Essentials for NX Designers

Student Guide
October 2009
MT10051_S — NX 7

Publication Number
mt10051_s NX 7
Proprietary and restricted rights notice

This software and related documentation are proprietary to Siemens Product

Lifecycle Management Software Inc.
© 2009 Siemens Product Lifecycle Management Software Inc. All Rights
Reserved.
All trademarks belong to their respective holders.

2 Essentials for NX Designers mt10051_s NX 7

Contents

Course overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15
Course objectives . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15
How to use this manual . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Lesson format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Activity format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Learning tips . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Common symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17
NX 7 Help Library . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17
Template parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
Teamcenter Integration for NX vs. native NX terminology . . . . . . . . . . . 19
Layer standards . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20
Implementing a layer standard . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20
Student responsibilities . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21

NX part files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-1

New file overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-2
Benefits of using templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-3
Use a template to create a new file . . . . . . . . . . . . . . . . . . . . . . . . 1-4
Save an unnamed template . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-5
Layers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-6
Activities: NX part files — Create new . . . . . . . . . . . . . . . . . . . . . . . . . . 1-7
Save As . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-8
Close selected parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-9
Exit NX . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-10
Activities: NX part files — Open, save, and close . . . . . . . . . . . . . . . . . . 1-11
Project: NX part files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-11
Summary: NX part files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-12

The NX user interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-1

Customize and display toolbars . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-2
Display toolbars . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-2
Display toolbars using the shortcut menu . . . . . . . . . . . . . . . . . . 2-3
Add or remove toolbar buttons . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-4
Access options on undocked toolbars . . . . . . . . . . . . . . . . . . . . . . 2-5
Command Finder overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-6
Search for a command . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-7
Dialog boxes and the Dialog Rail . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-8
Dialog Rail buttons . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-9

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Selection bar . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-10

Save toolbar configuration between sessions . . . . . . . . . . . . . . . . . . . . . 2-10
Roles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-11
Example roles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-11
Choose a role . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-11
Activities: User interface — Toolbars and Roles . . . . . . . . . . . . . . . . . . 2-12
Using the mouse . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-13
View shortcut menu . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-14
Radial menus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-16
Graphics window view manipulation . . . . . . . . . . . . . . . . . . . . . 2-17
Selecting objects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-19
Preview selection . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-21
QuickPick . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-22
Activities: User Interface — Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-23
Summary: User interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-24

Coordinate systems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-1

Overview of coordinate systems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-2

Absolute coordinate system . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-3
Work coordinate system . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-3
WCS options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-4
WCS Dynamics overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-5
Exit WCS Dynamics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-5
Move and orient the WCS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-6
Activities: Coordinate systems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-8
Summary: Coordinate systems . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3-9

Sketch Task Environment . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-1

Establishing design intent and a modeling strategy . . . . . . . . . . . . . . . . 4-2

Activities: Sketch creation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-3
Internal and external sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-4
Internal and external sketch status change . . . . . . . . . . . . . . . . . 4-5
Create points in Sketcher . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-6
Selection bar Snap Point options . . . . . . . . . . . . . . . . . . . . . . . . . 4-7
Activities: Sketch Profile . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-8
Activities: Fillet, Quick Trim, Quick Extend, Make Corner . . . . . . . . . . . 4-9
Constraints overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-10
Degree of Freedom Arrows . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-11
Geometric Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-12
Create geometric Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . 4-13
Geometric constraint types . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-14
Show All and Show No Constraints . . . . . . . . . . . . . . . . . . . . . . 4-16
Show and Remove Constraints . . . . . . . . . . . . . . . . . . . . . . . . . 4-17
Show and Remove Constraint options . . . . . . . . . . . . . . . . . . . . 4-18
Activities: Geometric constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-19

4 Essentials for NX Designers mt10051_s NX 7

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Dimensional constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-20

Sketch dimension types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-21
Inferred Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-22
Create Inferred Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-23
Edit sketch dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-24
Sketch Dimensions dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . 4-25
Retain Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-26
Attach Dimension overview . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-27
Attach a dimension . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-27
Convert To and From Reference . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-28
Convert curves and dimensions to reference . . . . . . . . . . . . . . . . 4-29
Sketch evaluation and update techniques . . . . . . . . . . . . . . . . . . . . . . . 4-30
Deleting or suppressing sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-30
Create Inferred Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-31
Activities: Dimensional constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-32
Project: Sketch Task Environment . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-32
Summary: Sketch Task Environment . . . . . . . . . . . . . . . . . . . . . . . . . . 4-33

Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-1

Expressions overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-2

Expression examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-2
Expressions case sensitivity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-3
Expressions dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-4
Creating expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-5
Create a numerical expression . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-5
Edit an expression . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-6
Listing expressions associated with features . . . . . . . . . . . . . . . . . . . . . . 5-7
List Referencers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-7
Insert Name . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-8
Parameter entry options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-8
Expression options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-9
Activities: Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-10
Project: Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-10
Summary: Expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5-11

Datum features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-1

Datum Plane overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-2

Datum plane types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-3
Datum plane options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-3
Applications for datum planes . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-4
Create a datum plane offset at a distance . . . . . . . . . . . . . . . . . . . . . . . . 6-5
Create a datum plane at an angle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-6
Create a bisector datum plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-7
Create a tangent datum plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-8
Create a datum plane through three points . . . . . . . . . . . . . . . . . . . . . . . 6-9

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Activities: Datum features — Relative . . . . . . . . . . . . . . . . . . . . . . . . . 6-10

Datum Axis overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-11
Datum axis types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-12
Datum axis options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-12
Applications for datum axes . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-13
Create a datum axis through two points . . . . . . . . . . . . . . . . . . . . . . . . 6-14
Create datum axis at an intersection . . . . . . . . . . . . . . . . . . . . . . . . . . 6-15
Create a datum axis on a curve or face axis . . . . . . . . . . . . . . . . . . . . . . 6-16
Datum CSYS overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-17
Activities: Datum features — cylindrical faces and other datums . . . . . 6-18
Project: Datum features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-18
Summary: Datum features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6-19

Swept features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-1

Types of swept features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-2

Extrude overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-3
Extrude start and end distances . . . . . . . . . . . . . . . . . . . . . . . . . 7-4
Create a simple extruded feature . . . . . . . . . . . . . . . . . . . . . . . . . 7-5
Body type . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-6
Revolve overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-7
Revolve start and end angles . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-8
Specifying vectors using the OrientXpress tool . . . . . . . . . . . . . . . 7-8
Create a simple revolved feature . . . . . . . . . . . . . . . . . . . . . . . . . 7-9
Activities: Swept features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-10
Project: Swept features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-10
Summary: Swept features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7-11

Part structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-1

Part Navigator overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-2

Main panel . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-2
Dependencies panel . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-3
Details panel . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-3
Preview panel . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-4
Timestamp order . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-5
Part Navigator shortcut menu . . . . . . . . . . . . . . . . . . . . . . . . . . 8-6
Feature Replay overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-8
Reorder feature overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-9
Feature and object information . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-10
Referenced expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-11
List referenced expressions . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-11
Measure Distance overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-12
Find the minimum distance between two objects . . . . . . . . . . . . 8-13
Measure Bodies overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-14
Assign a material to a solid body . . . . . . . . . . . . . . . . . . . . . . . . 8-15
Delayed updates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-16

6 Essentials for NX Designers mt10051_s NX 7

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Activities: Part structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-17

Summary: Part structure . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8-18

Using sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-1

Edit sketches with drag . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-2
Drag to assist sketch constraints . . . . . . . . . . . . . . . . . . . . . . . . . 9-3
Activities: Drag sketch objects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-4
Alternate Solution . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-5
Use Alternate Solution on tangent constraints . . . . . . . . . . . . . . . 9-6
Use Alternate Solution on a dimension . . . . . . . . . . . . . . . . . . . . 9-7
Activities: Alternate solutions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-8
Reattach a sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-9
Reattach a sketch on plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-10
Reorder an object in the Part Navigator . . . . . . . . . . . . . . . . . . . 9-11
Activities: Reattach sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-12
Sketcher Mirror Curve . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-13
Mirror sketch curves . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-13
Activities: Mirror sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-14
Project: Using sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-14
Summary: Using sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9-15

Trim Body . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-1

Trim Body overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-2
Trim a body . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-3
Activities: Trim Body . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-4
Summary: Trim Body . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10-5

Swept feature options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-1

Selection Intent . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-2
Curve rule options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-3
Curve collection modifiers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-4
Extrude start and end limits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-5
Extrude with offset . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-6
Two sided offset examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-7
Example: Start Offset Zero, End Offset Positive . . . . . . . . . . . . . 11-7
Example: Start Offset Zero, End Offset Negative . . . . . . . . . . . . 11-7
Example: Start Offset Negative, End Offset Positive . . . . . . . . . 11-7
Single-sided offset examples . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-8
Example: Offset value too large . . . . . . . . . . . . . . . . . . . . . . . . . 11-8
Example: Smaller positive offset . . . . . . . . . . . . . . . . . . . . . . . . 11-8
Example: Negative offset . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-9
Extrude with draft . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-10
Positive and negative draft angles . . . . . . . . . . . . . . . . . . . . . . 11-11
Draft and the extrude direction . . . . . . . . . . . . . . . . . . . . . . . . 11-11
Draft example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-12

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Example: Draft with offset . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-12

DesignLogic parameter entry options . . . . . . . . . . . . . . . . . . . . . . . . . 11-13
Reference existing parameters . . . . . . . . . . . . . . . . . . . . . . . . . 11-14
Activities: Swept feature options . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-15
Project: Swept features options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-15
Summary: Swept feature options . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11-16

Hole features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-1

Hole overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-2
Hole dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-3
Hole position and direction options . . . . . . . . . . . . . . . . . . . . . . 12-4
Hole form and dimension options . . . . . . . . . . . . . . . . . . . . . . . . 12-5
Create a general hole . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-6
Activities: Hole features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-7
Project: Hole features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-7
Summary: Hole features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12-8

Shell . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-1
Shell overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-2
Create a shell . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-3
Assign alternate thicknesses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-4
Shell options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-5
Selection Intent face rules . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-7
Activities: Shell . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-8
Project: Shell . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-9
Summary: Shell . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13-10

Associative copies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-1

Instance Feature overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-2
Instance array caveats . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-2
Instance array methods . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-3
Rectangular array . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-4
Rectangular array parameters . . . . . . . . . . . . . . . . . . . . . . . . . . 14-4
Create a rectangular array . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-5
Rectangular array example . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-5
Circular array . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-6
Circular array parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-6
Create a circular array . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-7
Circular array example . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-8
Activities: Associative copies — instance arrays . . . . . . . . . . . . . . . . . . 14-9
Mirror Body overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-10
Create a mirrored body . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-11
Edit a mirrored body . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-11
Mirror Body options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-12
Activities: Associative copies — mirror . . . . . . . . . . . . . . . . . . . . . . . . 14-13

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Project: Associative copies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-13

Summary: Associative copies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14-14

Edge operations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-1

Edge Blend overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-2

Edge Blend dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-3
Edge Blend preview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-4
Add New Set . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-5
Activities: Edge operations — blends . . . . . . . . . . . . . . . . . . . . . . . . . . 15-6
Chamfer overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-7
Create a Chamfer . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-8
Chamfer options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-9
Activities: Edge operations — chamfers . . . . . . . . . . . . . . . . . . . . . . . 15-10
Project: Blends and chamfers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-10
Summary: Edge operations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15-11

Introduction to Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-1

Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-2
Subassembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-2
Component objects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-3
Component parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-3
Introduction to assembly load options . . . . . . . . . . . . . . . . . . . . . . . . . . 16-4
Part Versions group . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-4
Load states . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-5
Scope group . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-6
Load Behavior . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-7
Reference Sets . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-7
Assembly Navigator . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-8
Node display . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-8
Icons and check boxes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-9
Assemblies application . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-10
Activities: Assemblies — load options and navigator . . . . . . . . . . . . . . 16-11
Select components in the Assembly Navigator . . . . . . . . . . . . . . . . . . . 16-12
Identify components . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-12
Select components using QuickPick . . . . . . . . . . . . . . . . . . . . . . . . . . 16-13
Design in context . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-14
The Displayed Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-14
Change Window dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-15
The work part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-16
Associativity between components and assemblies . . . . . . . . . . 16-16
Assembly Navigator shortcut menu . . . . . . . . . . . . . . . . . . . . . . . . . . 16-17
Pack and Unpack . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-17
Make Work Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-17
Make Displayed Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-17
Display Parent . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-17

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Activities: Assemblies — more navigator options . . . . . . . . . . . . . . . . 16-18

Save the work part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-19
Save . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-19
Save Work Part Only . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-19
Summary: Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16-20

Adding and constraining components . . . . . . . . . . . . . . . . . . . . . . 17-1

General assembly concepts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-2

Assemblies toolbar . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-2
Use the bottom-up construction method . . . . . . . . . . . . . . . . . . . 17-3
Add Component overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-4
Add components to an assembly . . . . . . . . . . . . . . . . . . . . . . . . 17-5
Activities: Adding and constraining components — create assembly . . . 17-7
Move Component overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-8
Assembly Constraints overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-9
Assembly Constraint types . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-10
Create a Touch Align constraint . . . . . . . . . . . . . . . . . . . . . . . . 17-11
Create a Concentric constraint . . . . . . . . . . . . . . . . . . . . . . . . 17-12
Create a Distance constraint . . . . . . . . . . . . . . . . . . . . . . . . . . 17-13
Create a Fix constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-14
Create a Parallel constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-15
Create a Perpendicular constraint . . . . . . . . . . . . . . . . . . . . . . 17-16
Create an Angle constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-17
Create a Center constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-18
Create a Bond constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-19
Create a Fit constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-20
Activities: Adding and constraining components — constrain . . . . . . . 17-21
Project: Assembly constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17-21
Summary: Adding and constraining components . . . . . . . . . . . . . . . . . 17-22

Introduction to Drafting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-1

Master model concept . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-2

Drawings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-3
New Sheet overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-4
Create a new drawing sheet . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-4
Open a drawing sheet . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-4
Edit a drawing sheet . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-5
Delete a drawing sheet . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-5
Activities: Drafting — Create drawings . . . . . . . . . . . . . . . . . . . . . . . . 18-6
Change drawing display to monochrome . . . . . . . . . . . . . . . . . . . . . . . . 18-7
View Preferences . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-8
Hidden Lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-8
Smooth Edges . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-8
Base View overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-9
Base View options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-10

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Projected View overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-11

Projection lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-12
Preview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-12
Projected View options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-13
Edit the style of an existing view . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-14
Drag views on a drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-14
Delete views on a drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-14
Activities: Drafting — add views . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-15
Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-16
Annotation Preferences . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-16
Dimension preferences and placement . . . . . . . . . . . . . . . . . . . 18-17
Annotation placement options . . . . . . . . . . . . . . . . . . . . . . . . . 18-18
Snap Point options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-18
Placement cues for dimensions . . . . . . . . . . . . . . . . . . . . . . . . 18-18
Append text to a dimension . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-19
Change text orientation and text arrow placement . . . . . . . . . . 18-19
Move a dimension . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-19
Editing an existing dimension . . . . . . . . . . . . . . . . . . . . . . . . . 18-20
Change the precision of a dimension . . . . . . . . . . . . . . . . . . . . 18-20
Inherit preferences from an existing dimension . . . . . . . . . . . . 18-20
Activities: Drafting — dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-21
Creating notes and labels . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-22
Helper lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-22
Create a note . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-23
Create a label . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-23
Edit an existing note or label . . . . . . . . . . . . . . . . . . . . . . . . . . 18-24
Create a Master Model Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-25
Activities: Drafting — Notes and labels . . . . . . . . . . . . . . . . . . . . . . . 18-26
Project: Drafting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-26
Summary: Drafting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18-27

Editing models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-1

Editing parametric models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-2

Synchronous modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-3
Move Face overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-4
Move Face options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-6
Resize Blend overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-7
Optimize Face overview . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-8
Activities: Editing models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-9
Summary: Editing models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19-11

Practice projects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-1

Practice Project 1 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-2

Practice Project 2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-3
Practice Project 3 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-4

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Practice Project 4 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-6

Practice Project 5 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-8
Practice Project 6 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-10
Practice Project 7 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-12
Practice Project 8 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-14
Practice Project 9 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-16
Practice Project 10 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-18
Practice Project 11 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-19
Practice Project 12 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-21
Practice Project 13 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-23
Practice Project 14 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-25
Practice Project 15 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-27
Practice Project 16 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-28
Practice Project 17 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-30
Practice Project 18 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-32
Practice Project 19 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-34
Practice Project 20 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-36
Practice Project 21 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-38
Practice Project 22 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-40

Expression operators . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-1

Operators . . . . . . . . . . . . . . .. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-2
Precedence and associativity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-3
Legacy unit conversion . . . . .. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-4
Built-in functions . . . . . . . . .. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-5
Scientific notation . . .. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-5

Point options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . C-1

Point dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . C-2
Point types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . C-3
WCS and absolute coordinates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . C-4

Primitive solids . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . D-1

Primitive solids . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . D-2
Block . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . D-3
Cylinder . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . D-4

Features with predefined shapes . . . . . . . . . . . . . . . . . . . . . . . . . . E-1

Boss . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-2
Slot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-3
Rectangular slot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-3
Other slot types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-4
Thru slot . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-4
Pocket . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-5
Rectangular pocket . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-5

12 Essentials for NX Designers mt10051_s NX 7

 Contents

Pad . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-6
Rectangular pad . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-6
Groove . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-7
Positioning a Groove . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-7
Positioning methods . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-8
Horizontal . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-8
Vertical . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-9
Perpendicular . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-10
Point onto Line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-10
Parallel . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-11
Point onto Point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-11
Parallel at a distance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-12
Line onto line . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-13
Angular . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-14
Edit positioning . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-15
Add dimension . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-16
Edit dimension value . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-16
Delete dimension . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-17
Display dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . E-17

Customer Defaults . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . F-1

Customer Defaults . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . F-2
Customer Defaults levels . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . F-3
Setting Customer Defaults . . . . . . . . . . . . . . . . . . . . . . . . . . . . F-5
Customer Defaults environment variables . . . . . . . . . . . . . . . . . F-6
USER, GROUP, and SITE directories . . . . . . . . . . . . . . . . . . . . F-7
Managing your changes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . F-8
Updating to a new release of NX . . . . . . . . . . . . . . . . . . . . . . . . F-9

Custom Roles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . G-1

User-Defined Roles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . G-2
Create a User Role . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . G-3
Activity: Create a User Role . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . G-5
Edit a User Role . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . G-7
Create a Group Role . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . G-8
Activity: Create a Role Palette with a Group Role . . . . . . . . . . . . . . . . G-10
Protected Roles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . G-13

Legacy mating conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-1

Mating Constraint types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-2
Selecting objects . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-2
Mate constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-3
Align constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-4
Angle constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-5
Parallel constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-6

Essentials for NX Designers 13

Contents

Perpendicular constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-7

Center constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-8
Create a Center constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-9
Distance constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-10
Tangent constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-10
Mating Conditions dialog box . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-11
Define mating constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-13
Degree of freedom indicators . . . . . . . . . . . . . . . . . . . . . . . . . . H-13
Vary Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-14
List Errors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-15
Tree listing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-16
Suppress/Unsuppress . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-16
Mating constraint shortcut menu . . . . . . . . . . . . . . . . . . . . . . . H-17
Mating condition shortcut menu . . . . . . . . . . . . . . . . . . . . . . . H-18
Reposition Component . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-19
Transform types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-20
Transform options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-21
Collision options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . H-22
Repositioning components using drag handles . . . . . . . . . . . . . H-23
Activities: Legacy mating conditions . . . . . . . . . . . . . . . . . . . . . . . . . . H-24

Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Index-1

14 Essentials for NX Designers mt10051_s NX 7

Course overview

Intended audience
This course is suited for designers, engineers, manufacturing engineers,
application programmers, NC programmers, CAD/CAM managers, and
system managers who need to manage and use NX.

Prerequisites

There are no prerequisites for this class.

Course objectives
After successfully completing this course, you should be able to:
• Open and examine NX models.

• Create and edit parametric solid models.

• Create and modify basic assembly structures.

• Create and modify simple drawings.

Essentials for NX Designers 15

Course overview

How to use this manual

The following guidelines describe how you can get the most benefit from your
use of the course guide and the accompanying HTML activities.

Lesson format

The general format for lesson content is:

• Instructor presentation

• One or more activities

• Project
Projects allow you to test your new skills without detailed instruction.
Consult your instructor for additional information.

• Summary

Activity format

Activities have the following format:

1. This is an example of a step. Numbered steps specify the actions you
will perform.
Action bullets detail how to complete the step.

Always read the Cue and Status information while working through
activities and as you perform your regular duties.

As you gain skills you may need only to read the step text to complete
the step.

Learning tips

• Ask questions.

• Confirm important facts by restating them in your own words.

It is important to use your Student Guide in the sequence it is written.

16 Essentials for NX Designers mt10051_s NX 7

 Course overview

Common symbols

The student manual uses special symbols as shown below.

Design Intent – Information about the task and what must be
accomplished.

Tip — Useful information or advice.

Note — Contains useful information that supplements or emphasizes

the main points.

Example — Shows a possible way that the current topic of discussion

could be used.

Caution — Contains important reminders or information about a task.

Warning — Contains information essential to your success.

NX 7 Help Library

The NX 7 Help Library is available online any time you need more
information about a function. To access the NX 7 Help Library; from the NX
menu choose Help→Documentation.
Throughout this course, specific online help paths may be displayed to help
you locate additional information.
The path names will be displayed in the following manner.
See Also:

NX Essentials→Introduction to NX→Using NX

Essentials for NX Designers 17

Course overview

Template parts
Template parts are an effective tool for establishing customer defaults or any
settings that are part-dependent (saved with the part). This may include
non-geometric data such as:
• A frame of reference, such as a datum coordinate system

• Commonly used expressions

• An initial application such as Modeling, Drafting, or Sheet Metal

• Part attributes, for example, attributes for a parts list

• Drawing formats

• User-defined views

• Layer categories

Choose a template from the New dialog box.

18 Essentials for NX Designers mt10051_s NX 7

 Course overview

Teamcenter Integration for NX vs. native NX terminology

Teamcenter Integration for NX Term Native NX Term
Item Part
Item revision Part revision
Dataset Part file
Item ID Part number
UGMASTER dataset Master part file
UGPART dataset Non-master part file
(specification or manifestation) (for example, a drawing or
manufacturing file)

When you work in NX, you manipulate parts, part revisions and part files.
These correspond to items, item revisions, and datasets in Teamcenter
Integration for NX and Teamcenter.

Essentials for NX Designers 19

Course overview

Layer standards
Parts used in this course were created using layer categories the same as or
very similar to those found in the Model template parts.
Layers provide an advanced alternative to display management (Show and
Hide) to organize data.

Layer categories in the Model template parts

Layers Category Description
1–10 Solids Solid bodies
11–20 Sheets Sheet bodies
21–40 Sketches All external sketches
41–60 Curves Non-sketch curves
61–80 Datums Planes, axes, coordinate systems
81–255 No category assigned

Implementing a layer standard

You may implement or enforce layer standards using some of the methods
below:
• Create NX Open programs to create a standard part organization and
verify it upon release.

• Use a macro to create layer categories: Tools→Macro→Playback.

• Your administrator can enforce company standards by providing suitable

templates.

In this course you may use a layer organization method you anticipate
using in your work.

20 Essentials for NX Designers mt10051_s NX 7

 Course overview

Student responsibilities
• Be on time.

• Be considerate of the needs of other students.

• Listen attentively and take notes.

• Ask questions.

• Practice what you learn.

• Have fun!

Essentials for NX Designers 21

 1
Lesson

1 NX part files

Purpose

This lesson is a fundamental introduction to working with NX part files.

Objectives
Upon completion of this lesson, you will be able to:
• Start an NX session.

• Create a new part file.

• Open a part file.

• Copy a part file.

• Close a part file and exit NX.

Essentials for NX Designers 1-1

 NX part files

1
New file overview
Use the New command to select a template and create a new product file.
• Standard templates are available and grouped by types, such as modeling,
drawing, simulation, and manufacturing.

• Use blank templates to create files with no custom content.

• When you create a new file from a template, it has a copy of all the objects
in the template and inherits all its settings.

• Your system administrator can create customized templates based on the

requirements at your site.

After you create the file, NX starts the appropriate application based on the
template. For example, if you select a modeling template, NX will start
Modeling.
A default name and location for the new file is assigned based on customer
default settings for each template type.
You can change the name and location:
• Before you begin work on the file.

• In native mode only, when you save the file for the first time.

You can specify a master part to reference when you create a new non-master
file.

Where do I find it?

Application Gateway

Toolbar Standard→New
Menu File→New

1-2 Essentials for NX Designers mt10051_s NX 7

 NX part files

1
Benefits of using templates

• Easy to use and help to enforce company standards.

• Automatically start the appropriate application.

• Simplify using master models by defining a master part reference as you

create a new file.

Essentials for NX Designers 1-3

 NX part files

1
Use a template to create a new file

1. On the Standard toolbar, click New .

2. Click the tab for the file type you want (1).

3. Select the template you want (2).

4. (Optional) Type the name and path information (3).

You can also type this information when you save the file.

1-4 Essentials for NX Designers mt10051_s NX 7

 NX part files

1
Save an unnamed template

1. On the Standard toolbar, click Save .

2. In the Parts to Name group, notice the name of the file for which you
must provide a name.
If you choose File→Save All, all unnamed parts will be listed. You
can provide new names for each one individually.

3. In the Name box, type the new name and press Enter.

4. Optionally, use the browse buttons to help to define the name and/or
folder.

5. Click OK.

Essentials for NX Designers 1-5

 NX part files

1
Layers
Use layers to organize geometry.
Use layer categories to organize and name layers.
To access the Layer Settings dialog box, choose Format→Layer Settings.
There are 256 layers in NX, one of which is always the work layer.
You can assign any of the layers to one of four classifications of status:
• Work
• Selectable
• Visible Only
• Invisible

The work layer is the layer that objects are created on and is always visible
and selectable.
When you create a new part file, layer 1 is the default work layer.
When you change the work layer, the previous work layer automatically
becomes selectable. You can then assign it a different status.
The number of objects on one layer is not limited. You may choose which
layers to create objects on and what the status will be.

Layer categories in the Model template parts

Layers Categories Description
1–10 Solids Solid bodies
11–20 Sheets Sheet bodies
21–40 Sketches All external sketches
41–60 Curves Non-sketch curves
61–80 Datums Planes, axes, coordinate systems
91–255 No category assigned

1-6 Essentials for NX Designers mt10051_s NX 7

 NX part files

1
Activities: NX part files — Create new
In the NX part files section, do the activity:
• Create new part files

Essentials for NX Designers 1-7

 NX part files

1
Save As
File→Save As allows you to save the current part under a different name
and/or in a different directory.
When you select Save As, a file selection dialog box displays asking for the
new name and location.
The name/location must be unique within the current directory. If you
specify a name that already exists, an error message displays. The current
part is filed under the new name, and the new part file name displays on
the graphics window.

1-8 Essentials for NX Designers mt10051_s NX 7

 NX part files

1
Close selected parts
1. Choose File→Close→Selected Parts.

2. In the Close Part dialog box, select parts to close from a list.

3. Click OK.

Essentials for NX Designers 1-9

 NX part files

1
Exit NX
End an NX session by choosing File→Exit.
If you modified any parts and did not save them, you get a warning message.

1-10 Essentials for NX Designers mt10051_s NX 7

 NX part files

1
Activities: NX part files — Open, save, and close
In the NX part files section, do the activity:
• Open, save, and close existing part files

Project: NX part files

In the Projects section, complete the Parts exercise.

Essentials for NX Designers 1-11

 NX part files

1
Summary: NX part files
In this lesson you:
• Started an NX session.

• Created, opened, and saved part files.

• Copied a part file.

• Closed a part file.

1-12 Essentials for NX Designers mt10051_s NX 7

Lesson

2 The NX user interface

2

Purpose

This lesson introduces the NX user interface.

Objectives
Upon completion of this lesson, you will be able to:
• Customize toolbars.

• Save and restore toolbars by applying a role.

• Select objects in the graphics window.

• Manipulate the orientation of the work view.

Essentials for NX Designers 2-1

 The NX user interface

Customize and display toolbars

• Each application has its own set of toolbars. You can hide or display
available toolbars for each application.
2 • You can either display or hide available buttons for each toolbar.

• For each toolbar you can add buttons from other toolbars, or remove them.

• You can save and share toolbar arrangements for all or selected
applications, using Roles.

Docking toolbars
• You can dock toolbars horizontally or vertically in the NX window.

• You can move undocked toolbars on your screen.

Display toolbars

1. Choose Tools→Customize from the main menu bar.

2. On the Toolbars (1) page, select check boxes (2) to display toolbars and
clear to hide them.
Select Text Below Icon (3) to display names on the buttons.

2-2 Essentials for NX Designers mt10051_s NX 7

 The NX user interface

Display toolbars using the shortcut menu

1. Right-click anywhere in the toolbar area (1) to display a shortcut menu of

all toolbars.

2. Select the listed toolbar names to display toolbars or clear the check boxes
2
to hide them (2).
Empty check boxes are not displayed beside menu items that are
not selected.

You can also select Customize (3) to open the Customize dialog box.

Essentials for NX Designers 2-3

 The NX user interface

Add or remove toolbar buttons

Toolbar options are an efficient way to turn on and off the display of buttons
within a toolbar.
2 1. Click Toolbar Options on a toolbar and select Add or Remove Buttons.

2. Select a toolbar to modify, or select Customize to open the Customize

dialog box.

3. Click an item with no check box to display it. Clear the check box to hide
an item.

2-4 Essentials for NX Designers mt10051_s NX 7

 The NX user interface

Access options on undocked toolbars

Access toolbar options on undocked toolbars as shown below.

Essentials for NX Designers 2-5

 The NX user interface

Command Finder overview

Use the Command Finder command to find and activate a specific NX
command that is associated with one or more words or phrases that you enter.
2 This includes commands that may not be active in the current application
or task environment.
From the list of commands you can:
• Display the command location, when it is available in the current
environment.

• Launch the command, if it is available.

• Turn on a toggle command, when it is available in the current environment

• Access the Help information for the command.

Where do I find it?

Application Gateway

Toolbar Standard→Command Finder

Menu Help→Command Finder

2-6 Essentials for NX Designers mt10051_s NX 7

 The NX user interface

Search for a command

1. On the Standard toolbar, click Command Finder , or choose

Help→Command Finder.
2
2. In the Search box, type one or more words or phrases.

3. Click Find Command or press Enter.

4. Place the cursor over any command presented in the Matches for list.

If the command is available for immediate use, the correct menu path or
toolbar button is highlighted.

5. (Optional) Click any available command in the list to immediately

activate it.

6. (Optional) Right-click a command in the list and choose Help to display

additional information about the command.

Essentials for NX Designers 2-7

 The NX user interface

Dialog boxes and the Dialog Rail

Dialog boxes that open when you choose an NX command are positioned by
default on a Rail Clip which slides on a Dialog Rail.
2 To position the Rail Clip along the Dialog Rail, either drag the center of the
Rail Clip or click the arrows to move it to default positions.

Dialog boxes are organized into groups that can be collapsed or expanded as
needed. These groups contain different types of information and options
The typical workflow is to interact with the dialog box from the top to the
bottom.

If you need to see behind the dialog box, either slide the Rail Clip to either
side or click the center of the Rail Clip to temporarily hide the dialog box.
Click again to show it.

2-8 Essentials for NX Designers mt10051_s NX 7

 The NX user interface

Dialog Rail buttons

Consistent options appear on the Rail Clip or on the dialog box title bar when
the dialog box is not clipped to the Dialog Rail.
2

Rail Clip buttons

Move Left Moves the dialog box along the Dialog Rail to
predefined positions.
Move Right

Clip Clips or unclips the dialog box to the Rail Clip.

Unclip When a dialog box is clipped, you can position
it by sliding the Rail Clip along the Dialog Rail
or by clicking the arrows to move the Rail Clip
to predefined locations.
When it is unclipped, the dialog box floats, and
you can position it anywhere on the screen by
dragging its title bar.
Reset Resets dialog box input values to the default
values. When editing a feature, the default
values are the values used when the feature was
created.
Hide Collapsed Shows or hides all dialog box groups that are
Groups currently collapsed.
Show Collapsed This simplifies the display of the dialog box.
Groups
Close Closes the dialog box.

Essentials for NX Designers 2-9

 The NX user interface

Selection bar
The Selection bar consolidates various selection options in a convenient
location.
2
The Selection bar provides the following types of options:
• Selection options to specify types of objects to select, for example, features
only, instead of faces, edges, bodies.

• Selection Intent options to determine how surfaces or curve segments

are chained together.

• Snap Point options to control the locations the cursor snaps to.

• Annotation placement options, available in the Drafting application.

The options that appear in the Selection bar will vary depending on the
command you are using.

Save toolbar configuration between sessions

When you exit an NX session, the current state of your toolbars is saved by
default. They will be the same when you start a new session.
You can control how this is saved:
1. Choose Preferences→User Interface.

2. On the Layout page, select Save layout at exit.

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 The NX user interface

Roles
As you define your own roles, you or your administrator can add them to a
palette for others to share.
2
Roles let you control the appearance of the user interface in a number of
ways. For example:
• The items displayed on the menu bar

• The buttons displayed on the toolbars

• Whether button names are displayed below the buttons

Example roles

NX comes with a number of example roles. These give you a choice of starting
points as you customize toolbars to meet your needs.
The roles palette includes these groups:
• System Defaults — generic roles for new and advanced users

• Industry Specific — examples of configurations for various industries

• User — exists after you save one or more personal configurations

For those starting to use NX or those who use NX infrequently, one of

the Essentials roles in System Defaults is recommended.
For more information about any role, hold your cursor over its button.

Choose a role

1. In the Resource bar, click the Roles tab to display the palette.

2. Click the role you want or drag it into the graphics window.

3. Click OK to accept the new role.

Essentials for NX Designers 2-11

 The NX user interface

Activities: User interface — Toolbars and Roles

In the NX user interface section, do the activities:
• Customize toolbars
2

• Create a new user role

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 The NX user interface

Using the mouse

There are three mouse configurations in common use.

On a two-button mouse, use the left (1) and right (3) buttons together when
you need the middle button.
On a three-button mouse, you can use combinations of mouse buttons.
• Use middle (2) plus right (3) buttons to pan.

• Use middle (2) plus left (1) buttons to zoom.

Mouse Button Action

Left mouse button (1) Select or drag objects.
Middle mouse button Click OK while in an operator.
(2)
Press and hold down while in the graphics window
to rotate the view.
Hold down Shift and the middle mouse button to
pan.
Hold down Ctrl and the middle mouse button to
zoom in or out.
Right mouse button (3) Display shortcut menu with various functions. Also
display action information for currently selected
objects.
Rotating mouse wheel Zoom in and out in graphics window. Scroll in lists,
(2) menus, and the Information window.

Here is a summary of things you can do by moving the mouse cursor.

Over buttons on a Display Balloon Help for the button.
toolbar
Over buttons in a Display the button name.
dialog box
Over objects, features Pre-highlight objects based on the Selection Type
or components in Filter.
graphics window

Essentials for NX Designers 2-13

 The NX user interface

View shortcut menu

Right-click in the background of the graphics window to display the View
shortcut menu (1). This menu lists frequently used NX commands.
2 The Selection MiniBar (2) is a compact version of the Selection bar that
displays in the graphics window whenever the View shortcut menu is
in use. This provides convenient access to selection options close to
your cursor location.

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 The NX user interface

Option Description
Refreshes the entire graphics window. Erases temporary
Refresh
display entities.
Fits the entire part to the view. Utilizes the fit percentage
Fit found in the Preferences→Visualization→Screen dialog
2
box.
Zoom Fits the view to a user specified rectangle.
Rotate Activates the rotate mode to rotate the view with the cursor.
Pan Activates pan mode to pan the view with the cursor.
Rendering Specifies the method of shading and hidden edges in which
Style the model is displayed.
Displays the current view in a canned view orientation. The
Orient View original visualization settings and view modifications are
retained. Active only in modeling view.
Set Rotate Defines a point about which the model is rotated. The point
Point may be defined on a curve, edge, face, or point in space.
Clear Rotate Removes a rotate point that was previously set.
Point
Undo Removes the effect of the last single operation performed.

Essentials for NX Designers 2-15

 The NX user interface

Radial menus

Radial menus provide quick access to frequently used options and commands.
When you press and hold down the right mouse button, depending on your
2 cursor location or selection, a radial menu displays up to eight buttons that
surround the cursor location.
These buttons differ depending what is beneath the cursor. As you learn the
position of the buttons, just moving the mouse in the appropriate direction
will choose the option.

1. Shaded
2. Shaded with Edges
3. Studio
4. Fit
5. Wireframe with Dim Edges
6. Face Analysis

You can also use the View toolbar to access the view commands found in
the view shortcut menu.

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 The NX user interface

Graphics window view manipulation

You can rotate the view by dragging with the middle mouse button. Release
the mouse button to stop rotating.
If the cursor is near the boundary of the graphics window, you can use 2
inferred rotation about a horizontal, vertical, or normal axis.
If the cursor is in the middle of the graphics window, the axis of rotation is
determined by the direction in which you drag the cursor.

Other options to manipulate the view orientation are described below.

Orient View button Modifies the orientation of a specified view to a

predefined view. Changes only the alignment of the
view, not the view name. This option can be invoked
from the View toolbar or from the shortcut menu.
Home key Orients the current view to Trimetric.
End key Orients the current view to Isometric.
Orients the current view to a selected planar face
or datum plane or the planar view (top, front, right,
F8 key
back, bottom, left) that is closest to the current view
orientation.

Essentials for NX Designers 2-17

 The NX user interface

View triad
Select an axis of the view triad to restrict middle mouse button dragging to
rotation about that axis only.
2

Click the middle mouse button, press Esc, or click the rotation triad origin
handle to return to normal rotation.

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 The NX user interface

Selecting objects

Use the Selection bar to identify the types of objects you want to select.

2
You may either select an object first and then choose a command to perform,
or, choose a command first and then select the required object.
The selection Type Filter allows you to control which type of objects you can
select. The content of the list changes with the active NX command.

The General Selection Filters allow you to further restrict what type of
objects you can select.

You can use toolbar options to add many additional buttons to the Selection
bar.

Essentials for NX Designers 2-19

 The NX user interface

If you right-click an object, a shortcut menu appears with commands for

the object type.
The cursor must be over the object, and the object must be highlighted.
2
The shortcut menu changes depending on the object. The following shortcut
menu is for a typical feature.

Options also vary with the application (Modeling, Drafting,

Manufacturing, etc.)

If you move the cursor over an object, then press the right mouse button and
hold, a radial menu appears.
The radial menu changes depending on the object. The following radial menu
is for a typical feature.

Deselecting objects

You can deselect and object by holding the Shift key as you click it.
To deselect all objects in the graphics window, press the Esc (Escape) key.

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 The NX user interface

Preview selection

Objects are highlighted in the preview selection color as the selection ball
passes over them.
By default, Preview Selection is enabled. Turn it off by choosing 2
Preferences→Selection from the menu bar.
The color of preview highlighting is determined by the Preselection setting
found under Preferences→Visualization→Color Settings.
When you hold the Shift key, the preselection color is applied to currently
selected objects that you can deselect.

Essentials for NX Designers 2-21

 The NX user interface

QuickPick

When you select objects, more than one object will often be within the selection
ball. QuickPick provides easy browsing through selection candidates.
2 If there is more than one selectable object at the selection ball location
and the cursor lingers for a short period of time, the cursor changes to a
QuickPick indicator:

This cursor display indicates that there is more than one selectable object at
that position. Click after the cursor changes to display the QuickPick dialog
box.

You can change the amount of time the cursor must be stationary for
the QuickPick indicator to appear.
• Choose Preferences→Selection.

• In the QuickPick group, change the Delay value (in seconds).

Use the middle mouse button to cycle through the items in the list and
then click when the desired object is highlighted.
Use the buttons in the dialog box to filter the list to include object types:
• All
• Construction
• Features
• Body objects
• Components
• Annotations

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 The NX user interface

Activities: User Interface — Views

In the NX user interface section, do the activity:
• Change the view display
2

Essentials for NX Designers 2-23

 The NX user interface

Summary: User interface

In this lesson you:
• Modified the location and contents of toolbars.
2
• Applied a role to restore saved toolbar settings.

• Manipulated the work view orientation.

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Lesson

3 Coordinate systems

Purpose 3
This lesson introduces the coordinate systems that are used in NX.

Objectives
Upon completion of this lesson, you will be able to:
• Describe the differences between the absolute coordinate system (ABS)
and the work coordinate system (WCS).

• Move the WCS.

• Obtain geometry information relative to the WCS.

Essentials for NX Designers 3-1

 Coordinate systems

Overview of coordinate systems

You can define planes and coordinate systems for constructing other geometry.
These planes and coordinate systems are completely independent of the
viewing direction. You can create geometry on planes that are not parallel
to the screen.
A three-axis symbol is used to identify a coordinate system. The intersection
of the axes is called the origin of the coordinate system. The coordinate values
of the origin are X=0, Y=0, and Z=0. The figure below illustrates that, starting
3 at the origin, the positive direction of each axis is represented by a line.

This lesson describes the following coordinate systems:

• Absolute coordinate system (ACS)

• Work coordinate system (WCS)

3-2 Essentials for NX Designers mt10051_s NX 7

 Coordinate systems

Absolute coordinate system

The absolute coordinate system, or model space, has the location and
orientation coordinate of a datum CSYS and the working coordinate system
in use when a new Model template is opened. The datum CSYS in the
template is actual model geometry; however, the absolute coordinate system
is a conceptual location and orientation.
Other coordinate systems may be defined, but one particular coordinate
system, called the work coordinate system or WCS, is used for construction.
You can always return the WCS to the absolute coordinate system in any
3
part, regardless of whether any geometric coordinate system exists with that
location and orientation.

Work coordinate system

You can locate and orient the WCS anywhere in model space.
The WCS is not itself a geometric entity; however, it can be positioned on
an existing coordinate system entity.
The WCS axes have identifying colors. X is red, Y is green, and Z is blue.
WCS axes also have the letter C appended to the axis name.

You must consider the location and orientation of the WCS when you:
• Create a fixed datum plane or fixed datum axis.

• Create a rectangular instance array.

Essentials for NX Designers 3-3

 Coordinate systems

WCS options
You can access WCS options from the Utility toolbar or by choosing
Format→WCS on the menu bar.
Options available to manipulate the WCS include:

Specify the location without changing the

Origin
orientation.

3 Dynamics
Use handles to adjust the origin and
orientation.

Rotate Specify rotations in a dialog box

Use a dialog box with Dynamic, Absolute,

Orient
Current View, and several other methods.

Change XC Use a dialog box with several options to specify

Direction the XC axis.

Change YC Use a dialog box with several options to specify

Direction the YC axis.

Display Show or hide the WCS.

Create a CSYS geometry entity at the current

Save
WCS origin and orientation.

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 Coordinate systems

WCS Dynamics overview

Use WCS Dynamics to manipulate the location and orientation of the WCS.
You can enter WCS Dynamics at any time and it supports the Undo function.

1 Translation
2 Rotation
3 Origin
3

Where do I find it?

Toolbar Utility→WCS Dynamics

Menu Format→WCS→Dynamics
Shortcut menu Double-click the WCS in the graphics window

Exit WCS Dynamics

You can exit WCS Dynamics mode in one of these ways:

• Click the middle mouse button.
• Press Esc.
• On the Utility toolbar, click WCS Dynamics .

Essentials for NX Designers 3-5

 Coordinate systems

Move and orient the WCS

Move the WCS (freeform)

1. Place the cursor over the origin handle (cube-shaped) on the WCS.

2. Drag the WCS to any location.

Move the WCS origin to a point

1. (Optional) Use the Snap Point options on the Selection bar to enable one
3 or more point selection methods.

2. Indicate the snap or screen position to which you want to move the WCS.

You can also use the Point Constructor .

The WCS moves to the specified point.

Drag the WCS along an axis

1. Place the cursor over any of the three translation handles on the WCS.

2. Drag the WCS in either direction along the axis.

Move the location of the WCS along an axis using an on-screen input box
1. Place the cursor over any of the three translation handles and click.

2. Type a value in the on-screen input box.

3. Press Enter.

Rotate the WCS

1. Place the cursor over any of the three rotation handles.

2. Drag to rotate the WCS around its axis.

On-screen input boxes indicate current angle and snap increment.

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 Coordinate systems

Orient the WCS to an object

1. Select one of the WCS axes.

2. Select an object, such as an edge, to which you want to align the WCS.
To specify a vector, in the WCS Dynamics dialog bar, click Vector

Constructor .

The WCS orients to be parallel with the object, without changing the
origin coordinates. 3
Reverse the direction of the WCS
To flip the WCS 180 degrees:
• Double-click one of the WCS axes.

Essentials for NX Designers 3-7

 Coordinate systems

Activities: Coordinate systems

In the Coordinate Systems section, do the activity:
• Move the working coordinate system (WCS)

3-8 Essentials for NX Designers mt10051_s NX 7

 Coordinate systems

Summary: Coordinate systems

The absolute coordinate system is a stationary coordinate system that defines
a fixed point in model space while the work coordinate system (WCS) is a
mobile coordinate system that may be moved and reoriented as necessary
to support other commands.
In this lesson you:
• Identified the difference between the absolute coordinate system and
the work coordinate system.
3
• Relocated, rotated, and reoriented the WCS.

• Obtained geometry information relative to the WCS.

Essentials for NX Designers 3-9

3
Lesson

4 Sketch Task Environment

Purpose

This lesson introduces the methods of creating a sketch.

Objectives

Upon completion of this lesson, you will be able to: 4

• Identify design intent and a modeling strategy

• Create a sketch.

• Create sketch curves.

• Apply dimensional constraints to sketches.

• Apply geometric constraints to sketches.

• Identify constraints.

• Convert sketch curves and constraints to reference status.

Essentials for NX Designers 4-1

 Sketch Task Environment

Establishing design intent and a modeling strategy

Before creating a parametric model, you should first establish the design
intent of the part. This is an important step that will determine the modeling
strategy to use and should be a standard practice.
There are two items to consider when establishing design intent:
• Design considerations
– What are the functional requirements of the part?

– What are the relationships between features on the part?

• Potential areas for change

– What portions of the model are subject to change?
4
– What is the scope of the changes? (Do you expect drastic topology
changes?)

– Will the model be copied and modified for other projects?

Design intent can be based on a number of factors:

• Known information

• Form, fit, and function requirements

• Manufacturing requirements

• External equations

The design intent will determine the modeling strategy and the following
types of tasks.
• Selecting feature types (features, feature operations, sketches)

• Establishing feature relationships (size, attachment, position, order)

• Defining sketch constraints

• Creating expressions (equations, conditions)

• Establishing relationships between parts (interpart expressions, linked

geometry)

It is possible to add design intent to a model after the initial

construction. However, the amount of rework will depend on the
modeling techniques originally used.

4-2 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Activities: Sketch creation

In the Sketch Task Environment section, do the activities:
• Create a sketch on a datum CSYS

4
• Sketch creation

Essentials for NX Designers 4-3

 Sketch Task Environment

Internal and external sketches

Sketches that you create from within NX commands like Variational Sweep,
Extrude, or Revolve are internal sketches. The owning feature manages
access to, and the display of, internal sketches. Use internal sketches when
you want to associate the sketch with only one feature.
In the following example, the sketch is only made visible when the
owning feature, in this case a Revolved feature, is activated.

Sketches that you create independently using the Sketch command are
external sketches, and are visible and accessible from anywhere within a
part. Use an external sketch to keep the sketch visible and to use it in more
than one feature.

Differences between internal and external sketches

• Internal sketches are visible in the graphics window only when you edit
the owning feature.

• You cannot open an internal sketch directly from the Sketcher task
environment unless you first make the sketch an external feature.

• You can view external sketches in the graphics window and open them for
editing without first opening the owning feature.

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 Sketch Task Environment

Internal and external sketch status change

Use this procedure to change the status of a sketch from internal to external
and vise versa.
To make an internal sketch external.
1. In the Part Navigator, select the owning feature of the sketch.

2. Right-click and choose Make Sketch External.

The sketch is placed before its former owner in timestamp order.

In the following navigator view, the external sketch is the fourth
feature in the list, SKETCH_VS, and the owning feature, Variational
Sweep, is fifth.
4

To reverse this operation, right-click the owning feature and choose Make
Sketch Internal.
When you internalize the sketch, it no longer appears in the Part Navigator.
Note that the Variational Sweep is now the fourth feature.

Essentials for NX Designers 4-5

 Sketch Task Environment

Create points in Sketcher

The Sketcher Point command provides you with a standard way to specify
points with the Point dialog box.
You can create points using existing geometry and in three dimensional space.
However, if you create a point off of the sketch plane, the system projects
that point back onto the sketch plane.
You can control point creation in sketcher by using the snap point
options on the Selection bar.

Where do I find it?

4 Task environment Sketcher

Toolbar Sketch Tools→Point

Menu Insert→Datum/Point→Point

4-6 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Selection bar Snap Point options

Button Name Description

Use this to turn the snap point options
Enable Snap Point
on and off.
Select end points of lines, arcs, conics,
End Point
splines, and all edge types.
Select mid points of lines, open arcs,
Mid Point
and all edge types.
Select a control point of a geometric
Control Point
object.
Select a point at the intersection of two
Intersection Point
curves. 4
Arc Center Select an arc center point.
Select one of four quadrant points of a
Quadrant Point
circle.
Existing Point Select an existing point.

Point on Curve Select a point on a curve.

Point on Surface Select a point on a surface.

Select a tangent point on circles, conics,
Tangent Point
and solid edges.
Select the intersection point of two
Two-curve
objects that do not fit within the
Intersection
selection ball by selecting two objects.
Point Constructor Open the Point dialog box.

Essentials for NX Designers 4-7

 Sketch Task Environment

Activities: Sketch Profile

In the Sketch Task Environment section, do the activity:
• Create a sketch profile

4-8 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Activities: Fillet, Quick Trim, Quick Extend, Make Corner

In the Sketch Task Environment section, do the activities:
• Create sketch fillets

4
• Quick Trim, Quick Extend, Make Corner

Essentials for NX Designers 4-9

 Sketch Task Environment

Constraints overview
Sketcher tools let you fully capture your design intent through geometric and
dimensional relationships that we refer to collectively as constraints.
Use constraints to create parameter-driven designs that you can update
easily and predictably.
Sketcher evaluates constraints as you work to update geometry without any
conflicts.
A fully constrained sketch has as many constraints as there are
degrees-of-freedom in the sketch, so that there can be no ambiguity in the
final shape.
While it is not required, we recommend that you fully constrain
sketches that define feature profiles.
4
Sketcher also offers you the flexibility to create as many, or as few, constraints
as your design requires. That means you can use Sketcher to create wireframe
drawings that can serve a wide variety of up-front design purposes, and are
not meant for downstream processing.

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 Sketch Task Environment

Degree of Freedom Arrows

Degree of Freedom Arrows (DOF) mark the points on your sketch curves
that are free to move.
These arrows can assist you in constraining a sketch by showing you the
directions you need to constrain for each point. When you constrain a
point from moving in a direction, the DOF arrow is removed. When all
degree-of-freedom arrows are removed, the sketch is fully constrained.
In the following example there are three types of positional DOF.

• Point one (1) is free to move in the X direction, horizontal.

• Point two (2) is free to move in the Y direction, vertical.

4
• Point three (3) is free to move in both the X and Y directions. In some
cases, the point is free to move in either X or Y directions but is limited by
a constraint. For example, a point with a Point on Curve constraint on a
line is only allowed to move along the direction of the line.

Essentials for NX Designers 4-11

 Sketch Task Environment

Geometric Constraints
You can use the Constraints command to create the geometric rules used
to define the shape of your sketch.
Sketcher uses geometric constraints, along with any dimensional constraints,
when analyzing your sketch for feature creation. Design intent determines
the type of constraints used and the relationships created within each sketch.
Examples of geometric constraints:
• Define a line as being horizontal or vertical.

• Ensure that multiple lines remain parallel to each other.

4 • Require that several arcs have the same radius.

• Position your sketch in space or relative to outside objects.

Where do I find it?

Task environment Sketcher

Toolbar Sketch Tools→Constraints

Menu Insert→Constraints
Right-click over a sketch curve and choose Add
Shortcut menu Constraints

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 Sketch Task Environment

Create geometric Constraints

1. On the Sketch Tools toolbar, click Constraints .

You can create multiple geometric constraints without reentering
the command by holding the Ctrl key while selecting the objects to
be constraints.

2. In the graphics window, select the sketch objects you want to constrain.
You can reverse step one and two and get the same results, use
what works best for you.

3. On the Constraints dialog bar, click one of the constraint options or

right-click the selected sketch objects and choose the constraint type from
the list.
4
4. Click Constraints or the middle mouse button to exit the command.

Essentials for NX Designers 4-13

 Sketch Task Environment

Geometric constraint types

Automatically created when the Recipe
Trim
Curve command is used.
Constrains two or more points as having the
Coincident
same location.
Constrains two or more linear objects as lying
Collinear on or passing through the same theoretical
straight line.
Constrains two or more circular or elliptical
Concentric
arcs as having the same center.
Constrains a line at the current angle without
Constant Angle
input of an angular value.
Constrains a line at the current length
Constant Length
without input of a length value.
4 Constrains two or more lines as being the
Equal Length
same length.
Constrains two or more arcs as having the
Equal Radius
same radius.
Defines fixed characteristics for geometry,
depending on the type of geometry selected.
Fixed These characteristics are unchangeable.
You can apply a fixed constraint to an
individual sketch point or to an entire object.
Creates sufficient fixed constraints to
Fully Fixed completely define the position and orientation
of sketch geometry in one step.
Constrains a line parallel to the sketch
Horizontal
X-axis.
Constrains the location of a point as
equidistant to the two end points of a line or
Midpoint a circular arc
Select the curve anywhere other than
at its end points.
Automatically created when the Sketcher
Mirror
Mirror Curve command is used.

Automatically created when the Offset Curve

Offset
command is used.

Constrains two or more linear objects or

Parallel
ellipses parallel to each other.
Constrains two linear objects or ellipses
Perpendicular
perpendicular to each other.

4-14 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Constrains the location of a point as lying on

Point on Curve
the path or projection of a curve.
Constrains the location of a point as lying on
Point on String
an extracted string.
Scales a spline in the horizontal direction
while keeping the original dimensions in the
Non-Uniform vertical direction during modification.
Scale You can not apply a Scale constraint to
a spline if any of its interior defining
points are constrained.
Scales a spline proportionally in both the
Uniform Scale horizontal and vertical when the horizontal
length changes.

Slope of Curve
Constrains a spline, selected at a defining
point, and another object as being tangential
4
to each other at the selected point.
Constrains two objects as being tangent to
Tangent
each other.
Constrains a line as being parallel to the
Vertical
sketch Y-axis.

Essentials for NX Designers 4-15

 Sketch Task Environment

Show All and Show No Constraints

The Show All Constraints command displays all geometric constraints

applied to an active sketch.

To hide all the constraint symbols, click Show No Constraints .

Unless Show No Constraints is on, you always see these constraint
symbols on an active sketch:

Coincident Concentric Midpoint

4
Point on
Tangent
Curve

If your sketch view is zoomed out, some symbols may not display. Zoom
in to see them, or clear the Dynamic Constraint Display check box on
the Session Settings page of the Sketch Preferences dialog box.

Where do I find it?

Task environment Sketcher

Sketch Tools→Show All Constraints Show No

Toolbar Constraints
Tools→Constraints→Show All Constraints/ Show No
Menu Constraints

4-16 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Show and Remove Constraints

The Show/Remove Constraints command displays geometric constraints

that are associated with selected sketch geometry or an entire sketch feature.
Show and Remove Constraints is often used as a tool to interrogate sketch
objects and resolve issues.
Use Show and Remove Constraints to:
• Familiarize yourself with existing constraints.

• You can remove existing geometric constraints.

• You can list all the geometric constraints associated to your sketch.
4
• Assist with sketch interrogation to resolve over constrained or conflicting
conditions.

• You can maintain design intent by checking for existing relationships to

outside features or objects.

Where do I find it?

Task environment Sketcher

Toolbar Sketch Tools→Show/Remove Constraints

Menu Tools→Constraints→Show/Remove Constraints

Essentials for NX Designers 4-17

 Sketch Task Environment

Show and Remove Constraint options

Show/Remove Constraints
Controls which constraints are listed in the Show
Constraints list window.
Selected Object lets you select only one object at
a time, this includes any adjacent curves that are
coincident or tangent to the selected object.
List Constraints for
Selected Objects lets you select multiple objects
by selecting them one by one, or at once using the
rectangle selection method.
All in Active Sketch lists all the constraints in the
active sketch.
4 Constraint Type
Filters the type(s) of constraints that are displayed
in the list.
Determines whether the specified constraint type
Include or Exclude is the only type displayed in the list. Include is the
default.

You can filter the constraints listed based on the

creation method.
Explicit displays all constraints created explicitly
or implicitly by the user.
Inferred displays all inferred coincident constraints
that are automatically created during curve
creation.
Show Constraints
Both displays both explicit and inferred types of
constraints.
Show Constraints list window lists the geometric
constraints of the selected sketch geometry.
Inferred coincident constraints create during curve
construction are appended with an "I" symbol in
parenthesis.
Remove
Removes one or more selected constraints.
Highlighted
Removes all of the listed constraints displayed in
Remove Listed
the show constraints list window.
Displays information about all geometric
Information constraints. This option is useful if you want to
save or print the constraint information.

4-18 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Activities: Geometric constraints

In the Sketch Task Environment section, do the activity:
• Add geometric constraints

Essentials for NX Designers 4-19

 Sketch Task Environment

Dimensional constraints
Dimensional constraints, also called sketch dimensions, establish the size
of a sketch object. You can establish the size of any sketch curve or the
relationship between two objects, such as the distance between two points.
Sketch dimensions, like drafting dimensions, have dimension text, extension
lines, and arrows. But with sketch dimensions if you change the dimension
constraint value, you also change the shape or size of the sketch objects. This
lets you control a feature derived from a sketch.
Sketch dimensions also create an expression you can edit in the Expressions
dialog box.

4-20 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Sketch dimension types

Sketch Dimension types
Infers a dimension type, based on the cursor position
Inferred
and the object(s) selected.
Creates a distance constraint parallel to the XC axis
Horizontal
between two points.
Creates a distance constraint parallel to the YC axis
Vertical
between two points.
Parallel Creates a distance constraint between two points.
Creates a perpendicular distance constraint from a
Perpendicular
line to a point.
Diameter Creates a diameter constraint for an arc or circle.
4
Radius Creates a radius constraint for an arc or circle.

Angular Dimensions an angle.

Creates a dimensions for the collected length of
Perimeter
selected curves.

Essentials for NX Designers 4-21

 Sketch Task Environment

Inferred Dimensions

The Inferred Dimensions command creates explicit dimensions, such as

horizontal or vertical, based on where you select sketch objects and how you
place the dimension.

Where do I find it?

Task environment Sketcher

Toolbar Sketch Tools→Inferred Dimensions

Menu Insert→Dimension
Right-click over a sketch curve and choose Add
Shortcut menu Dimensions

4-22 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Create Inferred Dimensions

1. Optional: Set your annotation preferences.

2. On the Sketch Tools toolbar, click Inferred Dimensions .

3. In the graphics window, select the sketch object(s) you want to dimension.

4. Drag the dimension preview and click to place it on the sketch.

5. Click Inferred Constraints or the middle mouse button to exit the

command.

Inferred Dimensions allow for the creation of many different kinds

of dimensions. 4
You can also create specific dimension types by selecting the dimension
type from the Inferred Dimensions list.

In the following example, you can dynamically edit the expression name
and value in the on-screen input box.

Essentials for NX Designers 4-23

 Sketch Task Environment

Edit sketch dimensions

Use this procedure to edit a sketch dimension using the on-screen input box.
1. In the graphics window, double-click the dimension.
You can also right-click over a dimension and choose Edit Value.

2. Edit the name or value in the on-screen input box.

To edit a formula value, click Launch the formula editor .

3. Press Enter.

To use the Dimensions dialog box options, on the

4
Dimensions dialog bar, click Sketch Dimensions Dialog .
To edit the dimension position, drag the dimension.

In the following example you can edit either the name of the sketch
dimension, a constant value, or a formula.
The name and value of a dimension may also be edited by using the
Expressions dialog box. As dimensions are edited, the constraints are
evaluated and the geometry is modified.

4-24 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Sketch Dimensions dialog box

Dimensions dialog box
Expressions List Lists the dimension’s name and value (p0=4.5).
Current Expression Edits the name and value of a selected dimension.
Remove Highlighted Deletes the currently selected dimension.

Value You can change the value of the selected dimensional

constraint by dragging the slider.
Dimension Placement Specifies where a dimension is placed:
• Auto Placement

• Manual Placement, Arrows In

4
• Manual Placement, Arrows Out
Leader Direction Specifies from which direction the leader extends
from the dimension text:
• Leader From Left

• Leader From Right

Fixed Text Height Maintains the text of dimensions at a constant size
when you zoom a sketch in or out.
If you clear the Fixed Text Height check box and zoom
in/out, the dimension text scales with the sketch
geometry.
Create Reference Use this to create reference (non-driving) dimensions.
Dimension
Create Alternate Used when you want to calculate the maximum
Angle dimension between sketch curves.

Essentials for NX Designers 4-25

 Sketch Task Environment

Retain Dimensions

Use this procedure to retain the display of your sketch dimensions outside
of the Sketcher task environment.
1. Enter the Sketcher task environment.

2. Choose Sketch→Sketch Style.

3. Select the Retain Dimensions check box.

4. Exit the Sketcher task environment.

Use the tips below when working with sketch dimensions outside of the
Sketcher.
4 • All of the sketch dimensions will be visible once you exit Sketcher.

• Use the Expressions dialog box to edit your sketch dimensions.

• Any edits made to the expression with update immediately, including any
dimensions or sketch data that has a relationship to the edited dimension.

4-26 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Attach Dimension overview

Use the Attach Dimension command to detach a dimension from the

geometry it references and attach it to different geometry.
You can:
• Retain the value of the expression and resize the target geometry to
match it.

• Measure the target geometry and assign that value to the expression.

Where do I find it?

Task Environment Sketcher 4

Toolbar Sketch Tools→Attach Dimension
Menu Tools→Constraints→Attach Dimension
right-click a sketch dimension and choose Attach
Shortcut menu Dimension

Attach a dimension

1. Right-click the dimension and choose Attach Dimension.

2. To select the dimension side to reattach, click the middle mouse button to
alternate between the default, Object 2, and Object 1.

3. In the Settings group, set the Expression Mode to Remove Expression,

Measure Geometry or Keep Expression, Adjust Geometry.

4. Select the new geometry.

Essentials for NX Designers 4-27

 Sketch Task Environment

Convert To and From Reference

The Convert To/From Reference command converts sketch curves and sketch
dimensions to and from reference status.
NX ignores reference curves in downstream operations like Extrude or
Revolve.
Reference dimensions update with any changes made to the parent features,
but do not control the curves they measure.
In the following example, the reference curves display in phantom line
font (1), the reference dimensions are displayed with no assigned name
(2) and with a different color then active sketch dimensions (3).

Where do I find it?

Task environment Sketcher

Toolbar Sketch Tools→Convert To/From Reference

Menu Tools→Constraints→Convert To/From Reference
Right-click over a sketch curve and choose Convert

Shortcut menu To/From Reference

4-28 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Convert curves and dimensions to reference

1. In the graphics window, select the sketch curves and/or dimensions.

2. From the Sketch Tools toolbar, click Convert To/From Reference .

You can also select objects in the graphics window, right-click and

choose Convert To/From Reference .

Use the same procedures to convert reference objects to active

objects. Perimeter dimensions cannot be converted to reference
objects.
To create sketch reference dimensions during creation, from the
4
Dimensions dialog bar, click Create Reference Dimension .

Essentials for NX Designers 4-29

 Sketch Task Environment

Sketch evaluation and update techniques

You would use this process to control when the system evaluates a sketch
for updating.

• Click Delay Evaluation .

• Create or edit sketch constraints or curves.

• Click Evaluate Sketch .

• Optional: To update the model while still in the sketcher, on the Sketcher

toolbar, click Update Model .

4 Update Model is not available when you use Edit with Rollback
to open your sketch for editing. However, all models are updated
as soon as you exit the sketcher.

Deleting or suppressing sketches

Since sketches are features, you can delete or suppress them.
From the menu bar:
• Choose Edit→Delete.

• Choose Edit→Feature→Suppress.

In the Part Navigator:

• Right click over any feature and choose Delete.

• To Suppress the feature, clear the feature check box .

In the graphics window, right click over the sketch and choose either Delete
or Suppress.

4-30 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Create Inferred Constraints

The Create Inferred Constraints command will either enable or disable
inferred constraints as you create or edit sketch geometry.
By default this option is turned on and creates the constraints defined in
the Inferred Constraints dialog box.
If you disable Inferred Constraints, you can take advantage of the constraints
as you work, but the actual constraints are not stored in your file.
When you preview a constraint, click the middle mouse button to lock the
constraint and prevent the sketch curve from moving in any other direction.
The settings for each sketch in a part file are saved.
4
Where do I find it?

Task environment Sketcher

Toolbar Sketch Tools→Create Inferred Constraints

Menu Tools→Constraints→Create Inferred Constraints

Essentials for NX Designers 4-31

 Sketch Task Environment

Activities: Dimensional constraints

In the Sketch Task Environment section, do the activities:

• Add dimensional constraints

4
• Constrain a profile

• Constraint conditions

Project: Sketch Task Environment

In the Projects section, complete the Sketch Task Environment exercise.

4-32 Essentials for NX Designers mt10051_s NX 7

 Sketch Task Environment

Summary: Sketch Task Environment

This lesson introduced the concept of creating a sketch.
Sketches may be used to define a base feature, guide paths, and additional
associative features to the base feature.
A sketch parametrically controls curves. It is defined on a sketch plane which
is fixed or associative to a datum plane or face of a model.
Constraints are applied to sketch objects in order to capture the design
intent. The number of constraints you choose to apply is determined by your
design intent.
In this lesson you:
• Created sketches on datum planes, solid faces, and a Datum CSYS.
4
• Created freehand curves in a sketch.

• Created and edited dimensional constraints.

• Created inferred and explicit geometric constraints.

• Converted sketch curves and dimensions to reference status.

Essentials for NX Designers 4-33

4
Lesson

5 Expressions

Purpose

This lesson introduces expressions which define characteristics of features.

Objectives
Upon completion of this lesson, you will be able to:
• Create expressions.

• Edit expressions.
5

Essentials for NX Designers 5-1

 Expressions

Expressions overview
Expressions are arithmetic or conditional formulas that define the
characteristics of features.
Software expressions are automatically created when you:
• Create a feature.

• Dimension a sketch.

• Position a feature.

• Constrain an assembly.

All expressions have a unique name and a formula that can contain a
combination of variables, functions, numbers, operators, and symbols.
Expression names are variables that you can insert in the formula strings
of other expressions. This can be used to break up lengthy formulas and to
define relationships that can be used in place of numbers.
5
Where do I find it?

Menu Tools→Expression
Shortcut menu Right-click an expression in the Part Navigator, either
in the Main panel or Details panel, and choose Edit in
Expression Editor
From supported Modeling dialogs, click parameter
entry options and choose Formula.

Expression examples

Here are some examples of expressions, their formulas and their resulting
values:

Expression Name Formula Value

length 5*width 20
p39 (Extrude(6) End Limit) p1+p2*(2+p8*sin(p3)) 18.849555921
p26 (Simple Hole(9) Tip Angle) 118 118

5-2 Essentials for NX Designers mt10051_s NX 7

 Expressions

Expressions case sensitivity

Expression names are not case sensitive, with the following exceptions:
• Expression names are case sensitive if their dimensionality is set to
Constant.
• Expression names are case sensitive if they were created before NX 3.

When expression names are case sensitive, the name must be spelled exactly
when used in other expressions.

Essentials for NX Designers 5-3

 Expressions

Expressions dialog box

(1) Listed Choose from User Defined, Named, Filter by
Expressions Name, Filter by Value, Filter by Formula,
Filter by Type, Unused Expressions, Object
Parameters, Measurements, and All
(2) Expression Columns for Name (followed by usage in the
list part), Formula, Value, Units, Type, Comment,
and Checks
(3) Accept Edit
(4) Reject Edit
(5) Less Options

5-4 Essentials for NX Designers mt10051_s NX 7

 Expressions

Creating expressions

• Software generated expressions are created for you automatically when

you create features and dimension sketches. They have the format p#,
where # represents a series of whole numbers.

• Enter user defined expressions in an on-screen input box as the name and
formula, separated by the equal symbol, for example Rad=5.00.

• In the Expressions dialog box, enter an expression name in the Name box
and the corresponding formula in the Formula box.

After you type the name of the expression, you may press the Tab, equal
sign, or Enter key to advance the cursor to the Formula box, or just
click in the Formula box.

Create a numerical expression

1. Choose Tools→Expression.

2. In the Name box, type the name of the expression and press Enter. 5
3. (Optional) Change the default values in the Dimensionality and Units
lists.

4. In the Formula box, type the formula for the expression and press Enter.

5. Click Apply or OK to save expression changes.

Essentials for NX Designers 5-5

 Expressions

Edit an expression

1. Choose Tools→Expression.

2. Select an expression to modify from the list.

3. Modify the Name, Formula, Dimensionality, or Units of the expression.

For software generated expressions, Dimensionality and Units are
not available for editing.

4. Press Enter or Accept Edit .

5. Click Apply or OK to save the expression.

When you edit the name of an expression, NX automatically updates

the formula of any expression that references it.

5-6 Essentials for NX Designers mt10051_s NX 7

 Expressions

Listing expressions associated with features

If Listed Expressions is set to All, all of the expressions in the part are listed.
If an expression defines a feature, the feature name is listed with it. For
example, p8 (Simple Hole(5) Diameter)
You can list all of the expressions associated with a feature in an Information
window:
• Choose Information→Feature and select the feature.

• Over a feature node in the Part Navigator, choose Information from the
shortcut menu.

List Referencers

The List Referencers command shows you if an expression is referenced in

another expression and what feature(s) use the expression.
Over a listed expression, from the shortcut menu, choose List Referencers.
5

Essentials for NX Designers 5-7

 Expressions

Insert Name
The Insert Name option places the name of a selected expression into a
formula you are editing.
Over a listed expression, from the shortcut menu, choose Insert Name.
Bold type on an option in the shortcut menu for an object, Insert Name
for an expression name, for example, means that the option in bold type
is preformed when you double-click the object.
When you are editing a formula, you can double-click a listed expression
to insert its name.

5
Parameter entry options
Access the Expressions dialog box as you create features by choosing
Formula from the parameter entry option menu.
You can specify a formula for the expression referenced by a feature
parameter.
Parameter entry options are available with most text input boxes.

5-8 Essentials for NX Designers mt10051_s NX 7

 Expressions

Expression options
Expression options that might be useful to you include:
Insert a math or engineering function
Functions
into your expression.
Measure the minimum distance between
Measure Distance
any two NX objects.
Remove a selected user-defined
Delete
expression.

You cannot delete an expression that is in use by a feature, sketch, assembly

constraint, etc.
Other options that appear in the Expressions dialog box are described
in the online Help, or in the course Intermediate NX Design and
Assemblies.

Essentials for NX Designers 5-9

 Expressions

Activities: Expressions
In the Expressions section, do the activity:
• Create and edit expressions

Project: Expressions
In the Projects section, complete the Expressions exercise.

5-10 Essentials for NX Designers mt10051_s NX 7

 Expressions

Summary: Expressions
Expressions are algebraic or arithmetic formulas that define the
characteristics of features.
In this lesson you:
• Created expressions.

• Edited expressions.

Essentials for NX Designers 5-11

5
Lesson

6 Datum features

Purpose

This lesson introduces the datum plane, datum axis, and datum CSYS
reference features.

Objectives

Upon completion of this lesson, you will be able to:

• Create a datum plane.

• Create a datum axis.

• Use datum features to position other features.

• Create a datum CSYS.

6

Essentials for NX Designers 6-1

 Datum features

Datum Plane overview

Use the datum plane command to create a planar reference feature to help
define other features, such as swept bodies and features at angles to the
faces of target solids.
Datum planes can be relative or fixed.
Relative datum planes reference curves, faces, edges, points, and other
datums. You can create relative datum planes across multiple bodies.
Fixed datum planes do not reference other geometry. Use any of the
relative datum plane methods to create fixed datum planes by clearing the
Associative check box in the Datum Plane dialog box.
You can also create fixed datum planes based on the WCS and absolute
coordinate system, or by using coefficients in an equation.

Where do I find it?

Application Modeling

Feature→Datum Plane
Feature Operation→General Datums and Points
Toolbar stack→Datum Plane
Menu Insert→Datum/Point→Datum Plane
Shortcut menu Right-click a planar face→Datum Plane

6-2 Essentials for NX Designers mt10051_s NX 7

 Datum features

Datum plane types

Select a plane type from the Type option list.

You can right-click the sizing handles, direction arrows, and points to
choose many of the following options.
When you edit a datum plane, you can change its type, defining objects,
and associative status.

Inferred Determine the best plane type to use based on objects

you select.
At Angle Create a datum plane using a specified angle.
At Distance Create a datum plane parallel to a planar face or another
datum plane at a distance you specify.
Bisector Create a datum mid way between two selected planar
faces or datum planes using the bisected angle.
Tangent Create a datum plane tangent to a non-planar surface,
and optionally a second selected object.

Datum plane options

Alternate Cycle through the possible different solutions for the 6

Solution plane, when an alternate solution to the previewed datum
plane is available.

Reverse Reverse the direction of the plane normal.

Plane Normal
Associative Clear this check box to create a fixed datum plane. If you
later edit a non-associative datum plane, it appears in
the Type list as Fixed.

Essentials for NX Designers 6-3

 Datum features

Applications for datum planes

• To define a sketch plane.

• To serve as the planar placement face for the creation of features with
predefined shapes.

• As a target edge for positioning features such as holes.

• For the mirror plane when using the Mirror Body and Mirror Featue
commands.

• To define the start or end limits when creating extruded and revolved
features.

• To trim a body.

• To define positioning constraints in assemblies.

• To help define a relative datum axis.

6-4 Essentials for NX Designers mt10051_s NX 7

 Datum features

Create a datum plane offset at a distance

1. On the Feature Operation toolbar, click Datum Plane , or choose

Insert→Datum/Point→Datum Plane.

2. In the Type group, click the At Distance button.

3. Select a planar face, datum plane, or plane.

4. Do one of the following:

• Click OK to accept a default value of 0 (zero).

• Type an offset value, press Enter, and click OK.

• Select the handle, drag the datum plane to the desired location and
click OK.

Inferred is the most commonly used datum plane type.

Essentials for NX Designers 6-5

 Datum features

Create a datum plane at an angle

1. Click Datum Plane .

2. In the Type group, expand the list and select At Angle.

3. Select a planar face, datum plane, or plane, to use as a reference for

measuring the angle.

4. Select a linear curve, edge, or datum axis, that defines the angle’s axis
of rotation.

5. Specify an angle using the on-screen input box or the drag handle.

6. Click OK.

6-6 Essentials for NX Designers mt10051_s NX 7

 Datum features

Create a bisector datum plane

1. Click Datum Plane .

2. In the Type group, expand the list and select Bisector.

3. Select a planar face.

4. Select a second planar face.

The faces do not need to be parallel.

5. Click OK.

Essentials for NX Designers 6-7

 Datum features

Create a tangent datum plane

1. Click Datum Plane .

2. In the Type group, expand the list and select Tangent.

3. (Optional) Specify a subtype; for example, Angle to Plane.

4. Select the required geometry for the subtype you chose.

5. (Optional) If it is available, click Alternate Solution until the correct

tangent datum plane is previewed.

6. Click OK.

6-8 Essentials for NX Designers mt10051_s NX 7

 Datum features

Create a datum plane through three points

1. Click Datum Plane .

2. In the Type group, expand the list and select Curves and Points.

3. In the Curves and Points Subtype group, expand the list and select
Three Points.

4. Set the snap point options as desired.

5. Select three points.

6. Click OK.

Essentials for NX Designers 6-9

 Datum features

Activities: Datum features — Relative

In the Datum features section, do the activity:
• Create relative datum planes

6-10 Essentials for NX Designers mt10051_s NX 7

 Datum features

Datum Axis overview

Use the datum axis command to define a linear reference to help you create
other objects, such as datum planes, revolved features, and circular arrays.
Datum axes can be either relative or fixed.
• A relative datum axis is associative to one or more other objects.

• A fixed datum axis is fixed in the position in which it was created. Fixed
datum axes are non-associative.
You can create a fixed datum axis using the XC, YC, and ZC axes of the
WCS, or by clearing the Associative check box when using one of the
relative axis types.

6
Where do I find it?

Application Modeling

Feature→Datum Axis
Feature Operation→General Datums and Points
Toolbar stack→Datum Axis
Menu Insert→Datum/Point→Datum Axis
Shortcut menu Right-click an edge or cylindrical face→Datum Axis

Essentials for NX Designers 6-11

 Datum features

Datum axis types

Select an axis type from the Type option list.

When you edit a datum axis, you can change its type, defining objects, and
associative status.
Inferred Determine the best datum axis type to use based on
objects you select.
Intersection Create a datum axis at the intersection of two planar
faces, datum planes, or planes.
Curve/Face Axis Create a datum axis on a linear curve or edge, or the axis
of a cylindrical or conical face or torus.
On Curve Vector Create a datum axis tangent, normal, or binormal to a
point on a curve or edge, or perpendicular or parallel to
another object.
Point and Create a datum axis from a point in a specified direction.
Direction
Two Points Create a datum axis by defining two points through which
the axis passes.

Datum axis options

6
Reverse Cycle through the possible directions for the axis normal.
Direction
Associative Clear this check box to create a fixed datum axis. 1

1. In the Part Navigator, an associative datum plane has the name Datum Axis, while a non-associative datum plane has the name
Fixed Datum Axis.

6-12 Essentials for NX Designers mt10051_s NX 7

 Datum features

Applications for datum axes

• Define an axis of rotation for revolved features.

• Define an axis of rotation for circular arrays.

• Define a relative datum plane.

• Provide a directional reference.

• Use as a target for feature positioning dimensions.

Essentials for NX Designers 6-13

 Datum features

Create a datum axis through two points

1. On the Feature Operation toolbar, click Datum Axis or choose

Insert→Datum/Point→Datum Axis.

2. In the Type group, click Two Points .

3. Set the snap point options as desired.

4. Select two different point locations.

5. Click OK.

6-14 Essentials for NX Designers mt10051_s NX 7

 Datum features

Create datum axis at an intersection

1. Click Datum Axis .

2. In the Type group, expand the list and select Intersection.

3. Select the planar faces, datum planes, or planes.

4. Click OK.

Essentials for NX Designers 6-15

 Datum features

Create a datum axis on a curve or face axis

1. Click Datum Axis .

2. In the Type group, from the option list, select Curve/Face Axis.

3. Select the linear curve or edge, or the axis of a cylindrical or conical face
or torus.

4. Click OK.

6-16 Essentials for NX Designers mt10051_s NX 7

 Datum features

Datum CSYS overview

Use the datum CSYS command to create an associative coordinate system
which consists of a set of reference objects. You can use the reference object to
associatively define the position and orientation of downstream features.
A datum CSYS consists of the following reference objects:
• A coordinate system

• Three datum planes

• Three datum axes

• An origin point

The datum CSYS appears as a single feature in the Part Navigator but its
objects can be selected individually to support the creation of other features,
to constrain sketches, and to position components in an assembly.

Where do I find it?

Application Modeling

Feature→Datum CSYS
Feature Operation→General Datums and Points
Toolbar stack→Datum CSYS
Menu Insert→Datum/Point→Datum CSYS
Shortcut menu Right-click edge or cylindrical face→Datum Plane

Essentials for NX Designers 6-17

 Datum features

Activities: Datum features — cylindrical faces and other datums

In the Datum features section, do the activities:
• Create datums on cylindrical faces

• Create an offset datum CSYS

Project: Datum features

In the Projects section, complete the Datums exercise.

6-18 Essentials for NX Designers mt10051_s NX 7

 Datum features

Summary: Datum features

Datums are reference features that you use to help construct other features
and sketches in locations and orientations where planar placement faces
do not exist.
In this lesson you:
• Created associative datum planes and datum axes.

• Used datum features to help position other features.

• Edited datum planes to see how associative features are affected.

• Created an associative datum CSYS.

Essentials for NX Designers 6-19

6
Lesson

7 Swept features

Purpose

This lesson introduces swept features that use a section string to define
a solid or sheet body.

Objectives
• Create an Extrude feature.

• Create a Revolve feature.

• Create a Sweep Along Guide feature.

• Combine bodies using a Boolean operation.

Essentials for NX Designers 7-1

 Swept features

Types of swept features

You create swept features by extruding, revolving, or sweeping a section
string. The section string may be composed of explicit curves, sketch curves,
edges, or faces.
Extrude – Sweep a section string (1) in a linear direction for a specified
distance.

Revolve – Rotate a section string (1) around a specified axis (2).

Sweep Along Guide – Sweep a section string (1) along a guide string (2).

Swept bodies are associative with both the section string and the guide string.
7

7-2 Essentials for NX Designers mt10051_s NX 7

 Swept features

Extrude overview
Use the Extrude command to create a body by sweeping a 2D or 3D section of
curves, edges, faces, sketches or curve features a linear distance in a specified
direction.

The example shows a section of curves (1) extruded (2) with threads added to
the final solid body (3).

Where do I find it?

Application Modeling

Toolbar Feature→Extrude 7
Menu Insert→Design Feature→Extrude
Shortcut menu Right-click sketch→Extrude

Essentials for NX Designers 7-3

 Swept features

Extrude start and end distances

To specify the start and end distances of an extrude feature:

• Use drag handles (1).
• Specify values in on-screen input boxes (2).
• Specify values in dialog boxes (3).

7-4 Essentials for NX Designers mt10051_s NX 7

 Swept features

Create a simple extruded feature

1. Click Extrude

2. Select a sketch, curves, or edges for the section.

Selection Intent is available.
The default direction of the extrude is normal to the plane of the section.

3. Specify Start and End limits by using the drag handles in the graphics
window or typing distance values.

4. Select a Boolean type.

To create a new solid body, select None.
To combine the feature with an existing solid body, select one of the other
Boolean types.

5. Click Apply or OK to create the extrude feature.

Essentials for NX Designers 7-5

 Swept features

Body type
You can use the Extrude and Revolve commands to create a solid body (1) or
a sheet body (2).

You create a solid body when you specify:

• a closed section with the Body Type option set to Solid.
• an open section with an offset.
• an open section and revolve a total angle of 360°.

You create a sheet body when you specify:

• a closed section with the Body Type option set to Sheet.
• an open section with no offset. For revolve, the total angle must be less
than 360°.

7-6 Essentials for NX Designers mt10051_s NX 7

 Swept features

Revolve overview
Use the Revolve command to create a feature by revolving section curves
sketches, faces, or edges of a face about a given axis through a nonzero angle.
The Revolve feature requires:
• A section (1)

• A location and direction for the rotation axis (2)

• Start and end angles

If the section crosses the axis of revolution you may get unexpected
results.

Where do I find it?

7
Application Modeling

Toolbar Feature→Revolve
Menu Insert→Design Feature→Revolve
Shortcut menu Right-click sketch→Revolve

Essentials for NX Designers 7-7

 Swept features

Revolve start and end angles

To specify the start and end angles of an revolve feature:

• Use drag handles (1).

• Specify values in on-screen input boxes (2).
• Specify values in dialog boxes (3).

Specifying vectors using the OrientXpress tool

7 Use the OrientXpress tool to quickly identify a principle axis.

The tool works in conjunction with NX commands that require an orientation

input. It will appear when you specify a vector for a revolve axis or an extrude
direction. You can select an axis on the tool to specify a vector.
You can move the tool by clicking one of the arrowheads and dragging it
to a new location.

7-8 Essentials for NX Designers mt10051_s NX 7

 Swept features

Create a simple revolved feature

1. Click Revolve .

2. Select a sketch, curves, or edges for the section.

Selection Intent is available.

3. Click the middle mouse button or click Specify Vector in the Axis group
in the dialog box.

4. Specify a rotation axis through one of the following:

• In the graphics window, select a curve, edge, relative datum axis or
plane about which to rotate the section.

• Define a rotation axis using vector methods or the Vector Constructor

in the Axis group in the dialog box. If the vector you specify does not
have an implied point, you may need to define one using Specify Point
or the Point Constructor.

5. Specify Start and End limits by using the drag handles in the graphics
window or typing angle values.

6. Select a Boolean type.

To create a new solid body, select None.
To combine the feature with an existing solid body, select one of the other
Boolean types.

7. Click Apply or OK to create the feature. 7

Essentials for NX Designers 7-9

 Swept features

Activities: Swept features

In the Swept features and Boolean operations section, do the activities:

• Extrude a sketch

• Revolve a sketch

• Sweep along an open guide

• Sweep along a closed guide

Project: Swept features

In the Projects section, complete the Swept features exercise.

7-10 Essentials for NX Designers mt10051_s NX 7

 Swept features

Summary: Swept features

Use swept features to define solid or sheet bodies using a section. A section
can be a sketch, or a collection of curves and face edges.
In this lesson you:
• Extruded a sketch.

• Revolved a sketch.

• Combined bodies using a Boolean operation.

• Swept sections along open and closed guide strings.

Essentials for NX Designers 7-11

7
Lesson

8 Part structure

Purpose

This lesson introduces tools to examine features, model construction, and

physical properties.

Objectives

Upon completion of this lesson, you will be able to:

• Access the Part Navigator.

• Replay model construction.

• Suppress and unsuppress features.

• Measure the distance between objects.

• Assign a material and calculate mass properties.

Essentials for NX Designers 8-1

 Part structure

Part Navigator overview

The Part Navigator displays your part in a detailed, graphical tree. Use the
Part Navigator to understand and update the part’s basic structure. You can
select and edit the parameters of items in the tree. You can rearrange how the
part is organized. You can view features, views, drawings, user expressions,
measurements, reference sets, cameras, and unused items in the tree.

To access the Part Navigator, click the tab on the Resource bar.
If the Resource is Bar is not visible, choose View→Show Resource
Bar to show it.

Main panel

Use the main panel to see an overall graphical representation of your part’s
structure, to edit the parameters of items, or to rearrange the feature history.
• Double-click nodes to edit the corresponding feature.

• Select features by their nodes during dialog box interactions.

• Right-click nodes for shortcut options.

• Select or clear green check boxes to control the suppression status of

features.

• Select or clear red check boxes to control the visibility of bodies.

8-2 Essentials for NX Designers mt10051_s NX 7

 Part structure

Dependencies panel

Use the Dependencies panel to view the parent-child relationships of the

feature geometry selected in the main panel.

Details panel

Use the Details panel to view, and in some cases edit, the parameters
belonging to the feature selected in the main panel.

Essentials for NX Designers 8-3

 Part structure

Preview panel

Use the Preview panel to see preview images of selected items in the main
panel.
The selected item must be one that has an available preview object,
such as a saved model view or drawing view.

8-4 Essentials for NX Designers mt10051_s NX 7

 Part structure

Timestamp order

Use Timestamp Order to display a linear listing of all features in the work
part as nodes in the order of their creation time stamp.
When Timestamp Order is inactive, the main panel is in the design view and
will include body nodes, reference sets, and unused features.

Essentials for NX Designers 8-5

 Part structure

Part Navigator shortcut menu

Right-click a feature node in the Part Navigator to display a feature specific

shortcut menu.
The options available depend on the type of feature you select.
Many options require the Modeling application to be active.

• Display Dimensions — Display the feature’s parameter values until you

refresh the display.

• Show Parents and Hide Parents — Display or hide parent curves,

sketches, or datums.

• Make Current Feature — Insert new features immediately after the

current feature.

• Select Whole Branch — Select the feature and all nodes with earlier
timestamps.

• Filter — Simplify the display tree by hiding features by type or timestamp

order.
To turn off a filter, place the cursor in the Part Navigator away from
a feature node, right-click and choose Apply Filter from the shortcut
menu to make it inactive.

• Edit Parameters — Edit the feature’s parameters, the same as

Edit→Feature→Edit Parameters.

• Edit with Rollback — Roll the model back to its state just before the
feature was created, and then open the feature’s creation dialog box.
Edit with Rollback is shown in bold type in the shortcut menu.
8 In any shortcut menu, the option in bold type is the default
double-click action.

• Suppress and Unsuppress — Temporarily remove and restore a feature

display from the part history.
A suppressed feature still affects some editing operations.

8-6 Essentials for NX Designers mt10051_s NX 7

 Part structure

• Reorder Before and Reorder After — Change the timestamp of features.

Creation order is important to permit use of a feature as a parent, and
in the Replace Feature command.
You can also drag nodes to valid locations.

• Group — Group features into a special collection called a Feature Set.

• Replace — Replace a feature’s definition by another feature.

• Make Sketch Internal and Make Sketch External — Internalize or

externalize a sketch that is a parent of the selected feature.

• Edit Sketch — Edit the parent sketch of the selected feature. This option
appears only when the feature has a parent sketch.

• Copy — Place a copy of a feature on a clipboard.

• Delete — Delete the selected feature, the same as Edit→Delete.

• Hide Body and Show — Hide or show the body containing the selected
feature.

• Rename — Append a user-defined name to the feature.

• Object Dependency Browser — Explore the parent and child

relationships of features.

• Information — Display information about the selected feature in the

Information window.

• Properties — Open the properties dialog box for the selected feature.
General properties include the feature name.
Attributes you assign appear in a column of the Part Navigator. See the 8
online Help for details.

Essentials for NX Designers 8-7

 Part structure

Feature Replay overview

Use the Feature Replay commands to review how features were used to
construct a model.

You can:
• Manually step through the features of a model using the commands on
the Feature Replay toolbar or Tools→Update menu.

• Play, pause, and select a starting feature for an uninterrupted replay of

the model using the Automatic Feature Replay command.

• Set a time-interval for each step in an automatic replay.

• Review features for problems during a feature replay, and fix them if
necessary. The feature on which you stop the replay automatically
becomes the current feature.

Feature Replay is not a feature validation tool. Use the Playback

command on the Insert→Feature menu for feature validation and
correction.

Feature Replay works by using the Part Navigator, Make Current Feature
command. If a feature does not appear in the Part Navigator, you cannot
step to it with Feature Replay.

Where do I find it?

Application Modeling
Toolbar Feature Replay
Menu Tools→Update→
Make First Feature Current
8 Make Previous Feature Current
Make Next Feature Current
Make Last Feature Current
Automatic Feature Replay

8-8 Essentials for NX Designers mt10051_s NX 7

 Part structure

Reorder feature overview

Use the Reorder Feature command to change the order in which a feature
is applied to a body. The desired feature can be reordered before or after
a selected reference feature.
As you create features, NX assigns a time stamp to each one. When you
modify a body, the update follows the order of the feature time stamps.

The example part consists of two extrusions, a blend, and a shell.

You can edit the part topology by moving the shell feature in the history
tree.

1. Extrude 1. Extrude 1. Extrude

2. Shell 2. Extrude 2. Extrude
3. Extrude 3. Shell 3. Edge Blend
4. Edge Blend 4. Edge Blend 4. Shell

Where do I find it?

Application Modeling

Toolbar Edit Feature→Reorder Feature

Menu Edit→Feature→Reorder
Right-click a feature node in the Part
Navigator→Reorder. 8
Shortcut menu In the Part Navigator, drag and drop feature nodes.

Essentials for NX Designers 8-9

 Part structure

Feature and object information

The Information menu offers a number of options to obtain information
about the model.

Information→Feature
Choose Information→Feature to open the Feature Browser dialog box. Use
this dialog box to identify parent/child relationships between a selected
feature and the other features in the model. You can display expressions that
control the feature in the graphics window by selecting Display Dimensions.
Click OK or Apply to display the Information window with the geometric data
and associated expressions.
Feature information may also be accessed by selecting the feature in the
Part Navigator and choosing Information from the shortcut menu, or by
selecting the feature in the graphics window and choosing Properties
from the shortcut menu.

Information→Object
This is used to display information about selected objects in an Information
window. Any type of geometric object may be selected including curves, edges,
faces, and bodies. The Information window displays information such as
name, layer, color, object type, and geometric properties (length, diameter,
start and end coordinates, etc.).

Information→Expression→List All
This lists all expressions in the part in the Information window. From the
Information window, you can print the listing or save it as a text file.

Information→Expression→List All by Reference

This is used to identify expressions that reference other expressions and
the features that they define. You can use the Edit→Find option on the
8 Information window menu bar to search for a specific expression.

8-10 Essentials for NX Designers mt10051_s NX 7

 Part structure

Referenced expressions
If an expression defines a feature directly, the feature name is listed with it in
the Expressions dialog box.
Any expression can be referenced by the formula of other expressions.
You can identify all referencing expressions by using List References in the
shortcut menu.

List referenced expressions

1. Choose Tools→Expression.

2. If necessary, change the Listed Expressions filter to list the expression.

3. Right-click the expression and choose List References.

An Information window lists the features and other expressions that
8
reference the selected expression.

Essentials for NX Designers 8-11

 Part structure

Measure Distance overview

Use the Measure Distance command to obtain the distance between any two
objects such as points, curves, planes, bodies, edges, faces, or components.
To specify units for distance measurements, choose Analysis→Units.

Where do I find it?

Application Gateway

Toolbar Utility→Measure Distance

Menu Analysis→Measure Distance

8-12 Essentials for NX Designers mt10051_s NX 7

 Part structure

Find the minimum distance between two objects

1. On the Utility toolbar, click Measure Distance or choose

Analysis→Measure Distance.

2. In the Measure Distance dialog box, from the Type list, select Distance.

3. In the Measurement group, from the Distance list, select Minimum.

4. Select the first point or object.

5. Select the second point or object.

A temporary ruler and measurement result are displayed in the graphics
window.
In the Results Display group, select the Show Information Window
check box to display result details in the Information window.

Essentials for NX Designers 8-13

 Part structure

Measure Bodies overview

Use the Measure Bodies command to calculate the volume, mass, surface
area, radius of gyration, weight, and centroid of selected bodies.
To specify units for body measurements, choose Analysis→Units.

There are two ways to assign a density to a solid body.

• Choose Tools→Material Properties and assign a material.

• Choose Edit→Feature→Solid Density.

The default density is specified in Modeling Preferences.

Where do I find it?

Application Gateway
Menu Analysis→Measure Bodies

8-14 Essentials for NX Designers mt10051_s NX 7

 Part structure

Assign a material to a solid body

1. Choose Tools→Material Properties.

The materials in the NX Material Library are listed by default. You may
create additional custom materials.

2. In the graphics window, select the solid body.

3. If the material is not listed in the Assign Material dialog box, expand the
Filters list and search for the material by name, category, or type.

4. In the Materials dialog box, select a material from the Materials list.

5. Click OK.

Essentials for NX Designers 8-15

 Part structure

Delayed updates
As you add features to your model, it may take noticeably longer to update.
You can delay updates until after edits are made.
From the main menu, choose Tools→Update→Delayed after Edit, or, on the

Edit Feature toolbar, click .

• If Delayed Update after Edit is inactive, the part is updated after the
completion of each edit operation. This is the default setting.

• If Delayed Update after Edit is active, feature updates are delayed while
edits are made.

When Delayed Update after Edit is active and edits are made, Update Model
is available.
Choose Tools→Update→Update Model, or, on the Edit Feature toolbar, click

.
The model is updated automatically when the part is saved.

8-16 Essentials for NX Designers mt10051_s NX 7

 Part structure

Activities: Part structure

In the Part structure section, do the activity:
• Examine part structure

Essentials for NX Designers 8-17

 Part structure

Summary: Part structure

In this lesson, you examined features, expressions, design intent, and
properties of a model. These skills are important to review models created by
other users.
In this lesson you:
• Accessed the Part Navigator.

• Identified expressions.

• Reviewed the model construction using Feature Replay, Suppress, and

Unsuppress.

• Measured a distance.

• Calculated mass properties.

8-18 Essentials for NX Designers mt10051_s NX 7

Lesson

9 Using sketches

Purpose

This lesson explains additional sketch editing methods.

Objectives
Upon completion of this lesson, you will be able to:
• Drag sketch objects

• Determine an alternate solution

• Reattach a sketch

• Mirror sketch curves

Essentials for NX Designers 9-1

 Using sketches

Edit sketches with drag

You can use drag to edit the location and shape of your sketch. You can drag
unconstrained sketch curves or points in unconstrained directions.
You can also use the Dimensions dialog box to edit a dimension by using
the value slider.
Techniques for editing sketch curves with drag.
• There is no dialog box for this command. You can just drag selected
objects in the graphics window.

• You can drag sketch curves that are partially constrained or

unconstrained.

• You can drag fully constrained sketches if they have not yet been
positioned.
When you drag constrained curves they are scaled as necessary to
preserve the constraints.

• You can apply Inferred constraints if you drag the free end of a line.

In the following example, L5 (1) is being dragged while L4 and L6

(2) stretch. L5 is constrained so it maintains its angular and length
relationship.

9-2 Essentials for NX Designers mt10051_s NX 7

 Using sketches

Drag to assist sketch constraints

You can drag curves to approximate the correct location before you constrain
them.
This is useful when constraining curves at their original location distorts the
sketch, making it difficult to continue.
The following example shows the distortion that can be caused when
you attempt to drag objects with too many applied constraints.

The following example shows the result of dragging an entire

unconstrained profile from one quadrant to another.

Essentials for NX Designers 9-3

 Using sketches

Activities: Drag sketch objects

In the Using sketches section, do the activity:
• Drag sketch geometry

9-4 Essentials for NX Designers mt10051_s NX 7

 Using sketches

Alternate Solution
The Alternate Solution command displays alternate solutions for both
dimensional and geometric constraints.
The number of alternate solutions provided will depend on the type of
constraints you have on your sketch.

Where do I find it?

Task Environment Sketcher

Toolbar Sketch Tools→Alternate Solution

Menu Tools→Constraints→Alternate Solution

Essentials for NX Designers 9-5

 Using sketches

Use Alternate Solution on tangent constraints

1. On the Sketch Tools toolbar, click Alternate Solution .

2. For Object 1, Select Linear Dimension or Geometry , select either the

line or arc.
If either curve does not have a tangency constraint you will not
be able to select the object. But you can select the geometry in
any order.

3. For Object 2, Select Tangent Geometry, select the corresponding line or

arc.
If the range of movement is limited to a single direction this step
may not be necessary.

4. Click Close.

In the following example, Alternate Solution was used to properly

create the fillet by modifying the tangent constraint.

9-6 Essentials for NX Designers mt10051_s NX 7

 Using sketches

Use Alternate Solution on a dimension

1. On the Sketch Tools toolbar, click Alternate Solution .

2. For Object 1, Select Linear Dimension or Geometry, select a sketch

dimension.
The change is immediate. Simply select the dimension again to
restore the previous solution.

In the following example, the sketch dimension p19 (1) was selected
and an alternate solution found. In this case the alternate solution was
to reverse the direction of the sketch curves (2).

Essentials for NX Designers 9-7

 Using sketches

Activities: Alternate solutions

In the Using sketches section, do the activities:
• Find an alternate solution for a dimension

• Find an alternate solution for a geometric constraint

9-8 Essentials for NX Designers mt10051_s NX 7

 Using sketches

Reattach a sketch
With the Reattach command you can move an existing sketch to a different
planar face, datum or path. You can also adjust the sketch orientation.
Use Reattach to:
• Move an existing sketch to a different plane, planar face, or path.
The target plane, face, or path must have an earlier timestamp
then the existing sketch.

• Switch a sketch in place to a sketch on path.

• Specify a new horizontal or vertical reference.

Where do I find it?

Task environment Sketcher

Toolbar Sketcher→Reattach
Menu Tools→Reattach

Essentials for NX Designers 9-9

 Using sketches

Reattach a sketch on plane

Use this procedure to reattach a sketch to a planar surface.

1. Open the target sketch for editing.

2. On the Sketcher toolbar, click Reattach .

3. Select the new target planar surface.

The preview sketch CSYS moves from the original face to the new
face.

4. Optional: Expand the Sketch Orientation group, from the Reference list,
choose either Horizontal or Vertical.

5. Optional: Click Select Reference and define the new reference direction

6. Click OK.

9-10 Essentials for NX Designers mt10051_s NX 7

 Using sketches

Reorder an object in the Part Navigator

To change an objects timestamp order, use this procedure to reorder an object

in the Part Navigator
1. In the Part Navigator, right-click the column heading and select
Timestamp Order.

2. Drag the object to reorder it to the timestamp you require.

If you attempt to create a circular relationship or position an object at

an invalid timestamp, your edit will be rejected.

Essentials for NX Designers 9-11

 Using sketches

Activities: Reattach sketches

In the Using sketches section, do the activity:
• Reattach a sketch

9-12 Essentials for NX Designers mt10051_s NX 7

 Using sketches

Sketcher Mirror Curve

The Mirror Curve command creates a mirrored copy of sketch geometry.
Mirrored sketch geometry is associative to the original curves and will reflect
any changes made.
Some of the existing sketch objects are modified after the sketch curves
have been mirrored.
• A mirror geometric constraint is applied to all the geometry associated
with the Mirror operation.

• The sketch curve used as the centerline are converted to a reference curve.

Where do I find it?

Task environment Sketcher

Toolbar Sketch Tools→Mirror Curve

Menu Insert→Curve from Curve→Mirror Curve

Mirror sketch curves

1. On the Sketch Tools toolbar, click Mirror Curve .

2. For the Mirror Centerline, select an existing sketch curve.

3. For the Curve to Mirror, select the curves you need to mirror.

4. Click OK.

Essentials for NX Designers 9-13

 Using sketches

Activities: Mirror sketches

In the Using sketches section, do the activity:
• Mirror sketch objects

Project: Using sketches

In the Projects section, complete the Using sketches exercise.

9-14 Essentials for NX Designers mt10051_s NX 7

 Using sketches

Summary: Using sketches

You can use Sketcher to plan, edit, and manipulate your design through every
phase of the design cycle.
In this lesson you:
• Dragged sketch curves.

• Applied alternate solutions to obtain appropriate profiles.

• Reattached sketches.

• Mirrored sketch curves.

Essentials for NX Designers 9-15

9
Lesson

10 Trim Body

Purpose

This lesson introduces the Trim Body command to define the topology of
a solid body.

Objectives

Upon completion of this lesson, you will be able to:

• Trim a solid body to a plane or sheet body.

10
Essentials for NX Designers 10-1
 Trim Body

Trim Body overview

Use the Trim Body command to trim one or more target bodies using a face,
datum plane, or other geometry.
• All parametric information is retained.

• You must select at least one target body, even when there is only one
possible target.

• You can select a single face, multiple faces from the same solid body, or a
datum plane to trim the target bodies.

Where do I find it?

Application Modeling

Toolbar Feature Operation→Trim Body

Menu Insert→Trim→Trim Body

10
10-2 Essentials for NX Designers mt10051_s NX 7
 Trim Body

Trim a body

1. On the Feature Operation toolbar, click Trim Body .

2. Select one or more target bodies to trim.

3. From the Tool Option list, select Face or Plane or New Plane.

4. Select an object with which to trim the target.

A vector points in the trimming direction.
If the sheet does not cut through a target body completely, the following
message is displayed:

If the sheet does not cut the target body at all, this message is displayed:

If a message appears, correct the problem before you continue.

5. (Optional) Click Reverse Direction to reverse the trimming direction.

6. Click Apply or OK to create the trim body feature.

10
Essentials for NX Designers 10-3
 Trim Body

Activities: Trim Body

In the Trim Body section, do the activity:
• Trim a solid body

10
10-4 Essentials for NX Designers mt10051_s NX 7
 Trim Body

Summary: Trim Body

Use the Trim Body command to define the topology of a body.
In this lesson you:
• Trimmed a solid body to a plane and a sheet body.

10
Essentials for NX Designers 10-5
10
 11
Lesson

11 Swept feature options

Purpose

This lesson introduces draft, offsets, and selection intent to define profiles and
swept features.

Objectives

Upon completion of this lesson, you will be able to:

• Apply selection intent to define sections from intersecting curves and
multiple loops.

• Create an extruded feature with offsets.

• Create an extruded feature with draft.

Essentials for NX Designers 11-1

 Swept feature options

11
Selection Intent
The Selection bar has rules you can use when you select curves.

Use these rules to help you to select curves or edges:

• In fewer steps than selecting them individually.

• When only part of some curves is needed.

• When a rule can determine which branch to take at multi-curve

intersections.

• When future model development or edits may change the number of

curves in the profile.

11-2 Essentials for NX Designers mt10051_s NX 7

 Swept feature options

11
Curve rule options

Single Curve Individually select one or more curves or edges with

no rule.

Connected Select a chain of curves or edges that share endpoints.

Curves
No rule is applied if the chained curves are
non-associative.
This rule does not grow or shrink the chain if curves
are added or no longer form a single chain after an
edit to the model.

Tangent Curves Select a tangent chain of curves or edges.

No rule is applied if the chained curves are
non-associative.
This rule does not attempt to grow or shrink the chain
if curves are added or no longer form a single chain
after an edit to the model.
Non-associative curves that are no longer tangent
after an edit are not discarded.

Face Edges Collect all edges of the face containing the edge you
select.
If you already selected an edge using another rule, you
can select an adjoining face to define a collection with
the Add All of Face rule.
When you select an edge, the cursor location
determines which face is selected.

Sheet Edges Collect all edges of the sheet body you select.

Feature Curves Collect all output curves from curve features, such as
sketches or any other curve features.

Region Select a profile that encloses an area with a single

Boundaries mouse click.

Essentials for NX Designers 11-3

 Swept feature options

11
Infer Curves Use the default intent method for the type of object
you select.
For example, with Extrude the default is Feature
Curves if you select a curve, and Single if you select
an edge.

Curve collection modifiers

Stop at Specify that auto chaining stops on

Intersection intersection points of wireframe.

Follow Fillet Automatically follow and leave fillets or

circular curves during section building.

Chain within Limit the chaining to collect curves only

Feature from the parent feature of the selected
curve.

11-4 Essentials for NX Designers mt10051_s NX 7

 Swept feature options

11
Extrude start and end limits
Use the limit options to define the overall construction method and the
extents of the extrude feature.

Options

Value Specify numeric values for the start or end of the extrusion.

Until Next Extends the extrude feature to the next body along the
direction path.

Until Extends the extrude feature to a face, datum plane, or

Selected body that you select.

Until Trims the extrude feature (if it is a body) to a face you

Extended select when the section extends beyond its edges.

Symmetric Converts the Start limit distance to the same value as the
Value End limit.

Through All Extends the extrude feature completely through all

selectable bodies along the path of the specified direction.

Essentials for NX Designers 11-5

 Swept feature options

11
Extrude with offset
The Offset options lets you specify up to two offsets to the profile for extruded
and revolved sections. You can assign unique values for both offsets.
You can:
• Type values for the offsets in the Start and End boxes in the dialog box.

• Type values in on-screen input boxes in the graphics window.

• Drag the offset handles.

Options

None Create no offset.

Single-Sided Add a single end offset to the extrude.

Two-Sided Add an offset with duplicate start and end values,

measured from opposite sides of the section.
The value for both start and end is determined by the last
one you specify.

Symmetric Add an offset with duplicate start and end values.

Start Start the offset at the value you specify, measured from
the section.

End End the offset at the value you specify, measured from the
section.

11-6 Essentials for NX Designers mt10051_s NX 7

 Swept feature options

11
Two sided offset examples
The start and end offset values may be positive or negative.
The positive direction is shown by the End Offset drag handle.

Example: Start Offset Zero, End Offset Positive

Example: Start Offset Zero, End Offset Negative

Example: Start Offset Negative, End Offset Positive

Essentials for NX Designers 11-7

 Swept feature options

11
Single-sided offset examples
The single-sided examples are based on offsets to the section shown.

Example: Offset value too large

If the end value becomes so large that a self-intersecting body is created, the
preview disappears.

Example: Smaller positive offset

In this example the offset is small enough to support a preview. The offset
body is valid.

11-8 Essentials for NX Designers mt10051_s NX 7

 Swept feature options

11
Example: Negative offset

In this example the offset is negative, and small enough to support a preview.
The offset body is valid.

Essentials for NX Designers 11-9

 Swept feature options

11
Extrude with draft
Use the Draft option to add a slope to one or more sides of the extrude feature,
in one or two directions from the section.
You can apply a draft only when the extruded section is planar.

Option Description
None No draft is created.
From Start Limit Maintain the original size of the extruded section
at the start limit.
From Section Maintain the original size of the extruded section
at the section plane.
From Section- Split the side faces into two sides at the section
Asymmetric Angle plane. You can control the draft angle separately
on each side of the section. 1
Front Angle and Back Angle options appear; one
pair with the Single option, and one pair for each
set of tangent curves for the Multipleoption.
From Section- Split side faces at the section plane, and use the
Symmetric Angle same draft angle on both sides. 1
From Section- Maintain the original size of the extruded section,
Matched Ends and split the side faces of the extrude feature at
the section plane.
Match the size of the shape at the end limit to
that of the start limit, and vary the draft angle to
maintain the matched shape at the end limit. 1
Angle Option Single — Specify a single draft angle for all faces
of the extrude feature.
Multiple — Specify unique draft angles to each
tangent chain of faces of the extrude feature.
Angle Specify a value for a draft angle.
List Examine the name and value for each draft angle.
The list appears when the Angle Option is set to
Multiple.

1. Available only when the extrude extends from both sides of the section.

11-10 Essentials for NX Designers mt10051_s NX 7

 Swept feature options

11
Positive and negative draft angles

If you look at the body with your eye positioned with respect to the draft
vector as shown, positive draft angles (1) enable you to see the draft feature
faces, and negative draft angles (2) hide the draft feature faces.

Draft and the extrude direction

Draft is measured with respect to the extrude direction. The extrude direction
does not need to be perpendicular to a planar section.

Essentials for NX Designers 11-11

 Swept feature options

11
Draft example
Draft examples are based on this extruded section.

Example: Draft with offset

In this example, the draft option is From Section-Asymmetric Angle.

The front angle value is set to 5° and the back angle value is set to 0°.
The offset option is Two Sided.
The start offset (1) is –0.2 and the end offset (2) is 0.2.

11-12 Essentials for NX Designers mt10051_s NX 7

 Swept feature options

11
DesignLogic parameter entry options
Parameter entry options let you define your model parametrically as you
specify feature values.

To access the options, click next to the text input box.

You may specify a value based on a:
• Measurement.

• Formula.

• Math or knowledge-based function.

• Reference to an existing value.

• Conversion of the above to a constant.

• Recently used value that you want to use again.

Essentials for NX Designers 11-13

 Swept feature options

11
Reference existing parameters

1. From the parameter entry options list, select Reference.

The Parameter Selection dialog box appears.
Initially, the list is empty.

2. Select an existing feature.

The list is populated with the feature’s parameters and their descriptions.

3. Select a parameter (1).

4. Click OK (2).
The parameter name now appears in the box (3).

11-14 Essentials for NX Designers mt10051_s NX 7

 Swept feature options

11
Activities: Swept feature options
In the Swept feature options section, do the activities:
• Extrude using selection intent

• Extrude with offsets

• Extrude with draft

Project: Swept features options

In the Projects section, complete the Swept feature options exercise.

Essentials for NX Designers 11-15

 Swept feature options

11
Summary: Swept feature options
Use selection intent to quickly specify sections by applying rules to complex
sets of curves.
Extrude or revolve with offsets to thicken simple sections or alter sections.
Incorporate draft in extruded features instead of using separate draft features
to simplify your history tree.
Use DesignLogic to increase productivity when modelling parametrically.
In this lesson you:
• Applied selection intent to define sections.

• Extruded with offsets.

• Extruded with draft.

11-16 Essentials for NX Designers mt10051_s NX 7

Lesson

12 Hole features
12

Purpose

This lesson introduces the general hole feature.

Objectives
Upon completion of this lesson, you will be able to:
• Create general hole features.

• Position hole features.

• Edit the parameters and location of hole features.

Essentials for NX Designers 12-1

 Hole features

Hole overview
Use the Hole command to add the following types of hole features to one or
more solid bodies in a part or assembly:
12
• General holes (simple, counterbored, countersunk, or tapered form)

• Drill size holes

• Screw clearance holes (simple, counterbored, or countersunk form)

• Threaded holes

• Hole Series (series of multi-form, multi-target body, aligned holes in the

work part or the assembly)

You can:
• Create holes on non-planar surfaces.

• Create multiple holes by specifying multiple placement points.

• Specify the position of holes using Sketcher. You can use the Snap Point
and Selection Intent options to select existing points or feature points.

• Create holes using formatted data tables for the Screw Clearance Hole,
Drill Size Hole, and Threaded Hole types.

• Use standards like ANSI, ISO, DIN, JIS and so on.

• Use the None and Subtract Boolean commands on the target bodies while
creating a Hole feature.

• Optionally add start, end, or relief chamfers to the hole feature.

Where do I find it?

Application Modeling

Toolbar Feature→Hole
Menu Insert→Design Feature→Hole

12-2 Essentials for NX Designers mt10051_s NX 7

 Hole features

Hole dialog box

The Hole dialog box includes four groups that are unique to hole features.
• Type
12
• Position

• Direction

• Form and Dimensions

The options available within the groups will change depending on which type
and form you select.

Essentials for NX Designers 12-3

 Hole features

Hole position and direction options

Position
Specifies the position of the Hole
feature.
12
Select Point You can use one of the following
methods to specify the center of the
hole:
• Sketch Section — Create a sketch
to define the location of the center
of the hole.

• Point — Specify the center of the

hole using existing points. Use
Snap Point and Selection Intent
options to select existing points or
feature points.
Direction
Hole Direction Specifies the hole direction. The
default hole direction is along the - ZC
axis. You can define the hole direction
using one of the following options:
• Normal to Face — Defines the
direction of the hole along the
direction opposite to the face
normal which is nearest to each of
the specified points.

• Along Vector — Defines the

hole direction along the specified
vector.

12-4 Essentials for NX Designers mt10051_s NX 7

 Hole features

Hole form and dimension options

Simple 1. Diameter
2. Depth
3. Tip Angle
12

Counterbore 1. C-Bore Diameter

2. C-Bore Depth
3. Depth

Countersink 1. C-Sink Diameter

2. C-Sink Angle
3. Depth

Tapered 1. Diameter
2. Taper Angle
3. Depth

Essentials for NX Designers 12-5

 Hole features

Create a general hole

1. Choose Insert→Design Feature→Hole or, on the Feature toolbar, click

Hole.
12
2. From the Type list, select General Hole.

3. Use the Position options to specify the center of the Hole feature.

• Click Sketch Section to create points in Sketcher.

• Click Point to select existing points or feature points.

A preview of the hole appears in the graphics window.

4. In the Direction group, select the required option from the Hole Direction
list.

5. Specify the form and dimensions.

6. Under Dimension, type the required parameter values.

7. (Optional) Specify the type of Boolean.

8. Click OK or Apply.

12-6 Essentials for NX Designers mt10051_s NX 7

 Hole features

Activities: Hole features

In the Hole features section, do the activities:
• Create holes
12

• Edit holes

Project: Hole features

In the Projects section, complete the Hole features exercise.

Essentials for NX Designers 12-7

 Hole features

Summary: Hole features

Hole features are one of several features with predefined shapes.
In this lesson you:
12 • Created general hole features.

• Positioned a hole using a sketch.

• Edited parameters and locations of holes.

12-8 Essentials for NX Designers mt10051_s NX 7

Lesson

13 Shell

Purpose 13
This lesson introduces the Shell command.

Objectives

Upon completion of this lesson, you will be able to:

• Create a shell feature.

• Specify faces to be removed, and apply an alternate thickness to a face.

Essentials for NX Designers 13-1

 Shell

Shell overview
Use the Shell command to hollow a solid body, or to create a shell around it.
You can assign individual thicknesses to faces and remove individual faces.

13

Where do I find it?

Application Modeling

Toolbar Feature Operation → Shell

Menu Insert →Offset/Scale→Shell
Shortcut menu Right-click a solid body→Shell

13-2 Essentials for NX Designers mt10051_s NX 7

 Shell

Create a shell

1. On the Feature Operation toolbar, click Shell .

2. Choose the type of shell you want to create:

• Remove Faces, Then Shell — Click Select Face in the Face to

Pierce group to specify one or more faces to remove from the target
solid.
13
• Shell All Faces — Click Select Body in the Body to Shell group
to select the body to shell.

3. In the Thickness group, type a distance value in the Thickness box.

4. (Optional) In the Thickness group, click Reverse Direction .

5. (Optional) Assign different thicknesses to different faces in the solid.

6. (Optional) Set or change the Approximate Offset Faces, Tangent Edges,

and Tolerance options in the Settings group.

7. Click OK or Apply to create the shell.

Essentials for NX Designers 13-3

 Shell

Assign alternate thicknesses

1. Click Select Face in the Alternate Thicknesses group and select the
faces for the first face set.

2. Type a thickness value in the Thickness n box.

You can also drag the thickness handle or type a value in its on-screen
input box.
13 Thickness n refers to Thickness 1, Thickness 2, Thickness 3, and
so on.

If the direction is wrong, click Reverse Direction for the face set.

3. Click Add New Set to complete the current face set and begin a new
set.
You can also complete the set by clicking the middle mouse button.

4. Repeat this sequence for each set of faces that require a unique wall
thickness.

13-4 Essentials for NX Designers mt10051_s NX 7

 Shell

Shell options
You can right-click the section, preview, axis vector, or handles to
quickly access many of the following options.

Option Description
Remove Faces, Then Remove some faces of the body before shelling
Shell is done.
Shell All Faces Shell all faces of the body.
Select Face Select one or more faces from a body you are 13
going to shell. 1
The first face selected sets the body to shell. 2

Select Body Select the body you want to shell. 3

Thickness Specify a thickness for the shell walls.

(Thickness group) Drag the thickness handle, or type a value in
the on-screen input box or in the dialog box.
Reverse Direction Change the direction of the thickness.
You can also right-click the thickness direction
cone head and choose Reverse Direction, or
double-click the direction cone head.
Select Face Select faces for a thickness set with a unique
thickness value for all faces in the set. 2
Complete the set by clicking Add New Set or by
clicking the middle mouse button.
You can add as many face sets as the model
allows.
Thickness n Specify an independent thickness value for the
currently selected thickness set in the List.
(Alternate Thickness
group) You can drag the face set handle, or type a value
in the on-screen input box or dialog box.
The Thickness n label changes to match
the currently selected Thickness set;
Thickness 1, Thickness 2, etc.

1. Appears only when the Type is Remove Faces, Then Shell.

2. Selection Intent for faces is available.
3. Appears only when the Type is Shell All Faces.

Essentials for NX Designers 13-5

 Shell

Option Description
Add New Set Complete the current face set.
You can also complete the current face set by
clicking the middle mouse button.
List Thickness sets appear in the list with their
name, value, and expression information.
To select a thickness set, click its on-screen
input box in the graphics window or click its
13 entry in the List.

Delete a thickness set in the list.

You can also delete a thickness set by
right-clicking it in the list and choosing Delete or
by right-clicking its handle and choosing Delete.
Approximate Offset Faces Require NX to repair self-intersections caused by
offsetting surfaces in the body, by approximating
the face within the specified Tolerance.
Use this option for complicated surfaces that
would fail due to self-intersections during shell
creation.
Tangent Edges Extend Shelf Face at Tangent Edge — Allow the
creation of edge faces along smooth boundary
edges.
Extend Tangent Face — Prevent the creation of
edge faces along smooth boundary edges.
Tolerance Enter a new tolerance value here to override
the modeling distance tolerance for the shell
operation.

13-6 Essentials for NX Designers mt10051_s NX 7

 Shell

Selection Intent face rules

When a feature requires a collection of faces, Face Rule options are available.
The list displays the face selection rules that are applicable to the feature
you are creating.

Rule Description

Single-select one or more faces as a simple list of

Single Face
objects without intent.
13
Specify a region of faces.
Region Faces Select a single seed face, and then specify the
boundary faces.

Select a single face that acts as the seed of a

Tangent Faces
collection of smoothly connected faces.

Tangent Region Select a seed face and then, optionally, one or

Faces more boundary faces.

Collect all faces of the body containing the single

Body Faces
face you select

Collect all faces that are immediately adjacent to

Adjacent Faces
the single face you select.

Collect all faces produced by the feature

Feature Faces
responsible for the face you select.

Essentials for NX Designers 13-7

 Shell

Activities: Shell
In the Shell section, do the activities:
• Create a shell

13

• Create a shell and edit direction

• Create a shell with alternate thickness

13-8 Essentials for NX Designers mt10051_s NX 7

 Shell

• Reorder features

13

Project: Shell
In the Projects section, complete the Shell exercise.

Essentials for NX Designers 13-9

 Shell

Summary: Shell
Use the Shell command to create a cavity inside, or a shell around an existing
solid body, based on a specified thickness.
In this lesson you:
• Created a shell with a uniform thickness.

• Created a shell and selected multiple faces to remove.

13 • Created a shell and specified an alternate thickness for a face.

13-10 Essentials for NX Designers mt10051_s NX 7

Lesson

14 Associative copies

Purpose

This lesson introduces the Instance Feature and Mirror Body commands.

Objectives
Upon completion of this lesson, you will be able to: 14
• Create a rectangular array of features.

• Create a circular array of features.

• Mirror a body.

Essentials for NX Designers 14-1

 Associative copies

Instance Feature overview

Use the Instance Feature command to duplicate the shape of existing features.
Use instance arrays to:
• Create patterns of features, such as bolt hole circles.

• Edit all members of an instanced feature array in one step.

The following instance array types are available:

Rectangular Create a linear array of instances from one or more
Array selected features.
Circular Array Create a circular array of instances from one or more
14 selected features.

Where do I find it?

Application Modeling

Toolbar Feature→Instance Feature

Menu Insert→Associative Copy→Instance Feature

Instance array caveats

Instanced features with a Boolean must intersect the parent solid body.
You cannot create instances of the following objects:
• Shells
• Blends
• Chamfers
• Offset sheets
• Datums
• Trimmed sheet bodies
• Instance sets
• Draft features
• Freeform features
• Trimmed features

14-2 Essentials for NX Designers mt10051_s NX 7

 Associative copies

Instance array methods

You can create three types of rectangular and circular instance arrays:

General Create an instance array with full

validation of all geometry.
Instanced geometry can cross an
edge of the face.
Instances can cross over from one
face to another.

Simple Create an instance array faster,

by eliminating excessive data
validation and optimizing
operations.
14
Identical Create an instance array by the
fastest method.
This method does the least amount
of validation.
Each instance is an exact copy of
the original.
Use this method when you have a
great many instances, and you are
sure they are all exactly the same.

When you use Simple and Identical, you should make sure that all new
geometry lies on the same face as the original feature.
If the new geometry touches or crosses the edges on the target body
or any other instance, use Analysis→Examine Geometry to validate
the geometry.
1. In the Examine Geometry dialog box, click Set All.

2. Select the geometry.

3. Click Examine Geometry.

If the array geometry fails a geometry check, click Undo and try a
General array.

Essentials for NX Designers 14-3

 Associative copies

Rectangular array
Use the Rectangular instance option to create a linear array of instances
from one or more selected features.
Rectangular instance arrays can be either two-dimensional in XC and
YC (several rows of features) or one-dimensional in XC or YC (one row of
features).
Rectangular instance arrays are generated parallel to the XC and/or YC axes
based on the number and offset distance you enter.
Change the orientation of the WCS (the XC and YC directions) by using

Format→ WCS options or WCS Dynamics .

14 Rectangular array parameters

After you select the desired features to instance, the following options appear:
Number Along XC Total number of instances parallel to the XC axis,
including the original feature.
XC Offset Spacing for the instances along the XC axis.
Number Along YC Total number of instances parallel to the YC axis,
including the original feature.
YC Offset Spacing for the instances along the YC axis.
The number of instances for both the XC and YC directions must be a
whole number greater than zero.
The offset values can be either positive or negative.

14-4 Essentials for NX Designers mt10051_s NX 7

 Associative copies

Create a rectangular array

1. In the Instance dialog box, click Rectangular Array.

2. Select the features you want to instance.

3. In the Enter Parameters dialog box, specify the method: General, Simple,
or Identical.

4. Type the Number Along XC, XC Offset, Number Along YC, and the YC
Offset.

5. Click OK to display a preview

6. Click Yes to create the instance array, or No to return to the Enter

Parameters dialog box. 14
Rectangular array example

(1) Hole selected for instance

Number Along XC = 3
XC Offset = 40
Number Along YC = 4
YC Offset = 50

Essentials for NX Designers 14-5

 Associative copies

Circular array
Use the circular instance array option to create circular array of instances
from one or more selected features.
You specify:
• The array method.

• The rotation axis about which the instances are generated.

• The total number of instances in the array, including the original feature.

• The angle between the instances.

14 Circular array parameters

After you select the desired features to instance, the following options appear:
Number Total number of instances created in the circular array,
including the existing feature you are instancing.
Angle The angle between the instances.
The number of instances must be a whole number greater than zero.
The angle can be either positive or negative.

14-6 Essentials for NX Designers mt10051_s NX 7

 Associative copies

Create a circular array

1. In the Instance dialog box, click Circular Array.

2. Select the features you want to instance.

3. In the Enter Parameters dialog box, specify the array method: General,
Simple, or Identical.

4. In the Number box, type the total number of instances in the array.

5. In the Angle box, type the angle between instances.

6. Click OK.

7. Choose Point & Direction or Datum Axis to establish the rotation axis.
14
• Point & Direction — Use the Vector dialog box to specify a direction
and the Point dialog box to specify a reference point. The selected
features are rotated about the reference point in a plane normal to
the vector direction.
When you use Point & Direction, the circular array is not
associated to geometry you select.

• Datum Axis — Select an existing datum axis.

The circular array is associated to the datum axis.

The radius of the array is the distance from the rotation axis to the
feature origin of the first feature you select. This radius value appears in
the Edit dialog box.
A highlighted representation of the array is displayed.

8. Click Yes to create the instance array, or No to return to Enter Parameters.

Essentials for NX Designers 14-7

 Associative copies

Circular array example

(1) Hole selected for instance.

(2) Rotation Axis (Datum Axis)
Number = 8
Angle = 45

14

14-8 Essentials for NX Designers mt10051_s NX 7

 Associative copies

Activities: Associative copies — instance arrays

In the Associative copies section, do the activities:
• Create a rectangular instance array

14
• Create a circular instance array

Essentials for NX Designers 14-9

 Associative copies

Mirror Body overview

Use the Mirror Body command to mirror an entire body through a datum
plane.
You can use this, for example, to form the other hand of a left hand or right
hand part.
You can timestamp the mirrored body. After you do so, any modification you
make to the original body is not reflected in the mirrored body. This is the
default mode.
When you mirror a body, the mirror feature creates a new body that is
associative to the original body. The mirrored body has no features of its own.
(1) Original body.
14
(2) Mirror datum
(3) Mirrored copy.

Where do I find it?

Application Modeling

Toolbar Feature Operation→Mirror Body

Menu Insert→Associative Copy→Mirror Body

14-10 Essentials for NX Designers mt10051_s NX 7

 Associative copies

Create a mirrored body

1. From the menu bar, choose Insert→Associative Copy→Mirror Body.

2. In the Mirror Body dialog box, click Select Body and select a body to
mirror.

3. Click Select Plane and select a datum plane.

4. (Optional) Clear the Fix at Current Timestamp check box if you want the
mirrored body to reflect subsequent features added to the parent body.

5. Click OK or Apply to create the mirrored body.

14
Edit a mirrored body

1. Right-click the mirrored body in the graphics window or in the Part

Navigator.

2. Choose Edit with Rollback from the shortcut menu

3. In the Mirror Body dialog box, edit the parent body, timestamp setting,
or the mirror plane.

Essentials for NX Designers 14-11

 Associative copies

Mirror Body options

Parent Part Available only during edit.

Work Part — Select a parent body from the work part.
Other Part — Select a parent body from another part.
The mirrored body then becomes a WAVE linked body.

Select Body
Lets you select a body in a part to mirror.

Reverse Available only during edit.

Direction Available only if you are mirroring a sheet body.
14 Reverses the surface normal of the mirrored body.

Select Plane
Select a datum plane through which to mirror a body.

Replacement Available only during edit and only if you select

Assistant geometry to replace the existing geometry.
Lets you select geometry to replace existing geometry.

WAVE This group is available only during edit and only when
Information the mirrored body is a WAVE linked body.
Parent Part displays the name of the parent part.
Object displays the name of the parent object.
Status displays the status of the WAVE link.

Fix at Current Select this option to fix the feature timestamp of the
Timestamp mirrored body.
When active, only changes made to the original body
prior to the timestamp are reflected in the mirrored
body. Changes made to the original body after the
timestamp are not reflected in the mirrored body.
When not selected, the mirrored body dynamically
changes its location in history. Changes made to the
original body are always reflected in the mirror body.

14-12 Essentials for NX Designers mt10051_s NX 7

 Associative copies

Activities: Associative copies — mirror

In the Associative copies section, do the activity:
• Mirror a solid body

14
Project: Associative copies
In the Projects section, complete the Associative copies exercise.

Essentials for NX Designers 14-13

 Associative copies

Summary: Associative copies

Use the Instance Feature and Mirror Body commands to duplicate existing
features.
In this lesson you:
• Created a rectangular instance array.

• Created a circular instance array.

• Mirrored a body.

14

14-14 Essentials for NX Designers mt10051_s NX 7

Lesson

15 Edge operations

Purpose

This lesson introduces the edge operation commands to provide additional

definition to the edges of a model. These commands include Edge Blend
and Chamfer.

Objectives
Upon completion of this lesson, you will be able to:
• Create edge blends.

• Create chamfers.
15

Essentials for NX Designers 15-1

 Edge operations

Edge Blend overview

Use the Edge Blend command to smooth selected edges that are shared by at
least two faces.
The Edge Blend command operates like a ball that rolls along an edge,
maintaining contact with the faces that meet the edge.
The blending ball rolls on the inside of faces to round the edges, removing
material (1), and the outside of faces to fillet the edges, adding material (2).

15

Where do I find it?

Application Modeling

Toolbar Feature Operation→Edge Blend

Menu Insert→Detail Feature→Edge Blend
Shortcut menu Right-click edges→Blend

15-2 Essentials for NX Designers mt10051_s NX 7

 Edge operations

Edge Blend dialog box

After you click Edge Blend a dialog box is displayed and you are prompted to
select a set of edges. You can type the radius in the Radius n box.
Radius n refers to Radius 1, Radius 2, Radius 3, and so on.

Use a Curve Rule to collect related edges or to speed up selection.

15

Essentials for NX Designers 15-3

 Edge operations

Edge Blend preview

As you select edges, the preview is updated. If the preview fails, it means the
blend will probably also fail. You should see a warning window explaining
the problem.
Adjust the radius by dragging one of the radius drag handles (1) or by typing
the value in the dynamic input field (2).

15

15-4 Essentials for NX Designers mt10051_s NX 7

 Edge operations

Add New Set

A single blend feature may consist of one or more sets of edges. Each set
may have a different radius value.
Click Add New Set in the dialog box (or click the middle mouse button once)
to select another set of edges.
You may continue to define another edge set or complete the blend operation
by clicking OK.

15

Essentials for NX Designers 15-5

 Edge operations

Activities: Edge operations — blends

In the Edge operations section, do the activities:
• Create edge blends

• Edit edge blends

15

15-6 Essentials for NX Designers mt10051_s NX 7

 Edge operations

Chamfer overview
Use the Chamfer command to bevel the edges of a solid body using chamfer
dimensions that you define.
Material is added or subtracted depending on the topology of the solid body.
In example (1) material is removed, and in example (2) material is added.

15
Where do I find it?

Application Modeling

Toolbar Feature Operation→Chamfer

Menu Insert→Detail Feature→Chamfer
Shortcut menu Right-click edges→Chamfer

Essentials for NX Designers 15-7

 Edge operations

Create a Chamfer

1. On the Feature Operation toolbar, click Chamfer , or choose

Insert→Detail Feature→Chamfer.

2. Select one or more edges.

3. In the Offsets group, specify an option from the Cross Section list;
Symmetric, Asymmetric, or Offset and Angle.

4. In the dialog box, type offset values that correspond to the cross section
option.

5. (Optional) In the Settings group, specify an option from the Offset Method
list, Offset Edges along Faces, or Offset Faces and Trim.

6. (Optional) In the Settings group, select Chamfer All Instances, if the

chamfered edge is, or may be, instanced.

15 7. (Optional) In the Preview group, select Preview to preview results, or

clear it to show only the drag handles.

8. (Optional) Use drag handles or on-screen input boxes to modify offsets.

9. (Optional) In the Offset group, click Reverse Direction to flip the chamfer.

10. Click OK or click the middle mouse button to create the chamfer.

15-8 Essentials for NX Designers mt10051_s NX 7

 Edge operations

Chamfer options
You can change the Cross Section option or click Reverse Direction in
the dialog box, or, you can use the shortcut menu over a drag handle.

Edge
Select one or more edges from the same body, using
Select Edge
a Curve Rule.
Offsets
Symmetric — Create a simple chamfer, using an
single, positive offset from a selected edge along
both of its faces.
Asymmetric Create a chamfer using two positive
Cross Section
values for the edge offsets.
Offset and Angle — Create a chamfer whose offsets
are determined by one positive offset value and a
positive angle.
Type a distance value for the offset when the Cross
Section is Offset and Angle or Symmetric.
Distance
You can also drag the distance handle to specify the
15
value.
Distance 1 Type distance values when the Cross Section is
Distance 2 Asymmetric, or drag the handles.
Type an angle value for the angle when the Cross
Section is Offset and Angle.
Angle
You can also drag the angle handle to specify the
angle.
Move the offsets or the offset and angle from one
Reverse Direction side of the chamfer edge to the other.
Not available when the cross section is symmetric.

Essentials for NX Designers 15-9

 Edge operations

Activities: Edge operations — chamfers

In the Edge operations section, do the activity:
• Create chamfers

Project: Blends and chamfers

In the Projects section, complete the Blends and Chamfers exercise.
15

15-10 Essentials for NX Designers mt10051_s NX 7

 Edge operations

Summary: Edge operations

Use the Edge Blend and Chamfer commands to alter the edges of a solid body.
All of the blended edges or chamfered edges created in a single operation are
considered to be one feature.
In this lesson you:
• Blended a single edge.

• Blended edges using a Selection Intent rule.

• Chamfered edges using different input options.

15

Essentials for NX Designers 15-11

15
Lesson

16 Introduction to Assemblies

Purpose

This lesson introduces the Assemblies application.

Objectives

Upon completion of this lesson, you will be able to:

• Set load options for an assembly.

• Work with the Assembly Navigator.

16

Essentials for NX Designers 16-1

 Introduction to Assemblies

Assembly
An assembly is a part which contains component objects.
Component objects are pointers to standalone parts or subassemblies.
In this illustration, the toy laser gun is an assembly consisting of many
components.

16 Subassembly
A subassembly is an assembly used as a component within a higher level
assembly.
This illustration shows the subassembly of the integrated circuit board for
the toy laser gun.

16-2 Essentials for NX Designers mt10051_s NX 7

 Introduction to Assemblies

Component objects
A component object links the assembly that contains it to another part file.
A component object can point to a part that is also an assembly; that is, a
subassembly with its own component objects.
1 Top level assembly.
Subassembly. This is a component part that is referenced by a higher
2
level assembly.
Standalone Parts. These are component parts that are referenced by
3
an assembly and are not themselves assemblies.
4 A Component Object.

16

Component parts
A component part is a part which is referenced by a component object within
an assembly.
Geometry stored in a component part is seen, but not copied, in the assembly.
The term “standalone part” refers to a part that it not itself an assembly.

Essentials for NX Designers 16-3

 Introduction to Assemblies

Introduction to assembly load options

When an assembly part is opened, or loaded, using File→Open, its component
parts must be found and loaded. Load Options establish how and from where
the component parts are loaded.
Access the Assembly Load Options dialog box by choosing
File→Options→Assembly Load Options or by clicking Options in the Open
Part File dialog box.

16
Part Versions group

The Part Versions group contains the Load list, with options to control how to
find component parts.
• As Saved loads parts from the directory in which they were saved.

• From Folder loads parts from the same directory as the parent assembly.

• From Search Folders loads parts from a list of search directories.

16-4 Essentials for NX Designers mt10051_s NX 7

 Introduction to Assemblies

Load states

NX parts can be fully loaded, partially loaded, or unloaded when an assembly

is opened.
• Fully loaded — All part data is loaded into memory.

• Partially loaded — Only the data required to display the part is loaded into
memory. The part will not update after certain changes that would affect
it if it was fully loaded, for example, with changes to interpart expression.
Any operations that need to load the feature data from components
will do so automatically, but can only do so if the component part
has not been modified since the first portion of it was loaded.

• Unloaded — The component part is not loaded into memory with the
assembly.

16

Essentials for NX Designers 16-5

 Introduction to Assemblies

Scope group

The Scope group in the Assembly Load Options dialog box allows you to
control the assembly configuration and the load state of parts:
• Load — Control which components are opened:
– All Components — Load all components.
– Structure Only — Load your assembly part, but no components.
– As Saved — Load the same components that were open when the
assembly was last saved.
– Re-evaluate Last Component Group — Load your assembly with the
component group used when the assembly was last saved.
Component groups are advanced functionality to let you
conditionally apply actions to all or part of the assembly
structure.

– Specify Component Group — Select from a list of available component

groups.

• Use Partial Loading — When selected, components will be partially

loaded unless the Load Interpart Data setting requires them to be fully
loaded. A partially loaded component will be fully displayed but the
underlying feature data is not loaded into system memory.

16 • Load Interpart Data — Find and load parents of interpart data, even if
the parts would be left unloaded by other rules.

16-6 Essentials for NX Designers mt10051_s NX 7

 Introduction to Assemblies

Load Behavior

The Load Behavior group controls optional actions that NX can take if there
are problems with the requested load configuration:
• Allow Replacement — Enable the assembly to be loaded with a component
that has the wrong internal identifier (but the correct name), even though
it is a completely different part. You receive a warning if this happens.

• Generate Missing Part Family Members — When NX determines that a

part family member is missing during the load:
– If it is selected, NX checks for newer versions of the current part
family template. If it finds a newer version of the template, the newest
version is used to generate the missing members.
– If it is clear, NX uses the current part family template to generate the
missing members.

• Cancel Load on Failure — NX cancels the entire load operation if it

cannot find one or more component part files.

Reference Sets
Use this area to specify a list of reference sets to be looked for, in order, when
an assembly is loaded. The first reference set found from the top of the list
reading downwards is the one that is loaded.
16
Think of a reference set as a subset of part geometry that you can load
in place of the entire part.
The Model reference set is meant to contain only a body that you wish
to place on a drawing.

Essentials for NX Designers 16-7

 Introduction to Assemblies

Assembly Navigator
The Assembly Navigator provides:
• A graphical display of the assembly structure of the displayed part.

• Methods to manage components.

To display the Assembly Navigator, click the Assembly Navigator tab

on the Resource bar.
If necessary, you may drag the Resource bar wider to see more information.

16 Node display

Each component of an assembly is displayed as a node in the assembly tree

structure.
Selecting a node is the same as selecting the corresponding component in
the graphics window.
Each node consists of a check box, an icon, the part name, and additional
columns.
If the part is an assembly or subassembly, an expand/collapse box will also be
present.

16-8 Essentials for NX Designers mt10051_s NX 7

 Introduction to Assemblies

Icons and check boxes

This assembly or subassembly is the work part, or a component of
the work part.
This assembly or subassembly is not the work part, and not a
component of the work part.
This assembly or subassembly is not loaded.

This standalone part is either the work part, or a component of

the work part.
This standalone part is not the work part, and not a component of
the work part.
This standalone part is not loaded.

This indicates a collapsed subassembly.

Click to expand the display.
This indicates an expanded subassembly.
Click to collapse the display.
The part is closed.
Click to load it.
Components will load according to assembly load options.
The part is hidden, and at least partially loaded.
Click to show it. 16
The part is visible, and at least partially loaded.
Click to hide it.

Essentials for NX Designers 16-9

 Introduction to Assemblies

Assemblies application

Start the Assemblies application like any other application, from the Start
list on the Standard toolbar. The Assemblies application can be active at the
same time as other applications such as Modeling or Drafting.
The Assemblies application name in the Start list has a check box beside
it when it is active. When the Assemblies application is active, you see
additional toolbars, and there are additional options in some menus.

16

16-10 Essentials for NX Designers mt10051_s NX 7

 Introduction to Assemblies

Activities: Assemblies — load options and navigator

In the Introduction to Assemblies section, do the activities:
• Assembly Load Options

• Assembly Navigator

16

Essentials for NX Designers 16-11

 Introduction to Assemblies

Select components in the Assembly Navigator

In any Assemblies function that requires you to select components, you may
also select the appropriate node in the Assembly Navigator.
To select multiple components in the Assembly Navigator, select the first
component and then:
• Hold the Shift key and click to select a range of nodes.

• Hold the Ctrl key and click to toggle selection of individual nodes.

You can also hold the Shift-key and click components in the graphics window
to deselect them.

Identify components

If you select a visible non-work part in the Assembly Navigator, the part is
highlighted.
If you hold the cursor over the node of a component that is not visible (e.g.,
hidden, on another layer, or unloaded), the bounding box of that component is
temporarily shown in the graphics window.
Temporary bounding box display is controlled by the Preselect Invisible
Nodes property of the Assembly Navigator.
16 To access Assembly Navigator properties, right-click in the background
and choose Properties.

16-12 Essentials for NX Designers mt10051_s NX 7

 Introduction to Assemblies

Select components using QuickPick

Once a component has been selected, you can use the shortcut menu over it in
the graphics window to select an available action.
The options in the component shortcut menu vary depending on the
active applications.

Selectable components appear in the QuickPick window.

Use the Components filter in the QuickPick dialog box to show only
components.

16

Essentials for NX Designers 16-13

 Introduction to Assemblies

Design in context
You design in context when you edit component geometry while a higher
level assembly is displayed.
The advantage is that you can see and, when necessary, select objects from
other components.

The Displayed Part

NX allows multiple parts to be open at the same time. These parts may have
been loaded:
• Explicitly — Loaded using the Open options on the Assembly Navigator,
or the File→Open command.

• Implicitly — Loaded as a result of being used by some other loaded

assembly.

The part currently displayed in the graphics window is called the displayed
part. You can make edits in parallel to several parts by switching the
displayed part back and forth among those parts.
Loaded parts do not have to belong to the same assembly.
There are several ways to change the displayed part:
16 • Select a component from the graphics window and use the shortcut menu.

• On the Assemblies toolbar, click Make Displayed Part .

• From the main menu, choose Window→More to open the Change Window
dialog box.

• Choose Window and select a part from the list.

• In the Assembly Navigator, open the shortcut menu over the node for a
part, and select Make Displayed Part.

• From the main menu, choose Assemblies→Context Control→Set

Displayed Part.

16-14 Essentials for NX Designers mt10051_s NX 7

 Introduction to Assemblies

Change Window dialog box

The Change Window dialog box lists all partially and fully loaded parts
except the displayed part.
Select a part by:
• Selecting from the list of loaded parts.

• Selecting geometry in the graphics window.

• Selecting the node in the Assembly Navigator.

Enter a portion of the part name in the Search Text box to help find the
part in the list.

16

Click the Options button to specify search methods.

Essentials for NX Designers 16-15

 Introduction to Assemblies

The work part

The part in which you create and edit geometry, and to which components
are added, is called the work part. The work part and the displayed part
need not be the same.
When the displayed part is an assembly, you can change the work part to any
of the components within that assembly, except for unloaded parts and parts
of different units. You can add or edit geometry, features, and components
within the work part.
You can reference geometry outside of the work part in many modeling
operations. For example, you can use control points on geometry outside of
the work part to position a feature within the work part.
When you open a part with File→Open it is both the displayed and the work
part.
If the displayed part is not the work part, the work part is, by default,
emphasized by retaining its normal colors while other components are
de-emphasized using a blend color. The blend color is specified on the Color
Settings page of the Visualization Preferences dialog box.
There are several ways to change the work part:
• In the graphics window, double-click the component.

16 • In the graphics window, select the component and use the shortcut menu.

• In the Assembly Navigator, double-click the node.

• In the Assembly Navigator, use the shortcut menu.

• On the Assemblies toolbar, click Make Work Part .

• Choose Assemblies→Context Control→Set Work Part.

Associativity between components and assemblies

Geometric changes made at any level within an assembly result in the update
of associated data at all other levels of affected assemblies.
An edit to an individual component part causes all assembly drawings that
use that part to be updated appropriately.

16-16 Essentials for NX Designers mt10051_s NX 7

 Introduction to Assemblies

Assembly Navigator shortcut menu

If you right-click a node in the Assembly Navigator that represents a
component, the shortcut menu shows component related options.
The options in the Assembly Navigator shortcut menu vary depending
on the status of the component and whether the Assemblies and
Modeling applications are active.

Pack and Unpack

The Pack option replaces multiple occurrences in the Assembly Navigator

display with a single node.
Multiple occurrences are components representing the same part, and
having the same parent.

Use the Unpack option to reverse the Pack option and show all occurrences.

Make Work Part

The Make Work Part command sets the part in which to create new geometry
or edit existing geometry.
When a component is the work part, the reference set is by default
changed to Entire Part. 16
This can result in the display of additional geometry.

Make Displayed Part

The Make Displayed Part command switches the display between currently
loaded parts.
The displayed part is always the top node in the Assembly Navigator.

Display Parent

The Display Parent command switches the displayed part from a component
or an assembly to a loaded parent assembly.
The Maintain option in the Assembly Preferences dialog box
determines the behavior when you make a parent the displayed part.
If Maintain is selected, the component remains the work part.
If Maintain is clear, the parent becomes both the displayed part and
work part.

Essentials for NX Designers 16-17

 Introduction to Assemblies

Activities: Assemblies — more navigator options

In the Introduction to Assemblies section, do the activity:
• Additional work with the Assembly Navigator

16

16-18 Essentials for NX Designers mt10051_s NX 7

 Introduction to Assemblies

Save the work part

After you edit it, save the work part to keep the modifications.
Use File→Save or File→Save Work Part Only.

Save

• If the work part is a standalone part, only that part is saved.

• If the work part is an assembly or subassembly, all modified component

parts below it are also saved.
File→Save does not save higher level parts and assemblies if they are
modified.
File→Save All saves all modified parts in the session regardless
of which part is the work part, even parts that do not belong to
the displayed assembly.

Open parts for which you do not have write privileges will not be
saved.
You will get a warning about parts that cannot be saved due to
permissions.

Save Work Part Only 16

Use File→Save Work Part Only saves only the work part, even if it is an
assembly or subassembly with modified components.

Essentials for NX Designers 16-19

 Introduction to Assemblies

Summary: Assemblies
An assembly is a file which contains component objects. It is a collection of
pointers to piece parts and/or subassemblies.
Assemblies provides the ability to design in context.
In this lesson you:
• Set Assembly Load Options.

• Worked with the Assembly Navigator.

16

16-20 Essentials for NX Designers mt10051_s NX 7

Lesson

17 Adding and constraining

components

Purpose

This lesson introduces commands to add components to an assembly, move

components, and define associative relationships between components.

Objectives
Upon completion of this lesson, you will be able to:
• Add components to an assembly.

• Move components.

• Create assembly constraints.

17

Essentials for NX Designers 17-1

 Adding and constraining components

General assembly concepts

There are two approaches to creating an assembly structure.
• Top-down modeling — Create component parts at the assembly level.

• Bottom-up modeling — Create individual models in isolation, then later

add them to assemblies.

You are not limited to one approach to build an assembly. For example, you
can initially work in a top-down fashion, then switch back and forth between
bottom-up and top-down modeling.

Assemblies toolbar
Button Description
Insert an existing component into your
Add Component
assembly.
Create New Create a new component and insert it into
17 Component your assembly.
Move selected components within their
Move Component
degrees-of-freedom in an assembly.
Assembly Define component positions using positioning
Constraints constraints.
Make Work Part Change the work part to the selected part.
Make Displayed
Change the displayed part to the selected part.
Part

17-2 Essentials for NX Designers mt10051_s NX 7

 Adding and constraining components

Use the bottom-up construction method

1. Create new part files using File→New.

2. Create the desired geometry.

3. Change the work part to the assembly file.

4. Position the new part in the assembly:

From the main menu choose Assemblies→ Components→ Add
Component.
or

On the Assemblies toolbar, click Add Component .

17

Essentials for NX Designers 17-3

 Adding and constraining components

Add Component overview

Use the Add Component command to create an assembly using a bottom-up
design method by adding one or more parts to the work part as components.
If the part to be added as a component has not already been loaded, it is
loaded when you use this option.

17

Where do I find it?

Application Assemblies

Toolbar Assemblies→Add Component

Menu Assemblies→Components→Add Component

17-4 Essentials for NX Designers mt10051_s NX 7

 Adding and constraining components

Add components to an assembly

1. On the Assemblies toolbar, click Add Component .

2. If you want to see a preview of the component, do both of the following:

• Choose Preferences→Assemblies and select the Preview Component
on Add check box.
• In the Add Component dialog box, select the Preview check box.

3. In the Add Component dialog box, while Select Part is active, select
one or more parts that you want to add. You can select a part from several
places, including:
• The graphics window.
• The Loaded Parts or Recent Parts lists in the Add Component dialog
box.
• The Assembly Navigator.

• The Part Name dialog box — Click Open , and browse to the
directory that has the part that you want to add.

4. (Optional) Under Duplicates, in the Count box, type a number of

instances to create. The default is 1.

5. Specify the Positioning method that is to be applied after you choose OK

or Apply in step 11:
• Absolute Origin — Place the added components at absolute 0,0,0.
• Select Origin — Place the added components at a selected point.
• By Constraints— Place the added components after you define their
17
assembly constraints with other components.
• Move — Place the added components after you define how they should
be positioned.

6. (Optional) Select the Scatter check box if you want to ensure that multiple
added components are initially positioned apart from each other.

7. (Optional) Under Replication, specify Multiple Add to define what NX

should do after you add the selected components. The Multiple Add options
provide shortcuts for common operations with newly-added components:
• None
• Repeat after Add — Immediately add another instance of each
newly-added component.
• Array after Add — Create an array of your newly-added components.

Essentials for NX Designers 17-5

 Adding and constraining components

8. (Optional) Under Settings, specify a Name if you want your added part
to have a different component name than the original part name. (Not
available if you select multiple parts.)

9. (Optional) Specify the Reference Set for your added components.

10. (Optional) Choose a Layer Option to define the layer where the
components should be located.
If your Layer Option is As Specified, type the layer number in the Layer
box.

11. Choose OK or Apply to add the selected components.

17

17-6 Essentials for NX Designers mt10051_s NX 7

 Adding and constraining components

Activities: Adding and constraining components — create assembly

In the Adding and constraining components section, do the activity:
• Create an assembly

17

Essentials for NX Designers 17-7

 Adding and constraining components

Move Component overview

Use the Move Component command to move components in an assembly.
• You can select components to move dynamically (such as with drag
handles), or you can create constraints to move the components into
position.

• You can move components on different assembly levels at the same time.

17 Where do I find it?

Application Assemblies

Toolbar Assemblies→Move Component

Menu Assemblies→Components→Move Component
Shortcut menu Right-click components→Move

17-8 Essentials for NX Designers mt10051_s NX 7

 Adding and constraining components

Assembly Constraints overview

Use the Assembly Constraints command to associatively define positions of
components in the assembly.
You specify constraint relationships between two components in the assembly.
For example, you can specify that a cylindrical face on one component is to be
coaxial with a conical face on another component.
Use combinations of constraints to completely specify a component’s position
in the assembly.
NX calculates a position for the components which satisfies the constraints
you specify.

Where do I find it? 17

Application Assemblies

Toolbar Assemblies→Assembly Constraints

Menu Assemblies→Components→Assembly Constraints
Shortcut menu Right-click component→Assembly Constraints

Essentials for NX Designers 17-9

 Adding and constraining components

Assembly Constraint types

Type Description
Constrain two components so they touch or align with
Touch Align each other.
Touch Align is the most common constraint.
Constrain circular or elliptical edges of two components
Concentric so the centers are coincident and the planes of the edges
are coplanar.
Distance Specify the minimum 3D distance between two objects.
Fix Fix a component at its current position.
Define the direction vectors of two objects as parallel to
Parallel
each other.
Define the direction vectors of two objects as perpendicular
Perpendicular
to each other.
Angle Define an angle dimension between two objects.
Center one or two objects between a pair of objects, or
Center
center a pair of objects along another object.
Bond “Weld” components together so they move as a rigid body.
Bring together two cylindrical faces with equal radii. This
constraint is useful for locating pins or bolts in holes.
Fit
If the radii later become non-equal, the constraint is
invalid.

17

17-10 Essentials for NX Designers mt10051_s NX 7

 Adding and constraining components

Create a Touch Align constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Touch Align.

3. Check the Settings and modify them as you require:

• Arrangements — Specify whether to apply the constraint to other
assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are retained after you close

the Assembly Constraints dialog box. If the check box is cleared,
constraints are temporary; they remain in effect only while the dialog
box is open.

4. Set Orientation to one of the following:

• Prefer Touch — Use a touch constraint when touch and align solutions
are both possible. (Touch constraints are more common than align
constraints in most models.)
The Prefer Touch option uses an align constraint if a touch constraint
would over-constrain the assembly.

• Touch — Constrain objects so their surface normals are in opposite

directions.

• Align — Constrain objects so their surface normals are in the same 17

direction.

• Infer Center/Axis — Specify that, when you select a cylindrical or

conical face, NX uses the face’s center or axis instead of the face itself
for the constraint.

5. Click Select Two Objects (if necessary), and select two objects for
the constraint.

You can use the Point Constructor to help you select objects.

6. If two solutions are possible, you can click Reverse Last Constraint to
flip between the possible solutions.

7. Click OK or Apply when you finish adding constraints.

Essentials for NX Designers 17-11

 Adding and constraining components

Create a Concentric constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Concentric.

3. Check the Settings and modify them as you require:

• Arrangements — Specify whether you want the constraint to be
applied to other assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are persistent after you close

the Assembly Constraints dialog box.

4. Click Select Two Objects (if necessary), and select two circular
curves for the constraint.
If the Accept Tolerant Curves assembly preference check box is selected,
you can also select elliptical or near-circular curves that are within the
modeling distance tolerance.

5. If two solutions are possible, click Reverse Last Constraint to flip

between the possible solutions.

6. Click OK or Apply when you finish adding constraints.

17

17-12 Essentials for NX Designers mt10051_s NX 7

 Adding and constraining components

Create a Distance constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Distance.

3. Check the Settings and modify them if you do not want to use their
defaults:
• Arrangements — Specify whether you want the constraint to be
applied to other assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are persistent after you close

the Assembly Constraints dialog box.

4. Click Select Two Objects (if necessary), and select two objects for the
distance constraint.

5. If two solutions are possible, you can click Reverse Last Constraint to
flip between the possible solutions.
If more than two solutions are possible, you can click Cycle Last
Constraint to cycle through the possible solutions.

6. Click OK or Apply when you finish adding constraints.

17

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 Adding and constraining components

Create a Fix constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Fix.

3. Check the Settings and modify them if you do not want to use their
defaults:
• Arrangements — Specify whether you want the constraint to be
applied to other assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are persistent after you close

the Assembly Constraints dialog box.

4. Click Select Object (if necessary), and select the object you want
to fix.

5. Click OK or Apply when you finish adding constraints.

17

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 Adding and constraining components

Create a Parallel constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Parallel.

3. Check the Settings and modify them if you do not want to use their
defaults:
• Arrangements — Specify whether you want the constraint to be
applied to other assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are persistent after you close

the Assembly Constraints dialog box.

4. Click Select Two Objects (if necessary), and select two objects that
you want to be parallel.

5. If two solutions are possible, you can click Reverse Last Constraint to
flip between the possible solutions.

6. Click OK or Apply when you finish adding constraints.

17

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 Adding and constraining components

Create a Perpendicular constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Perpendicular.

3. Check the Settings and modify them if you do not want to use their
defaults:
• Arrangements — Specify whether you want the constraint to be
applied to other assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are persistent after you close

the Assembly Constraints dialog box.

4. Click Select Two Objects (if necessary), and select two objects that
you want to be perpendicular.

5. If two solutions are possible, you can click Reverse Last Constraint to
flip between the possible solutions.

6. Click OK or Apply when you finish adding constraints.

17

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 Adding and constraining components

Create an Angle constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Angle.

3. Check the Settings and modify them if you do not want to use their
defaults:
• Arrangements — Specify whether you want the constraint to be
applied to other assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are persistent after you close

the Assembly Constraints dialog box.

4. Specify the Subtype:

• 3D Angle measures the angle constraint between two objects without
a defined axis of rotation.

• Orient Angle measures the angle constraint between two objects,

using a selected axis of rotation.

5. Select the objects for the angle constraint as follows:

• If Subtype is 3D Angle, the Select Two Objects option appears.

Select two objects for the angle constraint.
17
• If Subtype is Orient Angle, the Select Three Objects option
appears. Select an axis as the first object, and then select two objects
for the angle constraint.

6. If two solutions are possible, click Reverse Last Constraint to flip

between the possible solutions.

7. Click OK or Apply when you finish adding constraints.

Essentials for NX Designers 17-17

 Adding and constraining components

Create a Center constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Center.

3. Check the Settings and modify them if you do not want to use their
defaults:

• Arrangements — Specify whether you want the constraint to be

applied to other assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are persistent after you close

the Assembly Constraints dialog box.

4. Specify the Subtype:

• 1 to 2 — Center the first selected object between the next two selected
objects.

• 2 to 1 — Center two selected objects along the third selected object.

• 2 to 2 — Center two selected objects between two other selected

objects.

5. If Subtype is 1 to 2 or 2 to 1, set Axial Geometry to define what happens

17 if you select a cylindrical face or circular edge:

• Use Geometry — Use selected cylindrical faces for the constraint.

• Infer Center/Axis — Use the center or axis of the object.

6. Click Select Objects (if necessary), and select the appropriate number
of objects as defined by the Subtype.

You can use the Point Constructor to help you select objects.

7. If two solutions are possible, click Reverse Last Constraint to flip

between the possible solutions.

8. Click OK or Apply when you finish adding constraints.

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 Adding and constraining components

Create a Bond constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Bond.

3. Check the Settings and modify them if you do not want to use their
defaults:
• Arrangements — Specify whether you want the constraint to be
applied to other assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are persistent after you close

the Assembly Constraints dialog box.

4. Click Select Objects (if necessary), and select two or more objects
to bond.

5. Click Create Constraint when you are ready to create the constraint.

6. Click OK or Apply when you finish adding constraints.

17

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 Adding and constraining components

Create a Fit constraint

1. On the Assemblies toolbar, click Assembly Constraints .

2. In the Assembly Constraints dialog box, set Type to Fit.

3. Check the Settings and modify them if you do not want to use their
defaults:
• Arrangements — Specify whether you want the constraint to be
applied to other assembly arrangements.

• Dynamic Positioning — Specify that you want NX to solve the

constraints and move the components as you create each constraint.

• Associative — Specify that constraints are persistent after you close

the Assembly Constraints dialog box.

4. Click Select Two Objects (if necessary), and select two pieces of
geometry that are the same size.
The objects are fitted together.

5. If two solutions are possible, you can click Reverse Last Constraint to
flip between the possible solutions.

6. Click OK or Apply when you finish adding constraints.

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 Adding and constraining components

Activities: Adding and constraining components — constrain

In the Adding and constraining components section, do the following activity:
• Constrain and move components

Project: Assembly constraints

In the Projects section, complete the Assembly constraints exercise.

17

Essentials for NX Designers 17-21

 Adding and constraining components

Summary: Adding and constraining components

When you add components to an assembly, you reference other part files
or subassemblies.
You can move components or establish constraints to define the locations of
components.
In this lesson you:
• Added components to an assembly.

• Moved components.

• Defined assembly constraints.

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Lesson

18 Introduction to Drafting

Purpose

This lesson introduces the Drafting application and the master model concept.

Objectives
Upon completion of this lesson, you will be able to:
• Create a non-master file that references a master model.

• Open, create, and delete drawing sheets.

• Add and edit views on drawing sheets.

• Create dimensions.

• Create notes on a drawing sheet.

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Essentials for NX Designers 18-1

 Introduction to Drafting

Master model concept

You apply the master model concept by creating an assembly, or non-master
part, with exactly one component part. The component part is the master
model. Edits to the master model are updated in the non-master part.
The master model concept allows multiple design processes to access the
same geometry during development. Benefits of this include:
• It promotes concurrent engineering. You can begin downstream
applications such as drafting, manufacturing, and analysis during
geometry construction.

• The downstream users need not have write access to the geometry. This
prevents accidental modifications.

Drafting Assembly

Master Model

Analysis N/C

Each application uses a separate assembly part. When the master model is
18 revised, the other applications automatically update with minimal or no
associativity loss.
You can maintain the design intent of the various design applications by
restricting write permission on the master model.

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 Introduction to Drafting

Drawings
Use the Drafting application to create drawings of 3D parts.
Some of the benefits of the Drafting application are:
• You can add views to a drawing sheet by indicating their location with
the cursor.

• When you add projected views, they are automatically aligned with the
parent view.

• When you update the model, you can update the views either
automatically or manually.

• Drafting annotation is placed directly on the drawing sheet.

• Drafting annotation (dimensions, labels, and symbols with leaders) is

associative to the geometry you select.

• Associative view boundaries are calculated when the drawing sheet is

updated.

• Section views are fully associative to the model.

In NX, the term drawing sheet is used to define a collection of views. You
can think of each drawing sheet as a separate page in the drawing file. One
drawing file can contain many drawing sheets.

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 Introduction to Drafting

New Sheet overview

Use the New Sheet command to create a new drawing sheet with a specific
size, scale, name, unit of measure, and projection.
The new drawing sheet replaces the current display.
When you start the Drafting application, you will see either:
• An existing drawing sheet.

• The Sheet dialog box if there are no existing drawing sheets.

To control the automatic appearance of the Sheet dialog box:

1. From the Menu Bar, choose Preferences→Drafting.
2. Click the General tab.
3. In the Drawing Work Flow group, select the Automatically Start
Insert Sheet Command check box.

Where do I find it?

Application Drafting

Toolbar Drawing→New Sheet

Menu Insert→Sheet
Right-click Drawing node in Part Navigator→Insert
Shortcut menu Sheet

Create a new drawing sheet

1. On the Drawing toolbar, click New Sheet .

2. In the Sheet dialog box, define the drawing sheet size, scale, name, units
18 of measure and projection angle.

3. Choose OK.

Open a drawing sheet

Do one of the following:

• In the Part Navigator, double click the drawing sheet node.

• In the Part Navigator, right-click the drawing sheet node and choose Open.

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 Introduction to Drafting

Edit a drawing sheet

Do one of the following:

• In the Part Navigator, right-click the drawing sheet and choose Edit Sheet.

• Right-click the view border of a drawing sheet and choose Edit Sheet.

• On the Drafting Edit toolbar, click Edit Sheet

• From the menu, choose Edit→Sheet.

You can change the projection angle only if no projected views exist on
the drawing sheet.
You can edit the drawing sheet to a larger or smaller size. If you
edit the drawing sheet to a size so small that a member view falls
entirely outside the boundary of the drawing sheet, you will get an
error message.

If you need to edit the drawing sheet to a smaller size, but cannot due to
the current position of the views, move the views closer to the drawing
sheet’s origin at the lower left corner of the sheet.

Delete a drawing sheet

Do one of the following:

• Right-click the border of a drawing sheet and choose Delete.

• In the Part Navigator, right-click the drawing sheet node and choose
Delete.

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 Introduction to Drafting

Activities: Drafting — Create drawings

In the Introduction to Drafting section, do the activities:
• Create a new non-master drawing

• Open and edit drawings

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 Introduction to Drafting

Change drawing display to monochrome

The Monochrome Display option displays a drawing sheet in a single color.
1. Choose Preferences→Visualization.

2. Click the Color Settings tab.

3. In the Drawing Part Settings section, select the Monochrome Display

check box.
The default colors are black and gray. You can specify any line or
background color

In the Part Navigator, right-click the drawing node and choose

Monochrome.
Monochrome will be applied to all drawing sheets in the part.
In the Visualization Preferences dialog box, on the Line page, use the
Show Widths option to display of line widths and make the display
closely resemble a plotter output.

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Essentials for NX Designers 18-7

 Introduction to Drafting

View Preferences
Control the display of views by choosing Preferences→View.
Define the display of hidden lines, silhouettes, smooth edges, and section view
background lines by using the View Preferences dialog box.
Automatically create linear, cylindrical, and bolt circle centerlines when you
add a view by selecting the Centerlines check box on the General page.

Hidden Lines

If you clear the Hidden Line check box, hidden line processing is not
performed and all hidden lines in the view appear as solid lines.
If you select the Hidden Line check box, the color, font, and width of the hidden
lines are determined by the settings in the three lists below the check box.

The color, font, and width lists are not named or labeled. This
configuration is common in the dialog boxes in Drafting.
The color option is not applicable in monochrome mode.
Widths are displayed only if Show Widths is selected in the
Visualization Preferences dialog box.

Smooth Edges

Smooth edges are those whose adjacent faces have the same surface tangent
at the edge where they meet.
On the Smooth Edges page, select the Smooth Edges option to use the color,
font, and width settings to specify the appearance of smooth edges.
18 Use the End Gaps option to vary the edge intersection appearance.

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 Introduction to Drafting

Base View overview

Use the Base View command to add the first view to a drawing sheet.
You can project other views from a base view.
A drawing sheet can have more than one base view.
To control the automatic appearance of the Base View dialog box:
1. From the Menu Bar, choose Preferences→Drafting.

2. Click the General tab.

3. In the Drawing Work Flow group, select Automatically Start Base

View Command.
This will automatically open the Base View dialog box when you
start the Drafting application and there are no existing views on
any of the drawing sheets.

Where do I find it?

Application Drafting

Toolbar Drawing→Base View

Menu Insert→View→Base View
Right-click the sheet border→Add Base View
Right-click drawing sheet node in Part Navigator→Add
Shortcut menu Base View

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Essentials for NX Designers 18-9

 Introduction to Drafting

Base View options

(1) Part Add a view from a part that you specify

(2) Model View to Use Select the base view type from a list. Select NX
defined views or custom views.
(3) Orient View Tool Define a custom orientation for a view such as
perpendicular to a model face.
(4) Scale Select from a list of several preset scales, enter a
custom scale, or define the scale by an expression.
(5) View Style Opens the View Style dialog box. Settings you
make apply to the view you are adding.

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 Introduction to Drafting

Projected View overview

Use the Projected View command to create a projected view from an existing
parent view.
Immediately after you place a base view on a drawing sheet, create a
projected view by moving the cursor in the direction of the projection you
want, and click to place the view.
To control the automatic appearance of the Projected View dialog box:
1. From the Menu Bar, choose Preferences→Drafting.

2. Click the General tab.

3. In the Drawing Work Flow group, select Automatically Start

Projected View Command.

Where do I find it?

Application Drafting

Toolbar Drawing→Projected View

Menu Insert→View→Projected View
Right-click an existing view border→Add Projected
View
Right-click drawing view node in Part Navigator→Add
Shortcut menu Projected View

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 Introduction to Drafting

Projection lines

When you move the cursor while adding a projected view you see projection
lines. You can place the view at any angle from the base view. You can:
• Place the view manually. The angle snaps to 45° increments.

• Define a hinge line.

• Select a planar face and project perpendicular to it.

Preview

As you move the cursor the preview style can be:

• Border

• Wireframe

• Hidden Wireframe

• Shaded Image

To select a preview option, right-click before you place the view and
choose Preview Style.

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 Introduction to Drafting

Projected View options

(1) Parent View Select a different base view to use as the parent
view.
(2) Vector Option Infer a hinge line or explicitly define a fixed hinge
line.
(3) Reverse Projected Reverse the direction of the projected view.
Direction
(4) Associative Make the projected view associated to the defined
hinge line.
(5) Placement Align the projected view horizontally, vertically,
perpendicular to the hinge line, or infer the
placement based on the cursor location.
(6) Move View Move an existing view without interrupting the
interaction to place a projected view.
(7) View Style Open the View Style dialog box.

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 Introduction to Drafting

Edit the style of an existing view

There are several ways to change the style of an existing view.

• Double-click the view border.

• Right-click the view border and choose Style.

• In the Part Navigator, double-click a drawing view node.

• In the Part Navigator, right-click a drawing view node and choose Style.

• Choose Edit→Style.

Drag views on a drawing

1. (Optional) Select one or more views to move.

2. Hold the cursor over the border of a view (a selected view, if there are more

than one) until it changes to drag mode .

3. Drag the view as required.

As you move a view relative to others, alignment lines appear. When

you place a view with alignment lines visible it automatically snaps to
an aligned position.

Delete views on a drawing

There are several ways to remove a view from a drawing sheet.

• Right-click the view border and choose Delete.

18
• In the Part Navigator, right-click the view to be removed and choose
Delete.

• Choose Delete and select the view.

• Choose Edit→Delete and select the view.

Once a view is removed from a drawing sheet, all drafting objects or view
modifications associated to that view are deleted.

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 Introduction to Drafting

Activities: Drafting — add views

In the Introduction to drafting section, do the activity:
• Add views to a drawing

18

Essentials for NX Designers 18-15

 Introduction to Drafting

Dimensions
To use the various dimensions types:
• Choose Insert→Dimension and then choose the desired dimension type.

• Use the Dimensions toolbar. This toolbar offers a menu of the available
dimension types.

Annotation Preferences

Use the Annotation Preferences dialog box (Preferences→Annotation) to

configure global settings that affect dimensions.
The following pages in the Annotation Preferences dialog box apply to
dimensions:
Dimensions Control the display of extension lines and arrows,
orientation of text, precision and tolerance, chamfer
dimensions, and narrow dimensions.
Line/Arrow Control the style and size of leaders, arrows, and extension
lines for both dimensions and other annotations. A
preview area provides a rendition of the symbol with
leaders and dimensions.
Lettering Control the alignment, justification, size, and font of text.
Units Control the desired unit of measure for dimensions
and whether dimensions are created in single or dual
dimension format.
Radial Control the settings that are unique to diameter and
radius dimensions.

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 Introduction to Drafting

Dimension preferences and placement

When you select a dimension type, the corresponding dimension dialog bar
appears.
The settings that you set on the dialog bar affect only dimensions you are
currently creating. The settings return to global values when you exit
dimension creation or choose Reset.

1 Tolerance Types Select the tolerance type from a list.

Select the primary nominal precision from 0-6
Primary Nominal decimal places from a list. If the preferences
2
Precision format is fractional, then the list displays
fractional precision values.
Enter a tolerance value, or values, using
3 Tolerance Values
on-screen input boxes.
Set the primary tolerance precision from 0-6
4 Tolerance Precision
decimal places.
Display the full Text Editor dialog box where
5 Annotation Editor
you can enter symbols and appended text.
Open the Dimension Style dialog box. This
dialog box is a subset of the Annotation
Preferences dialog box, containing only the
property pages that apply to dimensions.
6 Dimension Style
Use this option to affect settings as you
create one or more dimensions.
The global settings are restored when
you exit from creating dimensions. 18
Reset local preferences to previous current
7 Reset
settings in the part and clear appended text.
Treat as a driving sketch dimension or as a
documentation dimension.
8 Driving Dimension
This option is only available when a sketch is
created on the drawing sheet.

Essentials for NX Designers 18-17

 Introduction to Drafting

Annotation placement options

When you select a dimension type to create, the annotation placement options
appear on the Selection bar.

Set the leader on the left side, right side, or

1 Leader Orientation
automatically infer the side.
Associate the entity origin so that it is always
2 Associative Origin
aligned with another dimension.
Specify the alignment position on object such
3 Alignment Position
as top-left, mid-center, bottom-right.
4 Origin Tool Open the Origin Tool dialog box.

Snap Point options

Snap point options appear on the Selection bar while you are working with
dimensions.
These options act as a filter for selecting geometric points. You can either
select or deselect any of these in order to limit your selection to specific types
of points.
Use the Two-curve Intersection button (at the right end of the toolbar) to
select any two edges whose intersection you cannot fit inside the select ball.
When you select it, all the other buttons are unavailable.
You can press the Esc key at any time to release all selected objects.

Placement cues for dimensions

As you create dimensions, you can align them with an existing dimension.
Graphical cues appear when the origins of two dimensions are vertically or
18 horizontally aligned.
If you want the new dimension associated with the existing dimension, make

sure the Associative Origin button is active.

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 Introduction to Drafting

Append text to a dimension

You can append text to a dimension while you are creating it.
If you want only one line of appended text, select the object(s) to dimension
and, before you place the dimension, choose one of the appended text options
in the shortcut menu.

If the text is complex, use the Text Editor .

To add appended text to a previously created dimension that does not already
have appended text, do one of the following:
• Double-click the dimension, and open the Text Editor from the dialog bar.

• Double-click the dimension, and use the Right (after), Left (before), Up
(above), or Down (below) arrow key on the keyboard to get the appended
text location you desire. Type the text and press Enter.

• Double-click the dimension, and use the shortcut menu to choose either
Appended Text (for a single line of text), or Text Editor (for complex text).

To edit existing appended text, do one of the following:

• Double-click the appended text.

• Double-click the dimension and use the Right (after), Left (before), Up
(above), or Down (below) arrow key on the keyboard to get the appended
text location you desire.

• Select the dimension, and open the shortcut menu over the appended text.

Change text orientation and text arrow placement

• To set the text orientation and text arrow placement as you create a
dimension, open the shortcut menu before you place the text.
18
• To change the text orientation and text arrow placement of an existing
dimension, edit the dimension style.

Move a dimension

To change the origin of an existing dimension, simply drag it when no

command is active.

The cursor will change to when you are in the move mode.

Essentials for NX Designers 18-19

 Introduction to Drafting

Editing an existing dimension

There are two possible shortcut menus that can be displayed over an existing
dimension.

• One shortcut menu appears over a dimension, when dimension creation

is inactive.

• The other menu appears when you double-click an existing dimension (to
edit it) and then open the shortcut menu.
When you edit a dimension the dimension dialog bar appears.

The cursor changes to indicate that you are in the editing mode.

Change the precision of a dimension

1. Double-click the dimension.

2. Do one of the following:

• Choose Nominal Precision from the shortcut menu.

• From the Edit Dimension dialog bar, in the Value group, click the
precision list.

• On the keyboard, press the number key that corresponds to the

desired precision.
18
Inherit preferences from an existing dimension

After you create a dimension, you can edit its preference settings to match
another dimension:

1. Double-click the dimension you want to change.

2. Right-click the dimension and choose Inherit.

3. Select the dimension that has the desired preference settings.

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 Introduction to Drafting

Activities: Drafting — dimensions

In the Introduction to drafting section, do the activity:
• Create dimensions

18

Essentials for NX Designers 18-21

 Introduction to Drafting

Creating notes and labels

The Note dialog box provides options for creating notes, labels, and symbols.
You enter text and symbols for your notes and labels in the Text Input box.

Helper lines

Helper lines act as a guide to allow you to align notes, labels, dimensions,
symbols, and views with other objects on the drawing sheet. Helper lines
appear as a dashed line.
18
To use helper lines, move the cursor over the object to which you want to
align as you are placing the new annotation. The note highlights and helper
lines appear.

Click to place the annotation at the desired location.

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 Introduction to Drafting

Create a note

1. Click Note from the Annotation toolbar or choose Insert→Note.

2. Enter the desired text into the text box. Text displays in the text box
and on the graphics window.

3. Click the left mouse button at the location where you wish to place the
note.
After you position text, it remains in the edit window for you to use again
or edit for the next annotation.

You can also create a note on a drawing sheet by dragging a text file
(.txt) from an operating system window to the drawing sheet.

Create a label

1. Type the desired text.

2. Locate the cursor on the curve/edge/face where you want to place the
arrowhead (with the cursor displayed as shown below).

3. Drag the cursor away from the selection point.

18
4. Click the location for the text.

Essentials for NX Designers 18-23

 Introduction to Drafting

Edit an existing note or label

1. Right-click the existing note or label.

2. Choose the appropriate option from the shortcut menu.

You can display the Note dialog box and edit text by double-clicking
the note or label.

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 Introduction to Drafting

Create a Master Model Drawing

1. Open the master model part file. (File→Open)

2. Start the Assemblies application. (Start→Assemblies)

3. Create a new parent part. (Assemblies→Components→Create New

Parent, xxxxx_dwg)
You can also create a drawing file using by choosing File→New and
selecting a Drawing template.

4. Start the Drafting application. (Start→Drafting)

5. Adjust the sheet; name, units, size, and projection angle. (Edit→Sheet)

6. Add the drawing formats; title block, border, revision block, standard
notes.

7. Set view display preferences; hidden line removal, section backgrounds,

and threads. (Preferences→View)

8. Add the base view, typically the top or front view. (Insert→View→Base
View and select the model view to use)

9. Add more views; projected, detail, section, isometric, and exploded.

(Insert→View)

10. Adjust the view display; size, orientation, etc. (Edit→Style or Edit→View)

11. Clean up individual views with view dependent edits; erase object, edit
entire object, and edit object segment. (Edit→View→View Dependent
Edit)

12. Add utility symbols; centerlines, target symbols, and intersection symbols.
(Insert→Centerline or Insert→Symbol) 18
13. Add dimensions. (Insert→Dimension)

14. Add the notes, labels, and GD&T symbols. (Insert→Note or

Insert→Feature Control Frame)

Essentials for NX Designers 18-25

 Introduction to Drafting

Activities: Drafting — Notes and labels

In the Introduction to drafting section, do the activity:
• Create notes and labels

Project: Drafting
In the Projects section, complete the Drafting exercise.

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 Introduction to Drafting

Summary: Drafting
Use the Drafting application to create and edit drawing sheets. Views and
dimensions on a drawing sheet are associative to the solid model and update
when changes are made to the model.
Use the Note command to create notes and labels.
In this lesson you:
• Applied the master model concept to create a drawing.

• Modified a drawing sheet.

• Added views to a drawing sheet.

• Created dimensions.

• Added notes to a drawing sheet.

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Essentials for NX Designers 18-27

18
Lesson

19 Editing models

Purpose

This lesson introduces editing techniques.

Objectives
Upon completion of this lesson, you will be able to:
• Edit a master model and update an associated non-master part.

• Edit a model using synchronous modeling techniques.

19

Essentials for NX Designers 19-1

 Editing models

Editing parametric models

The techniques you use to edit an existing parametric model depend on the
modeling strategy used to create the part and feature history. The modeling
strategy is determined by the design intent which considers the requirements
of the part, relationships between features, and potential changes.
The following changes are typical for a parametric model.
• Edit sketch dimensions and constraints

• Edit feature parameters (extrude distance, edge blend radius, or hole

diameter for example)

• Edit expression values or formulas

• Reattach or replace features

• Add or delete features

19

19-2 Essentials for NX Designers mt10051_s NX 7

 Editing models

Synchronous modeling
You can use Synchronous Modeling commands to modify a model regardless
of its origins, associativity, or feature history.
You could apply Synchronous Modeling to:
• Edit a model that was imported from another CAD system and has no
feature history or parameters.

• Edit a model due to a change in design intent that was not anticipated
when it was created. Incorporating the change into the existing
construction history would require a lot of rework and loss of associativity.

Synchronous Modeling is primarily suited for use on models composed of

analytic faces types like plane, cylinder, cone, sphere, torus. This does not
necessarily mean “simple” parts, since models with many thousands of faces
are composed of these face types.

19

Essentials for NX Designers 19-3

 Editing models

Move Face overview

Use the Move Face command to move a set of faces and automatically adjust
adjacent blend faces.
You can use linear or angular transform methods to move the selected faces.
Move Face is a useful design tool that facilitates easy design change during
the design process. It is also useful in downstream applications like Tooling,
Manufacturing, and Simulation, where you can directly make changes to the
model, regardless of feature history.
Some scenarios where you can use the Move Face command are:
• To relocate a group of faces to a different position to meet design intent.

• To relocate a series of faces in several components of an assembly. (All

components and assembly must be in History-Free mode.)

• To change the bend angle of a sheet metal part that has no history.

• To rotate a face or set of faces about a given axis and about a point. For
example, to change the angular position of a keyway slot.

• To change the orientation of an entire solid body, irrespective of its history,

to a different orientation.

19

19-4 Essentials for NX Designers mt10051_s NX 7

 Editing models

Where do I find it?

Application Modeling and Shape Studio

Toolbar Synchronous Modeling→Move Face

Menu Insert→Synchronous Modeling→Move Face

19

Essentials for NX Designers 19-5

 Editing models

Move Face options

1 Select Face Lets you select a face or faces to move.

2 Face Finder Lets you select faces based on how their geometry
compares with the selected face.
3 Motion Provides linear and angular transform methods for the
faces you select to move.

19

19-6 Essentials for NX Designers mt10051_s NX 7

 Editing models

Resize Blend overview

Use the Resize Blend command to change the radii of blend faces regardless
of their feature history.
The Resize Blend command works with translated files and unparameterized
solids.

In this example, the red face in the body on the left is resized using Resize
Blend.
The dependent blue face updates automatically.

Where do I find it?

Application Modeling

Toolbar Synchronous Modeling→Resize Blend

Menu Insert→Synchronous Modeling→Resize Blend

19

Essentials for NX Designers 19-7

 Editing models

Optimize Face overview

Use the Optimize Face command to simplify surface types, merge faces,
improve edge accuracy, and recognize blends.

Use this command on models imported into NX to convert B-surface faces

to analytic faces.

Where do I find it?

Application Modeling and Shape Studio

Prerequisite You must be in History-free mode

Toolbar Synchronous Modeling→Optimize Face

Insert→Synchronous Modeling→Optimize→Optimize
Menu Face

19

19-8 Essentials for NX Designers mt10051_s NX 7

 Editing models

Activities: Editing models

In the Editing models section, do the activities:
• Edit the parameters of a master model

• Move faces using synchronous modeling

• Resize blends using synchronous modeling

19

Essentials for NX Designers 19-9

 Editing models

• Optimize faces to analytic surfaces using synchronous modeling

19

19-10 Essentials for NX Designers mt10051_s NX 7

 Editing models

Summary: Editing models

Synchronous Modeling commands can be used to quickly edit a model that
has no feature history or that requires a change in the design intent which
was not anticipated when it was constructed.
In this lesson, you:
• Edited a model parametrically by modifying existing expressions and
features.

• Edited models using Synchronous Modeling commands.

19

Essentials for NX Designers 19-11

19
Appendix

A Practice projects

This appendix contains additional practice projects.

A
Essentials for NX Designers A-1
 Practice projects

Practice Project 1

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 Practice projects

Practice Project 2

A
Essentials for NX Designers A-3
 Practice projects

Practice Project 3

A
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 Practice projects

A
Essentials for NX Designers A-5
 Practice projects

Practice Project 4

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 Practice projects

A
Essentials for NX Designers A-7
 Practice projects

Practice Project 5

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 Practice projects

A
Essentials for NX Designers A-9
 Practice projects

Practice Project 6

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 Practice projects

A
Essentials for NX Designers A-11
 Practice projects

Practice Project 7

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 Practice projects

A
Essentials for NX Designers A-13
 Practice projects

Practice Project 8

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 Practice projects

A
Essentials for NX Designers A-15
 Practice projects

Practice Project 9

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 Practice projects

A
Essentials for NX Designers A-17
 Practice projects

Practice Project 10

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 Practice projects

Practice Project 11

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Essentials for NX Designers A-19
 Practice projects

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 Practice projects

Practice Project 12

A
Essentials for NX Designers A-21
 Practice projects

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 Practice projects

Practice Project 13

A
Essentials for NX Designers A-23
 Practice projects

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 Practice projects

Practice Project 14

A
Essentials for NX Designers A-25
 Practice projects

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 Practice projects

Practice Project 15

A
Essentials for NX Designers A-27
 Practice projects

Practice Project 16

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 Practice projects

A
Essentials for NX Designers A-29
 Practice projects

Practice Project 17

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 Practice projects

A
Essentials for NX Designers A-31
 Practice projects

Practice Project 18

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 Practice projects

A
Essentials for NX Designers A-33
 Practice projects

Practice Project 19

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 Practice projects

A
Essentials for NX Designers A-35
 Practice projects

Practice Project 20

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 Practice projects

A
Essentials for NX Designers A-37
 Practice projects

Practice Project 21

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 Practice projects

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Essentials for NX Designers A-39
 Practice projects

Practice Project 22

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Essentials for NX Designers A-41
A
 B
Appendix

B Expression operators

This appendix describes the operators and functions that you can use in
expressions.

Essentials for NX Designers B-1

 Expression operators

B
Operators
There are several types of operators that you may use in the expression
language.

Arithmetic operators Example

+ Addition p2=p5+p3
- Subtraction and Negative Sign p2=p5–p3
* Multiplication p2=p5*p3
/ Division p2=p5/p3
% Modulus p2=p5%p3
^ Exponential p2=p5^2
= Assignment p2=p5

Relational and Boolean operators

> Greater Than
< Less Than
>= Greater Than or Equal
<= Less Than or Equal
== Equal
!= Not Equal
! Negate
& or && Logical AND
| or || Logical OR

B-2 Essentials for NX Designers mt10051_s NX 7

 Expression operators

B
Precedence and associativity
In the table below, operators in the same row have equal precedence while
operators in the following rows have less precedence.

Precedence and associativity

Operators Associativity
^ Right to left
– (change sign)
* / % Left to right
+ –
> < >= <=
== !=
&&
||
= Right to left

When using operators with the same precedence in an equation without

parameters, use left-to-right or the right-to-left rule from the table. For
example:
X = 90 – 10 + 30 = 110 (not 50)

X = 90 – (10 + 30) = 50

Essentials for NX Designers B-3

 Expression operators

B
Legacy unit conversion
Although when dimensionality is specified and units are assigned the
system handles conversions, legacy parts may have used functions for unit
conversion. For legacy compatibility these functions are supported.

Functions for unit conversion

cm cm(x) converts x from centimeters to the default units of the part
ft ft(x) converts x from feet to the default units of the part
grd grd(x) converts x from gradients to degrees
in in(x) converts x from inches to the default units of the part
km km(x) converts x from kilometers to the default units of the part
mc mc(x) converts x from microns to the default units of the part
min min(x) converts x from minutes to degrees.
ml ml(x) converts x from mils to the default units of the part
mm mm(x) converts x from millimeters to the default units of the part
mtr mtr(x) converts x from meters to the default units of the part
sec sec(x) converts x from seconds to degrees
yd yd(x) converts x from yards to the default units of the part

B-4 Essentials for NX Designers mt10051_s NX 7

 Expression operators

B
Built-in functions
Built-in functions include math, string, and engineering functions.

Scientific notation
You may optionally enter numbers in scientific notation. The value you enter
must contain a positive or negative sign. For example, you can enter:
2e+5 which is the same as the value 200000

2e-5 which is the same as the value .00002

Built-in functions
abs Returns the absolute value of a given number
arccos Returns the inverse cosine of a given number in degrees
arcsin Returns the inverse sine of a given number in degrees
arctan Returns the inverse tangent of a given number in degrees
from –90 to +90
arctan2 Returns the inverse tangent of a given delta x divided by a
given delta y in degrees from –180 to +180
ASCII Returns the ASCII code of the first character in a given
string or zero if the string is empty
ceiling Returns the smallest integer that is bigger than a given
number
Char Returns the ASCII character for a given integer in the
range 1 to 255
charReplace Returns a new string from a given source string, character
to replace and the corresponding replacement characters.
compareString Case sensitive compare of two strings
cos Returns the cosine of a given number in degrees
dateTimeString Returns the system date and time in the format “Fri Nov
21 09:56:12 2005/n”
floor Returns the largest integer less than or equal to a given
number
format Returns a formatted string, using C-style formatting
specification
getenv Returns the string value of a given environment variable
string
hypcos Returns the hyperbolic cosine of a given number
hypsin Returns the hyperbolic sine of a given number
hyptan Returns the hyperbolic tangent of a given number

Essentials for NX Designers B-5

 Expression operators

B
Built-in functions
log Returns the natural logarithm of a given number
log10 Returns the logarithm base 10 of a given number
MakeNumber Returns the number or integer of a given numerical string
max Returns the largest number from a given number and
additional numbers
min Returns the smallest number from a given number and
additional numbers
mod Returns the remainder (modulus) when a given numerator
is divided by a given denominator (by integer division)
NormalizeAngle Normalizes a given angle (degrees) to be between 0 and
360 degrees
pi() Returns pi
Radians Converts an angle in degrees into radians
replaceString Replaces all occurrences of str1 with str2
round Returns the integer nearest to a given number, returns the
even integer if the given number ends in .5
sin Returns the sine of a given number in degrees
sqrt Returns the inverse square root of a given positive number
StringLower Returns a lowercase string from a given string
StringUpper Returns an uppercase string from a given string
StringValue Returns a string containing a textual representation of a
given value
subString Returns a new string containing a subset of the elements
from the original list
tan Returns the sine of a given number
ug_ functions see the documentation for descriptions of dozens more
specialized math and engineering functions

B-6 Essentials for NX Designers mt10051_s NX 7

Appendix

C Point options
C

This appendix describes the options to create points.

Essentials for NX Designers C-1

 Point options

Point dialog box

Use the Point dialog box to create point objects or specify locations in
three-dimensional space.
C You specify a point by choosing a type and selecting geometry or by typing X,
Y, and Z coordinates directly.

C-2 Essentials for NX Designers mt10051_s NX 7

 Point options

Point types
The Type group of the Point dialog box has buttons representing various
methods for specifying a point. As the cursor is passed over these buttons,
text shows the name of the method.
C
Inferred Point Specifies the point option to use based on your
selection.
Cursor Location Specifies a position at the location of the cursor. The
location lies in the plane of the WCS.
Existing Point Specifies a position by selecting an existing point
object.
End Point Specifies a position at the end points of existing lines,
arcs, conics, and other curves.
Control Point Specifies a position at the control points of geometric
objects.
Intersection Point Specifies a position at the intersection of two curves or
at the intersection of a curve and a surface or plane.
Arc/Ellipse/Sphere Specifies a position at the center of an arc, ellipse,
Center circular or elliptical edge, or sphere.
Angle on Arc/Ellipse Specifies a position at an angular position along an
arc or an ellipse.
Quadrant Point Specifies a position at the quarter points of an arc or
an ellipse. You can also define a point on the extension
of an arc.
Point on Curve/Edge Specifies a position on a curve or edge. The U
parameter can be edited.
Point on Face Specifies a position on a face. The U and V parameters
can be edited.
Between Two Points Specifies a position mid way between two points.
By Expression Specifies a point using an expression of the type Point.

Essentials for NX Designers C-3

 Point options

WCS and absolute coordinates

When Associative is inactive in the settings group, you can, in the
Coordinates group, select Relative to WCS or Absolute (the default) to
specify the coordinate system to reference.
C
Enter values in the X, Y, or Z boxes.

C-4 Essentials for NX Designers mt10051_s NX 7

Appendix

D Primitive solids

This appendix describes the common commands to create primitive solids. D

Essentials for NX Designers D-1

 Primitive solids

Primitive solids
A primitive is a solid body that is has an basic mathematical shape.
As an alternative to sketching when the model is quite simple, you could use
a primitive as the base feature of your solid model.
When you create a primitive body, you specify its type, size, location, and
orientation.
The four types of primitives are:
D • Block

• Cylinder

• Cone

• Sphere

Although NX allows the use of multiple primitives, the practice is not

recommended.

D-2 Essentials for NX Designers mt10051_s NX 7

 Primitive solids

Block
Create a Block by specifying the size and location.
The orientation is inferred from the WCS.
There are three Type options you can use to create a Block:
• Origin and Edge Lengths

• Two Points and Height D

• Two Diagonal Points

Essentials for NX Designers D-3

 Primitive solids

Cylinder
Create a Cylinder by specifying the axis vector, location, and size.
There are two Type options you can use to create a Cylinder:
• Axis, Diameter, and Height

• Arc and Height

D

D-4 Essentials for NX Designers mt10051_s NX 7

Appendix

E Features with predefined shapes

This appendix discusses additional features that can be associatively

positioned. Features formerly called form features include holes, slots, bosses,
pads, pockets and grooves.

Essentials for NX Designers E-1

 Features with predefined shapes

Boss
The Boss feature is used to add a cylindrical shape with a specified height to
a model, having either straight or tapered sides.
1 — Diameter
2 — Height
3 — Taper Angle

E
A positive or negative value may be entered depending on which way the wall
is to incline. A zero value results in a vertical cylinder wall.

E-2 Essentials for NX Designers mt10051_s NX 7

 Features with predefined shapes

Slot
This option allows you to create a slot in a solid body as if cut by a milling
machine tool. In each case, the shape of the cutting tool corresponds to the
slot type and dimensions.
The slot feature will be created so that the axis of the cutting tool is normal to
the face or datum plane selected. Initially, the path of the slot will be parallel
to the selected Horizontal Reference.
There are several different slot types available. You will be prompted for the
parameters that apply to the type of slot chosen.

Rectangular slot
The Rectangular slot type uses a tool that has cylindrical end faces and will E
produce sharp edges along the bottom of the slot.
1 — Length
2 — Width
3 — Depth

The Width of the rectangular slot represents the diameter of the cylindrical
cutting tool.
The Depth of the slot is measured in a direction parallel to the tool axis from
the placement face to the bottom of the slot. Depth values must be positive.
The Length is measured parallel to the horizontal reference (X in the feature
coordinate system). Length values must be positive.

Essentials for NX Designers E-3

 Features with predefined shapes

Other slot types

The other available slot profiles are shown below.

Ball-End

U-Slot

T-Slot

E Dove-Tail

Thru slot

The Thru Slot option can be applied to all slot types and extends the length of
the slot along the placement face in the direction of the horizontal reference
between two specified faces.
You will be prompted to select starting and ending thru faces instead of a
length parameter. The two thru faces cannot be parallel to the placement face.
The rectangular slot shown below was created with the Thru Slot option
enabled. The selected starting and ending thru faces are shaded.

You should not dimension to the end arcs of the slot when positioning a Thru
Slot. The length of a Thru Slot is determined by the selected thru faces. The
only positioning dimension required is to locate an edge or centerline along
the length of the slot (tool) to a target edge or datum. Parallel at a Distance
can be used to constrain the feature and control the two remaining degrees
of freedom.

E-4 Essentials for NX Designers mt10051_s NX 7

 Features with predefined shapes

Pocket
The pocket feature is used to create a cavity in a solid body.
There are three types of pockets:
• Cylindrical (not covered in this lesson)

• Rectangular

• General (not covered in this lesson)

Rectangular pocket

This option allows a rectangular pocket to be defined to a specified depth, with

or without a floor and/or corner radius, having either straight or tapered walls.
E
The following parameters may be specified:
1 — Length
2 — Width
3 — Depth
4 — Corner Radius
5 — Floor Radius
6 — Taper Angle

The pocket is initially oriented so that the Length is parallel to the

selected Horizontal Reference.

Pocket features may be positioned from a tool edge or from the centerlines
provided for this purpose.

Essentials for NX Designers E-5

 Features with predefined shapes

Pad
This option allows a raised pad on a solid body.
There are two types of pads:
• Rectangular

• General (not covered in this lesson)

Rectangular pad

This option allows a rectangular pad to be defined to a specified height, with

or without a corner radius and/or taper.
E The following parameters may be specified:
1 — Length
2 — Width
3 — Height
4 — Corner Radius
5 — Taper Angle

The pad is initially oriented so that the Length is parallel to the

selected Horizontal Reference.

E-6 Essentials for NX Designers mt10051_s NX 7

 Features with predefined shapes

Groove
The groove feature requires a cylindrical or conical placement face. A groove
can be thought of as a feature that would result from a part being cut in a
lathe. After specifying the groove parameters, you will be shown a preview
of the tool solid. The tool solid can be thought of as the path that the lathe
would make as it cuts the solid.

Positioning a Groove

You only have to position a groove along the axis of the cylindrical or conical
placement face. The Positioning dialog box will not appear. Instead, you are
only required to specify a horizontal dimension along the axis by selecting a
target edge followed by a tool edge or centerline.
E
Two grooves are shown in the following example.
1 — Target Edge
2 — Tool Edge (or centerline)

Essentials for NX Designers E-7

 Features with predefined shapes

Positioning methods
Positioning is a legacy method used to place the legacy form features relative
to other geometry.

Horizontal

Specifies the horizontal distance between two points, one on the target solid
and the other on the tool solid. Horizontal is measured along the X-axis of the
feature coordinate system (the Horizontal Reference). As edges are selected,
the nearest valid point is selected (midpoints are not selectable).
1 — Horizontal Reference
2 — Target Edge (End Point)
E
3 — Tool Edge (Tangent Point)

E-8 Essentials for NX Designers mt10051_s NX 7

 Features with predefined shapes

Vertical

Specifies the vertical distance between two points, one on the target solid and
the other on the tool solid. Vertical is measured along the Y-axis of the feature
coordinate system (perpendicular to the Horizontal Reference). As edges are
selected, the nearest valid point is selected (midpoints are not selectable).
1 — Horizontal Reference
2 — Target Edge (End Point)
3 — Tool Edge (Arc Center)

Essentials for NX Designers E-9

 Features with predefined shapes

Perpendicular

Specifies the shortest (normal) distance between a linear edge on the target
solid (also datum planes or axis) and a point on the tool solid. The linear
target edge is always selected first.
1 — Target Edge
2 — Tool Edge (Arc Center)

Point onto Line

Specifies that the distance between an edge on the target solid (also datum
planes or axis) and a point on the tool solid is zero.
Point onto Line is the same as the Perpendicular positioning dimension
with the value automatically set to zero. You can change it to a non-zero
value when you edit the feature.

1 — Target Edge (Datum Plane)

2 — Tool Edge (Arc Center)

E-10 Essentials for NX Designers mt10051_s NX 7

 Features with predefined shapes

Parallel

Specifies the shortest distance between two points, one point on the target
solid and the other point on the tool solid. As edges are selected, the nearest
valid point is selected (midpoints are not selectable).
1 — Target Edge (Arc Center)
2 — Tool Edge (Arc Center)

Point onto Point

Specifies the distance between a point on the target solid and a point on the
tool solid is zero. This is commonly used to align arc centers (concentric) of
cylindrical or conical features. This method fully constrains their location
since rotation is not a degree of freedom for cylindrical or conical features.
Point onto Point is the same as the Parallel positioning dimension with
the value automatically set to zero. You can change it to a non-zero
value when you edit the feature.

1 — Target Edge (Arc Center)

2 — Tool Edge (Arc Center)

Essentials for NX Designers E-11

 Features with predefined shapes

Parallel at a distance
Specifies that a linear edge on the target solid (also a datum plane or datum
axis) and a linear edge on the tool solid must be parallel and at a given
distance. This is typically used for features with length (slot, pocket or pad).
Using Parallel at a Distance will solve two of the three degrees of freedom
necessary to fully specify a feature having a length (rotation and translation
in one direction). Adding another Parallel at a Distance or Line onto Line
dimension would overspecify the location of the feature.
To fully specify the feature in the example an additional positioning
dimension is required to solve the final degree of freedom (i.e. Horizontal,
Vertical, Perpendicular).
1 — Target Edge
E
2 — Tool Edge (Centerline of Slot)

E-12 Essentials for NX Designers mt10051_s NX 7

 Features with predefined shapes

Line onto line

Specifies that the distance between a linear edge on the target solid (or a
datum plane or datum axis) and a linear edge on the tool solid is zero and
they are constrained parallel to each other. This is typically used for features
with length (slot, pocket, or pad).
Using Line onto Line will solve two of the three degrees of freedom necessary
to fully specify a feature having a length (rotational and translation in one
direction). Adding another Line onto Line or Parallel at a Distance dimension
would overspecify the location of the feature. To fully specify the feature in
the above example an additional positioning dimension is required to solve
the final degree of freedom (i.e. Horizontal, Perpendicular, or Point onto Line).
Line onto Line is the same as the Parallel at a Distance positioning
dimension with the value automatically set to zero. This zero value can E
be changed to a non-zero value when editing the feature.

1 — Target Edge (Datum Plane)

2 — Tool Edge (Centerline of Slot)

Essentials for NX Designers E-13

 Features with predefined shapes

Angular

Specifies that a linear edge on the target solid (also a datum plane or datum
axis) and a linear edge on the tool solid must be at a given angle to each
other. The angle is measured in a counter-clockwise direction (with respect to
the feature coordinate system), from the ends of the edges nearest to where
they are selected.
1 — Target Edge
2 — Tool Edge (Edge of Pocket)

E-14 Essentials for NX Designers mt10051_s NX 7

 Features with predefined shapes

Edit positioning
As features are created the parametric data is captured in expressions.
The parametric data consists of the actual feature size definition (i.e.
diameter, height, length) as well as the positional data that is captured in
the positioning dimensions.
This option allows a feature to be moved by editing its positioning dimensions.
In addition, positioning dimensions may be added to features that are either
underspecified or were not given any positioning dimensions at the time
of creation.
Once the feature has been selected, the following options are offered based
upon the positioning status of the selected feature:
• Add Dimension

• Edit Dimension Value E

• Delete Dimension

Essentials for NX Designers E-15

 Features with predefined shapes

Add dimension

This option may be used to add a positioning dimension to a feature.

When adding positioning dimensions, any edge (1) resulting from the
intersection of the feature being positioned (2) and a face on the target solid
(3) may not be selected as the tool edge.

Valid target edges for positioning purposes must belong to features existing
E in the feature creation list of the model before the feature being positioned.

Edit dimension value

Features may be moved by changing the values of the feature’s positioning
dimensions.
To use this option:
• Select the dimension to edit (if there is only one positioning dimension, it
is selected automatically).

• Type the new value.

Continue editing as many dimension values as desired. Once all the desired
dimension values have been edited, click OK.

E-16 Essentials for NX Designers mt10051_s NX 7

 Features with predefined shapes

Delete dimension

Use this option to delete a positioning dimension from a feature. The feature
will then remain in its current location as its position is no longer associated
to the model.
If you are replacing a dimension, add the new dimension before deleting
the old one. The Edit Positioning dialog box is maintained when you
add a dimension but is automatically dismissed when you delete a
dimension.

Display dimensions

The Display Dimensions option in the Feature Browser temporarily displays

the parameters of size and location in the graphics window for the feature.
Refreshing the graphics window removes the temporary display of the E
parameters.
Display Dimensions can also be accessed using the Part Navigator.

Essentials for NX Designers E-17

E
Appendix

F Customer Defaults

This appendix describes utilities and customization files which affect the
default interface and behavior of NX. These topics would normally be the
responsibility of a system administrator.

Essentials for NX Designers F-1

 Customer Defaults

Customer Defaults
Customer defaults are accessed by choosing File→Utilities→Customer
Defaults.
When NX is first started (out-of-the-box) the defaults are set to User and a
variable points to a user file which may or may not exist. This is an extract
from the log file for a user named “nxuser” after logging in and starting NX
for the first time:
Processing customer default values file
C:/Documents and Settings/nxuser
/Local Settings/Application Data/Unigraphics Solutions
/NX7/nx7_user.dpv
User customizations file
C:/Documents and Settings/nxuser
/Local Settings/Application Data/Unigraphics Solutions
/NX7/nx7_user.dpv does not exist

The fact that the file does not exist is of no concern because the path is
writable for the person logged in.
NX will create the file nx7_user.dpv when and if the user makes a change to
F the defaults.
If the administrator wishes to prevent the user from changing the defaults,
i.e., set them as User (Read Only), there are various ways to accomplish it:
• Create the file and customize it as you wish, and then make it read only.

• Define the file in a path to which the user cannot write. The file and the
path need not exist.

• Lock one or more defaults at a higher level, i.e. group or site level.

F-2 Essentials for NX Designers mt10051_s NX 7

 Customer Defaults

Customer Defaults levels

Customer defaults can be controlled at three levels: Site, Group, and User.
Site is the highest level, User is the lowest. Any or all of these levels may be
available to you, based on how the customer default environment variables
are defined at your site. If none of the environment variables are defined, the
level is Shipped (read-only).

System administrators or managers at a higher level can lock the settings of F

customer defaults that they do not want anyone at the lower levels to change.
The Group level can lock customer defaults at the User level, and the Site
level can lock defaults at the Group and User levels. You cannot lock defaults
at the User level.
When a lock is active not only is the text de-emphasized but value change
is prohibited. Even if the site (or a lower) DPV file is writable the value of
a locked default can not be changed until the lock icon has been toggled off
for the given default).

Essentials for NX Designers F-3

 Customer Defaults

For example, to lock out the ability to create promoted bodies, the manager
clicks the lock beside promotions at the site or group level. The icon changes
color and the text is de-emphasized.

At the user level, that default is de-emphasized an a padlock is displayed

beside it.

The manager can use the Default Lock State option to set the global locked
status for all of the customer defaults on all defaults pages. This allows
strategies like All are locked except...or All are unlocked except... instead of
requiring the assertion of 5000+ individual locks.
Locks at the group level change color and the text is de-emphasized.
The user then sees all options for Site Standards de-emphasized and
padlocked. This prevents Site Standards from being changed at the user level.

F-4 Essentials for NX Designers mt10051_s NX 7

 Customer Defaults

Setting Customer Defaults

Customer defaults have as-shipped default settings that are hard-coded.

When you change defaults at any level (assuming you have write permission
and the levels are defined) a file is created to save the settings. By default the
file is called nx7_user.dpv, nx7_group.dpv, or nx7_site.dpv.
Only the defaults that are changed from the hard–coded settings are saved,
thus the DPV files can be very small in size.
Customer defaults files are defined by environment settings. These are
typically set in ugii_env.dat on Windows systems; however, the administrator
may prevent a user from spoofing these settings by creating a file named
ugii_env.master in the UGII directory where NX is installed to define these
particular environment settings. When this file exists any attempt to redefine
the environment variables will be ignored.
When you change defaults the changes are NOT effective immediately.
They will be in effect the next time NX is started.

Essentials for NX Designers F-5

 Customer Defaults

Customer Defaults environment variables

To set up a User, Group, or Site level, you must define the appropriate
environment variable with a directory. You must first create a directory
named startup where you want to store the customer defaults file for that
level.

Level Variable Defaults File

(in the startup directory)
User UGII_USER_DIR nx7_user.dpv
Group UGII_GROUP_DIR nx7_group.dpv
Site UGII_SITE_DIR nx7_site.dpv

If you are already using the UGII_USER_DIR environment variable for other
purposes, you can use the UGII_LOCAL_USER_DEFAULTS environment
variable. When you define the environment variable, you must point it to the
.dpv file you will use (instead of just the directory, as done with the other
environment variables).

F If both of these environment variables are defined, the system uses

the UGII_LOCAL_USER_DEFAULTS environment variable to define
the customer defaults User level. NX is shipped with this variable
defined, so if you want to use a common user directory (i.e., the one
defined by UGII_USER_DIR), you must remove the definition for
UGII_LOCAL_USER_DEFAULTS from your environment variables
file.

F-6 Essentials for NX Designers mt10051_s NX 7

 Customer Defaults

USER, GROUP, and SITE directories

There is a standard structure for customer site installation of menu files and
shared libraries. This directory structure defines three subdirectories. For
the purpose of this discussion only the startup folder need exist; however, you
might encounter the others if you have site customization.

startup Contains site-specific menu files, defaults files, and shared

libraries of menu actions to be loaded automatically at NX
startup to customize Gateway.
application Contains site-specific files defining menus and shared
libraries of menu actions for customizing NX or third-party
applications, such as NX Open programs. Loading of each
shared library is deferred until you enter the application that
names the library on the LIBRARIES statement in the menu
file definition for the Application Button for the application.
User Tool Definition files, GRIP programs, User Function
programs that are referenced by menu file actions.
udo Contains the shared libraries defining methods for
site-specific User Defined Objects (another NX Open topic.) F

Essentials for NX Designers F-7

 Customer Defaults

Managing your changes

The DPV files contain only the defaults that are changed from the hard–coded
settings.
You may review your changes at any time:
• Set the Defaults Level to the level you want to examine, Site, Group,
or User.

• On the Customer Defaults dialog box, click Manage Current Settings.

Here is an example of standard classroom defaults at the group level:

F-8 Essentials for NX Designers mt10051_s NX 7

 Customer Defaults

Updating to a new release of NX

To update to a new release, you need only define the DPV files you want to
use at whatever levels your organization uses.
When you receive the new software use Import Defaults to validate your

previous settings against the new release.

Importing Customer Defaults values file: <full path specification of DPV
file.>

Total settings and locks imported: 10

Total settings rejected due to values not valid in this release: 0

Total settings rejected due to values being locked at the higher level: 0

Total settings already set to the same value and lock status: 0

Total settings not recognized in this release: 0

Essentials for NX Designers F-9

F
Appendix

G Custom Roles

Roles provide a method to create a custom user interface based on a user

or departments needs.
In this appendix, you will create user and group roles.

Essentials for NX Designers G-1

 Custom Roles

User-Defined Roles
By default, when you begin an NX session you are presented with a core set
of functionality but more specific Roles (sets of tools) can be accessed through
the Resource bar.
These prepackaged roles are a starting point from which you can customize
the NX user interface and save as a personal user role.
As a user, there are two different repositories for user-defined roles:
• The User folder where you can store your individual roles that reflect your
personal user interface layouts with their specific menus, toolbars etc.

G
Because these are your personal roles, the .mtx files that define them
reside in a user directory. In Windows, these roles reside in /Documents
and Settings/<yourname>/Local Settings/Application Data/Unigraphics
Solutions/NX7/Roles/

• A new palette which references roles in a directory.

You can use these palettes to store departmental/group specific roles and
put permission restrictions on their respective directories.

G-2 Essentials for NX Designers mt10051_s NX 7

 Custom Roles

Create a User Role

It is important to customize the interface (toolbars, menus, etc.) the
way you want it before you create a role.

1. On the Resource bar, click the Roles tab .

2. Right-click in the background of the Roles palette and choose New User
Role.
This displays the Role Properties dialog box.

3. Specify the role properties.

1. Name of the .mtx file as

stored
2. Name of Role as referenced
in your NX interface
3. Graphic for the Role icon;
type in name or Browse
4. Description of the role.
5. Application(s) referenced in
Role G
6. Toggles to structure Role;
Current Only is used
to capture a customized
interface
7. If selected, the settings for all
dialog boxes in the selected
applications are stored with
the Role.

Essentials for NX Designers G-3

 Custom Roles

4. Click OK to create new ’User’ role.

G-4 Essentials for NX Designers mt10051_s NX 7

 Custom Roles

Activity: Create a User Role

In this activity you will create a user role.
Step 1: Open roles_1.
The buttons and menu options you see here reflect the base
functionality of Gateway when you start a new part.

Step 2: Select a Role.

Choose the Roles tab on the Resource bar and pin the
Roles pane.

From the System Defaults folder, click the Advanced role.

In the Load Role message box, click OK.

Choose Tools→Customize and change your user interface

(menus, options, toolbars) as desired.
Disregard the Roles tab in the Customize dialog box; you
will learn about its purpose later in the activity.

Step 3: Create a User role to store your customized user interface. G

Right-click in the background of the Roles pane and choose
New User Role.

The Role Properties dialog box is displayed.

Step 4: Define your User role properties.

In the Name box, type role_1_xxx, where xxx are your initials.

This is the name of your role as it will appear in the Resource bar
Roles pane.
The name of the .mtx file (top of dialog) is system-assigned.
The name of your role must be assigned by you.

Click Browse and navigate to the parts directory; that’s where

the image files are.

Set the Files of type to JPEG Files.

Select a role_image_xx file and click OK.

Essentials for NX Designers G-5

 Custom Roles

In the Description box, type the date <mmddyyyy> – <your

last name, first name> – first user role. (Example: 07042008
– Doe, John – first user role)
Your company may set description standards in place
for this data.

Select the Current Only check box.

Notice the Current Only option captures your current,

customized user interface, by application.

Click OK.

Your user role is created.

Step 5: Close the part.

G-6 Essentials for NX Designers mt10051_s NX 7

 Custom Roles

Edit a User Role

After a user role is created, changes can be made by using the Edit
option.

1. Make the toolbar changes that you want to incorporate.

2. On the Resource bar, click the Roles tab .

3. On the Roles palette, in the User group, right-click your role and choose
Edit.
This displays the Role Properties dialog box.

4. From the Toolbar Layout, Menus and Dialog Memory group, select the
Use Current Session radio button.

5. Click OK to update ’User’ role with the changes.

Essentials for NX Designers G-7

 Custom Roles

Create a Group Role

It is important to customize the interface (toolbars, menus, etc.) before
you create a role. If you decide later you want additional customizations
saved with a specified role, you will have to recreate the role.

1. Create a folder to store group roles in a writable directory.

2. Choose Preferences→Palettes.

3. Click Open Directory as Role Palette .

4. Navigate to the directory you want the new Role palette to point to. This
creates a tab on the Resource bar.

5. Choose Tools→Customize and customize your interface however you

wish.

6. In the Customize dialog box, click the Roles tab.

7. Click Create.

8. Navigate to your roles directory.

9. Type a File name for your role and click OK.

10. In the Role Properties dialog box, specify the role definition.
Name of role
Image for icon
Description
Application check boxes

11. Click OK to create the role.

G-8 Essentials for NX Designers mt10051_s NX 7

 Custom Roles

12. On the Resource bar, in your new palette, right-click and choose Refresh
to see the icon of the new role.

Essentials for NX Designers G-9

 Custom Roles

Activity: Create a Role Palette with a Group Role

In this activity, you will create a role palette with a group role that could
be shared with other users.
Step 1: Create a new folder for the group roles.
In a writable directory, create a folder named grp_role_xxx,
where xxx is your initials.

The group-specific roles will be stored here. The group role palette
will point to this directory.

Step 2: Open roles_1.

Step 3: Customize the user interface.

This interface would be based on the design needs of the group.

Choose Tools→Customize and customize the user interface.

Step 4: Create your role.

In the Customize dialog box, select the Roles tab.

On this page, you can Load an existing user role (.mtx file), create a
new role, and define keyboard accelerators associated with the role.
Click Create.
G
The New Role File dialog is displayed.

Step 5: Define your new role file.

Expand the Save in list and navigate to the writable directory
you created.

In the File name box, type custom_role_1_xxx, where xxx

are your initials, and click OK.
This will be the name of your custom .mtx file. In the first
(user) role you created, this action was done internally by
NX.

Step 6: Define the properties of the new role.

In the Role Properties dialog box, in the Name box, type
custom_1_xxx, where xxx are your initials.

This is the name of your role as it will appear in the Resource bar
Roles pane.
The Role Properties dialog is displayed.

G-10 Essentials for NX Designers mt10051_s NX 7

 Custom Roles

Click Browse and navigate to the parts directory where the

image files are located.

Set the Files of type to JPEG Files.

Select a role_image_xx file and click OK.

In the Description box, type in the date <mmddyyyy> – <a

short description of role>. (Example: 11032005 – custom UI
for xyz project)

In the Role Properties dialog box, select the Current Only

check box.

Click OK.

Your custom role is created and is now located in the writable

directory you defined.

Close the Customize dialog box.

Step 7: Define your new Role palette

Choose Preference→Palettes.

Click Open Directory as Role Palette.

G
Browse to the writable directory where your custom .mtx file
resides.

Select your custom_role_1_xxx.mtx file and click OK.

If you do not see any entries, make sure Files of type is
set to All Files (*.*)

If your directory is correct, OK the Open Directory as Role

Palette dialog box.

Essentials for NX Designers G-11

 Custom Roles

A new tab is added to the Resource bar and your custom role is
displayed.

1. Directory you created to hold

your custom roles

2. Property name of your

custom role

3. Role palette tab created

Close the Palettes dialog box.

Step 8: Close the part.

G

G-12 Essentials for NX Designers mt10051_s NX 7

 Custom Roles

Protected Roles
The power of Roles can be extended throughout your industry enterprise,
on several levels, by having your company’s systems administrator create
’protected’ roles for authorized workflows.
One Possible Scenario: — Adding System Default Roles
• Have the group leaders of various departmental processes/disciples
customize the NX user interface to reflect the design needs of that group;
e.g. assemblies, design review, drafting etc. (Activity procedure)

• The group leaders then create individual Roles for each of the
processes/disciplines.

• The group leaders alert the NX Systems Administrator where these

role (.mtx) files are located and asks for them to be moved into
the /UGII/menus/roles directory within the NX release. This is a
permissions-protected area.

• Once the .mtx files are moved into the /UGII/menus/roles directory, they
will be available as Roles in the System Defaults folder.

Essentials for NX Designers G-13

G
Appendix

H Legacy mating conditions

By applying mating conditions to components in an assembly, you establish

parametric, positional relationships between objects in the components.
These relationships are termed mating constraints.
In the example shown, if you align the cylindrical face of a bolt to the
cylindrical face of a hole in a block and then move the hole, the bolt will
automatically move with it.

Essentials for NX Designers H-1

 Legacy mating conditions

Mating Constraint types

A mating condition is made up of one or more mating constraints. There
are eight types of constraints.

1 — Mate 4 — Parallel 7 — Distance

2 — Align 5 — Perpendicular 8 — Tangent
3 — Angle 6 — Center

To make the Mating Conditions dialog box available, choose

Preferences→Assemblies, and from the Interaction list, choose Mating
Conditions.

Selecting objects

FROM / TO

When selecting objects to mate, the Cue line will be directing you to
select FROM and TO objects. The FROM object is part of the component that
is going to move to a new position. The TO object is part of the component
that is remaining in its present location.

H-2 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Mate constraint
When applying the Mate constraint to components using planar faces and
datum planes, the objects will be oriented so that their normals are parallel
and point in opposite directions. The components will not necessarily have
physical contact but will be coplanar. By definition, a face normal in a solid
body points away from the solid.

When mating non–planar faces (i.e. cylindrical to cylindrical, spherical to

spherical) the radii must be the same; for conical to conical faces, the taper
must be the same.

Essentials for NX Designers H-3

 Legacy mating conditions

Align constraint
When you apply the Align constraint to components using planar objects
(planar faces and datum planes), the objects will be oriented so that their
normals are parallel and point in the same direction. The components will
not necessarily have physical contact but will be coplanar.

When aligning non-planar faces, i.e. cylindrical to cylindrical, spherical to

spherical, or conical to conical, the radii and/or taper do not have to be the
same.

The Align constraint can also be used to position an edge or curve object of
a component with a planar object (planar face or datum plane) of another
component. A vector will be determined from the edge or curve object and
H the objects will be oriented so that the vector and the planar object lie on the
same plane (same behavior as with mate constraint).

Using the CSYS filter

The Align constraint allows existing coordinate systems to be used as
FROM/TO selection objects. When using the CSYS option, select the FROM
CSYS and then immediately select the TO CSYS. This constraint will remove
all DOFs between the two components.

H-4 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Angle constraint
Use the Angle constraint when you need to control specific angles between
objects of components.
The example below illustrates an angle constraint that is being applied in
conjunction with two other constraints. The two planar faces of the blocks
must always be coplanar by virtue of the Mate constraint. The pivot for the
Angle constraint is determined by the Align constraint that is applied to
the two edges.

Essentials for NX Designers H-5

 Legacy mating conditions

Parallel constraint
Use the Parallel constraint when you need to establish parallelism between
objects of components. Objects that have surface normals associated to them
will be oriented parallel based on those normals.
When applying the Parallel constraint to position a planar object of a
component (planar face or datum plane) with an edge or curve object of
another component; a vector will be determined from the edge or curve object.
The vector and the planar object’s normal will then become parallel.

H-6 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Perpendicular constraint
Use the Perpendicular constraint when you need to establish perpendicularity
between objects of components. Objects that have surface normals associated
to them will be oriented perpendicular based on those normals.
When applying the Perpendicular constraint to position a planar object of a
component, (planar faces and datum planes), with an edge or curve object of
another component; a vector will be determined from the edge or curve object,
that vector and the planar object’s normal will then become perpendicular.

Essentials for NX Designers H-7

 Legacy mating conditions

Center constraint
Use the Center constraint to center 1 or 2 objects of a component to 1 or 2
objects of another component.

Center Objects 1 to 1

Center Objects 1 to 2

H-8 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Center Objects 2 to 2

Create a Center constraint

1. Choose the Center constraint.

2. Set the Object filter.

3. Specify the number of objects to use (Center Objects 1 to 1, 1 to 2, 2

to 1, or 2 to 2).

4. Select the objects as instructed in the Cue line.

H

Essentials for NX Designers H-9

 Legacy mating conditions

Distance constraint
Use the Distance constraint to define a distance between two geometric
objects. The sign (+/-) of the dimension controls which side of the object the
solution is on.

Tangent constraint
Use the Tangent constraint to define a physical contact between two geometric
objects. There can be multiple solutions to a tangent constraint. To specify
which solution is desired, a help point will be computed from the pick position
on the surface and used to find a unique solution to the tangent constraint.
The following are some examples of tangent constraints:
• Point on Surface.

• Line tangent to Surface.

• Plane tangent to Sphere.

• Plane tangent to Cylinder.

H-10 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Mating Conditions dialog box

Mating conditions are applied from the Mating Conditions dialog box and can
be accessed by clicking Mate Component on the Assemblies toolbar or by
choosing Assemblies→Components→Mate Component from the menu bar.
1 — Mating Conditions Tree Listing
2 — Mating Constraint Types
3 — Selection Steps
4 — Expression Value (for Angle and Distance constraints)

Essentials for NX Designers H-11

 Legacy mating conditions

Preview
The Preview option becomes active after all the objects have been correctly
selected for a constraint. This option lets you preview the solution by
actually moving the component based on the existing constraints. Additional
constraints may still be applied. After previewing the constraint, click Apply
or OK to accept the constraint or continue creating another constraint. If
the constraint is not correct, click Unpreview and use the Selection Steps to
define different FROM and TO faces.

OK, Apply, and Cancel

• OK — This should be selected only after all constraints have been applied.
This will save the mating condition (and its constraints) and dismiss the
Mating Conditions dialog box.

• Apply — This will apply the constraint and the dialog box will remain
open.

• Cancel — This will dismiss the dialog box without saving any of the
constraints you added.

H-12 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Define mating constraints

1. Select a Mating Type.

2. Select an object type from the Filter list (optional).

3. In the graphics window, select an object FROM component to be mated

(component you are moving).

4. In the graphics window, select an object on the component to mate TO

(component that will remain stationary).

5. Click Preview and then click Apply (the dialog box remains open to let
you add more constraints) or click OK to accept the constraint and dismiss
the dialog box.

Degree of freedom indicators

Temporary arrows are displayed to indicate the remaining degrees of freedom.

The Show Degrees of Freedom/Remove Degrees of Freedom options in the
Mating Condition shortcut menu may be used to turn on and off the display
of these arrows.
A Mate constraint applied to the faces shown below, constrains the small
block in the direction normal to the faces. The small block is still free to
translate and rotate in the plane that the two shaded faces have in common.

Essentials for NX Designers H-13

 Legacy mating conditions

Vary Constraints

The Vary Constraints option can be used to reposition the active component in
the Mating Conditions dialog box. Existing mating constraints will limit the
freedom of movement. This dialog box is similar to the Reposition Component
dialog box. A different component can be selected and repositioned by clicking
Select Component.

H-14 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

List Errors

If there are no degree of freedom indicators visible and the Preview option is
unavailable, you may have tried to define an invalid mating constraint. This
will activate the List Errors button. Clicking it will present information about
the error. The constraint must be deleted and recreated.

Essentials for NX Designers H-15

 Legacy mating conditions

Tree listing
The Mating Conditions Tree Listing list all of the assemblies mating
conditions and constraints. Several options and viewing preferences may
be controlled from the Listing Tree.
1 — Mating Condition expanded to display constraint
2 — Mating Constraint suppression toggle
3 — Mating Condition
4 — Mating Constraints
5 — Mating Constraint shortcut menu

Suppress/Unsuppress

Mating Conditions or individual Mating Constraints may be suppressed or

H unsuppressed using the check box.
• A suppressed mating constraint is ignored during geometric edits.

• If a mating constraint is being unsuppressed, the mating condition must

be solved again.

H-16 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Mating constraint shortcut menu

The mating constraints shortcut menu is activated by using the shortcut

menu over a mating constraint.
• Alternate Solution – Produces any other solution that is applicable to the
selected constraint.

• Convert To – Allows the constraint to be changed to another applicable

constraint, i.e. Mate to Distance.

• Delete – Removes the selected mating constraint.

• Rename – Allows the renaming of a mating constraint.

Essentials for NX Designers H-17

 Legacy mating conditions

Mating condition shortcut menu

The mating condition shortcut menu is activated by using the shortcut menu
over a mating condition.

Highlight/Unhighlight – will highlight or unhighlight the current condition.

• From – Highlights the FROM object for all constraints of the selected
condition.

• To – Highlights the TO object for all constraints of the selected condition.

• With/Without Direction – Controls the display of the object normal or

direction vectors.

Show/Remove Degrees of Freedom – Controls the display of the remaining

Degrees of Freedom (DOF).

H Suppress/Unsuppress – Controls the suppression status of the selected

condition. Can also be performed by using the suppression toggle in front
of the condition name.
• A suppressed mating condition is ignored during geometric edits.

• No error messages will be displayed for suppressed mating conditions.

• If you modify a component creating a failed constraint, that constraint

must be deleted before the mating condition can be unsuppressed.

Delete – Removes the selected mating condition.

Rename – Allows the renaming of a mating condition.
Remember Constraints – Mating constraints may be saved for a selected
mating condition within the assembly part. This allows “learned” or
automatic mating when the same component is added to the assembly again.

H-18 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Reposition Component
The Reposition Component option may be used on a component that does not
have any mating conditions, has suppressed mating conditions, or is only
partially constrained. If the component is partially constrained, its mating
constraints will be enforced within the reposition function.
To reposition a component click Reposition Component on the Assemblies
toolbar or choose Assemblies→Components→Reposition Component from
the menu bar.

Essentials for NX Designers H-19

 Legacy mating conditions

Transform types

The Reposition Component dialog box includes the following transform types:
1 — Point to Point 5 — Reposition
2 — Translate 6 — Rotate Between Axes
3 — Rotate About a Point 7 — Rotating Between Points
4 — Rotate About a line

H-20 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Transform options

Move Objects or Move Handles Only

These radio buttons let you specify whether you want to move the component
along with the drag handles or just the drag handles. The drag handles can
be repositioned to a specific orientation and used to drag the component along
a specific vector direction or about a specific axis.

Distance or Angle

The Distance input field (or Angle field if a rotation is being defined) lets you
define a distance (or angle) for movement.

Snap Increment
Snap Increment allows snapping to “whole-multiple” distances when using
the direction or rotation drag handles.

Vector Method
Provides options to define a vector when moving a component using one of
the direction drag handles.

Snap Handles to WCS

Provides a means for moving the handles to the origin and orientation of
the current WCS.

Motion Animation
This slider lets you specify how finely the motion is animated (from Fine to
H
Coarse) during the motion that you have defined.

Essentials for NX Designers H-21

 Legacy mating conditions

Collision options

Collision Action
Specifies what the system will do if a collision occurs.

• None — no action is taken.

• Highlight Collision — you can continue moving the components, and the
areas that collided are highlighted.

• Stop Before Collision — the motion stops just before a collision occurs.
The distance between the components when the motion stops depends
on the setting of the Motion Animation slider. The closer the slider is
to Fine, the shorter the distance.

Collision Checking Mode

Allows you to specify what types of objects will be checked for clearance while
repositioning.

H-22 Essentials for NX Designers mt10051_s NX 7

 Legacy mating conditions

Repositioning components using drag handles

Components can be repositioned quickly and easily using drag handles.

When the Reposition Component dialog box is displayed, the graphics window
displays a set of handles.

There are several ways to reposition a component with the drag handles.
• To move the origin of the component to a specific point, select the origin
drag handle (filled square) and then select a destination point. The
destination points that can be selected are determined by the Snap Point
toolbar.

• To drag the component to an arbitrary cursor location, select the origin

drag handle (filled square) and drag to a new cursor location.

• To translate the component along an axis, select a translation drag handle

(cone head) and drag the component.

• To rotate the component about an axis, select a rotation drag handle

(filled circle) and drag the component.

• To orient the component to a saved coordinate system, select the origin

drag handle (filled square) and then select the saved coordinate system.
H
The Move Handles Only option is used to first move the drag handles to
a specific orientation before using them to move the component.

Essentials for NX Designers H-23

 Legacy mating conditions

Activities: Legacy mating conditions

In the Legacy mating conditions section, do the activity:
• Mating Conditions

H-24 Essentials for NX Designers mt10051_s NX 7

Index

A fit . . . . . . . . . . . . . . . . . . . 17-20
Absolute coordinate system . . . . . . . 3-3 fix . . . . . . . . . . . . . . . . . . . 17-14
Activity parallel . . . . . . . . . . . . . . . 17-15
Creating a Role Palette with a Group perpendicular . . . . . . . . . . 17-16
Role . . . . . . . . . . . . . . . . . . . . G-10 touch align . . . . . . . . . . . . . 17-11
Creating a User Role . . . . . . . . . . G-5 types . . . . . . . . . . . . . . . . . 17-10
Analysis Constraints . . . . . . . . . . . . . . . . 17-9
assign material properties . . . . . 8-15 general concepts . . . . . . . . . . . . . 17-2
Distance . . . . . . . . . . . . . . . . . . . 8-12 Load options
Measure Bodies . . . . . . . . . . . . . 8-14 Reference Sets . . . . . . . . . . . 16-7
Annotation Load Options . . . . . . . . . . . . . . . 16-4
dimension preferences and Load Behavior . . . . . . . . . . . 16-7
placement . . . . . . . . . . . . . . 18-17 Load states . . . . . . . . . . . . . 16-5
placement . . . . . . . . . . . . . . . . . 18-18 Part Versions . . . . . . . . . . . . 16-4
helper lines . . . . . . . . . . . . 18-22 Scope . . . . . . . . . . . . . . . . . . 16-6
preferences . . . . . . . . . . . . . . . . 18-16 master model . . . . . . . . . . . . . . . 18-2
preferences and placement Move Component . . . . . . . . . . . . 17-8
placement cues for Selecting Components in the
dimensions . . . . . . . . . . 18-18 navigator . . . . . . . . . . . . . . . 16-12
snap point options . . . . . . . 18-18 Subassembly . . . . . . . . . . . . . . . 16-2
Application Top down and bottom up
Assemblies . . . . . . . . . . . . . . . . 16-10 modeling . . . . . . . . . . . . . . . . 17-2
Drafting . . . . . . . . . . . . . . . . . . . 18-3 Assembly Navigator . . . . . . . . . . . . 16-8
Assembly . . . . . . . . . . . . . . . . . . . . 16-2 Display Parent . . . . . . . . . . . . . 16-17
Add Component . . . . . . . . . . . . . 17-5 Icons and check boxes . . . . . . . . . 16-9
Assemblies application . . . . . . . 16-10 Identifying components . . . . . . . 16-12
Assemblies toolbar . . . . . . . . . . . 17-2 Make Displayed Part . . . . . . . . 16-17
Associativity . . . . . . . . . . . . . . . 16-16 Make Work Part . . . . . . . . . . . . 16-17
Bottom-up construction method . . 17-3 Node display . . . . . . . . . . . . . . . . 16-8
Component object . . . . . . . . . . . . 16-3 Pack and Unpack . . . . . . . . . . . 16-17
Component parts . . . . . . . . . . . . 16-3 Selecting Components . . . . . . . . 16-12
constraints shortcut menu . . . . . . . . . . . . . 16-17
angle . . . . . . . . . . . . . . . . . 17-17
bond . . . . . . . . . . . . . . . . . 17-19 B
center . . . . . . . . . . . . . . . . 17-18
concentric . . . . . . . . . . . . . 17-12 Block . . . . . . . . . . . . . . . . . . . . . . . . D-3
distance . . . . . . . . . . . . . . . 17-13 Boss . . . . . . . . . . . . . . . . . . . . . . . . E-2

Essentials for NX Designers Index-1

Index

C Tangent to Face at Point, Line or

Face . . . . . . . . . . . . . . . . . 6-8
Chamfer . . . . . . . . . . . . . . . . . . . . 15-7 Options . . . . . . . . . . . . . . . . . . . . 6-3
creating . . . . . . . . . . . . . . . . . . . 15-8 Types . . . . . . . . . . . . . . . . . . . . . . 6-3
options . . . . . . . . . . . . . . . . . . . . 15-9 Delayed Update after Edit . . . . . . . 8-16
Command Finder . . . . . . . . . . . . . . . 2-6 Delayed Updates . . . . . . . . . . . . . . 8-16
Coordinate Systems . . . . . . . . . . . . . 3-2 Deselecting objects . . . . . . . . . . . . . 2-20
Absolute . . . . . . . . . . . . . . . . . . . . 3-3 Design in Context . . . . . . . . . . . . 16-14
WCS . . . . . . . . . . . . . . . . . . . . . . . 3-3 Design intent . . . . . . . . . . . . . . . . . . 4-2
Customer Defaults DesignLogic . . . . . . . . . . . . . . . . . 11-13
Directory Structures . . . . . . . . . . . F-7 Parameter Entry Options
DPV . . . . . . . . . . . . . . . . . . . . . . . F-5 Formula . . . . . . . . . . . . . . . . . 5-8
Files . . . . . . . . . . . . . . . . . . . . F-3, F-5 Dimensions
Setting Levels . . . . . . . . . . . . . . . F-3 appended text . . . . . . . . . . . . . . 18-19
Cylinder . . . . . . . . . . . . . . . . . . . . . D-4 creating . . . . . . . . . . . . . . . . . . 18-16
edit . . . . . . . . . . . . . . . . . . . . . 18-20
D change precision . . . . . . . . 18-20
inherit preferences . . . . . . . 18-20
Datum Axis . . . . . . . . . . . . . . . . . . 6-11 placement cues . . . . . . . . . . . . . 18-18
Applications . . . . . . . . . . . . . . . . 6-13 preferences and placement . . . . 18-17
Creating text orientation and text arrow
Curve/Face Axis . . . . . . . . . . 6-16 placement . . . . . . . . . . . . . . 18-19
Intersection . . . . . . . . . . . . . 6-15 Displayed Part . . . . . . . . . . . . . . . 16-14
Two Points . . . . . . . . . . . . . . 6-14 Distance between objects . . . . . . . . 8-12
Curve/Face Axis . . . . . . . . . . . . . 6-16 Drawings
Intersection . . . . . . . . . . . . . . . . 6-15 adding a base view . . . . . . . . . . . 18-9
Options . . . . . . . . . . . . . . . . . . . 6-12 adding projected views . . . . . . . 18-11
Two Points . . . . . . . . . . . . . . . . . 6-14 project view options . . . . . . 18-13
Types . . . . . . . . . . . . . . . . . . . . . 6-12 projection lines . . . . . . . . . . 18-12
Datum CSYS . . . . . . . . . . . . . . . . . 6-17 adding views
Datum Plane preview . . . . . . . . . . . . . . . 18-12
At Angle . . . . . . . . . . . . . . . . . . . . 6-6 annotation preferences . . . . . . . 18-16
At Distance . . . . . . . . . . . . . . . . . 6-5 See also Annotation
Bisector . . . . . . . . . . . . . . . . . . . . 6-7 create new sheet . . . . . . . . . . . . . 18-4
Curves and Points deleting a sheet . . . . . . . . . . . . . 18-5
Three Points . . . . . . . . . . . . . 6-9 edit notes . . . . . . . . . . . . . . . . . 18-24
Tangent to Face at Point, Line or edit sheet . . . . . . . . . . . . . . . . . . 18-5
Face . . . . . . . . . . . . . . . . . . . . 6-8 edit views . . . . . . . . . . . . . . . . . 18-14
Datum planes . . . . . . . . . . . . . . . . . 6-2 drag . . . . . . . . . . . . . . . . . . 18-14
applications . . . . . . . . . . . . . . . . . 6-4 editing views . . . . . . . . . . . . . . 18-14
Creating monochrome display . . . . . . . . . . 18-7
At Angle . . . . . . . . . . . . . . . . 6-6 open sheet . . . . . . . . . . . . . . . . . 18-4
At Distance . . . . . . . . . . . . . . 6-5 removing views . . . . . . . . . . . . . 18-14
Bisector . . . . . . . . . . . . . . . . . 6-7 text . . . . . . . . . . . . . . . . . . . . . 18-22
Curves and Points, Three leaders . . . . . . . . . . . . . . . . 18-23
Points . . . . . . . . . . . . . . . . 6-9 note . . . . . . . . . . . . . . . . . . 18-23

Index-2 Essentials for NX Designers mt10051_s NX 7

 Index

view creation options . . . . . . . . 18-10 Using . . . . . . . . . . . . . . . . . . . . . . 1-4

view preferences . . . . . . . . . . . . . 18-8
G
E Gateway
Edge blend Roles . . . . . . . . . . . . . . . . . . . . . . G-2
add new set . . . . . . . . . . . . . . . . 15-5
dialog box . . . . . . . . . . . . . . . . . . 15-3 H
preview . . . . . . . . . . . . . . . . . . . 15-4
Hole . . . . . . . . . . . . . . . . . . . 12-2–12-3
Edge Blend . . . . . . . . . . . . . . . . . . 15-2
Creating . . . . . . . . . . . . . . . . . . . 12-6
Edge operations
Forms . . . . . . . . . . . . . . . . . . . . . 12-5
Chamfer . . . . . . . . . . . . . . . . . . . 15-7
options . . . . . . . . . . . . . . . . . . . . 12-4
Edge Blend . . . . . . . . . . . . . . . . . 15-2
Edit
Positioning . . . . . . . . . . . . . . . . . E-15 I
Edit Feature
Information . . . . . . . . . . . . . . . . . . 8-10
Reorder . . . . . . . . . . . . . . . . . . . . 8-9
Instance Feature . . . . . . . . . . . . . . 14-2
Editing models . . . . . . . . . . . . . . . . 19-2
array methods . . . . . . . . . . . . . . 14-3
Exit NX . . . . . . . . . . . . . . . . . . . . . 1-10
caveats . . . . . . . . . . . . . . . . . . . . 14-2
Expressions
circular array . . . . . . . . . . . . . . . 14-6
case sensitivity . . . . . . . . . . . . . . . 5-3
creating . . . . . . . . . . . . . . . . 14-7
creating . . . . . . . . . . . . . . . . . . . . 5-5
example . . . . . . . . . . . . . . . . 14-8
dialog box . . . . . . . . . . . . . . . . . . . 5-4
parameters . . . . . . . . . . . . . 14-6
editing . . . . . . . . . . . . . . . . . . . . . 5-6
rectangular array . . . . . . . . . . . . 14-4
examples . . . . . . . . . . . . . . . . . . . 5-2
creating . . . . . . . . . . . . . . . . 14-5
functions . . . . . . . . . . . . . . . . . . . B-5
example . . . . . . . . . . . . . . . . 14-5
insert name . . . . . . . . . . . . . . . . . 5-8
parameters . . . . . . . . . . . . . 14-4
list referencers . . . . . . . . . . . . . . . 5-7
List References . . . . . . . . . . . . . . 8-11
listing expressions associated with L
features . . . . . . . . . . . . . . . . . . 5-7 Layers . . . . . . . . . . . . . . . . . . . . . . . 1-6
operators . . . . . . . . . . . . . . . . . . . B-2
options . . . . . . . . . . . . . . . . . . . . . 5-9
overview . . . . . . . . . . . . . . . . . . . . 5-2 M
precedence and associativity . . . . . B-3 Make Current Feature . . . . . . . . . . . 8-6
Extrude . . . . . . . . . . . . . . . . . . . . . . 7-3 Master model . . . . . . . . . . . . . . . . . 18-2
Draft . . . . . . . . . . . . . . . . . . . . 11-10 drawing guidelines . . . . . . . . . . 18-25
limits . . . . . . . . . . . . . . . . . . . . . 11-5 Material Properties . . . . . . . . . . . . 8-15
Offset . . . . . . . . . . . . . . . . . . . . . 11-6 Mating Conditions . . . . . . . . . . . . . . H-1
start and end distance . . . . . . . . . 7-4 Align . . . . . . . . . . . . . . . . . . . . . . H-4
Angle . . . . . . . . . . . . . . . . . . . . . . H-5
F Center . . . . . . . . . . . . . . . . . . . . . H-8
Distance . . . . . . . . . . . . . . . . . . . H-10
Feature Replay . . . . . . . . . . . . . . . . 8-8 Mate . . . . . . . . . . . . . . . . . . . . . . H-3
File Templates . . . . . . . . . . . . . . 1-2–1-3 Parallel . . . . . . . . . . . . . . . . . . . . H-6
Saving unnamed template files . . . 1-5 Perpendicular . . . . . . . . . . . . . . . . H-7

Essentials for NX Designers Index-3

Index

Tangent . . . . . . . . . . . . . . . . . . . H-10 Preview panel . . . . . . . . . . . . . . . . 8-4

Vary Constraint . . . . . . . . . . . . . H-13 Shortcut menu . . . . . . . . . . . . . . . 8-6
Measure Bodies . . . . . . . . . . . . . . . 8-14 Timestamp order . . . . . . . . . . . . . 8-5
Mirror Body . . . . . . . . . . . . . . . . . 14-10 Pocket . . . . . . . . . . . . . . . . . . . . . . . E-5
creating . . . . . . . . . . . . . . . . . . 14-11 Positioning
editing . . . . . . . . . . . . . . . . . . . 14-11 Edit
options . . . . . . . . . . . . . . . . . . . 14-12 Add Dimension . . . . . . . . . . E-16
Modeling strategy . . . . . . . . . . . . . . 4-2 Delete Dimension . . . . . . . . . E-17
Mouse . . . . . . . . . . . . . . . . . . . . . . 2-13 Edit Dimension . . . . . . . . . . . . . E-16
Preview selection . . . . . . . . . . . . 2-21 Positioning Methods
QuickPick . . . . . . . . . . . . . . . . . . 2-22 Angular . . . . . . . . . . . . . . . . . . . E-14
Radial menus . . . . . . . . . . . . . . . 2-16 Horizontal . . . . . . . . . . . . . . . . . . E-8
Selecting objects . . . . . . . . . . . . . 2-19 Line onto Line . . . . . . . . . . . . . . E-13
View manipulation . . . . . . . . . . . 2-17 Parallel . . . . . . . . . . . . . . . . . . . E-11
View shortcut menu . . . . . . . . . . 2-14 Parallel at a Distance . . . . . . . . . E-12
View triad . . . . . . . . . . . . . . . . . 2-18 Perpendicular . . . . . . . . . . . . . . . E-10
Mouse Buttons . . . . . . . . . . . . . . . . 2-13 Point onto Line . . . . . . . . . . . . . . E-10
Mouse shortcut menu Point onto Point . . . . . . . . . . . . . E-11
Display Mode . . . . . . . . . . . . . . . 2-15 Vertical . . . . . . . . . . . . . . . . . . . . E-9
Fit . . . . . . . . . . . . . . . . . . . . . . . 2-15 Preferences
Orient View . . . . . . . . . . . . . . . . 2-15 view . . . . . . . . . . . . . . . . . . . . . . 18-8
Pan . . . . . . . . . . . . . . . . . . . . . . 2-15 Preview selection . . . . . . . . . . . . . . 2-21
Refresh . . . . . . . . . . . . . . . . . . . 2-15 Procedure
Rotate . . . . . . . . . . . . . . . . . . . . 2-15 Creating a Group Role . . . . . . . . . G-8
Set Rotate Point . . . . . . . . . . . . . 2-15 Creating a User Role . . . . . . . . . . G-3
Undo . . . . . . . . . . . . . . . . . . . . . 2-15 Edit a User Role . . . . . . . . . . . . . . G-7
Zoom . . . . . . . . . . . . . . . . . . . . . 2-15
Q
O
QuickPick . . . . . . . . . . . . . . . . . . . 2-22
Online Help . . . . . . . . . . . . . . . . . . . 17
OrientXpress tool . . . . . . . . . . . . . . . 7-8 R
Reference Features
P
Datum Axis . . . . . . . . . . . . . . . . 6-11
Pad . . . . . . . . . . . . . . . . . . . . . . . . . E-6 Datum CSYS . . . . . . . . . . . . . . . 6-17
Parameter Entry Options . . . . . . . 11-13 Datum Planes . . . . . . . . . . . . . . . . 6-2
Formula . . . . . . . . . . . . . . . . . . . . 5-8 Referencing Existing
Parametric models Parameters . . . . . . . . . . . . . . . . 11-14
editing . . . . . . . . . . . . . . . . . . . . 19-2 Reorder features . . . . . . . . . . . . . . . 8-9
Part Files Replay
Close Selected . . . . . . . . . . . . . . . 1-9 feature . . . . . . . . . . . . . . . . . . . . . 8-8
Save As . . . . . . . . . . . . . . . . . . . . 1-8 Reposition Component . . . . . . . . . . H-19
Part Navigator . . . . . . . . . . . . . . . . . 8-2 Revolve . . . . . . . . . . . . . . . . . . . . . . 7-7
Dependencies panel . . . . . . . . . . . 8-3 start and end angles . . . . . . . . . . . 7-8
Details panel . . . . . . . . . . . . . . . . 8-3 Roles . . . . . . . . . . . . . . . . . . . . 2-11, G-2
Main panel . . . . . . . . . . . . . . . . . . 8-2 Choosing . . . . . . . . . . . . . . . . . . 2-11

Index-4 Essentials for NX Designers mt10051_s NX 7

 Index

creating group . . . . . . . . . . . . . . . G-8 Edit . . . . . . . . . . . . . . . . . . . 4-24

creating user . . . . . . . . . . . . . . . . G-3 Retain dimensions . . . . . . . . 4-26
editing user . . . . . . . . . . . . . . . . . G-7 Types . . . . . . . . . . . . . . . . . . 4-21
Examples . . . . . . . . . . . . . . . . . . 2-11 Drag . . . . . . . . . . . . . . . . . . . . . . . 9-2
Protected . . . . . . . . . . . . . . . . . . G-13 Constraint assistance . . . . . . . 9-3
User-Defined . . . . . . . . . . . . . . . . G-2 Geometric Constraints
Show or remove . . . . . . . . . . 4-18
S Internal and external . . . . . . . . . . 4-4
Status change . . . . . . . . . . . . 4-5
Save Work Part . . . . . . . . . . . . . . 16-19
Mirror . . . . . . . . . . . . . . . . . . . . 9-13
Save . . . . . . . . . . . . . . . . . . . . . 16-19
Point . . . . . . . . . . . . . . . . . . . 4-6–4-7
Save Work Part Only . . . . . . . . 16-19
Reattach . . . . . . . . . . . . . . . . . . . . 9-9
Selection
Sketch in place . . . . . . . . . . . 9-10
QuickPick . . . . . . . . . . . . . . . . . . 2-22
Retain dimensions . . . . . . . . . . . 4-26
Selection bar . . . . . . . . . . . . . 2-10, 2-19
Show All/Show No Constraints . . 4-16
filter components . . . . . . . . . . . 16-13
Show/Remove Constraints . . . . . 4-17
Point
Suppress . . . . . . . . . . . . . . . . . . 4-30
Snap Point options . . . . . . . . . 4-7
Timestamp and dependencies . . . 9-11
Selection Intent . . . . . . . . . . . . . . . 11-2
Slot . . . . . . . . . . . . . . . . . . . . . . . . . E-3
Curve rule options . . . . . . . . . . . 11-3
positioning . . . . . . . . . . . . . . . . . . E-4
face options . . . . . . . . . . . . . . . . 13-7
Swept Features
Follow Fillet . . . . . . . . . . . . . . . . 11-4
Body types . . . . . . . . . . . . . . . . . . 7-6
selecting sketches . . . . . . . . . . . . 11-4
Revolve . . . . . . . . . . . . . . . . . . . . 7-7
Stop at Intersection . . . . . . . . . . 11-4
Types . . . . . . . . . . . . . . . . . . . . . . 7-2
Selection MiniBar . . . . . . . . . . . . . 2-14
Synchronous Modeling . . . . . . . . . . 19-3
Shell . . . . . . . . . . . . . . . . . . . . . . . 13-2
assign alternate thicknesses . . . . 13-4
creating . . . . . . . . . . . . . . . . . . . 13-3 T
options . . . . . . . . . . . . . . . . . . . . 13-5 Templates . . . . . . . . . . . . . . . . . 1-2–1-3
Sketch Toolbars
Constraints Customizing . . . . . . . . . . . . . . . . . 2-2
Geometric . . . . . . . . . . . . . . 4-12 Add or remove buttons . . . . . . 2-4
Geometric creation . . . . . . . . 4-13 Displaying toolbars . . . . . . . . 2-2
Geometric list . . . . . . . . . . . 4-14 Rail . . . . . . . . . . . . . . . . . . . . 2-8
Inferred . . . . . . . . . . . . . . . . 4-31 Saving configuration . . . . . . . . . . 2-10
Constraints overview . . . . . . . . . 4-10 Selection . . . . . . . . . . . . . . . . . . 2-19
Convert To/From Selection bar . . . . . . . . . . . . . . . 2-10
Reference . . . . . . . . . . . 4-28–4-29 Trim Body . . . . . . . . . . . . . . . . . . . 10-2
Create Inferred Constraints . . . . 4-31
Degrees of freedom . . . . . . . . . . . 4-11 U
Delay Evaluation
Update Model . . . . . . . . . . . . . . . . 8-16
Evaluate process . . . . . . . . . 4-30
Delete . . . . . . . . . . . . . . . . . . . . 4-30
Dimensional Constraints . . 4-20, 4-22 V
Attach dimension . . . . . . . . . 4-27 vector
Create inferred . . . . . . . . . . 4-23 OrientXpress tool . . . . . . . . . . . . . 7-8
Dimensions Dialog box . . . . . 4-25 View Preferences . . . . . . . . . . . . . . 18-8

Essentials for NX Designers Index-5

Index

Hidden Lines . . . . . . . . . . . . . . . 18-8 Move, freeform . . . . . . . . . . . . 3-6

Smooth Edges . . . . . . . . . . . . . . . 18-8 Move, origin to a point . . . . . . 3-6
View shortcut menu . . . . . . . . . . . . 2-14 Orient to object . . . . . . . . . . . 3-7
Reverse axis . . . . . . . . . . . . . . 3-7
W Rotate . . . . . . . . . . . . . . . . . . 3-6
WCS . . . . . . . . . . . . . . . . . . . . . . . . 3-4 Move . . . . . . . . . . . . . . . . . . . . . . 3-5
Dynamics WCS Dynamics . . . . . . . . . . . . . . . . 3-5
Drag along axis . . . . . . . . . . . 3-6 Work part . . . . . . . . . . . . . . . . . . 16-16
Move on axis using on-screen input
box . . . . . . . . . . . . . . . . . . 3-6

Index-6 Essentials for NX Designers mt10051_s NX 7

Siemens Learning Advantage
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PLM Software
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STUDENT PROFILE
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will be kept confidential and will not be shared with anyone outside of Education Services.
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Course Title/Dates Essentials for NX Designers / thru

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Please verify/add to this list of training for NX, I-deas, Imageware, Teamcenter Mfg., Teamcenter Engineering, Teamcenter Enterprise, Tecnomatix or
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Please “check”! your ability/knowledge in the following…
Subject None Novice Intermediate Advanced
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PDM – system management o o o o
PDM – customization o o o o

Thank you for your participation. We hope your training experience will be an outstanding one.

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 Course Agenda
Essentials for NX Designers
Essentials for NX Designers with Teamcenter Integration
Monday Morning
• Introduction & Course overview
• Lesson 1. NX part files
• Project – Parts
• Lesson 2. The NX User Interface

Afternoon
• Lesson 3. Coordinate systems
• Lesson 4. Sketch Task Environment
• Project – Sketch Task Environment

Tuesday Morning
• Lesson 5. Expressions
• Project – Expressions
• Lesson 6. Datum features
• Project – Datums
• Lesson 7. Swept features

Afternoon
• Project – Swept features
• Lesson 8. Part structure
• Lesson 9. Using sketches
• Project – Using sketches

Wednesday Morning
• Lesson 10. Trim Body
• Lesson 11. Swept feature options
• Project – Swept feature options
• Lesson 12. Hole features

Afternoon
• Project – Hole features
• Lesson 13. Shell
• Project – Shell
• Lesson 14. Associative copies
• Project – Associative copies

Thursday Morning
• Lesson 15. Edge operations
• Project – Blends and Chamfers
• Lesson 16. Introduction to Assemblies

Afternoon
• Lesson 17. Adding and constraining components
• Project – Assembly constraints

Friday Morning
• Lesson 18. Introduction to Drafting
• Lesson 19. Editing models

Afternoon
• Project – Drafting

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•

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Accelerators
The following Accelerators can be listed from within an NX session by choosing
Information→Custom Menubar→Accelerators.

Function Accelerator
File→New... Ctrl+N
File→Open... Ctrl+O
File→Save Ctrl+S
File→Save As... Ctrl+Shift+A
File→Plot... Ctrl+P
File→Execute→Grip... Ctrl+G
File→Execute→Debug Grip... Ctrl+Shift+G
File→Execute→NX Open... Ctrl+U
Edit→Undo Ctrl+Z
Edit→Redo Ctrl+Y
Edit→Cut Ctrl+X
Edit→Copy Ctrl+C
Edit→Paste Ctrl+V
Edit→Delete... Ctrl+D or Delete
Edit→Selection→Top Selection Priority - Feature F
Edit→Selection→Top Selection Priority - Face G
Edit→Selection→Top Selection Priority - Body B
Edit→Selection→Top Selection Priority - Edge E
Edit→Selection→Top Selection Priority - Component C
Edit→Selection-Select All Ctrl+A
Edit→Show and Hide→Show and Hide... (by type) Ctrl+W
Edit→Show and Hide→Hide... Ctrl+B
Edit→Show and Hide→Invert Shown and Hidden Ctrl+Shift+B
Edit→Show and Hide→Immediate Hide… Ctrl+Shift+I
Edit→Show and Hide→Show... Ctrl+Shift+K
Edit→Show and Hide→Show All Ctrl+Shift+U
Edit→Transform... Ctrl+T
Edit→Move Object Ctrl+Shift+M
Edit→Object Display... Ctrl+J
View→Operation→Zoom... Ctrl+Shift+Z
View→Operation→Rotate... Ctrl+R
View→Operation→Section... Ctrl+H
View→Layout→New... Ctrl+Shift+N
View→Layout→Open... Ctrl+Shift+O
View→Layout→Fit All Views (only with multiple views) Ctrl+Shift+F
View→Layout→Fit Ctrl+F
View→Visualization→High Quality Image... Ctrl+Shift+H
View→Information Window F4
Hide or show the current dialog box F3
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View→Reset Orientation Ctrl+F8
Insert→Sketch... S
Insert→Design Feature→Extrude... X
Insert→Design Feature→Revolve... R
Insert→Trim→Trimmed Sheet... T
Insert→Sweep→Variational Sweep... V
Format→Layer Settings... Ctrl+L
Format→Visible in View... Ctrl+Shift+V
Format→WCS→Display W
Tools→Expression... Ctrl+E
Tools→Update→Make First Feature Current Ctrl+Shift+Home
Tools→Update→Make Previous Feature Current Ctrl+Shift+Left Arrow
Tools→Update→Make Next Feature Current Ctrl+Shift+Right Arrow
Tools→Update→Make Last Feature Current Ctrl+Shift+End
Tools→Journal→Play... Alt+F8
Tools→Journal→Edit Alt+F11
Tools→Macro→Start Record... Ctrl+Shift+R
Tools→Macro→Playback... Ctrl+Shift+P
Tools→Macro→Step... Ctrl+Shift+S
Tools→Movie→Record Alt+F5
Tools→Movie→Stop Alt+F7
Information→Object... Ctrl+I
Analysis→Curve→Refresh Curvature Graphs Ctrl+Shift+C
Preferences→Object... Ctrl+Shift+J
Preferences→Selection... Ctrl+Shift+T
Start→Modeling... M or Ctrl+M
Start→All Applications→Shape Studio... Ctrl+Alt+S
Start→Drafting... Ctrl+Shift+D
Start→Manufacturing... Ctrl+Alt+M
Start→NX Sheet Metal... Ctrl+Alt+N
Start→Assemblies A
Help→On Context... F1
Refresh F5
Fit Ctrl+F
Zoom F6
Rotate F7
Orient View-Trimetric Home
Orient View-Isometric End
Orient View-Top Ctrl+Alt+T
Orient View-Front Ctrl+Alt+F
Orient View-Right Ctrl+Alt+R
Orient View-Left Ctrl+Alt+L
Snap View F8

Rev-10/23/09-jab
 PLM Software
Evaluation – Delivery
Name: NX 7 ESN___________ Course #: TR10051/TR10051_TC
Start Date: ____________ Through: __________
Please share your opinion in all of the following sections with a “check” in the appropriate box:

SOMEWHAT

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Instructor:

STRONGLY

STRONGLY
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DISAGREE
If there were 2 instructors, please evaluate the 2nd instructor with “X’s”

AGREE

AGREE

AGREE
Instructor: 7

1. Clearly explained the course objectives

2. Was knowledgeable about the subject
3. Answered my questions appropriately
4. Encouraged questions in class
5. Was well spoken and a good communicator
6. Was well prepared to deliver the course
7. Made good use of the training time
8. Conducted themselves professionally
9. Used examples relevant to the course and audience
10. Provided enough time to complete the exercises
11. Used review and summary to emphasize important information
12. Did all they could to help the class meet the course objectives

Comments on overall impression of instructor(s):

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Suggestions for improvement of course delivery:

What you liked best about the course delivery:

Class Logistics:
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3. The software performed properly
4. The overhead projection unit was clear and working properly
5. The registration and confirmation process was efficient

Hotels: (We try to leverage this information to better accommodate our customers)
1. Name of the hotel Best hotel I’ve stayed at
2. Was this hotel recommended during your registration process? YES NO
3. Problem? (brief description)

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 PLM Software
Evaluation - Courseware
Name: NX 7 ESN___________ Course #: TR10051/TR10051_TC
Dates: ____________ Through: __________
Please share your opinion for all of the following sections with a “check” in the appropriate box:

SOMEWHAT

SOMEWHAT
STRONGLY

STRONGLY
DISAGREE

DISAGREE

DISAGREE

AGREE

AGREE

AGREE
Material:
1. The training material supported the course and lesson objectives
2. The training material contained all topics needed to complete the projects
3. The training material provided clear and descriptive directions
4. The training material was easy to read and understand
5. The course flowed in a logical and meaningful manner

6. How appropriate was the length of the course relative to the material? Too short Too long Just right

Comments on Course and Material:

Overall impression of course Poor Excellent

Student:
1. I met the prerequisites for the class (I had the skills I needed)
2. My objectives were consistent with the course objectives
3. I will be able to use the skills I have learned on my job
4. My expectations for this course were met
5. I am confident that with practice I will become proficient

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