Sketcher Fundamentals

Student Guide
February 2006
MT10028 — NX 4

Publication Number
mt10028_g NX 4
Manual History

Manual Unigraphics Publication

Revision Version Date
Version 16.0 May 2000
Version 17.0 December 2000
Version 18 November 2001
Unigraphics NX October 2002
Unigraphics NX 2 December 2003
NX 3 January 2005
NX 4 February 2006

This edition obsoletes all previous editions.

Proprietary & Restricted Rights Notice

This software and related documentation are proprietary to UGS Corp.

© 2006 UGS Corp. All Rights Reserved.
All trademarks belong to their respective holders.

©2006 UGS Corp.

All Rights Reserved.
Produced in the United States of America.

2 Sketcher Fundamentals – Student Guide mt10028_g NX 4

Contents

Overview ........................................................................................................... 7

Intended Audience ........................................................................................ 7

Course Objectives .......................................................................................... 7
Prerequisites ................................................................................................. 8
How to Use This Course ............................................................................... 8
Class Standards ............................................................................................ 9
About Part File Naming ............................................................................... 9
Seed Part ......................................................................................................... 10
Definition of Terms......................................................................................... 11
Classroom System Information .................................................................. 12

Sketching....................................................................................................... 1-1

Sketching Overview ...................................................................................1-2

Sketches and the Part Navigator ........................................................1-6
Sketch Visibility ...................................................................................1-7
Creating a New Sketch ..............................................................................1-8
The Active Sketch .............................................................................. 1-12
Sketch Creation Steps ....................................................................... 1-13
Activity — Sketch Creation ............................................................... 1-14
Sketch Curves .......................................................................................... 1-21
Activity — Using the Sketch Profile Tool ...........................................1-28
Creating Fillets .................................................................................. 1-33
Trimming and Extending Curves ...................................................... 1-34
Activity — Creating Fillets................................................................ 1-37
Activity — Using Quick Trim and Quick Extend ............................. 1-42
Sketch Points ........................................................................................... 1-46
Dimensional Constraints ......................................................................... 1-48
Activity — Adding Dimensional Constraints ................................... 1-54
Editing Dimensions............................................................................ 1-57
Activity — Editing Sketch Dimensions............................................. 1-59
Geometric Constraints ............................................................................. 1-63
Show/Remove Constraints ................................................................. 1-66
Constraint Conditions........................................................................ 1-69
Activity — Adding Constraints ......................................................... 1-71
Activity — Constraining a Profile ..................................................... 1-76
Activity — Sketching and Constraining a Gasket ............................ 1-85
Convert To/From Reference ............................................................... 1-92
Activity — Constraint Conditions ..................................................... 1-93
Contents
 Summary .................................................................................................. 1-99

Constraining Sketches ............................................................................... 2-1

Drag ............................................................................................................2-2
Create Inferred Constraints ......................................................................2-5
Activity - Dragging Sketch Objects ...........................................................2-6
Activity - Adding Constraints .................................................................. 2-15
Automatic Constraint Creation ............................................................... 2-22
Sketch Operations — Project................................................................... 2-23
Activity - Projecting Objects into a Sketch ............................................. 2-25
Activity - Auto Creating Constraints ...................................................... 2-32
Add Existing Curves to a Sketch............................................................. 2-36
Activity - Adding and Constraining Curves............................................ 2-37
Activity - Design Change ......................................................................... 2-40
Activity - Another Design Change........................................................... 2-41
Activity - Constraining the Perimeter of a Sketch ................................. 2-44
Activity - Controlling Heat Transfer in a Cooling Pipe .......................... 2-49
Summary .................................................................................................. 2-58

Constraint Management ............................................................................ 3-1

Alternate Solution ...................................................................................... 3-2
Activity - Alternate Solution ...............................................................3-4
Placing Sketches Where They Are Needed ............................................. 3-11
Activity - Creating and Positioning a Sketch ................................... 3-12
Activity - Positioning a Sketch .......................................................... 3-20
Activity - Using Positioning Dimensions .......................................... 3-28
Reattach ................................................................................................... 3-38
Reordering Sketches ................................................................................ 3-40
Activity - Reattaching a Sketch ............................................................... 3-41
Activity - Moving Sketches ...................................................................... 3-45
Mirroring in a Sketch .............................................................................. 3-62
Activity - Mirroring Sketch Objects .................................................. 3-63
Summary .................................................................................................. 3-66

Sketch on Path Overview .......................................................................... 4-1

Sketch on Path ...........................................................................................4-1
Summary ....................................................................................................4-3

Additional Sketching Techniques ........................................................... 5-1

Edit Defining String...................................................................................5-2
Deleting or Suppressing Sketches .............................................................5-4
Activity - Edit Defining String ..................................................................5-5
Activity - Suppressing and Deleting Sketches ........................................ 5-10
Animate .................................................................................................... 5-14
Activity - Animating Sketch Dimensions ................................................ 5-15
Contents
 Summary .................................................................................................. 5-19

Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Index-1
About Part File Naming
The following is a sample usage of a file naming standard:

TIP
Currently up to 128 characters are valid for file names. A four character
extension (.prt) is automatically added to define the file type.
 Overview

Definition of Terms
Explicit Modeling
1. Explicit modeling is modeling that is not parametric.
2. Objects are created relative to model space, not each other.
3. Changes to one or more objects do not necessarily affect other objects
or the finished model.
4. Examples of explicit modeling include creating a line between two
existing points, or creating an arc through three existing points. If one
of the existing points were moved, the line/arc would not change.

Parametric Modeling
1. A parametric model is one in which the values (parameters)
used for the definition of the model are stored with the model for
future editing.
2. Parameters may reference each other to establish relationships
between the various features of the model.
3. Examples include the diameter and depth of a hole, or the length,
width, and height of a rectangular pad.
4. The designer’s intent may be that the hole is always as deep as the
pad is high. Linking these parameters together may achieve the
desired results. This is not easily accomplished with an explicit model.
Constraint-based Modeling
1. A constraint-based model is one in which the geometry of the model is
driven, or solved, from a set of design rules applied to the geometry
defining the model as constraints.
2. These constraints might be dimensional constraints (such as sketch
dimensions or positioning dimensions) or geometric constraints (such
as parallelism or tangency).
3. Examples include a line tangent to an arc, where the designer intends
for that tangent condition to be maintained even though the angle of
the line may change, or a perpendicular condition being maintained as
angles are modified.
Hybrid Modeling
1. Hybrid modeling refers to the selectively combined use of the three
types of modeling described above.
2. Hybrid modelers allow designers to use parametric modeling where
needed, without requiring that the entire model be constrained before
proceeding.

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3. The Uni-graphics NX hybrid modeler supports traditional explicit geometric modeling
along with constraint-based sketching and parametric feature modeling. All tools are
integrated so they can be used in combination.

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 1
Lesson

1 Sketching
Purpose

This lesson introduces the method of creating a sketch and free hand
sketching of curves.

Objectives

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

• Create a sketch.

• Create sketch curves.

• Apply dimensional constraints to sketches.

• Apply geometric constraints to sketches.

• Identify constraints.

• Convert a sketch curve to reference.

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Sketching Overview

What is a sketch?

 A sketch is a collection of two-dimensional geometry within a part.

Each sketch is a named collection of 2D curves and points residing on a
plane that you specify.

 You can use sketches to address a wide variety of design needs. For
example, you might create.

 Detailed part features by sweeping, extruding, or revolving a sketch

into a solid or a sheet body.

 Large-scale 2D concept layouts.

 Construction geometry, such as a path of motion, or a clearance arc,

that is not meant to define a part feature.

This lesson will focus on the use of sketches to define detailed part
features.

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 Sketching

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An important aspect of modeling that will help you decide how to use a
sketch is defining the design intent of the model. The design intent consists
of two items:
• Design Considerations — The geometric requirements on the actual
part, including engineering and design rules that determine the detail
configuration of the part.

• Potential Areas for Change — Known design changes or iterations, and

their effects on the part configuration.

As a general rule, the more design considerations and potential areas for
change, the more likely there are benefits from sketching.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 1-5
 Sketching

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Sketches and the Part Navigator
Sketches can be created by choosing the Sketch Section icon in certain feature
creation dialogs such as Extrude and Revolve, choosing the Sketch icon
directly in the Form Feature toolbar, or by choosing Insert→Sketch.
If you create a sketch from within a feature creation dialog, the sketch of the
section remains internal to the feature. It does not display in the graphics
window or in the Part Navigator. You can edit the sketch by accessing
the associated feature. If the same sketch is required to create additional
features, you can choose the Make Sketch External option from the MB3
popup menu in the Part Navigator and it will appear in the graphics window.

If a sketch is not created from within a feature creation dialog, it will appear
as a separate feature in the Part Navigator.

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Sketch Visibility

Organizing the data in a part is an important aspect of modeling. The

sketcher helps in this endeavor by automating the visibility of sketches are
activated and deactivated.
• If a standalone sketch is created by choosing the Sketch icon in the Form
Feature toolbar (or InsertSketch), the current work layer is assigned to
the sketch as it is created. When you subsequently activate the sketch,
the work layer is set to the layer assigned to the sketch so that you do not
accidently construct objects in the active sketch across multiple layers.

• If the sketch is created internal to a feature, it automatically becomes

visible when you edit the feature and choose the Sketch Section icon in
the feature dialog.

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 Sketching

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Creating a New Sketch

Defining a Sketch Plane

1 – Sketch in Place 4 – YC–ZC Plane 7 – Datum CSYS

2 – Sketch Plane 5 – XC–ZC Plane 8 – OK
3 – XC–YC Plane 6 – Datum Plane 9 – Cancel

Defining the Sketch as the Base Feature

• XC-YC Plane
• YC-ZC Plane
• ZC-XC Plane
• Datum CSYS

Initially, the XC-YC plane will be highlighted in the graphics window.

1
Defining the Reference Direction

 The reference direction is used to specify the horizontal direction on the

sketch plane. When there is no linear object pointing in the desired horizontal
direction, a vertical reference may be defined.

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Sketching

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Sketch Curves
Sketch curves are created via the Sketch Curve toolbar. As curves are
created geometric constraints are assigned to the curves relative to the Infer
Constraints Settings.
1 – Profile
2 – Line
3 – Arc
4 – Circle

Infer Constraint Settings

The Infer Constraints Settings dialog determines which constraints are
automatically created during curve creation. It is accessed by choosing
the Infer Constraint Settings icon from the Constraints toolbar or
ToolsConstraintsInfer Constraint Settings.

As you create the curves a symbol will appear near the curve being created to
represent the constraint that will be applied, if any.

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Sketching

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 Sketching

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Creating Lines

Line creation is accessed by choosing the Line icon on the Sketch Curve
toolbar.
Once in line creation, the icons in the upper left corner of the graphics window
provide two options: Coordinate Mode (by cursor location or keying in an XC
and YC coordinates) and Parameter Mode.

There are several ways to create a line:

• Locate the start, and then locate the end.

• Locate the start, and then enter the length and angle parameters.

• Locate the start, enter one parameter, and then locate the end.

• Key in the parameters and then locate the start.

Once you indicate a start location, the system will switch to the Parameter
Mode. But, you can still specify an end location without switching back to
Coordinate Mode.

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 Sketching

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Creating Arcs

Arc creation is accessed by choosing the Arc icon on the Sketch Curve toolbar.
Once in arc creation, the icons in the upper left corner of the graphics window
give you two sets of options. The first is creation method, and the second is
for the Coordinate/Parameter Mode.

There are two different arc creation methods:

Arc by 3 Points — There are several ways to create the arc with
this method:
• Locate the start, locate the end, and then locate a point on the arc.

• Locate the start, enter a radius value and press Enter, locate the end
point, and then move the cursor to preview and choose which of the
four possible solutions to create.

• The same as the previous, but enter the radius value after locating the
end point, but before the point on arc.

Arc by Center and End Points — There are several ways to create
an arc with this method:
• Locate the center, locate the start point, and locate the end point. (The
start point location determines the radius.)

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 • Locate the center, locate the start point, enter a radius value and press
Enter, locate the end point.

• Locate the center, enter radius and sweep angle values and press
Enter, locate the start of the sweep, and specify the direction for the
sweep.

Once you indicate a first location, the system will switch to Parameter
Mode. But you can still specify locations with the cursor without switching
back to Coordinate Mode.

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 Sketching

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Creating Circles

There are two different circle creation options:

Circle by Center and Diameter — There are a few ways to create a

circle with this option:

Circle by 3 Points — There are two ways to create a circle with

this option:

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 1-27
 Sketching

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Activity — Using the Sketch Profile Tool

In this activity, you will use the Profile tool to create sketch geometry.

Step 1: Open seedpart_in and save it as ***_sketch_profile_1 where ***

represents your initials.

Step 2: Start the Modeling application.

Step 3: Change the Work Layer to 21.

Step 4: Create a sketch on the XC-YC plane.

Choose the Sketch icon. (InsertSketch)

Choose OK to accept the XC-YC Plane.

Step 5: Add icons to the Sketch Constraints toolbar.

Select the Toolbar Options area of the Sketch Constraints

toolbar and choose Add or Remove Buttons→Sketch
Constraints.

Make sure the Infer Constraint Settings and Create Inferred

Constraints icons are toggled on.

You may have to move the toolbar to see the icons after
they are added.

Step 6: Set the Infer Constraints Settings.

This is done so that only the constraints that you may want to
apply will be available during curve creation.

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 Sketching

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Choose the Infer Constraint Settings icon.
(ToolsConstraintsInfer Constraint Settings)

Turn on only the following constraints.

Horizontal
Vertical
Tangent
Parallel
Perpendicular
Coincident
Dimensional Constraints

Choose OK.

Step 7: Create a Profile.

In this step you will create the sketch curves shown below using
the Profile tool.

Choose the Profile icon (InsertProfile) and move the

cursor into the graphics window.

Select a start location with the cursor near the bottom left
corner of the graphics window (approximately XC=-4, YC=-2)

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 Sketching

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Move the cursor so that the rubber-banding line snaps to the
horizontal orientation and the horizontal symbol displays (1)
as shown below.

Notice the horizontal symbol indicating the constraint that is

going to be applied to the line.

Press MB2 to lock in the horizontal constraint.

Now notice that as you move the cursor around, the
rubber-banding line remains horizontal.

Key in 3 for the Length and press Enter.

Notice that a dimensional constraint is created automatically.

This is because a Length value was explicitly entered and
the Dimensional Constraints option was turned on in the
Infer Constraint Settings dialog.

Hold MB1 down and drag the cursor straight up from the end
point of the last line and then release.
You are now in Arc creation mode.

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 Sketching

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Key in 1 for the Radius and press Enter.

Key in 180 for the Sweep Angle and press Enter.

Click MB1 in the graphics window to apply.

Continue using the Profile tool to create the remaining curves

in the sketch as shown below. You do not have to key in exact
values but just create the approximate shape.
Close the profile by selecting the end point of the first line.

Dimensions maybe added at a later time to constrain

the remaining curves to specific sizes.

Choose the Finish Sketch icon.

Step 8: Save and close the part.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 1-31
 Sketching

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Optional Challenge
Practice sketching the following profiles:

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 Sketching

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Creating Fillets

Fillet creation is accessed by choosing the Fillet icon on the Sketch Curve
toolbar.
Once in fillet creation, icon options appear in the upper left corner of the
graphics window. The Trim Inputs option (1) determines whether or not the
original curves are trimmed. The Delete Third Curve option (2) determines
whether the middle curve is deleted in a three-curve fillet. The Create
Alternate Fillet option (3) will produce a complementary solution for the fillet
(e.g. a 270 degree arc instead of the default 90 degree arc).

You can create fillets between lines, arcs or conics. You can also create a fillet
between two parallel lines.
There are several ways to create Fillets:
• Select two curves with a single selection (at their intersection), and then
drag the size and quadrant.

• Select two curves individually, and drag the size and quadrant.

• Select one curve, enter a radius value, and select the second curve.

• Select two curves individually, enter a radius value, and the indicate the
desired quadrant.

• Drag (with MB1) across the two curves you want to fillet. The size of the
fillet is determined by where the curves are selected.

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 Sketching

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Trimming and Extending Curves

Quick Trim

This option will allow you to trim any curve to the closest curve in the sketch
and preview the results in preselection color.

You can trim multiple curves at one time, by using the "crayon" select method.
Hold down MB1 and drag across the portion of curves you want to trim away.

You can select a specific curve to trim to, by using Ctrl-select to select the
desired boundary curve. More than one bounding curve can be selected using
this method.
In the example below, both the arc on the left and the spline on the right were
Ctrl-selected as boundary curves. With the cursor on the top line, (between
the two boundary curves), the center section is previewed as the portion to
be removed.

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When a curve is trimmed, appropriate constraints are automatically created.
In the previous example, two Point on Curve constraints and one Collinear
constraint are added. If one of the boundary curves is later trimmed to the
line, the Point on Curve constraint would change to Coincident.

If you trim an arc to a line that is tangent, the tangency constraint is retained.

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 Sketching

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Quick Extend

This option will extend lines, arcs and conics to the closest curve in the
sketch. The system will preview the results in the preselection color.
The curve being extended must extend to an actual intersection with the
boundary curve.
You can extend multiple curves at one time, by using the "crayon" select
method. Hold down MB1 and drag across the ends of curves you want to
extend.

You can also select specific boundary curves by using the control-select
method.
As with Quick Trim, when you use Quick Extend, appropriate constraints are
automatically created.

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Activity — Creating Fillets

In this activity, you will create fillets in an existing sketch.

Step 1: Open the sketch_fillet_1 part.

Step 2: Start the Modeling application.

Step 3: Activate the sketch.

Double-click on any of the sketch curves.

Step 4: Set the Infer Constraints Settings.

Choose the Infer Constraint Settings icon.

(ToolsConstraintsInfer Constraint Settings)

Turn off the Dimensional Constraints setting.

Choose OK.

Step 5: Create a 4 mm radius fillet using lines L16 and L20 with a single
selection and trimming the lines.

Choose the Fillet icon. (InsertFillet)

Make sure Trim Inputs is on (highlighted background).

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 Sketching

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Key in 4 in the Radius field on the graphics window, and press
Enter.

Select both lines at the same time, by selecting at their

intersection.

Drag the cursor around the screen and notice that you can
select which quadrant you want.

Select in the lower right quadrant to place the fillet in the

desired quadrant.

Step 6: Create a 4 mm fillet using lines L16 and L17 with a single selection
and do not trim the lines.

Turn off Trim Inputs. (background not highlighted)

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Select the two lines at their intersection.

Select in the upper right quadrant.

Step 7: Create a 4 millimeter fillet between lines L17 and L18. Select by
dragging across the two lines.
The 4.0 Radius value should still be in the text field on the
graphics window.

With MB1 held down, drag across the two lines as below: (This
is another method of selecting the curves to be filleted. The
curves crossed with the "crayon" are the curves selected.)

Notice that the 4 millimeter radius was used.

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 Sketching

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Step 8: Create another fillet between lines L18 and L20 by using the
"crayon", but this time do NOT use a radius value.
Use Backspace to erase the 4 in the text field.

Drag (with MB1), as shown below:

It used the selection location of the curves to determine the

radius.

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Step 9: Create a fillet between lines L18 and L19, and drag the size and
quadrant.
Individually select the lines L18 and L19.

Drag the cursor around the screen.

Select a location to create an arc similar to the one shown below.

Choose the Finish Sketch icon.

Step 10: Close the part.

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Activity — Using Quick Trim and Quick Extend
In this activity, you will trim and extend existing sketch geometry.
Step 1: Open the sketch_quick_1 part.

Step 2: Start the Modeling application.

Step 3: Trim curves with Quick Trim.

Double-click on one of the sketch curves to activate the sketch.

Choose the Quick Trim icon. (EditQuick Trim)

Select the line at the location of the arrow below.

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Hold MB1 down and drag the cursor across the two curves as
shown below.

Ctrl-Select the curves (1) and (2) for boundaries. Select on

curves (3) and (4) to trim the center portion.

Step 4: Extending curves with Quick Extend.

Choose the Quick Extend icon. (EditQuick Extend)

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 Sketching

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Place the cursor on the arc at location (1) shown below.

The status line informs you that the curve cannot be extended.
This is because there is no other curve that would intersect
the arc.

Place the cursor on the arc at location (2) shown below.

This time, an intersection is found and a preview is provided.

Select the arc at location (2) to create the extension.

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Step 5: Continue to experiment with Quick Trim and Quick Extend until
the instructor is ready to continue.

Step 6: Choose the Finish Sketch icon.

Step 7: Close the part.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 1-45
 Sketching

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Sketch Points
Sketch objects are defined by theoretical points. A line, for instance, is defined
by two points. The sketcher attempts to mathematically solve for the location
of the points by analyzing the constraints (rules) that are placed on objects.
The points that the sketch solver analyzes are referred to as sketch points.
By controlling the locations of these sketch points the curve itself may be
controlled. There are various ways to control these points. The sketch points
associated with different types of curves are illustrated in the graphic below.

Line Arc Circle Fillet

Spline Point Ellipse

Degree-of-Freedom (DOF) Arrows

Degree of freedom arrows are displayed at a sketch point when the solver is
unable to fully determine where the sketch point is located on the sketch
plane based on existing constraints and dimensions. They are only displayed
during the creation of dimensions or constraints.
The DOF arrows can point in both the horizontal and vertical directions. An
arrow pointing to the right means that the sketch point is free to move left or
right in the horizontal direction. An arrow pointing up means that the sketch
point is free to move up or down in the vertical direction.
These arrows provide visual feedback while you are constraining the sketch.

Undefined Undefined in Undefined in Defined in

in X and Y Y Direction X Direction X and Y
Directions Directions

(no display)

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DOF arrows are removed as rules are written that define the location of the
sketch points.
• Arc - Arcs have sketch points at the center and at either end. These
sketch points as well as the radius of the arc may be defined.

• Circle - Circles may have the center point as well as a radius or diameter
defined.

• Ellipse - An ellipse may have the location of its center defined; also, the
parameters for the size and orientation of the ellipse are stored for future
editing.

• Fillet - A Fillet is a special case of arc. By definition a fillet is tangent to

the objects with which it is associated and this rule is applied as it is
created. Fillets are also defined by the center and end points but the
tangency will help determine the location of these points.

• Line - Lines may have the sketch points at either end defined.

• Point - Points may be defined relative to other objects or at specific

locations in space.

• Spline - Degree three splines may have their defining points located.
Slopes of the spline at the defining points may also be defined. Splines
that are of a degree other than three may be added to sketches; however,
since their defining points are not located at their knot points, there is no
way to locate their defining points using constraints.

If any of the sketch points that define a curve are unconstrained, the curve is
displayed in the color specified by the Partially Constrained Curves setting
in PreferencesSketchColors. When all defining points are constrained,
the curve will change to the color specified by the Fully Constrained Curves
setting in PreferencesSketchColors. Theses colors only apply during the
creation of dimensions or constraints.

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Dimensional Constraints
Design Intent
The power in sketching is derived from the ability to capture design intent.
You do this by creating rules, called constraints, that dictate how sketch
objects will react to changes.
As many or as few constraints as necessary may be applied to cause the
sketch profile to update in the manner desired.
NX sketches are not required to be fully constrained.
There is one case where a sketch should always be fully constrained:
a sketch-on-path used for a variational sweep.

Creating Sketch Dimensions

A dimension controls the size of a sketch object, such as the length of a line or
radius of an arc, or the relationship between two objects, such as a distance
or angle.
Dimensions appear in the graphics window. Unlike drafting dimensions,
changing the value of the sketch dimensions changes the shape and or size of
dimensioned objects. This changes any features, such as extrude or revolve
features, that the sketch curves control.

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Dimensions may be applied by using
the dimension menu on the Sketch
Constraints toolbar.
1 — The default Inferred Dimensions icon
infers the dimension type based on the
objects that are selected and the position
of the cursor.
2 — The other dimension icons are useful
when the system is unable to infer the
desired dimension type. These different
options are "filters" that when selected
will only allow a specific dimension type
to be created.
Certain types of geometry may not be
selectable if they do not coincide with the
dimension type selected.

As dimensions are being created, the dimension, its extension lines, and
arrows are displayed as soon as the geometry has been selected.
• Drag the dimension until it is the correct type, for example horizontal
or parallel.

• Place the dimension by clicking MB1.

• Click and drag the dimension to the desired location.

Sometimes, a dimension type may be inferred before all of the geometry has
been selected. In this case, continue to select geometry until the correct
dimension type is displayed, or select the icon for the dimension type you
desire and select the geometry again.

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An expression is also created for each dimension. The name (1) and value
(2) of the expression appear in a text box in the graphics window after the
dimension has been placed. You may key in a new name or value. Press
the Enter key to activate the change.

Sketch Dimension Dialog

The Sketch Dimensions Dialog icon accesses the Dimensions dialog.

You can use the dialog to help create and edit dimensions. You can change the
value of a dimension by either keying it in or using the slider bar.

There are also two option menus to change the appearance of the dimension.
The Placement option menu is for defining how the text and arrows of the
dimension will be displayed. Options are for automatic placement of text and
arrows (1), manual text placement with arrows inside the extension lines (2),
or manual text placement with the arrows outside the extension lines (3).

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The Leader option menu is for defining whether the dimension’s leader is
attached to the left (1) or right (2) of the dimension text.

Both of these option menus may be used before, during or after dimension
creation.

Text Height
The Text Height controls the displayed height of the dimension text.
Modifying this value will affect the display of all dimensions in the active
sketch.
The Text Height option can also be accessed by choosing
PreferencesSketch.

The Fixed Text Height option in Sketch→Preferences controls the size of

the dimension text when you zoom. If this option is turned on, the text will
remain the same size relative to the screen as you zoom in and out.

Dimension Types

Inferred — The dimension type (except perimeter) is inferred based on

the objects selected and the cursor location.

Horizontal — Specifies a distance constraint between two points with

respect to the X-axis of the sketch coordinate system. Points, points on sketch
curves, edges, lines, and arcs are selectable.

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Vertical — Specifies a distance constraint between two points with
respect to the Y-axis of the sketch coordinate system. Points, points on sketch
curves, edges, lines, and arcs are selectable.

Parallel — Specifies a constraint for the shortest distance between two

sketch points. All sketch objects are selectable using this method. The points
selected will be inferred from the objects selected.

Perpendicular — Specifies a distance constraint measured

perpendicular to a selected line and a point. If the desired point is an
endpoint of a line, this endpoint must be selected as the second object.

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Angular — Specifies an angular constraint between two linear objects.

Radius — Specifies a radial size constraint for an arc or circle.

Diameter — Specifies a diameter size constraint for an arc or circle.

Perimeter — Constrains the collective lengths of lines and arcs to a

desired value. After selecting the curves and choosing MB2, an expression
is automatically generated with a “Perimeter_” prefix added to the name.
(i.e. Perimeter_p7=6.456). There will be no graphical representation of this
constraint in the graphics window.

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Activity — Adding Dimensional Constraints

In this activity, you will capture the design intent for a part by adding rules
that will control how the part is to change. These rules allow the part to be
easily modified.
The included angle of the adjustment slot should change from 45° to
75° by dimensional constraints.

Step 1: Open angle_adj_1.

Step 2: Start the Modeling application.

Step 3: Add the required dimensions.

Double-click on one of the sketch curves to activate the sketch.

Choose Preferences→Sketch.

Verify the Text Height is set to .10 and choose OK.

Choose the Inferred Dimensions icon.

(InsertDimensionsInferred)

Select the lower angled line (1, not endpoint).

The system infers that you wish to create a horizontal, vertical,

or parallel dimension depending on the placement of the cursor
relative to the geometry. DO NOT PLACE THE DIMENSION!

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Select the upper angled line (2, not endpoint).

Select a cursor location to place the dimension.

Select the horizontal line (1, not endpoint) across the bottom.

Select the lower angled line (2, not endpoint).

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Select a cursor location to place the dimension.

Choose MB2 to exit dimension creation mode.

Step 4: Change the viewpoint.

Choose MB3→Orient View to Model.

Choose the Finish Sketch icon.

There are times, such as geometry creation, when looking directly

at the plane of the sketch is beneficial. At other times, it may
help to change the view point to see the effects of changes on the
geometry.

Step 5: Close the part.

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Editing Dimensions
The editing of dimensions may be achieved as follows:
• To edit the value or the name, simply double-click on the dimension and
edit the value or the name in the text box and press Enter.

• To edit the position, place cursor over a dimension, press and hold down
MB1, and simply drag the dimension’s location.

• Additional editing that may be done with the Dimensions dialog as listed
below:
Name — Key in a new name in the text entry field.
Value — Key in a new value in the text entry field or use
the slider.
Position — Click and hold MB1 on the dimension and drag
to new position.
Text placement — Select a different option from the option menu.
Leader side — Select a different option from the option menu.
Text height — Key in a new text size in the text entry field.

The name and value of a dimension may also be edited by using the
Expressions dialog. As dimensions are edited, the constraints are
evaluated and the geometry is modified.

Delay Evaluation
Delay Evaluation prevents geometry changes as one or more dimensions are
modified. This is available as an icon on the Sketcher toolbar or by choosing
ToolsDelay Sketch Evaluation.

Evaluate Sketch
Evaluate Sketch controls sketch evaluation when Delay Evaluation is on.
(Sketches are evaluated automatically when you exit from the Constraints
dialog.) This is available as an icon on the Sketcher toolbar or by choosing
ToolsEvaluate Sketch

Update Model
Update Model forces the model to update without leaving the sketch
function. (The model is updated automatically when you exit from the sketch
environment.) This is available as an icon on the Sketcher toolbar or by
choosing ToolsUpdate Model.

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Retain Dimensions

When a sketch is deactivated the dimensions are normally hidden.

Retain Dimensions is a toggle in the Sketch Preferences dialog to retain
dimension display after the sketch is deactivated.

Retain Dimensions applies only to the active sketch, thus to suit your needs
you may have a mixture of sketches with and without retained dimensions.
Use this setting when you need to display dimensions without an active
sketch, for example to reference expression names between sketches, when
creating features, or for plotting.

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Activity — Editing Sketch Dimensions

In this activity, you will edit dimensional constraints and see that they do not
sufficiently control the angle bracket from the previous activity.
Step 1: Open angle_adj_2.

Step 2: Start the Modeling application.

Step 3: Change the layer settings.

Make layer 1 Selectable.

Fit the view. (MB3Fit)

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Step 4: Edit a dimension.
Place the cursor over a sketch curve and choose MB3→Edit.

Choose MB3→Orient View to Model.

Double-click on the 45° dimension.

In the dynamic input field, key in 75 and press Enter.

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Step 5: Edit another dimension.
Double-click on the 15° dimension.

In the dynamic input field, key in 25° and press Enter.

Notice how the geometry updates.

Basic geometric assumptions that we make when we look at this
geometry are not specified to the system, i.e. the bottom line has
no horizontal constraint applied.
If the geometry had been created in the sketch rather than added to
the sketch some of these geometric assumptions would have been
added to the geometry as constraints during the creation process.

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Step 6: Close the part.

Choose Undo twice. (MB3Undo)

Choose the Finish Sketch icon.

Close the part.

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Geometric Constraints
A geometric constraint establishes a geometric characteristic of a sketch
object (such as defining a line as being horizontal) or the type of relationship
between two or more objects (such as requiring that two lines be parallel or
perpendicular, or that several arcs have the same radius).
Unlike dimensional constraints, geometric constraints have no editable
numeric values; a constant angle constraint, for instance, simply dictates that
the line stay at the angle it is at when the constraint is applied.
To create geometric constraints, choose the Constraints icon, select the
objects, and choose the desired constraint from the icon option bar that
appears in the upper left corner of the graphics window. Only icons for
constraints that apply to the selected geometry will be displayed.

You may also choose the constraint from an MB3 pop-up menu after selecting
the geometry.

To assign multiple constraints at one time, press the Ctrl key while
selecting the objects. The icon option bar for the constraints will
then remain in the upper left corner of the graphics window after
you choose the first constraint. You can use MB2 or the Esc key to
cancel creation of constraints.

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Types of Geometric Constraints

Coincident Constrains two or more points as having the

same location.

Collinear Constrains two or more linear objects as lying on

or passing through the same theoretical straight
line.
Concentric Constrains two or more arcs as having the same
center.

Constant Angle Constrains a line so as to remain in its current

orientation without input of an angular value.

Constant Length Constrains a line so as to remain at its current

length without input of a length value.

Equal Length Constrains two or more lines as being the same

length.

Equal Radius Constrains two or more arcs as having the same

radius value.

Fixed Constrains unchangeable characteristics for

geometry, depending on the type of geometry
selected. You can apply a Fixed constraint to an
individual sketch point or to an entire object.
Horizontal Constrains a line as being parallel to the FCS
X-axis.

Midpoint Constrains the location of a point to be

equidistant from both ends of the curve.
Select the curve anywhere other than at
its end points.
Parallel Constrains two or more linear objects as being
parallel to each other.

Perpendicular Constrains two linear objects as being

perpendicular to each other.

Point on Curve Constrains the location of a point as lying on the

path or projection of a curve.

Point on String Constrains the location of a point as lying on an

extracted string.

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Scale, Non– When applied, a spline will scale in the horizontal
Uniform direction while keeping the original dimensions
in the vertical direction during modification.
Scale, Uniform A spline will scale proportionally in both the
horizontal and vertical when the horizontal
length changes.
Slope of Curve Constrains a spline, selected at a defining point,
and another object as being tangent to each other
at the selected point.
Tangent Constrains two objects as being tangent to each
other.

Vertical Constrains a line as being parallel to the FCS

Y-axis.

Displaying Constraint Symbols

Constraint symbols are displayed when a sketch is active. Symbols for
Coincident, Point on Curve, Midpoint, Tangent, and Concentric are always
displayed.

The Show All Constraints option will display the symbols for all the
constraints in the active sketch.
The various constraint symbols are shown below:

Fixed Constant Angle

Collinear Concentric
Horizontal Tangent
Vertical Equal Radius
Parallel Coincident
Perpendicular Point on Curve
Equal Length Midpoint of Curve
Constant Length Point on String
Mirror Scale, Uniform
Slope of Curve Scale, Non-Uniform

If the sketch curves are relatively small (the view is zoomed out), the
symbols may not be displayed. You may need to zoom in to see them.

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Show/Remove Constraints
Show/Remove Constraints helps you manage constraints. The constraints
may be listed by object(s) or all of the constraints of the active sketch may
be listed at once.

1 — List all constraints

or by object(s).

2 — Filter for the type

of constraint to list.

3 — Determines if the
filtered constraint types
will be included or excluded.

4 — Category of
constraints to list.

5 — Actions to take on the

listed constraints.

Constraint Interrogation

While the Show/Remove dialog is displayed, you can determine what

constraints are present by passing the selection ball over a sketch object. If
the object has an associated constraint, the object will be pre-highlighted
along with any other objects that share the constraint. The constraint symbol
will appear next to the sketch objects. If an object which has no constraints
associated with it, it will not highlight.

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Constraint Categories

There are two major categories of constraints, Explicit and Inferred.

Explicit constraints are constraints that you create by assignment using the
constraints dialog or by virtue of the creation method. Inferred constraints
are Coincident constraints that the system has inferred and created
during the curve creation process. You have the option to list only Explicit
constraints, only Inferred constraints, or both.

Constraint Listing

The constraints may also be listed in the Show/Remove Constraints dialog by

selecting one of the three options at the top of the dialog window.

Selected Object Once an object is selected, the associated

constraints, depending on the selected constraint
category, are listed in the dialog. To view
constraints associated with a different sketch
object, simply select the new object.
Selected Objects Allows the selection of multiple objects; the
associated constraints, depending on the selected
constraint category, are listed in the dialog. Objects
may be deselected by holding the shift key down
and selecting the object.
All in Active List all the constraints of the active sketch,
Sketch depending on the selected constraint category.

Listing Box

Any time there are constraints listed in the list box they may be browsed by
selecting the constraint to highlight it. When the constraint is highlighted in
the list box, the sketch object(s) that is associated with it is also highlighted
in the graphics window. The Step Up the List and Step Down the List buttons
allow easy navigation through the various constraints. The Up and Down
arrows on most keyboards will mimic this behavior.

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Information

The Information button located on the Show/Remove Constraints dialog will

list all of the constraints in the active sketch to the information window.
This is useful should there be a need to make a hard copy of the constraints
or save them as a text file.

Removing Constraints

Constraints may be deleted by these methods:

• Highlight them in the Show/Remove Constraints dialog List box and select
Remove Highlighted Constraint(s), or just double click them in the list.

• Turn on Select Constraints (on the Selection toolbar), select the constraint
symbol on the graphics window, and then choose the Delete icon.

• Turn on Select Constraints, select the constraint symbol on the graphics

window, and then use MB3Delete to delete selected constraint.

Undo

Undo from the Edit pull-down menu, the Undo icon on the Standard toolbar,
the MB3 pop-up menu, or the accelerator keys. Undo takes the user actions
back one step at a time.
After an Undo is performed, the Redo option is available in the Edit
pulldown menu or Standard toolbar.

Dragging Geometry

Under constrained geometry can be dragged only when not in a constraint

creation mode. Simply hold down and drag MB1 while on the selected
curve(s) or point(s).

Selection

When in the Sketcher Task Environment, the selection toolbar changes. It

has two icons that are only available in the Sketcher.
Select Sketch Objects allows selection of curves and dimensions
in the sketch.
Select Constraints allows selection of constraint symbols in the
graphics window.

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Constraint Conditions

When either the Dimensions or Constraints option is chosen, the Status line
lists the constraint condition for the active sketch. A sketch may be fully
constrained, under constrained, or over constrained. When the sketch is
under constrained the Status line will indicate the number of constraints
needed.

Sketch needs 4 constraints

Sketch is fully constrained
Sketch contains over constrained geometry

A sketch is evaluated each time a constraint is placed upon the sketch. Each
time a sketch is evaluated, the system attempts to solve the set of constraints
that describe how the geometric objects are positioned and their relationships
with each other.

Fully Constrained
In order to completely capture the design intent of a particular profile, it may
be beneficial to fully constrain the sketch. This occurs when the solver is able
to completely define all sketch geometry.
There is no requirement to fully constrain a sketch. The design intent has
been captured sufficiently when the constraint set applied to the profile
causes it to update in the intended manner.

Under Constrained
A sketch is under constrained when there is insufficient information to
completely locate each sketch point. Degree-of-freedom arrows are displayed
at each point that can not be solved to identify the direction in which that
point remains free to move.

Over Constrained

A sketch is over constrained when too much constraint information is

supplied to the solver. For example, if an Equal Length constraint is applied
to two lines and then dimensions are added to each to constrain their length,
the sketch would be over constrained.
The geometry and dimensional constraints that are causing the over
constrained condition are highlighted in a different color to help you identify
and resolve the issue. This color is determined by the Overconstrained Curves
and Dimensions setting in the Sketch Preferences.
An unwanted constraint must be removed before the system will change the
geometric configuration. The sketch remains in the last solved condition.

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Conflicting Constraints
Dimensional constraints and geometry that are in conflict in the current
configuration with the current constraint set are also highlighted in a
different color. This indicates that the constraint set that has been supplied is
not solvable with the geometry in its current configuration. Constraints may
need to be added or removed in order for the sketcher to be able to solve the
constraint set. The highlight color is determined by the Conflicting Curves
and Dimensions setting in the Sketch Preferences.

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Activity — Adding Constraints

In this activity you will add constraints to the angle adjustment bracket to
cause the expected update to occur when a dimension is modified.
Step 1: Open angle_adj_3.

Step 2: Start the Modeling application.

Step 3: Add the required constraints.

Place the cursor over a sketch curve and choose MB3→Edit.

Choose MB3→Orient View to Model.

Fit the view. (MB3Fit)

Choose the Constraints icon. (InsertConstraints)

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Select the line (1) at the bottom of the sketch.

Choose Horizontal in the upper left corner of the graphics

window. (MB3Horizontal)
This constraint will keep the line from rotating around when
dimensions are modified.
There are six places where the curvature transitions need to
maintain tangency.

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Select the six tangent curve pairs near the six points shown
below, two adjacent curves at a time, and apply aTangent
constraint to each pair. Be careful to select on the correct half
of the arc.

Lastly, the two arcs at the top of the slot should remain
concentric.

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Select the two upper arcs (1) and apply a Concentric constraint.

The slot should now be constrained such that the angle may be
adjusted while the configuration remains as intended.

Choose MB2 to turn the Constraints option off.

Step 4: Edit the dimensions.

Double-click on the 45° dimension and change it to 75°.
The sketch geometry changes in the expected manner.

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Step 5: Apply the change to the solid geometry.

Choose the Update Model icon. (ToolsUpdate Model)

Choose the Finish Sketch icon.

Step 6: Close the part.

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Activity — Constraining a Profile

Constrain the pipe vise sketch to satisfy the stated design intent.

Apply constraints to the curves so that the following may be

controlled:
• The outside envelope of the part.

• The included angle of the angled lines.

• The angled lines must remain centered in the part horizontally.

• The width of the slot at the bottom of the angled lines is controlled
by the radius at the bottom of the slot.

Step 1: Open pipevise_1.

Step 2: Start the Modeling application.

Step 3: Activate the sketch.

Double-click on a sketch curve.

Step 4: View the system applied constraints.

Choose the Show/Remove Constraints icon.

(ToolsConstraintsShow/Remove Constraints)

Choose All In Active Sketch in the List Constraints For: area

of the dialog.

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Verify the Show Constraints option is set to Explicit.
The system created constraints are now displayed in the list
box. The dialog should look similar to the graphic shown below.

Choose the first constraint in the list.

The object referred to in the list is highlighted in the graphics
window. There should be one horizontal line highlighted.

Use the UP and DOWN arrow buttons located to the right of

the list box to browse through the constraint list.

Cancel the Show/Remove Constraints dialog.

Step 5: View the degree of freedom arrows.

Turn on the Constraints icon. (InsertConstraints)

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Notice that there are degree of freedom arrows at each of the
sketch points. Even though most of the objects in the sketch have
constraints associated with them, the sketch points are free to
move in all directions. This is because the system cannot locate
any of the points relative to model space.

Step 6: Constrain the location of a point.

Select the lower endpoint of the left vertical line.

Select the vertical datum axis.

Choose the Point on Curve icon in the upper left corner

of the graphics window.
The geometry now changes to follow the constraint. The point
at the bottom of the left vertical line is now constrained in the
horizontal direction.

Select the left endpoint of the bottom horizontal line.

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Select the horizontal datum axis.

Choose the Point on Curve icon.

The geometry now changes to follow the new constraint. The
shared sketch point at the bottom of the left vertical line is now
constrained in both the horizontal and vertical directions. The
degree of freedom arrows go away and, due to the horizontal
and vertical constraints on the lines that share the sketch
point, one of the arrows on the opposite end of those lines has
disappeared.

Choose MB2 to cancel the Constraints mode.

Fit the view. (MB3Fit)

Step 7: Move the datum planes and axes to layer 61.

The datums have served their purpose of locating the sketch. You
will now move them to ease selection of objects and clean up the
screen display.

Choose Edit→Object Display.

Choose the Class Selection icon in the upper left corner of the

graphics window.

Choose Type.

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Choose Datums and choose OK.

Choose Select All and OK.

Key in 61 for the Layer in the dialog and press Enter.

Step 8: Continue adding constraints to satisfy the stated design intent.

Turn on the Constraints icon. (InsertConstraints)

Hold the Ctrl key down and select the two horizontal lines (1)
at the top of the profile.

Choose Collinear and Equal Length.

Use the Esc key to deselect all the curves.

(EditSelectionDeselect All).

Select the right side of the arc at the bottom of the slot (1).
Select the short right vertical line (2, but not on the end point).

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Choose Tangent.

Create another Tangent constraint on the other side of the slot,

selecting the left side of the arc and the left vertical line.

Hold the Ctrl key down and select the bottom horizontal line
and the lower endpoint of the line originating from the arc
center.

Choose Point on Curve.

Choose Midpoint.

Use the Esc key to deselect all the curves.

(EditSelectionDeselect All).

Select the line (1), shown below, between the midpoint and
the arc center.

Choose Vertical.

Adding dimensional constraints to satisfy the controlling

portions of the design intent will allow the profile to be changed
by modifying the numerical values.

Choose the Inferred Dimensions icon.

(InsertDimensionsInferred)

Select the bottom horizontal line. Drag the dimension to

position it and select with MB1 to place it.

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Key in a value of 5 and press Enter.
Notice the curves change color as they become constrained.

Fit the view if necessary.

Select the left vertical line and place the dimension for it.
Change the value to 3.75.

Select the top left horizontal line and place the dimension.
Change its value to .5.

Fit the view if necessary.

Select the left angled line (1) and the top left horizontal line
(2), avoiding the end points. Place the angular dimension and
change its value to 45°.

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Select the right angled line and the top right horizontal line,
avoiding the end points. Place this angular dimension and
change its value to the ’p’ number assigned to the other angular
dimension.

Select the arc at the bottom of the slot. Place the radius
dimension and change its value to .25.

Select the line connecting the arc center and the midpoint
and place this vertical dimension. Change its value to 1.5 and
choose Enter.
The Status line now informs you that the sketch is fully
constrained. Remember that it is not necessarily required
to fully constrain the profile if it is updating in the manner
desired.

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Step 9: Change the constraints on the sketch to alter the included angle in
the notch.
Click on the first angular dimensional constraint that was
created and change it from a 45° to 30°.

Notice that the depth of the notch is unchanged as a result of

this edit. Should that have not been our intent, we would have
to constrain the sketch in a different manner.

Choose the Finish Sketch icon.

Step 10: Close the part.

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Activity — Sketching and Constraining a Gasket
In this activity, you will create and constrain a gasket. To efficiently capture
the design intent, constraints and dimensions will be added progressively.
The center hole is the origin of the gasket. The three holes are located
on a horizontal axis. The lines on the outer boundary of the profile
are tangent to the arcs.

Step 1: Open the seedpart_in part and save it as ***_gasket_1 where ***
represents your initials.

Step 2: Start the Modeling application.

Step 3: Create the sketch on a Datum CSYS.

Change the Work Layer to 21 so that the part will be compliant
with class standards.

Choose the Sketch icon. (InsertSketch)

Click on the sketch name; key in s21_profile and press Enter.

Choose Datum CSYS.

Choose Absolute CSYS.

Choose OK.

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The X-Y plane of the Datum CSYS is highlighted as the default
sketch plane.

Choose OK to accept the default plane.

Step 4: Set the Infer Constraint Settings.

Choose the Infer Constraint Settings icon.

(ToolsConstraintsInfer Constraint Settings)

Verify that the following constraints are turned on.

Concentric
Coincident
Dimensional Constraints

Choose OK.

Step 5: Create the circles in the center of the gasket.

Choose the Circle icon. (InsertCircle)

Verify that Control Point is turned on in the Snap Point

toolbar.

Select the existing point at the origin of the Datum CSYS.

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Drag the cursor to preview circle as shown below. Key in a
Diameter value of 2 and press Enter.

The first circle is created.

Key in a Diameter value of 3 for the second circle and press

Enter.

Select the existing point at the origin of the Datum CSYS.

Choose MB2.

The two circles are fully constrained because of the dimensional

and geometric constraints that were inferred as you created them.

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Step 6: Create a circle representing the hole on the left side.

Choose the Circle icon. (InsertCircle)

Click and drag to create a circle near on left side of the graphics
window. Key in a Diameter value of 0.5 and press Enter.

Choose the Constraints icon. (InsertConstraints)

Select the arc center of the circle and the horizontal datum axis.

Choose Point on Curve .

Choose the Inferred Dimensions icon.

(InsertDimensionsInferred)

Create a perpendicular dimension from the vertical datum

axis to the arc center of the left circle. Change the value of
the dimension to 2.625.

Step 7: Create a circle for the outer boundary on the left side.
Create another circle in the left side of the graphics window
with a diameter of 1.

Choose the Constraints icon. (InsertConstraints)

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Select the two circles on the left side and choose Concentric.

Step 8: Create circles representing the hole and outer boundary on the
right side.
Create two circles on the right side of the graphics window
representing the hole and the outer boundary of the gasket. Do
not explicitly enter the diameter values. You will constrain
them to be equal to existing circles.

Choose the Constraints icon. (InsertConstraints)

Select the two new circles on the right and choose Concentric.

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Select the arc center of the circles on the right and the

horizontal datum axis and choose Point on Curve.

Select the smaller circle on the left and the smaller circle on

the right and choose Equal Radius.

Select the larger circle on the left and the larger circle on the

right and choose Equal Radius.

Choose the Inferred Dimensions icon.

(InsertDimensionsInferred)

Create a horizontal dimension from the arc center of the left

circles to the arc center of the right circles. Change the value of
the dimension to 5.25.

Step 9: Set the Infer Constraint Settings before creating the lines.

Choose the Infer Constraint Settings icon.

(ToolsConstraintsInfer Constraint Settings)

Disable all constraints except Point on Curve and Tangent.

Choose OK.

Step 10: Create the tangent lines on the outer boundary of the gasket.

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Choose the Line icon. (InsertLine)

In the Snap Point toolbar, disable all options except Point on

Curve.

Create the lines by selecting the circles representing the outer

boundary of the gasket. Select the circles by placing the cursor
near the expected tangency.

You should see Point on Curve and Tangent constraint symbols

on each end of the lines as they are created.

The Quick Trim option could be used to trim the circles.

However, when extruding the sketch to create a solid
body, it is possible to define the correct boundary of the
gasket without trimming.

Step 11: Choose the Finish Sketch icon.

Step 12: Choose File→Close→Save and Close.

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Convert To/From Reference
At times it is useful to add a dimension to a sketch to see the effect of a
change numerically. Adding a dimensional constraint, however, would cause
the sketch to become over constrained. It also may be necessary to add
sketch curves to aid in the construction and constraining of a profile without
representing a portion of the swept feature.
To support these needs, curve and dimensional constraints within a sketch
may be converted to and from a Reference status.
• To convert objects, select them in the graphics window and choose Convert
To/From Reference from the MB3 pop-up menu.

• You may access a dialog by choosing the Convert To/From

Reference icon from the Sketch Constraints toolbar
(Tools→Constraints→Convert To/From Reference).

• Reference curves are displayed in a phantom line font and are ignored
during sweep operations.

• Reference curves and dimensions are displayed in colors specified

by the Reference Curves and Reference Dimensions settings in
Preferences→Sketch→Colors.

• Reference dimensional constraints are displayed with only the value

portion of the expression. The values will be updated as the sketch is
changed, but they do control the sketch geometry with which they are
associated.
Dimensions can be made reference as they are created by choosing

Create Reference Dimension in the icon option bar.

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Activity — Constraint Conditions
In this activity, you will constrain and edit a simple sketch to change the
design intent. This configuration is not one that you would likely sketch, but
its simplicity illustrates the concept of an over-constrained condition.
Apply constraints to control the length and width of the sketch. The
shape of the sketch should remain rectangular.

Step 1: Open seedpart_in.

Step 2: Start the Modeling application.

Step 3: Create a sketch on Layer 21.

Change the work layer to 21.

Choose the Sketch icon. (InsertSketch)

Choose Datum CSYS.

Choose Absolute CSYS.

Choose OK.
The X-Y plane of the Datum CSYS is highlighted as the default
sketch plane.

Choose OK.

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Step 4: Set the Infer Constraints Settings.

Choose the Infer Constraints Settings icon.

(ToolsConstraintsInfer Constraint Settings)

Verify that the following constraints are turned on.

Horizontal
Vertical
Parallel
Perpendicular
Coincident

Choose OK.

Step 5: Create a rectangle.

Choose the Rectangle icon. (InsertRectangle)

Verify that Control Point is turned on in the Snap Point

toolbar.

Select the existing point at the origin of the Datum CSYS.

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Drag the cursor to preview the rectangle and select a cursor
location near the upper right corner of the graphics window.

Step 6: Interrogate the constraints that currently exist for this sketch.

Choose the Show/Remove Constraints icon.

(ToolsConstraintsShow/Remove Constraints)

Choose All In Active Sketch.

Set the Show Constraints to Explicit.

Highlight the first constraint in the list and use the down
arrow button to browse the constraints.

Choose Cancel.

Step 7: Apply dimensional constraints to control the length and width of

the rectangle as per the design intent.

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Choose the Inferred Dimensions icon.
(InsertDimensionsInferred)

Select the left vertical line and place the dimension. Change
the value to 2.75.

Select the bottom horizontal line and place the dimension.

Change the value to 4.5.

As dimensional constraints are being created, the

degree-of-freedom arrows are eliminated and the curves change to
the fully constrained color. The sketch is fully constrained with one
vertical and one horizontal dimensional constraint, along with the
geometric constraints inferred when the lines were constructed.
Design Change — Modify the sketch so that it can be
controlled by the angle and length of a diagonal line.

Step 8: Create a diagonal line in the sketch and convert it to reference.

Choose the Line icon. (InsertLine)

In the Snap Point toolbar, disable all options except Control

Point.

Select the lower left endpoint and the upper right endpoint of
the rectangle to define the line.

Step 9: Convert the diagonal line to Reference status.

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Choose MB2 to exit the line creation mode.

Select the diagonal line.

Choose MB3→Convert To/From Reference.

Step 10: Apply an angular dimensional constraint.

Choose the Inferred Dimensions icon.

(InsertDimensionsInferred)

Select the lower horizontal line (not the endpoint) and the
diagonal line (not the endpoint). Indicate a location for the
angular dimension and change the value to 35°.
The Status line indicates that sketch is now over constrained.
The sketch objects associated with the over constrained
condition change to the color specified by the Overconstrained
Curves and Dimensions setting in the Sketch Preferences.
To correct the over constrained condition, one or more of the
offending constraints must by removed. The new design intent
is to control the sketch with angular and diagonal length
dimensions.

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Step 11: Apply a parallel dimensional constraint.
Select the diagonal line and place a parallel dimension. Change
the value of the dimension to 6.5.

Notice that the sketch configuration does not change when the
value is modified. The system leaves the geometry in its last
solved state until the over constrained condition is resolved.

Step 12: Convert sketch dimensions to reference.

Choose MB2 to exit the dimension creation mode.

Select the horizontal and vertical dimensions.

Choose MB3→Convert To/From Reference.

The sketch is returned to a fully constrained condition. The
reference dimensions reflect the value only. They do not control
the geometry to which they are attached.
The over constrained condition could also have been resolved
by deleting the horizontal and vertical dimensions.

Choose the Finish Sketch icon.

Step 13: Close the part.

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Summary
This lesson introduced the concept of sketch creation.
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 can also be defined on a sketch
plane which is associative to a datum plane/face of a model. Both of these
benefits allow you to capture and maintain design intent.
Constraints are applied to sketch objects in order to capture the design intent.
The level of constraint, partial or full, is determined by the design intent
and what is necessary to capture it.
In this lesson you:
• Created sketches on datum planes, solid faces, and a Datum CSYS.

• 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.

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Lesson

2 Constraining Sketches
2

Purpose

This lesson describes creating and modifying sketch constraints.

Objectives

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

• Create Geometric Constraints

• Work with System Applied Constraints

• Auto Create and Display Constraints

• Work with Constraint Conditions

• Convert Sketch Curves To Reference Curves

• Update The Model

• Add Objects to Sketch

• Constrain the Perimeter of a Sketch

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 Constraining Sketches

Constraints
NX provides a variety of feedback about a sketch.
You can see color coded information about the constraint condition of a curve,
2 list current constraints, or view information about how many constraints are
needed to fully constrain the sketch.

Drag
You might consider a sketch sufficiently constrained, but the system still
lists the status as under constrained.
One method of interrogating the sketch is to drag the geometry. Dragging
allows under constrained geometry to be moved in the unconstrained
directions.
To drag a single curve or point move the cursor over it, click, and drag. For
multiple objects first select curves or end points and then click and drag
all selected objects. Objects that share sketch points with the object being
dragged remain connected to the object and stretch to accommodate the
movement.
If an object has no freedom to move due to constraints, it will not drag.

In the example below, L6 (1) is being dragged while L4 and L5 (2) stretch to
accommodate the movement of the line. L6 is constrained so it maintains its
angular and length relationship during the drag operation.

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Drag may be used to drag multiple sketch curves. Select the curves to be
dragged, then use the left mouse button to click and drag to move the objects
in their unconstrained directions. Selecting two or more objects to drag
causes different results as the constraints applied to different curves have
different effects on how the group of curves react. 2
In the example below, the two lines L4 and L6 (1) are selected to drag causing
L5 and the upper horizontal line (2) to stretch.

Drag may be used to drag a single sketch point. Move the cursor to
pre-highlight the point, then click and drag to move it in its unconstrained
directions. Objects that share the sketch point stretch to accommodate the
movement.

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 Constraining Sketches

In the example below, the sketch point V1 is being dragged. The lines that
share the sketch point stretch to accommodate the movement of the point.
Their angle and length are modified by the drag operation.

Drag may also be used to approximate the correct location of a sketch profile
relative to other objects. This may be useful when the process of constraining
distorts the sketch profile so that it would be difficult to undo.

Undesired Results

Distortion caused by the act of constraining.

Desired Results
Desired results when entire profile dragged from quadrant to quadrant.

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 Constraining Sketches

Create Inferred Constraints

Create Inferred Constraints lets you toggle inferred constraints on or off as
you create and/or edit sketch geometry. 2
Create Inferred Constraints is active by default. The icon is available (but by
default not displayed) in the Sketch Constraints toolbar.
When you drag a sketch object you can make use of Inferred Constraints,
such as horizontal or vertical.
If Create Inferred Constraints is inactive (off), the system uses the constraints
only to place the geometry, but does not store the constraints in your file.
If Create Inferred constraints is active (on), the system creates and stores
constraints as shown by constraint symbols you see on the screen.

You control which constraints can be inferred during curve

creation via Inferred Constraint Settings.

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Activity - Dragging Sketch Objects

Step 1: Open the part file drag_1.

Step 2: Activate the sketch.

2
Choose Start→Modeling.

Double-click on a sketch curve.

Zoom out the view to give yourself some working room around
the geometry.

Toggle Show All Constraints to active.

In Preferences→Sketch make sure that Dynamic Constraint

Display is inactive (off).

Notice that the constraint set is presently made up of one vertical

and several tangent and coincident constraints.

Step 3: Drag a curve.

Place the cursor over the curve at location (1) shown below.
Hold MB1 down and drag the curve to location (2).

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Notice how the vertical and tangent constraints impacted the drag
operation. Also notice the circle was left behind.

Choose Undo.

Choose Constraints.

Select the arc (1) and circle (2) shown below. Apply a

Concentric constraint.

Toggle Constraints off (or MB2).

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Place the cursor over the curve at location (1) shown below.
Hold MB1 down and drag the curve to location (2).

Notice that the circle moved with the drag operation.

Choose Undo.

Step 4: Dragging curves versus endpoints.

Place the cursor over the curve at location (1) shown below.
Hold MB1 down and drag the curve to location (2).

The line with a constraint remains tangent to the arc, while the
other line may not remain tangent.

Choose Undo.

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Select and drag the endpoint shown below from location (1)
to (2).

When you select an end point the radius of the arc changes
dramatically as you drag. You are effectively dragging the radius
along with the end point.

Choose Undo.

Step 5: Drag a line to horizontal, and create a horizontal constraint.

Display Create Inferred Constraints in the Sketch
Constraints toolbar, or use ToolsConstraints.

Verify that Create Inferred Constraints is active.

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Drag the endpoint (1) shown below from location (1) to (2).
End the dragging action only when you can see a horizontal
constraint symbol.

Notice that the line snaps to horizontal within the snap angle.

Notice also that the horizontal constraint becomes permanent

when you release the end point you were dragging.

Choose Undo.

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Step 6: Drag a line to horizontal without creating a constraint.

Toggle Create Inferred Constraints to inactive.

Once again, drag the endpoint from location (1) to (2). End the
dragging action only when you can see a horizontal constraint 2
symbol.

Notice that, just as before, the line snaps to horizontal within the
snap angle and the horizontal symbol appears.
Notice that this time no horizontal constraint is created.

Choose Undo.

Toggle Create Inferred Constraints to active. (Restore the

default setting.)

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Step 7: Drag several curves at one time.

Select the curves shown below by dragging a rectangle around
them.

Drag the selection to the left as shown below.

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Step 8: Drag all of the sketch geometry to a new position.

Drag a rectangle around the entire sketch and drag the
geometry to the location shown below.

Step 9: Locate the sketch.

Choose Constraints.

Select the arc center of the arc (1) and the horizontal datum
axis (2).

Apply a Point on Curve constraint.

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 Constraining Sketches

Select the same arc center and the vertical datum axis.

Apply a Point on Curve constraint.

2 Notice what happened to the sketch geometry. The arc center
moved to the prescribed location and the vertical line still
meets the vertical and tangent constraints assigned to it.

Toggle Constraints off (or MB2).

Fix the geometry by dragging the vertical line to the other side
of the arc. Try to maintain the same size of the upper and
lower arcs.

Choose Finish Sketch.

Step 10: Close the part.

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Activity - Adding Constraints

As a design evolves two angles that determine the extents of a
circular slot may be changed.
When changes are made, the update must not fail, and the following 2
conditions must be met:
• When the angles change, it is necessary that the slot retain its
current width.

• The slot must remain centered in the arm with its upper end
concentric with the end of the arm.

• All arcs that are currently tangent must remain tangent.

You will verify that this sketch needs additional constraints to control
it as it updates.
You will add enough geometric constraints to fully capture the design
intent.

Step 1: Open angle_adj_4 and choose Start→Modeling.

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Step 2: Examine the sketch.

Double-click on a sketch curve.

If necessary, toggle Show All Constraints to active.

2

In PreferencesSketch, if necessary, toggle Dynamic

Constraint Display to inactive.

Are there any geometric constraints in the sketch?

What do you think would happen if you edited one of the
dimensions?

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Step 3: Edit the angle p68 to 35 and observe the update behavior.

Double-click on p68 to enter edit mode.

Change the value to 35 and press enter.

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What happens to the sketch?

The unite between the shape extruded from the sketch and the rest
of the model will fail, thus the model cannot update successfully
with the sketch in this condition.
In addition, one of the end arcs of the slot has lost its tangency.

Step 4: Drag a curve end to see if the sketch deforms.

Drag the end point indicated by the square dot in the direction
of the black arrow.

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Step 5: Undo the changes.

Choose Edit→Undo List and choose Edit Sketch Dimension,
the entry just above Enter Sketcher.

You could also press Ctrl+Z until all of the edits you made 2
are undone

Step 6: Constrain the line adjacent to the part.

Choose Constraints.

Select the line (1) at the bottom of the sketch.

Select the solid edge behind the line.

Choose Collinear.
This constraint will keep the line from rotating around when
dimensions are modified.

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Step 7: Constrain the arcs to maintain tangency in six places.

Select the six tangent curve pairs near the six points shown
2 below, two adjacent curves at a time, and apply Tangent
constraints to each pair. Be careful to select on the correct half
of the arc.

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Step 8: Make the two arcs at the top of the slot concentric.
Select the two upper arcs and apply a Concentric constraint.

The slot should now be constrained such that the angle may be
adjusted while the configuration remains as intended.

Choose MB2 to toggle the Constraints icon off.

Step 9: Edit the p68 dimension to 75.

Double-click on the 45° dimension and change it to 75°.

Step 10: Apply the change to the solid geometry.

Choose Finish.

Step 11: Close the part.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 2-21
 Constraining Sketches

Automatic Constraint Creation

The system can create certain types of constraints automatically. This is
2 especially useful when geometry is added to a sketch rather than created
as sketch objects.
You can enable the Automatic Constraints icon on the Sketch constraints
toolbar, or use Tools→Constraints→Automatic Constraints.

Procedure

1. Choose Automatic Constraint Creation.

2. Toggle the desired constraints to on.

3. Ensure that the proper distance and angle tolerances are set.

4. Choose Apply or OK.

The Set and Clear buttons, on the Auto Create Constraints dialog, may be
used to turn all of the constraint fields on or off.
When using the horizontal, vertical, parallel, and perpendicular auto create
options, the system evaluates lines using the specified Angle tolerance to
apply the proper constraints.
Other types of auto create constraints, such as coincident and concentric, use
the Distance tolerance to apply the constraints.
Using the Distance tolerance with the Coincident constraint will have the
effect of closing gaps. This condition is common with objects that have been
translated from other systems.
Allow Remote constraints permits automatic constraints to be created
between curves that do not actually touch. Currently, tangency between
curves that would be tangent if they were extended is supported.

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Sketch Operations — Project

Project lets you create extracted curves or strings of curves by projecting
external objects onto a sketch along the normal of the sketch plane. You can 2
project a curve associatively or non-associatively onto a sketch.
Objects available for projection include:
• Curves, associative and non-associative

• Edges

• Faces (selecting a face automatically selects its edges for projection)

• Other sketches or the curves within the sketches

• Points

Procedure
1. Set the selection filter to the desired object type.

2. Select a curve string, face, edges or points you want to project onto the
sketch plane.

3. Set the Associate option as desired.

4. Set the Output Type option as desired.

5. Click OK.
A curve string is projected onto the sketch plane from the selected curves,
face or edges. If you selected points, the points are projected onto the
sketch.

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Output Types

The extracted curves are created with their original

Original
geometry types.
2 Spline The extracted curves are represented by individual
Segment splines.
Single The extracted curves are connected and
Spline represented by a single spline

Editing Projected Curves

You can add, remove, or replace curves projected into a sketch by displaying
and using the Edit Curve icon on the Sketch Operations toolbar, or Edit→Edit
Curve. You cannot edit projected points.
When you choose Edit Curve and select a non-associated projected curve
string, the normal edit curve dialog displays.
Editing an associated projected curve string displays the Project options.

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Activity - Projecting Objects into a Sketch

You have a part that was translated from another system. It is
necessary to use the imported curves to create an extrude body.
You will: 2
• add the curves to a sketch.

• repair objects that are not suitable.

• create enough constraints to make the geometry usable with the

extrude function.

Step 1: Open iges_1 and if necessary choose Start→Modeling.

Step 2: Create sketch s21_profile on layer 21.

Change the Work Layer to 21.

Choose Sketch.

Click on the sketch name; key in s21_profile and press Enter.

Choose OK to accept the XC-YC plane.

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Step 3: Verify whether or not the existing curves lie on the sketch plane.
Imported curves should always be checked for being planar
and for gaps at “adjacent” end points.

2 Choose Analysis→Distance.

Alternately select the sketch datum plane and points on

various lines and arcs.

Do the curves lie on the sketch plane?

If the distance between any point on a curve and the
sketch plane is not zero, then that curve does not lie on
the sketch plane.

Step 4: Add the existing curves to the sketch.

Fit the view.

If necessary display the Sketch Operations toolbar.

If necessary, use Add or Remove buttons to display the Project

icon.

Choose Project.

If necessary, toggle Associative to inactive.

Associative sketch curves are constrained automatically by
the curves they were projected from. You will not be able
to alter their constraint condition from inside the sketch.
When you project curves associatively they are treated as
a single feature.
You will need to access the curves individually, so you do
not want associative projection.

Press the key combination Ctrl+A (Select All).

Choose OK to add the curves.

Step 5: Verify the types of curves that were created.

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If imported curves are not parallel with the sketch plane,

arcs may become conic curves.
It is also prudent to verify that imported curves that
appear to be lines or arcs are not in fact splines.
2
Move the cursor over the entire string of curves while observing
the status line.

What curve type is the curve shown below?

Step 6: Remove the conic curve.

Make layer 41 invisible.

Move the cursor over the highlighted curve shown below so

that it prehighlights, press and hold MB3 until the radial
popup icons appear, and slide to the left over the delete icon. .

Step 7: Create an arc to replace the conic.

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Choose Arc.
Make sure End Point is enabled on the Snap Point toolbar.
2
Indicate the two end points in the order shown.

For the third point, indicate any point that creates an inferred
tangency constraint at one end of the arc.

Click MB2 to exit from arc creation.

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Step 8: Analyze the curves.

Choose Analysis→Distance.

Select pairs of endpoints from several adjacent curves, any

place where there is not a coincident symbol. 2
Make sure that Point on Curve is inactive on the snap
point toolbar.
End Point is the only necessary option.

Notice that the curves are not contiguous. This is common when
geometry is translated into a double precision system, like NX,
from a single precision system. These values are fractions of a
millimeter in this case; however, trying to extrude these curves
into a solid body will fail because of gaps and overlaps.

Cancel from Analysis.

Display the Automatic Constraints Creation icon on the

Sketch Constraints toolbar, or use ToolsConstraints.

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Step 9: Close the gaps between the curves.

Choose Automatic Constraints Creation.

2 Choose the Clear button to clear all constraint types.

Choose the Coincident constraint to toggle it to active.

Change the Distance tolerance value to .25.

Choose OK to create the constraints.

NX interrogates each sketch point for other sketch points within

the Distance tolerance and combines the points to one.
Observe the display of coincident constraints that were added.

The profile will now extrude properly to create a solid body.

Choose Finish Sketch.

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Step 10: Extrude the sketch into a solid feature.

Orient the view to Trimetric. (HOME key.)

Move the cursor over any sketch curve until it pre highlights.
2
Hold MB3 until the radial pop-ups appear, and slide right to

choose Extrude.

NX treats sketches as collective strings of curves for swept features.

Enter an End distance of 200 mm.

Enter a Start distance of 50 mm.

Choose OK to create the body.

Fit the view.

The solid body is created.

Additional sketch constraints can now be added to capture
design intent. The body will update when you choose
Update Model or Finish.

Step 11: Optional challenge: You saw that the sketch does not have to be
fully constrained to be extruded.
Now, optionally, add all tangent constraints and any others needed
to fully constrain the sketch.

Step 12: Close the part.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 2-31
 Constraining Sketches

Activity - Auto Creating Constraints

You can use auto constraint creation to quickly create or recreate most
constraints in a reasonably accurate sketch.
2 In this part, you will pretend that there is an obscure problem with
constraints that someone else has created. Since the sketch is fairly
simple, you decide to remove all constraints and replace them with
new ones.
Auto Constraint Creation will save a lot of time and effort as you
complete your goal.

Step 1: Open the part.

Open pipevise and choose Start→Modeling.

Step 2: Activate the sketch.

Double-click on a sketch curve.

Step 3: Analyze the existing constraint set.

Ensure Show all Constraints is toggled to active.

Choose the Show/Remove Constraints icon.

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Ensure the radio button for All In Active Sketch is active.

Change the Show Constraints option to Both.

Notice the different types of Explicit and Inferred constraints
that exist in this part.

Step 4: Remove the constraints.

Select Remove Listed.

Choose OK.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 2-33
 Constraining Sketches

Step 5: Selectively Auto Create the constraints.

Choose Automatic Constraint Creation.

2 Choose the Clear button in the All Constraints area of the
dialog.

Toggle on the buttons for Horizontal, Vertical, Coincident, and

Tangent only.

Check or ensure that the Distance Tolerance is .001.

Choose OK to create the constraints.

Step 6: Manually create the rest of the constraints.

Choose Constraints.

Select the left-most vertical line.

Select the vertical datum axis.

Choose Collinear.

Select the bottom horizontal line.

Select the horizontal datum axis.

Choose Collinear.

Hold the Ctrl key down and select the two horizontal lines at
the top of the profile.

Choose Collinear and Equal Length.

If necessary, display the Deselect All icon on the

Selection toolbar.

Choose Deselect All .

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 Constraining Sketches

Hold the Ctrl key down and select the bottom end point of
the vertical line controlling the slot location and the bottom
horizontal line.

2
Choose Midpoint and Point on Curve.
The Status line should now inform you that the sketch is fully
constrained.

Click MB2 to exit the function.

Windows users may also use the ESC key.

Choose Finish.

The sketch is now fully constrained.

Step 7: Close the part.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 2-35
 Constraining Sketches

Add Existing Curves to a Sketch

If you initially decide not to control a swept feature with a sketch, or if you
2 obtain a wireframe part from a translator, you may create a sketch and
add the geometry to it at a later date. You do this by displaying and using
Add Existing Curves on the Sketch Constraints toolbar, or Insert→Existing
Curves.
An example could be that you have a general idea of what a cross sectional
profile looks like, but do not quite understand how form, fit, and function
of the part will drive the design intent. As the design matures and you
recognize the intent, you may then create a sketch and add already swept
curve geometry to it.
Curves that are added to a sketch have their layer reassigned to that of the
sketch.
The only constraints that will be applied to Existing Curves that are
added to a sketch are Inferred Coincidence, regardless of how the
curves were originally created.

Associative curves may not be directly added to sketches. The shape of

these curves are controlled by other means, such as the associative faces for
projected points or curves, or the law functions that control certain types
of splines and helices.

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Activity - Adding and Constraining Curves

Apply dimensions and constraints to control the following:

• The width of the slot (1). 2

• The total length of the slot (2).

Step 1: Open straightslot_1 and choose Start→Modeling.

Step 2: Create a sketch in layer 21.

Make 21 the Work Layer.

Choose Sketch.

Click on the sketch name; key in s21_slot and press Enter.

Select the front face (1) as the sketch plane.

Select the horizontal sketch axis (2) as shown above.

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Choose OK.

Step 3: Add the curves to the sketch.

2
Display the Add Existing Curves icon in the Sketch
Operations toolbar, or use InsertExisting Curves.

Choose Add Existing Curves.

Press the key combination Ctrl+A and then choose OK.

Step 4: List the constraints currently on the sketch.

Choose Show/Remove Constraints.

Ensure the radio button for All In Active Sketch is toggled on.
There are four inferred coincident constraints.
No explicit constraints exist in this sketch because the curves
were added to the sketch and not created with the sketch active.

Cancel the Show/Remove Constraints dialog.

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Step 5: Fully constrain the sketch according to the design intent.

Use dimensions to locate the left arc center 1 inch from the left
side of the part and 2 inches from the bottom of the part.

Add the following constraints:

Horizontal constraint to both lines
Tangent constraint to arcs and lines (4 places)
Remember Automatic Constraints.

Add the following dimensions:

Step 6: After constraining the sketch, edit the dimensions for the slot to
ensure that it updates properly. Use any reasonable values of your
choice.

Step 7: Close the part.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 2-39
 Constraining Sketches

Activity - Design Change

Change the design intent on the previous sketch: modify dimensions
and constraints so that one end may be made larger than the other
(1, 2).
2
The total length (3) still needs to be controlled. Examine the diagram
below and follow the steps to perform the design change.

Step 1: Open straightslot_2 and if necessary choose Start→Modeling.

Step 2: Double-click on any sketch curve to activate the sketch.

Step 3: Identify and delete constraints that do not meet the new design
intent, and add new constraints.

Select the Show/Remove Constraints icon.

Verify the radio button for All In Active Sketch is selected.

Delete the horizontal constraints.

Delete the slot width dimension and replace it with a radius

dimension on each arc.

The sketch is not fully constrained but it does meet the design
intent; one end may be made larger than the other.

Step 4: Edit the dimensions for the slot to ensure it updates properly.
Assign a value of .5 to the left radius dimension.

Assign a value of .25 to the right radius dimension.

Choose Finish Sketch and close the part.

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Activity - Another Design Change

Change the sketch design so that it may be oriented at various angles
(1) other than horizontal. The total length of the shape should still be
controlled.
2

Step 1: Open straightslot_3 and if necessary choose Start→Modeling.

Step 2: Double-click on any sketch curve to activate the sketch.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 2-41
 Constraining Sketches

Step 3: Create reference geometry.

Check your Snap Point settings to assure Arc Center is
active.
2 Create a line (1) from arc center to arc center.

Create another line (2) and apply Vertical (if necessary) and
Constant Length constraints.

Exit from constraint creation.

Step 4: Converting Curves to Reference Lines.

Select the two lines just created.

Hold MB3 over either one of the lines until the radial popup
options appear.

Slide to the right and down to choose Convert To/From

Reference.

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Step 5: Add or edit dimensions as shown below.

If a horizontal dimension for the slot length was inferred

or manually defined, delete it and replace with a parallel
dimension.

Step 6: After constraining the sketch, edit the dimensions for the slot to
ensure that it updates properly. Use any reasonable values of your
choice.

Step 7: Close the part.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 2-43
 Constraining Sketches

Activity - Constraining the Perimeter of a Sketch

The design intent for swimming pool requires that:
• The two larger radii are equal and must be controlled by a
2 dimension.

• The four corner radii are equal and must be controlled by a

dimension.

• The perimeter must be a constant value.

Step 1: Open the part file skt_perimeter and choose Start→Modeling.

Step 2: Activate the SWIMMING_POOL sketch.

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Step 3: Investigate the existing constraints using Show/Remove

Constraints.

Choose the Show/Remove Constraints icon.

2
If necessary, toggle on All in Active Sketch.

Verify the Constraint Type is set to All.

Verify the Show Constraints option is set to Explicit.

Choose the first constraint in the list, A5 Equal radius to A7.

Investigate the highlighted curves on the screen.

Select the Step Down the List button or use your down arrow
key and read through the constraints to get an idea of the
existing constraints in the sketch. Then Cancel the dialog.

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Step 4: Add the two dimensions shown.

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 Constraining Sketches

Step 5: Constrain the perimeter of the sketch.

Choose the Perimeter icon from the dimension pull-down

icon. 2
Select all of the active curves, a total of eight.

Choose the Sketch Dimensions Dialog icon.

Choose MB2 to create a perimeter dimension for the selected

curves.

Verify that a Perimeter dimension appears in the Dimensions

list. (It may be a different "p"-number.)

If you did not get all of the curves selected, highlight the
perimeter constraint in the Dimensions list and choose the
Delete button in the dialog.

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 Constraining Sketches

Step 6: Edit the perimeter.

Slide the slider bar to the left and right and observe the
changes in the sketch.

Edit the Perimeter and other dimensions by entering values

and/or using the slider bar.

Step 7: Close the part.

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Activity - Controlling Heat Transfer in a Cooling Pipe

The design intent for cooling fins on a length of pipe requires that the
cross sectional area of the fins should be controlled by the volume of
fluid in the pipe. Each fin’s perimeter should equal 1.25 times the
cross sectional flow area. 2
You will:
• Use a perimeter dimension to control the total perimeter.

• Equate the expression for the perimeter to 1.25 times the cross
sectional area of the pipe.

Step 1: Open the part file perim_1 and if necessary choose Start→Modeling.

This part contains the following features:

Cylinder

Thru Hole - The diameter of the thru hole controls the diameter of
the cylinder by maintaining a constant wall thickness.

Sketch

Using ToolsExpressions, examine the areaRatio

expression.

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 Constraining Sketches

Step 2: Interrogate the sketch.

Activate the FIN sketch.

2 Fit the view.

The sketch is located by two constraints. The reference curve and

datum plane (layer 61) are collinear (1) and the sketch arc and OD
of the cylinder feature are concentric (2).

The sketch is not yet totally constrained.

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Step 3: Add a perimeter dimension to the sketch.

Make layer 1 invisible.

2
Choose the Perimeter icon from the dimension pull-down
icon.

Choose the Sketch Dimensions Dialog icon.

Individually select the curves shown below.

Click MB2 to create the perimeter dimension.

Note that there is a new dimension called Perimeter_p## and that

the sketch is now fully constrained.

Choose Close.

You cannot edit the curves of a Perimeter constraint.

If you miss a curve or get an extra, delete the constraint
by highlighting it in the Dimensions list and choosing the
Delete button in the dialog.

Choose Finish.

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 Constraining Sketches

Step 4: Extrude the sketch.

Hold MB3 over a sketch curve until the radial pop up options
appear.

2
Slide to the right to choose Extrude.

The default extrude direction is normal to the plane of the sketch,

ZC+ in this case.

Double-click the direction vector arrow to reverse the extrusion

vector to the negative ZC direction.

Change the Boolean to Unite.

Notice that since there is only one body available as a

target, the system does not require you to select it.

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Use MB3 over the End symbol to change the option to Until
Extended.
You choose Until Extended so that the system knows the
face you will select must be extended beyond its current
boundary to trim the extruded sketch. 2

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 Constraining Sketches

Select the bottom planar face of the solid (1).

Choose OK.

Step 5: Create a circular array of the extruded fin.

Make layer 61 Selectable.

Choose Insert → Associative Copy → Instance.

Choose Circular Array.

Select the Extrude feature and choose OK.

Enter:
Number = 8
Angle = 360/8

Choose OK.

Choose Datum Axis.

Select the datum axis in the graphic window.

Choose Yes.

Choose Cancel.

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Make all but the work layer invisible.

Step 6: Capture the design intent for the fin.

Choose Tools→Expression.

If necessary choose More Options.

If necessary change the Listed Expressions option until ID is

listed.

Select the ID (SIMPLE_HOLE(1) Diameter) expression and

change it to 4 and Accept Edit.

Choose Apply.

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 Constraining Sketches

Fit the view.

Notice that the fins have retained their original profile. If

the cooling pipe’s volume is going to increase the cooling
fins will also need to increase.
Recall that an expression, areaRatio, relates each fin’s
profile to the cross sectional flow area.
This expression is associative to the hole feature and will
update automatically.
You need to link this value to the perimeter constraint.

Undo the last expression operation to return the heat

pipe to its original configuration.

Select the expression called Perimeter_p3 (FIN:SKETCH(5)

Perimeter Dimension) (the digit following the _p in your
expression may be different).

Change the Formula to areaRatio and Accept Edit.

While editing the ID expression highlight areaRatio in
the list. Use MB3  Copy Name to assure that the
spelling is correct, then type the rest of the expression.

Choose Apply.

The fins become slightly smaller.

In a real life situation you might tweak the formula until the ratio
exactly matches cooling requirements.
Select the ID expression, change it to 4, and Accept Edit.

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Choose OK.

Fit the view.

2

Notice how the fins have updated to meet the new flow
requirement.

Step 7: Close the part.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 2-57
 Constraining Sketches

Summary
Sketch constraints allow you to capture and maintain design intent even
after design changes occur. Through dimensions and constraints, you can
adapt your solid models to the design intent of the final product.
2
In this lesson you:
• Applied Design Intent.

• Created Geometric Constraints.

• Auto Created Constraints.

• Displayed Constraints.

• Converted Sketch Curves To Reference Curves.

• Updated a Model.

• Added Objects to a Sketch.

• Constrained a Sketch by its perimeter.

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Lesson

3 Constraint Management

Purpose 3
This lesson describes other constraint management tools as well as additional
ways to use sketches.

Objectives

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

• Create an Alternate Solution

• Reorder sketches

• Position Sketches on a Solid Body

• Locate a Sketch with Constraints

• Move a sketch using Reattach

• Mirror a sketch

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 3-1
 Constraint Management

Alternate Solution
Constraint sets may be valid in one or more configurations depending on the
given geometry. Scalar dimensions have no positive or negative sign, they
specify only an absolute value. This absolute value may be applied to specify
a given distance between objects in one direction or the other.
There are times when multiple solutions may be available for a given
constraint set. At these times there is a need to ask the system to change
3 the configuration based on the given set of constraints. NX provides this
functionality as an Alternate Solution.
Selecting the Alternate Solution icon from the Sketch Constraints toolbar will
bring up a small dialog containing the options OK, Back, or Cancel. The Cue
line prompts the user to "Select a dimension or circle/arc".

One alternate solution as it applies to a dimension would be the fairly simple

case illustrated below. Constraints for horizontal and vertical have been
applied to the appropriate lines, as well as collinearity between the two
horizontal segments as shown. The dimension is selected for an alternate
solution with the results as shown. The vertical dimension is valid in either
case when it is applied as an absolute value.

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 Constraint Management

A second form of alternate solution can be applied to a circle or an arc, for

example when two circles are constrained tangent to each other or a line is
constrained tangent to an arc. This is illustrated below. In the case of the
two circles, either solution is valid given the constraints supplied. Alternate
Solution may be used to switch between the two if some other constraint
causes the system to select the wrong configuration.

Two Tangent Circles

Select the large circle (1) first and the small circle (2) second.
3

Line Tangent to an Arc

Select the arc (1) first and the horizontal line (2) second.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 3-3
 Constraint Management

Activity - Alternate Solution

In this activity you will explore alternate solutions to constraint sets and the
effects that different constraints have as they are applied.
Step 1: Open alternate_1.

Step 2: View the constraints.

Choose Start→Modeling.

Double-click on a sketch curve.

If necessary toggle Show All Constraints to active and make

sure Dynamic Constraint Display is inactive.

Choose the Show/Remove Constraints icon.

Ensure the List Constraints for radio button is set to All In

Active Sketch.

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Change the Constraint Type to Tangent.

Select A1 Tangent to L6 to see the only tangent constraint in

the sketch.

Choose Cancel.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 3-5
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Step 3: Add dimensions.

Choose the Inferred Dimensions icon.

Select the bottom horizontal line and place a horizontal

dimension on the screen.

Select the circle and place a radius dimension on the screen.

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Step 4: Obtain an Alternate Solution.

Display the Alternate Solution icon
on the Sketch Constraints toolbar.
Optionally, you can use the ToolsConstraints
menu.

Choose the Alternate Solution icon.

The Cue line prompts you to "Select a dimension or circle/arc". 3
Select the circle and the center vertical line.

The circle flips to the other side of the line. This is a valid alternate
solution, the circle is still tangent to the line.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 3-7
 Constraint Management

Step 5: Obtain another Alternate Solution.

Select the circle and the center horizontal line.

3
Since there is no constraint associated to the two objects selected,
there is no alternate solution available. NX displays a message
stating that there is no valid alternate solution for the selected
objects.

Choose OK to dismiss the message.

Choose Cancel in the Alternate Solution dialog.

Step 6: Add a Tangency constraint.

Choose the Constraints icon.

Select the circle and the center horizontal line.

Apply a Tangent constraint.

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Step 7: Obtain an Alternate Solution.

Choose Alternate Solution.

Select the circle and the center horizontal line.

Here’s what happened. The center horizontal line has six

constraints associated to it:

Horizontal
Tangent to the arc
Left endpoint is located midpoint of the left vertical line.
Left endpoint is located on the left vertical line.
Right endpoint is located midpoint of the right vertical line.
Right endpoint is located on the right vertical line.

When the alternate solution is applied to the line and circle, the
top horizontal line collapses onto the bottom horizontal line. The
two vertical lines now have a theoretical length of 0 (zero), which
allows the middle horizontal line to meet its midpoint, point on
curve, and tangent constraints.

Choose Undo to restore the geometry.

Step 8: Add constraints to the center horizontal and vertical lines.

Choose the Constraints icon.

Select the left vertical line and the bottom horizontal line and

apply an Equal Length constraint to them.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 3-9
 Constraint Management

Step 9: Obtain an Alternate Solution.

Choose Alternate Solution.

Select the circle and the center horizontal line.

With the addition of the Equal Length constraint, the geometry

now updates in the desired manner.
3

Choose Finish Sketch.

Step 10: Close the part.

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 Constraint Management

Placing Sketches Where They Are Needed

Sketches require a placement plane, which can be a solid face or a datum
plane.
Sketches may be located in their plane by constraints with datum axes, datum
planes, objects belonging to other sketches, non-sketch curves, or solid edges.
Only features that are earlier in the Timestamp order (have a lower time
stamp number) may be selected to constrain a sketch.
Sketches may be located by one of two methods: 3
• Sketch constraints (dimensional and geometric)

• Positioning dimensions

These two methods are mutually exclusive.

If you use Positioning Dimensions, you cannot reference external
objects when creating Dimensions or Constraints.
If you reference external objects when creating Dimensions or
Constraints, then you cannot use Positioning Dimensions.

Positioning is supported by the sketcher primarily to permit sketches

to be used in User Defined Features.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 3-11
 Constraint Management

Activity - Creating and Positioning a Sketch

The function of this part requires a triangular pocket located relative
to an angled face. The sketch position should update automatically
if the angle of the face changes.

Step 1: Open fence_1.

Step 2: Choose Start→Modeling.

Step 3: Make layer 21 the Work Layer.

Step 4: Create a sketch of the pocket.

Choose Sketch.

Click on the sketch name, key in s21_pocket and press Enter.

Select the larger top face of the block as the sketch plane.

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 Constraint Management

Select the upper half of the angled edge of the pad as the
horizontal sketch axis.

You assure that the positive direction of XC will point away from
the “more pointed” end of the pad by selecting the edge at the end
shown below.

You can reverse the direction by double-clicking the head

of the x-axis vector.

Choose OK.

If your display does not look like the graphic below, start over
(choose FileCloseReopen Selected Parts).

Blend features are more intuitively edited as blends than

as sketch curves. You will define the shape of the pocket in
this sketch with only three lines, and add the corner radii
of the pocket later using blends.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 3-13
 Constraint Management

The sketcher is automatically in profile mode as you start a new

sketch.
Display the Create Inferred Constraints icon in the Sketch
Constraints toolbar. Alternatively, you may use the
ToolsConstraints menu.

Toggle Create Inferred Constraints to inactive. (off)

3 In the middle of the placement face, create the three lines as
shown below.

Length values are approximate.

Allow the first line to snap to horizontal.

Allow the second line to snap to vertical.

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Be sure to snap the third end point to the starting point of the
first line.

3
Step 5: List the current constraints.

Choose Show/Remove Constraints.

Ensure List Constraints for is set to All in Active Sketch,

Constraint Type is set to All, and Show Constraints is set to
Both.

There should be no constraints, because Create Inferred

Constraints was inactive when you created the lines.

Choose Cancel.

Step 6: Add geometric constraints.

Add coincident constraints only, using automatic constraints.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 3-15
 Constraint Management

Add a perpendicular constraint between the two lines shown.

Add a parallel constraint between the “horizontal” line and the

long edge of the pad, as shown.

Step 7: Add dimensional constraints.

By design, the size of the pocket should be controlled by
defining the lengths of the “horizontal” and “vertical” sides.

Choose Parallel.

Select the horizontal line and place the dimension.

Change the value to 6 and press Enter.

Select the vertical line and place the dimension.

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 Constraint Management

Change the value to 4 and press Enter.

Choose Finish Sketch.

Step 8: Extrude the sketch.

Hold down MB3 to open the radial pop up menu over any of
the sketch curves.

Slide right to choose Extrude.

Extrude the sketch to a depth of 1 inch and subtract it to create

a pocket.

Step 9: Add a .5 inch blend to the inside pocket corners.

Step 10: Constrain the sketch position.

Locate the sketch .75 inch away from the pad.

Double-click on a sketch curve.

Choose Fit.

Choose Perpendicular.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 3-17
 Constraint Management

Create the dimension from the horizontal sketch line to the

edge of the solid (1) shown below.

Locate the 90 degree corner of the pocket 1 inch from the

edge of the part shown below.

Select the edge at the edge of the part (1) as shown.

Select an end point at the 90° corner.

Use a cursor location to place the dimension.

Enter a value of 1 and press the Enter key.

The sketch automatically moves into position.

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Notice that all three sketch curves change to the fully constrained
color, and the status line reports that the sketch is fully
constrained.

Choose Finish Sketch .

Review the updated model.

Step 11: Verify the sketch positioning by editing the angle of the pad. 3
Choose Tools→Expression.

The pad has been positioned relative to the block. Its

angle may be changed by editing an expression named
fence_angle.

Change the value for fence_angle to –35, press Enter and

choose OK.

Note that the sketch remains parallel to the pad, .75 inch away,
and remains 1 inch from the back of the part.
In some cases if the edit to an edge used to position
the sketch is great enough, an Alternate Solution to a
dimension may occur. If either of the locating dimensions
flips, perform an Alternate Solution on the applicable
dimension to resolve the flip.

Step 12: Close the part.

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 Constraint Management

Activity - Positioning a Sketch

This structural frame requires pockets to minimize its weight.
You will control the thickness of the walls and the webs by adding
appropriate sketch constraints.
Drag and Alternate Solution will be useful tools as you work on the
sketch.

Step 1: Open frame_1.

Step 2: Constrain the sketch using both dimensions and constraints to

position the sketch curves relative to the solid edges and datum
planes.

Choose Start→Modeling.

Set the Rendering Style to Wireframe with Dim Edges.

Double-click on a sketch curve.

Choose Fit.

Choose Constraints.

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Select the three sketch arcs (1) and the solid edge (2) shown
below and apply a Concentric constraint.

Select the three sketch arcs and Apply an Equal Radius

constraint.

Choose Inferred Dimensions.

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Add a Radius constraint with a value of 2.25 to the arc (1)

shown below.

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When you use a dynamic input window end each value

entry with the enter key.
For example, in the next step, use enter to complete the
dimension value 0.2, and then activate the name field and
select all of the existing text.
Next, type the name wall and again use enter to complete
the edit.

Create the wall dimension as shown below. Remember to name 3

the expression wall.

If the sketch line is lying off the solid face instead of over
the face, use Alternate Solution to flip the wall dimension.

Choose Constraints.

When you apply constraints between datum features

and sketch curves the constraints have to be applied
individually.
In the next example, select one line and one datum plane
and apply a parallel constraint. Repeat for the rest of the
lines.

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 Constraint Management

Apply Parallel constraints to the objects as shown below.

You may avoid needing to use Alternate Solution later:

drag these curves to their proper relationships after
applying geometric constraints and before dimensioning.

Apply the dimensions as shown below.

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When you key in the first letter of wall you will have
the option of choosing from a list of all functions and
expressions. Since no function names or other variables
start with “w” there will be only the one list entry to select.
Click on your selection in the list, or use the arrow keys
and enter to make a selection.
When the value appears in the dynamic input window,
use enter twice: one time to place the value in the input
window and again to record the value and update the 3
sketch.

Apply the remaining dimensions as shown below.

The sketch is now fully constrained and positioned on the solid

body.

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Step 3: Extrude the sketch and subtract it from the solid to create the
pockets. Use a Start distance of 0 and an End distance of 0.56.

Step 4: Edit the chamfer feature.

Choose Edit→Feature→Edit Parameters.

Select the Chamfer feature and choose OK.

Change the First Offset value to 1.5.

Tab to the Second Offset and change it to 2.0.

Choose OK twice.

Examine the part to ensure the update was correctly applied.

Look to see if any Alternate Solutions need to be applied to the
dimensions from the datum planes.

Step 5: Optional: Add blends to the solid edges.

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For the first set of the first blend, specify 0.125 on the vertical
edges of the pockets.

For the second set of the first blend, specify 0.325 on the outer
vertical edges of the solid.

For the second blend, using selection intent Tangent Curves,

specify 0.0625 on the floors of the pockets.

Step 6: Close the part.

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Activity - Using Positioning Dimensions

The design requirements for this part will eventually require the
sketch to be used as a user defined feature or UDF. When you use a
sketch in a UDF, it is convenient to use positioning as an intuitive
tool for placing and aligning the feature.
First you will fully constrain the sketch using constraints. Next
you will replace constraints that are specific to this solid body with
flexible positioning dimensions.
3
Step 1: Open position_1.

Step 2: Choose Start→Modeling.

Step 3: Use dimensional constraints to locate the sketch on the placement

plane.

Double-click on a sketch curve.

Choose Fit.

Choose Show All Constraints.

Notice that there are two vertical, one horizontal and two
tangent constraints.

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Choose Inferred Dimensions.

Select the arc center and the bottom horizontal edge of the
solid body.

Place a vertical dimension to the right of the part.

Change the value to 3 and press Enter.

Notice that the status line indicates that 1 constraint is needed.

Also notice that the vertical DOFs no longer appear.

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Select the arc center again and the right vertical edge of the
solid body.

Place a horizontal dimension above the part.

Change the value to 2 and press Enter.

The sketch is now fully constrained

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Step 4: Test the sketch to see if more flexible positioning can be added
with the current constraints.
In some instances the sketch needs to be rotated 20
degrees as shown below.

Choose the Angular dimension type.

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Select the objects in the order and at the locations as shown

below.

Place the dimension to the right of the part.

Notice how the dimension and horizontal constraint are displayed

in the over constrained color.
Also notice that the status line indicates that the sketch is over
constrained.
The angular dimension and horizontal constraint are presently
redundant (over constrained).
If you were to change the angular dimension value, the dimension
would then be in conflict with the horizontal and both vertical
constraints.

Choose Undo.

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Step 5: Prepare to create positioning dimensions.

Add Positioning Dimensions on the Sketcher
toolbar. (Actually, there is a stack of three icons.)
Alternatively you could use ToolsPositioning
Dimensions.

Choose Create Positioning Dimensions.

An error window pops-up informing you that you cannot apply

3
positioning dimensions when there are sketch constraints to
external objects. This message is referring to the dimensions going
to the solid body.

Choose OK.

You will now remove the dimensional constraints to the

solid body and replace them with Positioning Dimensions.
In a future UDF, users who create instances of your sketch
would apply similar positioning dimensions to meet their
design intent.

Select the two dimensions that position the sketch to the solid
body.

Choose Delete.

Choose Constraints.

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Choose the endpoint (1) shown below and apply a Fixed

constraint.

Notice that the sketch curves change to the fully constrained color,
and all degree of freedom indicators are removed.
The sketch is now fully constrained with no external references.
When you use positioning it will apply to the entire sketch.

Step 6: Use a Positioning Dimension to define the distance from the arc
center to the lower edge of the solid body.

Choose Create Positioning Dimensions.

Choose Perpendicular.

Select the bottom horizontal edge of the solid body.

Select the arc and choose Arc Center.

Choose OK to accept the value of 3.

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Step 7: Create a Positioning Dimension to define the distance from the arc
center to the right hand edge of the solid body.

Choose Perpendicular.

Select the right vertical edge of the solid body.

Select the arc and choose Arc Center.

Choose OK to accept the value of 2. 3

Step 8: Create a Positioning Dimension to define the angle of the sketch
with respect to the lower edge of the solid body.

Choose Angular.

Select the objects in the order and at the locations as shown

below.

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Key in 20 and choose OK.

Notice how the sketch rotated even though there are vertical
and horizontal constraints present. This is because positioning
dimensions operate on the entire sketch as a feature.

Choose Orient View to Sketch.

3 Choose Fit.

Now you can see that the sketch was rotated and that the vertical
and horizontal constraints are still valid relative to the sketch
plane.

Step 9: Edit the angle positioning dimension.

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Choose Edit Positioning Dimensions from the pull-down.

In the graphic window, select the angle positioning dimension.

Key in a value of 45 and choose OK twice.

Choose Orient View to Sketch.

Fit the view.

Choose Finish Sketch.

Step 10: Close the part.

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Reattach
You can reattach a sketch to a different planar face or datum plane than the
one on which it was created. You can only reattach to a plane or face with
an earlier time stamp.
The Reattach option also displays any for the sketch, and lets you redefine
the geometry referenced by them.
After you choose the Reattach icon, the reattach input boxes display.
3

Sketch in place

These options are from left to right:

• Sketch type – Lets you change between Sketch in place and Sketch on
path.

• Sketch Plane – Lets you choose a new sketch plane or planar face.

• OK – Lets you execute the reattachment.

• Cancel – Quits the reattachment operation.

To reattach a Sketch in place:

1. Select a new datum plane or planar surface (optional).

2. Select a horizontal or vertical reference (optional).

3. Choose OK.

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Sketch on path

These options are from left to right:

• Sketch type – Lets you change between Sketch in place and Sketch on
path.
3
• Path – Lets you choose a new path or edit the existing one.

• Positioning Method – Lets you change the positioning method.

• Alternate Solution – This will be available when there are multiple

positioning possibilities.

• OK – Lets you execute the reattachment.

• Cancel – Quits the reattachment operation.

To reattach a Sketch on path:

1. Select a new path or modify the existing path (optional).

2. Modify the sketch plane orientation: Normal to Path, Normal to Vector,

Parallel to Vector, or Through Axis (optional).

3. Modify the placement of the sketch by dragging or choose among:

ArcLength, % ArcLength, or Through Point (optional).

4. Choose OK.

To redefine a positioning dimension:

1. Select a displayed positioning dimension to redefine. The original dialog
used to define the positioning dimension displays.

2. Follow the prompts to choose new reference objects for the positioning
dimension.

For information on positioning methods see the Modeling Online Help.

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Reordering Sketches
In order to attach a sketch to a face or datum or define a horizontal reference,
the geometry must come before the sketch in Timestamp order. Reordering
accomplishes this.
Reordering is also necessary when you attempt to add generating or guide
curves of a swept feature that occurs before the sketch. The sketch must
be reordered before (earlier than) the swept feature that is generated or
guided by the curves. Once the timing of the sketch relative to the swept
3 feature is resolved, and the curves are added to the sketch, the curves may be
constrained just as any other sketch curve.
Sketches appear in the Part Navigator and the list of features presented
when performing an Reorder. A sketch can be located anywhere after its
reference geometry in the creation order.

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Activity - Reattaching a Sketch

Step 1: Open reattach_1.
In this activity you will reattach a sketch that defines two
cam blocks (1). The design has changed so that the blocks
must be mounted on the opposite face, as shown below.

Step 2: Investigate the current placement face and horizontal reference

of the sketch.

Choose Start→Modeling.

Change the Rendering Style to Wireframe with Dim Edges.

Make the sketch layer 22 and datum layer 62 selectable.

Use the push pin icon to lock the Part Navigator in the

open position.

Make sure the Part Navigator is in the Design View; i.e.,

Timestamp Order does not have a check beside it.

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Expand the nodes Solid Body, Unite (13), Solid Body, Extruded
(11), Direction, and Sketch (9) until the Horizontal Reference
and Placement Face of Sketch (9) “INSERT_RELIEF” are
displayed, as shown below.

One at a time, select Datum_Plane(2) and the Face node

under Placement face, noting which entities highlight in the
graphics window.

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Double-click the sketch icon beside Sketch (9)

“INSERT_RELIEF” to activate the sketch.

Unpin the Part Navigator to expand the graphics viewing area. 3

Step 3: Reattach the sketch.
Display Orient View to Model on the Sketcher toolbar, or
use the View menu.

Choose Orient View to Model.

Choose Reattach.

Select the face shown below.

Click on the Y axis of the coordinate system.

Select the datum plane to define the vertical direction.

Choose OK.

Choose Finish Sketch.

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Shade the model and review the part.

The sketch is now reattached to the defined face and the cam block
features are rebuilt.

Step 4: Close the part.

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Activity - Moving Sketches

The part for this activity contains two dimensional geometry for a switch
base. The data may have originated from another system.
You will selectively eliminate some of the geometry and constrain
the remainder in sketches so that parametric control over the model
may be defined by the geometry.
You will initially create the sketches on the same plane. Later you
will move two of the sketches into the proper orthogonal planes and
extrude them to define a solid model.
3

Step 1: Open switchbase_1.

Step 2: Move the curves required for each profile sketch to separate layers.

Choose Start→Modeling.

Choose Format→Move to Layer.

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Select only the two circles in the "top" view and choose OK.

3
Key in 21 and choose Apply.

Choose Select New Objects and move the lines shown below in
the "front" view to layer 22.

Move the curves shown below in the "right" view to layer 23.

Step 3: Create expressions for the diameter and height.

Choose Tools→Expression.

Create expressions:

Name Formula Dimensionality Units

dia 3.75 Length Inches
h 5.75 Length Inches

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Step 4: Create a sketch for the top profile.

Change the work layer to layer 21 and make all other layers
invisible.

Create a sketch named S21_TOP on the XC-YC plane.

Choose Fit.

Add the two circles to the sketch.

3
Step 5: Constrain the sketch for the top profile.
Add constraints to position the sketch so that both circle
centers are aligned with the two datum axes.

Add a dimension for the outer diameter. Change the value of

this expression to dia to associate it to the expression.

Choose Finish.

Choose Fit.

Step 6: Move the datum plane and two datum axes to layer 61.
They are no longer required for this sketch but will be referenced
by the other sketches.

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Step 7: Create an extruded feature using the top profile.

Change the work layer to layer 1 and keep layer 21 selectable.

Change to a Trimetric view orientation. (HOME key.)

Extrude the sketch S21_TOP in the default (+ZC) direction

using an End distance of h and a Start distance of 0.

Step 8: Create a sketch for the front profile.

Change the work layer to layer 22. Make layer 61 selectable

and all other layers invisible.

Choose Fit.

Create a sketch named S22_FRONT. Select the existing datum

plane as the sketch plane and select the datum axis parallel to
the XC axis as the horizontal sketch axis.

Choose Fit.

Add all of the curves on layer 22 to the sketch.

Step 9: Constrain the front profile sketch.

In Sketch→Preferences make sure Dynamic Constraint

Display is inactive (off) so you can see all of the constraints.

Use the Automatic Constraints to create horizontal and

vertical constraints.

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Add dimensions for the total height and width as shown below.
The numeric suffixes you see may differ from the
illustration.

Test the behavior of the sketch by changing the height

constraint to 7.0 and the width to 5.0.

Notice that the sketch does not satisfy the design intent and
remain symmetrical when the expressions are changed. To satisfy
the design intent you can add a reference line and additional
constraints.

Choose Undo (twice if necessary) to change the

dimensions back to their original values.

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Create a vertical line between the midpoints of the two

horizontal lines shown below and convert it to reference. After
you create the line verify the inferred constraints and Undo to
try again if necessary.

You may need to enable Mid Point in the Snap Point

toolbar so that the system can infer the correct constraints.

3 Remember that you can add multiple constraints to

selected curves if you hold the Control (Ctrl) key as you
select the curves.

Add the new dimension as shown below and make the two
pairs of lines (1) and (2) both Collinear and Equal Length.

Change the value of the expression for the total width to dia
and the total height to h.

Choose Finish.

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Step 10: Create associative reference features to be used as attachment

faces for the front and right profile sketches, and as location aids.
Change the work layer to layer 62. Make sure layers 1 and 61
are selectable to display the solid and the other datum objects.

Choose Datum Plane and create a datum plane through

the axis of the outer cylindrical face of the solid.

Create another datum plane through the axis of the cylindrical

3
face and at a 90 degree angle to the plane you just created.

Choose Datum Axis and create a datum axis through the

axis of the cylindrical face of the model pointing in the ZC+
direction.

The front profile sketch will be attached to the datum plane that
is parallel to the ZC-XC plane. However, the plane was created
after the sketch and cannot be referenced as a target face unless it
precedes the sketch.

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Step 11: Reorder the sketch after the datum planes.

Choose the Part Navigator icon.

In the Part Navigator, place the cursor on the

S22_FRONT:SKETCH node. The sketch will appear under
Unused Items in the Design View.

Press the right mouse button to display the pop-up menu, slide
3 the cursor down to the Reorder After option, and select the last
datum axis from the cascading menu.

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Step 12: Attach the front profile sketch to a datum plane.

Make layer 22 selectable to display the sketch.

Double-click on a sketch curve.

Enable Orient View to Model on the Sketcher toolbar.

Choose Orient View to Model. 3

Choose Reattach.

Select the datum plane that lies in the ZC-XC plane as the
sketch plane.

Notice the Datum Axis used for the horizontal sketch axis is still
valid. It is not necessary to redefine all steps during the reattach
operation.

Choose OK.

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Step 13: Position the sketch.

Choose Fit.

Add a constraint to make the centerline of the sketch Collinear

with the datum axis through the cylindrical face axis (1).

Add another constraint to make the lower horizontal line in

the sketch Collinear with the datum axis that is parallel to
3 the XC-axis (2).

Choose Finish Sketch.

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Step 14: Extrude the front profile sketch.

Extrude the sketch S22_FRONT along the default direction
(YC axis) using Start and End values Through All and choose
the Boolean option Intersect.

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Step 15: Create the sketch for the right profile.

Change the work layer to layer 23, make layer 61 selectable,
and all other layers invisible.

Create a sketch named S23_RIGHT. Once again, define the

sketch plane with the datum plane defined for the S21_TOP
sketch and select the datum axis parallel to the XC axis as the
horizontal sketch axis.

3
Choose Fit.

Add all the curves to the sketch.

Step 16: Constrain the right profile sketch.

Choose Automatic Constraints.

Set the Distance value to .01.

Toggle on: Horizontal, Vertical, Coincident, Parallel, Tangent,

and Equal Length.

Choose OK.

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Create two vertical reference lines between the midpoints of

the horizontal lines as shown below.

Add the dimensions as shown above.

The numeric suffixes you see may differ from the
illustration.

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 Constraint Management

Change the value of the expression for the width to "dia" (1)
and the value of the expression for the height to "h" (2) to
associate them to the other sketches.

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Step 17: Attach the right profile sketch to the other new datum plane.
Make layers 1 and 62 selectable.

Choose Orient View to Model.

Choose Fit.
3
Choose Reattach.

Select the datum plane that lies parallel to the four flat faces
of the model.

Choose OK.

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Step 18: Add constraints to position the sketch.

Choose Orient View to Model.

Choose Fit.

Add a constraint to make the centerline of the sketch collinear

3 with the datum axis through the cylindrical face axis (1).

Add another constraint to make the lower horizontal line in

the sketch collinear with the datum axis that is parallel to the
XC axis (2).

Choose Finish Sketch.

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Step 19: Extrude the right profile sketch.

Change the work layer to layer 1.

Choose Fit.

Extrude the sketch S23_RIGHT along the default direction

(XC axis) using a Start and End distances of Through All and
choose the Intersect Boolean option.
3
Make all layers invisible.

Note that the work layer is never affected when you

select the layer category All and then choose Invisible.

Step 20: Edit the expressions to modify the part.

Choose Tools→Expression.

If necessary choose More Options.

Set Listed Expressions to User Defined.

Change the value of the expression dia to 4.25 and the value
of the h to 6.5.

Choose OK to update the model.

Step 21: Close the part.

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 Constraint Management

Mirroring in a Sketch
The sketch mirror functionality provides a means for copying geometry and
constraints within the context of a sketch whenever the sketch design intent
is meant to be symmetrical. The mirror function may provide a time saving
option.
To mirror sketch curves:

3 • Choose Mirror.

• Select the mirror centerline.

• Select the curves to be mirrored.

• Choose OK or Apply.

The mirror centerline you select will be automatically converted to

reference status if it is not already a reference line.

A Mirror constraint is created between each new curve created

through the Mirroring process and the original curve.

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Activity - Mirroring Sketch Objects

Step 1: Open mirror_1 and if necessary choose Start→Modeling.

This part file contains a sketch and an extruded solid body

that represent half of a V-Block. You will mirror the sketch
and update the model.

Step 2: Activate the sketch.

Double click on a sketch curve.

The status line indicates that the sketch is fully constrained.

Step 3: Mirror the sketch curves.

Choose Mirror.

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 Constraint Management

Select the vertical line (1) as the mirror centerline.

Click MB2 to advance the selection step to Mirror Geometry.

Press the key combination Ctrl+A to select the remaining

sketch geometry.

Choose OK.

Step 4: Edit the angle of the V-block.

Double-click on the p2=60.000 dimension.

In the dynamic input box key in 50 and press Enter.

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Notice that both sides of the sketch updated.

Choose Finish Sketch.

In the part navigator (Design View) verify that there is still only
one solid body.
After the mirror centerline was converted to reference status the
remaining curves and their mirror images created a single closed
loop. 3
Step 5: Close the part.

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Summary
Sketches can be reconfigured by using an alternate solution when more than
one configuration applies to a given set of constraints.
Sketches also can be dragged to other locations or in relation to their own
members. Managing sketches will allow you more flexibility when you create
your designs.
Positioning sketches using dimensions or constraints or a combination of both
can help you maintain design intent when related features change.
3
Reattaching a sketch to another sketch plane offers you greater flexibility
in your final configuration.
In this lesson you:
• Applied Alternate Solutions to obtain the appropriate profile.

• Located sketches using constraints.

• Located sketches using positioning dimensions.

• Reattached sketches.

• Reordered sketches.

• Mirrored sketches.

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Lesson

4 Sketch on Path Overview

Purpose
This lesson provides an introduction to the Sketch on Path option available
within the Variational Sweep operator.
For more detailed information, use the following NX help
documentation Design ModelingCreating Objects From the Insert
MenuSweepVariational Sweep.
4
Objectives
Upon completion of this lesson, you will be able to:
• Understand When this Option is Available

• Understand the Sketch on Path Geometry Elements

Sketch on Path
Sketch on Path provides a single definition process that allows you to create a
datum plane perpendicular to a string of curves or edges and a sketch with
origin and orientation related to both the path and the datum.
• Sketch on Path makes it easy to create input for the Variational Sweep
or V-Sweep command

• Sketch on Path captures the master section

• Guide curves such as curves or edges can be captured by the sketch using
Intersect

• Choose from several orientation functions to control the sketch plane

relative to the path:
– Normal to Path

– Normal to Vector

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 4-1
 Sketch on Path Overview

– Parallel to Vector

– Through Axis

• The datum axes are automatically calculated by face properties adjacent

to the path

• Easily move the sketch plane along the path using the Reattach function

• Reattach a template Sketch in place to make it into a Sketch on path

• The location of the sketch on its path is defined by a pair of expressions,

one for arclength and one for the percentage.

• If used in dimensions of the sketch on path, these arclength and

4 percentage expressions will update the sketch dimensions according to
the current position of the sketch
– The arclength and percentage expressions can be used to define design
intent in a v-sweep

– V-sweep generates the full range of values of the arclength and

percentage expressions corresponding to all positions of the section
along the path

– The percentage expression divided by 100 is a fraction between 0 and

1; thus pn/100 (where pn is the name of the percentage expression)
can be used identically to the controlling parameter in law curves

4-2 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Sketch on Path Overview

Summary
The Sketch on Path option provides you with the ability to create associative
Guide Curves and Section Strings within the Variational Sweep operator.
When the feature is completed editing is assessable through familiar NX
Sketch tools such as expressions, reattach and relative datum features.
In this lesson you:

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 4-3
4
Lesson

5 Additional Sketching Techniques

Purpose

This lesson describes additional techniques that may be used to manipulate

sketches.

Objectives

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

• Edit a Defining String

• Suppress and Delete Sketches 5

• Animate Sketch Dimensions

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-1
 Additional Sketching Techniques

Edit Defining String

Overview
Sketches may be used to define profiles for extruded, revolved, or swept
features and paths for swept features. Profiles are called Section Strings and
the paths are called Guide Strings.
Sketch objects that define another feature of the solid model cannot simply be
deleted due to the parent/child dependency relationship.
Edit Defining String is accessed by displaying the icon in the Sketch
Operations toolbar or via Edit→Edit Defining String in the sketch
environment.
This option allows objects to be added to or removed from a string of objects
defining a Section String or Guide String that has been used to create a solid
feature.
When the Edit String dialog displays, the system shows a list of features
5 associated with the active sketch. By default, the top feature in the list is
highlighted in the dialog and the sketch objects associated with the feature
are highlighted in the graphics area.

To add objects to the defining string, simply select them.

To remove objects from the defining string, hold down the Shift key while
selecting them.

5-2 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Additional Sketching Techniques

An option menu is provided to allow filtering of selectable objects. Options

are provided for All (the default), Curve, Edge, Face, and Sketch.
The radio buttons at the top of the dialog, Section and Guide, are for instances
where sketches are used both as a section string for one feature and as a
guide string for another feature. In these cases the system provides for
editing of defining strings of the non-active sketch because of the associativity
of the sweep along guide feature.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-3
 Additional Sketching Techniques

Deleting or Suppressing Sketches

Overview

Since sketches are features of the model, they may be deleted or suppressed
by choosing Edit→Delete or Edit→Feature→Suppress.

Sketches may also be deleted or suppressed from the Part Navigator.

5-4 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Additional Sketching Techniques

Activity - Edit Defining String

In this activity you will modify the profile of a part that already exists by
changing the curves that define the profile.

Step 1: Open bbqcover_1.

5
Step 2: Activate the sketch defining the profile.

Choose Start→Modeling.

Choose Edit→Sketch.

Since S21_CROSSSECTION is the only sketch available, it is

automatically opened for editing.

Step 3: Change the profile defining the part.

Make layer 1 Invisible.

Choose Studio Spline on the Sketch Curve toolbar.

Use the Through Points method.

Verify that the degree is 3.

Make sure that End Point is active on the snap point toolbar.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-5
 Additional Sketching Techniques

Start with the upper left endpoint on the sketch as shown.

Follow with points 2, 3, and 4 as cursor locations. Finish with
the upper right endpoint as shown.
3
2 4

1 5

Choose OK to signal the end of point specification.

5
Choose Constraints.

Select the left angled line and the left endpoint of the spline
as shown below. Make sure the spline is highlighted when
selecting the left endpoint.

Apply a Slope of Curve constraint to these objects.

Repeat the previous action for the right angled line and the
right endpoint of the spline.

5-6 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Additional Sketching Techniques

Step 4: Add six new dimensional constraints to the spline points as shown
below.
Your numeric suffixes may differ. Be careful to preserve
the relationships illustrated.

Step 5: Edit the defining string for the model.

Display the Edit Defining String icon in the Sketch
Operations toolbar.

Choose the Edit Defining String icon.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-7
 Additional Sketching Techniques

In the dialog the Section string for EXTRUDED(4) is the only

choice available.

With the Edit String dialog still displayed, select the spline
to add it to the string.

Hold down the Shift key and select the top horizontal sketch
line to remove it from the string.

Choose OK.

5-8 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Additional Sketching Techniques

Step 6: Convert the extraneous line to a reference line.

This line is still needed because the spline is dimensioned to it.
Hold down MB3 over the line until the radial pop up options
appear.

Slide down and to the right to chooseConvert To/From

Reference.

Choose Finish Sketch.

Examine the new and improved barbecue cover.

Step 7: Close the part.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-9
 Additional Sketching Techniques

Activity - Suppressing and Deleting Sketches

In this activity you will suppress and delete a sketch and observe the effects
on features that depend on it.
Step 1: Open delete_1.

Step 2: Suppress a sketch.

Choose Start→Modeling.
5
Choose Edit→Feature→Suppress.

Choose the sketch named S21_CAM from the Feature Selection

dialog.
The dependents of the sketch are also selected. This includes
all of the features except the datum plane and axes used to
define the sketch plane.

Choose OK, and observe the effect on the model.

Step 3: Unsuppress the sketch.

Choose Edit→Feature→Unsuppress.

Choose all of the suppressed features from the Feature

Selection dialog (Choose the top feature in the list and drag
with MB1 to the bottom of the list).

Choose OK and again observe as the model updates.

Step 4: Delete a sketch.

Pin the Part Navigator in the open position.

5-10 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Additional Sketching Techniques

Make sure that you are in the Design View, with Timestamp
Order inactive.

Expand the Dependencies window.

Expand the node for the bottom feature in the hierarchy,

Extruded(4).

Note that the arcs and lines that make up the extruded section are
all named, and all nodes can be further expanded.

Make sure the Extruded(4) node is selected, so that Details

are visible.

If necessary, expand the Details window

In the Dependencies window, note that both the Children and

Parents nodes can be expanded.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-11
 Additional Sketching Techniques

If necessary, expand the Parents node in the Dependencies

window.

Examine the parent-child relationships of the feature.

Expand any one of the nodes for lines or arcs under Extruded(4).

Note that Sketch(3) “S21_CAM” is the parent of the root feature

of the solid body, Extruded(4). Note that the only parents of the
sketch are the datums used to position it.
Place the cursor over either of the Sketch(3) nodes, then click
MB3 and choose Delete.

A Notification window pops up informing you that deleting this

feature will affect other features.

Choose Information

The Information window lists the other features that will also be
deleted, every feature except the datums.
Close the Information window

Choose OK in the Notification window.

Note that all dependents of the sketch are also deleted.

There is nothing under the Model Node.
The datums now appear under the Unused Items node.

5-12 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Additional Sketching Techniques

Step 5: Close the part.

Step 6: Examine the customer defaults that affect the behavior of the
system as you delete features.
Choose File→Utilities→Customer Defaults.

Choose Modeling→General, and click the Delete and Suppress

tab.

On the Delete and Suppress page hover the cursor over

the question mark icon for each option to examine a brief

explanation of what the option does.

Cancel the dialog without saving any changes.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-13
 Additional Sketching Techniques

Animate
The Animate function dynamically displays the effect of varying a given
dimension over a specified range. Any geometry affected by the selected
dimension is also animated. The behavior of the animation is relative to the
existing dimensions and constraints.
Access Animate by displaying the Animate Dimension icon in the Sketch
Constraints toolbar, or via Tools→Constraints in the sketch environment.

Dimensions list box: Lists the dimensions that can be animated.

Value: The value of the currently selected dimension.
Lower Limit: The smallest value that the dimension will be during the
animation. The default limit is the selected dimension value minus 10%.
Upper Limit: The largest value that the dimension will be during the
animation. The default limit is the selected dimension value plus 10%.
Steps/Cycle: The number of times that the dimension value changes when it
moves from the upper limit to the lower limit (or vice versa).
Display Dimensions: Optional: lets you display the original sketch
dimensions during the animation.

5-14 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Additional Sketching Techniques

Activity - Animating Sketch Dimensions

Step 1: Open animate_1.

Step 2: Animate the first sketch.

Choose Start→Modeling.

Double-click on a sketch curve.

Toggle Show All Constraints to enabled.

The constraints that presently exist in this sketch are:

Lines are either horizontal or vertical.

Lines are equal length to each other.

Arcs are equal radius to each other.

Lines and adjacent arcs are tangent.

Display Animate Dimension in the Sketch Constraints

toolbar.

Choose Animate Dimension.

Pan the sketch so that none of the geometry is hidden behind

the dialog.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-15
 Additional Sketching Techniques

Select the p5=1 dimension.

Type the following values:

• Lower Limit = 0.25
• Upper Limit = 2.75
• Steps/Cycle = 20

Choose Apply.

The sketch animates the radius dimension within the animate

limits and the present constraints of the sketch.

Choose Stop.

Change the Steps/Cycle value to 40 and choose OK.

Changing the number of steps per cycle slows down the

animation.
Remember to start relatively fast (low step count) and
5 increase step count only within the ability of your computer
to meet your needs.

Choose Stop

Choose Finish.

Step 3: Animate the second Sketch.

Change the work layer to 22 and make layer 21 Invisible.

Double-click on a sketch curve.

The constraints in the sketch consist of a fixed horizontal line and

4 angular dimensions that are associative to each other.

5-16 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Additional Sketching Techniques

Choose Animate Dimension.

Select the p0=43.2 dimension.

Choose OK to use the default values.

If you are using a space ball, you may zoom and pan
during the animation so that you can see the entire range
of motion.

Choose Stop

Edit the p2 dimension formula to read p1*9 .

Use the sketch dimension dialog or the formula editor.

Choose Animate Dimension.

5
Select the p0=43.2 dimension.

Set the Steps/Cycle back to the default value, 20.

Choose OK to accept the remaining defaults.

The animation now dynamically reflects the new dimensional

value.

Choose Stop

Choose Finish.

Step 4: Animate the third Sketch. (Optional)

Change the work layer to 23 and make layer 22 Invisible.

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-17
 Additional Sketching Techniques

Double-click on a sketch curve.

Review the sketch constraints. Notice the reference line with

the constant length constraint.
5
Choose Animate Dimension.

Select the p9=3 dimension.

Choose OK to accept the defaults.

Choose Stop when you are done viewing the animation.

Choose Finish.

Step 5: Close the part.

5-18 Sketcher Fundamentals – Student Guide ©UGS Corp., All Rights Reserved mt10028_g NX 4
 Additional Sketching Techniques

©UGS Corp., All Rights Reserved Sketcher Fundamentals – Student Guide 5-19
Summary
Index
A
Alignment Lines ...................................1-22
Animate Sketch Dimension .................5-14

D
Delay Evaluation ..................................1-57
Delete Sketch ......................................... 5-4
DOF .......................................................1-46

E
Edit Defining String .............................. 5-2
Evaluate Sketch ...................................1-57

I
Infer Constraint Settings .....................1-21

Q
Quick Extend ........................................1-36
Quick Trim............................................1-34

S
Show/Remove Constraints ...................1-66
Sketch
Add Existing Curves .........................2-36
Alternate Solution ............................. 3-2
Automatic Constraint Creation ........2-22
Constraining .....................................1-48
 Constraints........................................1-63
Convert To/From Reference ............. 1-92
Create Inferred Constraints .............. 2-5
Creating . . . . . . . . . . . . . . . . 1-8, 1-13
Curve Creation ................................. 1-21
Arc .............................................. 1-26
Circle .......................................... 1-27
Fillets ......................................... 1-33
Line ............................................ 1-24
Profile ......................................... 1-23
Dimensions ....................................... 1-48
Editing ....................................... 1-57
Types .......................................... 1-51
Drag .................................................... 2-2
Mirror ................................................ 3-62
Naming ............................................. 1-11
Overview ............................................. 1-2
Positioning ........................................ 3-11
Project ............................................... 2-23
Reference Direction .......................... 1-10
Reordering ........................................ 3-40
Show/Remove Constraints ............... 1-66
Text Height ....................................... 1-51
Sketch on Path ....................................... 4-1
Sketch Points ....................................... 1-46
Snap Angle ........................................... 1-22
Suppress Sketch ..................................... 5-4

U
Update Model ....................................... 1-57
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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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BlankBlank... Ctrl+B
EditBlankReverse Blank All Ctrl+Shift+B
EditBlankUnblank Selected... Ctrl+Shift+K
EditBlankUnblank All of Part Ctrl+Shift+U
EditTransform... Ctrl+T
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 Ctrl+Shift+F
ViewVisualizationHigh Quality Image... Ctrl+Shift+H
ViewInformation Window F4
ViewCurrent Dialog F3
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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
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
StartGateway... Ctrl+W
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