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Lesson 3: Surface Creation
In this lesson, you will learn how to create surfaces from wireframes.
Lesson 3: Surface Creation
Lesson content:
Case Study: Surface Creation
Design Intent
Stages in the Process
Choice of Surface
Sweeping a Profile
Create a Multi-Section Surfaces
Create a Adaptive Sweep Surface
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Case Study: Surface Creation
Case Study: Surface Creation
The case study for this lesson is the Car Door substrate with Arm rest. The focus of this case study is the
creation of Surfaces from a given wireframe data to check the Design feasibility. Your goal is to achieve
the editable model of Car Door substrate with Arm rest. which incorporates the design intent of the part.
The focus of the case study in this lesson is to understand, how to access Surface Design workbench and
to manage a few basic tools.
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Design Intent (1/2)
Create a Door Substrate. The substrate profile needs to be
adaptable for design modification & changes without replacing
the original input .
Create an Adaptive Sweep
Create a broad cross-section surface for an Arm rest
attached to the front door for design feasibility study.
Create a profile sweep with single guide curve option.
Create a cross-section surface for Key-pad (for
Electronic control ) at a measured distance from the Arm rest
ankle point.
Create a profile sweep from a given sketch with single guide
curve.
Attain a single merged part by using Arm rest and the key
pad component.
Create a Multi-section surface between two different profiles
of Armrest and Key-pad to form an integrated single part.
Close the end of the Arm rest & Key-pad with rounded end.
Use the revolve option to attain the rounded ends.
The intent is to create surfaces for design feasibility study for given components. The surfaces should
meet the following given design intents.
Case Study: Surface Creation
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Design Intent (2/2)
Design the door latch .
Create Multi-Section Surface to attain the variable shapes,
along the flow.
Design a Map-Pocket with the rounded edges.
Use a circle sweep tool with single guide and tangency
surface option.
Case Study: Surface Creation
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Stages in the Process
The following steps are used to perform the case study:
Adaptive Sweep Surface
Sweep a Profile
Revolve Surface
Create Multi section Surface
Arm Rest area
Door Substrate
Key Pad Area
Merge between
Armrest & Key
Pad
Map-Pocket
Latch
Rounded Ends
Case Study: Surface Creation
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Step 1: Choice of Surfaces
In this section, you will be introduced to the different types of surface creation
tools available in Generative Shape Design.
Use the following steps to get
familiar with Surface creation.
1. Choice of Surfaces
2. Extruding or Revolving a Profile
3. Sweep a Profile
4. Create Multi-Section Surface
5. Create an Adaptive Sweep Surface
Step 1 :Choice of Surface
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Choice of Surface (1/2)
Creates a surface offset from an existing
surface
Offset Surfaces offset from
an existing surface
Creates a surface inside a closed
boundary
Fill Surfaces filling a gap
Sweeps a parametric profile along a path,
allowing the parameters to evolve along
the path
Adaptive
sweep
Sweeps a profile along a path (the profile
is predefined or user defined)
Sweep Surfaces sweeping a
profile along a guide
curve
Surface passing through multiple sections Multi-section
surface
Surfaces connecting
existing sections
Full or partial spherical surface. It works
as circular profile revolved around an
axis.
Sphere
Revolve a user defined profile around an
axis
Revolve Surfaces revolved
around an axis
Extrudes an implicitly circular profile in a
specified direction.
Cylinder
Extrudes a user defined profile in a
specified direction.
Extrude Surfaces extruded in
a direction
Illustration Description Icon Name Category
Step 1 :Choice of Surface
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Choice of Surface (2/2)
The choice of the surface can be done in regards to the wireframe features available.
The following table shows what are the wireframe required for each type of surface:
Section
Optional Optional Loft
Revolve
Sweep
Cylinder
Sphere
Extrude
Spine Guide Curve Direction/Axis Profile
Mandatory
Not Applicable
Inputs
Tools
Loft => Multi-Section Surface
Step 1 :Choice of Surface
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Step 2: Extruding or Revolving Profile
In this section, you will learn to create a basic surfaces.
Use the following steps to get
familiar with Surface creation.
1. Choice of Surfaces
2. Extruding or Revolving a
Profile
3. Sweep a Profile
4. Create Multi-Section Surface
5. Create an Adaptive Sweep Surface
Step 2 :Extruding or Revolving Profile
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Profiles that can be used
An Extrude or a Revolve tool uses a profile to create a surface.
A Profile can be a Sketch, 3D curve, edge of an existing surface or solid.
Revolve
Extrude
Solid edge profile Surface edge profile 3D profile Sketch profile
Inputs
Surface
Step 2 :Extruding or Revolving Profile
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Extruding or Revolving a Profile(1/2)
An extruded surface is created by extruding a
user defined profiles in a specified direction.
Use the following steps to create an extruded
surface:
1. Select the Extrude icon.
2. Select the profile to extrude.
3. Specify the direction to extrude. The direction can
be specified using a line, plane, or edge. Direction
can also be defined using the contextual menu.
4. Enter limits.
5. Click OK to generate the feature.
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2
3
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4
Step 2 :Extruding or Revolving Profile
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Extruding or Revolving a Profile(2/2)
A Revolve feature is created by revolving a profile
about an axis.
Use the following steps to create a revolve feature:
1. Select the Revolve icon.
2. Select the profile to revolve.
3. Select the axis of revolution.
4. Enter the angle limits.
5. Click OK to generate the feature.
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3
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2
Step 2 :Extruding or Revolving Profile
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Step 3: Sweeping a Profile
In this section, you will learn about different types of Sweep surface tools.
Use the following steps to get
familiar with Surface creation.
1. Choice of Surfaces
2. Extruding or Revolving a Profile
3. Sweeping a Profile
4. Create Multi-Section Surface
5. Create an Adaptive Sweep Surface
Step 3 :Sweeping a Profile
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Computation of Sweep
Sweep is a surface generated by sweeping a profile along a guide curve with respect to a spine. The profile
can be a user-defined or pre-defined profile.
Sweeping a profile along a guide curve with respect to a
spine means,
The Planes are calculated in regards to the tangent to the
spine and to the mean plane of the spine. The sweep profile
is repeated on these planes along the guide curve. Then a
surface is swept passing through these profiles. This surface
is the sweep (or swept surface).
Profile
Spine
Guide
Profiles repeated in the
planes
Surface passing through
the repeated sections
Step 3 :Sweeping a Profile
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Why is the Choice of the Spine Important ?
The quality of the spine defines the quality of the sweep: Tangency discontinuities on the spine
impact the quality of the final sweep:
The spine is not tangency continuous
The sweep inherits the faults of the
spine.
The same spine has been made
continuous. The default is gone.
A B
Step 3 :Sweeping a Profile
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Spine Calculation
Spine can be calculated using the Spine tool available in the
Generative Shape Design workbench.
Using the Spine tool, you can calculate,
A. The spine in regards to end or intermediate planes.
B. The spine in regards to two or more guide curves
facilitating the creation of swept surface which runs
along the guide curve.
Spine computed using
intermediate planes.
Spine computed using
guide curves.
Section
Sweep computed
using explicit spine
Guide Curves
Sweep computed
using explicit spine
Step 3 :Sweeping a Profile
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Calculating a Spine Regards to Plane or Guide Curve
1
2
1. Select the Spine icon.
2. Select the first Plane.
3. Successively, select the Planes through which the
spine should pass.
4. Select the Start point (if required).
5. Select OK to generate the feature.
Use the following steps to create a revolve feature:
Planes to compute spine
Spine computed using
intermediate planes
Step 3 :Sweeping a Profile
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Explicit Sweep
Following is the list of user-defined sweep options available in a sweep tool.
Profile
An explicit profile is
swept along the guide
curve at an angle of 20
deg with respect to
pulling direction.
With Pulling
Direction
An explicit profile is
swept along the two
guide curve. Anchor
points decides the start
point and orientation of
the sweep.
With Two
Guide curves
An explicit profile is
swept along the guide
curve at an angle of 45
deg with respect to
reference surface.
Guide curve lies on
reference surface.
With
Reference
surface
Illustration Description
Sweep Sub
Types
Sweep Type
Guide Curve 1
Guide Curve 2
Guide Curve
Pulling
Direction
Reference Surface
Profile
Profile
Guide curve
Anchor Points
20 Deg
Step 3 :Sweeping a Profile
45 Deg
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Sweeping a Profile (1/2)
Use the following steps to apply a reference surface to a swept surface feature:
1. Select the sweep Icon.
2. Select the With Reference Surface option from
the dialog box.
3. Select the Profile and Guide curve.
4. Select the surface.
5. If necessary, enter an angle. This angle is
measured between the profile and the reference
surface.
6. Select OK to create a swept surface.
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3
2
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6
Step 3 :Sweeping a Profile
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Sweeping a Profile (2/2)
Use the following steps to add a second guide curve to a swept surface feature:
1. From the Subtype pull-down menu, select the
With two guide curves option.
2. Select the profile.
3. Select the first guide curve. This guide curve,
by default, will also act as the spine.
4. Select the second guide curve.
5. Select the 1
st
and 2
nd
anchor points (If you do
not explicitly select anchor points or anchor
direction, they are automatically computed if the
profile is planar ).
6. Select OK to generate the feature.
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5
3
2
4
Step 3 :Sweeping a Profile
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You can manipulate the orientation and position of the swept surface without actually moving the
parent curves. This is done by selecting the positioned profile option in swept surface dialog box.
Profile Positioning
Before Positioning
A. Using no positioning:
B. Using positioning:
C. Rotate the positioning axis system
D. Translate the position of the origin of the
positioning axis system
After Positioning
Rotating the surface
Profile
Guide
Modifying the Position axis
system
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Linear Sweep (1/2)
Pre-defined profiles are the Implicit profiles like line, Circle and Conic which are used to compute the
sweep. The other inputs are specified by the user variably, keeping the profile type as constant.
Following is the list of sub -options available to perform a pre-defined Line sweep.
Guide Curve (G)
Reference
surface (S)
An implicit line profile is swept
along the guide curve at an
specified angle with respect to
reference surface.
With
Reference
Surface
Guide Curves
( G1 and M )
A swept surface is created
using two guide curve. The
second guide can be opted to
be a middle curve of the
generated surface.
Limits and
Middle
Guide Curves
( G1 and G2)
A swept surface is created
between two guide curves With Two
Limits
Illustration
Inputs
required
Description Type
G1
G2
G1
M
G1
S
Step 3 :Sweeping a Profile
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Linear Sweep (2/2)
Following is the list of sub -options available to perform a pre-defined Line sweep (Continued).
Tangent
Surface
(T1 and T2).
Spine (C)
A swept surface is created
using two tangent surfaces and
a Spine.
With Two
Tangency
Surface
Guide Curve (G)
Draft direction
(D)
A swept surface is created at
an angle with the specified
pulling direction.
With Draft
Direction
Guide Curve (G)
Tangent
Surface (S)
A swept surface is created
using guide curve and a
tangent surface.
With
Tangency
Surface
Guide Curves
(G1 and G2)
A swept surface is created at a
specified angle with the line
joining the two guides.
With
Reference
Curve
Illustration
Inputs
required
Description Type
G1
G2
Line joining two
guides
A
G
S
T1
T2
C
D
G
A
Step 3 :Sweeping a Profile
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Circle Sweep
Following is the list of sub -options available to perform a pre-defined Circle sweep.
Center Guide
(GC).
Radius (R)
A circle swept surface
(complete round) of specified
radius is created using center
guide as tube axis.
Center and
Radius
Center Guide
(GC).
Reference Guide
(GR). Angle (A)
A circle swept surface is
created using center guide as
axis and reference guide
profile.
Center and
Two Angle
Guide Curve
(G1 and G2)
Reference
Surface (S)
A circle swept surface is
created along the two guide
curve and reference surface.
One Guide
and
Tangency
Surface
Guide Curve (G) A circle swept surface of
specified radius is created
between two guide curve.
Two Guide
and Radius
Guide Curves
(G1, G2 and G3)
A circle swept surface is
created using three guide
curves.
With Three
Guide
Curves
Illustration
Inputs
required
Description Type
G1
G2
G3
G1
G2
GR
GC
A1
GC
A2
R
R
G1
G2
S
Step 3 :Sweeping a Profile
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Conical Sweep
Following is the list of sub -options available to perform a pre-defined Conic sweep.
Guide Curve
(G1, G2, G3, G4
and G5)
A conic sweep surface is
created by passing through five
guide curve.
Five Guide
curves
Guide Curve
(G1, G2, G3, G4)
Tangent surface
(T1)
A conic sweep surface is
created by passing through four
guide curve and tangent
surface.
Four Guide
Curves
Guide Curves
(G1, G2 and G3)
Tangent surface
(T1)
A conic sweep surface is
created by surface passing
through three guide curve and
tangent surface.
Three
Guide
Curves
Guide Curves
(G1 and G2)
Tangent surface
(T1 and T2)
A conic swept surface is
created by passing through two
guide curves. The tangent
surface is specified at each
curve.
Two Guide
Curves
Illustration
Inputs
required
Description Type
G1 G2
T1 T2
T1
G1
G2
G3
G4
G1
G2
G3
G4
G5
Step 3 :Sweeping a Profile
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What are Laws
d
L
Advance Law
Reference
Curve
Definition Curve
Parametric surface created require certain input parameters to
define them. An input parameter can be length or angle value.
By default, this value remains constant while computing the
surface. By using Laws you can vary these parameters as per
desired results.
Laws can be used in the situations where the curve or the
surface that are being created vary according to pattern or a
mathematical equation.
There are basically three types of Laws :Linear, S type and
Advanced
A. Linear
B. S type of Laws
C. Advanced Laws
Linear Law
S type Law
The Law define the variation of d along L
Step 3 :Sweeping a Profile
A
C
B
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Sweeping a Profile Using Law
You can use Law in a sweep functionality to vary the parameters
such as angle, length and radius along the Sweep.
Use the following steps to create a profile sweep using law
definition.
1. Select the Sweep icon.
2. Select Pre-defined profile Line option.
3. From the Subtype pull-down menu, select the With Draft
Direction option.
4. Select the first guide curve.
5. Select the Draft direction.
6. Select the Draft button.
a. Select the S type option.
b. Specify the Start angle and End angle. (The draft angle
transits with respect to S path from start value to end value.
You can inverse the law by selecting Inverse check box).
7. Select close in the law definition panel.
8. Specify the length parameter of the surface
9. Click OK in the Sweep panel
0 degrees at
start end
45 degrees at end
Step 3 :Sweeping a Profile
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Errors you can encounter while computing the Sweep
Step 3 :Sweeping a Profile
Solution
The problem would be due to,
too short spine compared to
guide curves, Guides parallel
to the moving Plane or due to
a large spine curvature.
modify the spine (with less
curvature variation) or expand
the guide curves
Error/Warning
The moving plane
(perpendicular to the Spine)
and the guides do not always
intersect.
Change the sweep parameters
or reduce the guide or spine
curvature variations
The surface is pre-computed to show
the place where the curvature variation
of the guide curve is too important to
show you the cusp and help you to
solve the problem
.
The Extrusion of the
vertex of a profile leads to a
cusp. Use a guide with smaller
curvature.
The plane on the spine that does not
intersect the guide is shown to help you
solve the problem.
Description
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Exercise 3A
Recap Exercise
15 min
In this exercise, you will create a profile sweep. You will create base surface of Phone
receiver. The intent of this exercise is to understand the role of spine in creating a
swept surface.
Detailed instructions for this exercise are provided.
By the end of this exercise you will be able to:
Sweep a profile along a guide curve.
Understand that Spine controls the orientation
and shape of the surface.
Exercise 3A
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Exercise 3A (1/5)
1. Create a new part.
To create a new part file, select Part from the New
dialog box.
a. Click File > New.
b. Choose Part from the New dialog box.
c. Click OK.
d. Enter the new part name as Table Lamp
e. Click OK.
1b
1c
1d
2. Access Generative Shape Design
workbench.
To access workbench from start menu.
a. Click Start > Shape >Generative
Shape Design
1e
Exercise 3A
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Exercise 3A (2/5)
3. Create a Sketch.
Create a conic section in a sketch on YZ plane.
a. Click on Sketch Icon.
b. Draw a Conic curve in to the sketch as shown.
c. Specify dimensions as shown.
d. Click Exit the Sketcher.
3b
3a
3c
4. Create Planes at both end of the sketched curve at
10 deg angle.
Create a Line normal to the curve at its end point
as shown. You will use these lines as axis to
create an angular plane at both ends of the
curve.
a. Click on Line Icon.
b. Specify the Point and direction as end point of
sketched curve along X direction.
c. Specify length as 15 mm.
d. Select OK.
Similarly, create a line at other end of the of the
sketched curve.
Create angular planes at both ends of the curve.
3d
Exercise 3A
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Exercise 3A (3/5)
5. Create a Profile Sketch.
Create a conic section in a sketch on YZ plane.
a. Click on Sketch Icon.
b. Draw a Conic curve in to the sketch as
shown.
c. Specify dimensions as shown.
d. Click Exit the Sketcher.
6. Create a Spine curve .
Create Spine curve using intermediate planes
a. Click on Spine Icon.
b. Select Plane 1, ZX Plane and Plane 2
consecutively, as shown.
c. Select OK.
5a
5d
Plane.1
ZX Plane
Plane.2
Spine
6a
Exercise 3A
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Exercise 3A (4/5)
7. Create a Profile sweep .
Create a base surface of Telephone receiver. Use
Sketch.2 as Profile and Sketch.1 as a guide. Use the
default spine.
a. Click on Sweep Icon.
b. In Explicit sweep option, select the sub-option with
reference surface.
c. Specify sketch.2 as profile.
d. Specify Sketch.1 as guide curve.
e. Select OK.
Similarly, create a sweep using Sketch.3 as profile and
Sketch.2 as guide curve. Use the default spine.
7a
7b
7c
7e
7d
Sweep.1
Sweep.2
Exercise 3A
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Exercise 3A (5/5)
7. Modify the Profile sweep .
Replace the Spine explicitly.
a. Double click on swept surface.
b. Select the spine.1 curve as a spine..
c. Select OK.
Similarly, replace the spine of second sweep with
Spine.1 curve.
Sweep without spine
Sweep with spine
Observation:
You can observe that the shape and orientation of the
swept surface changes when you add a spine.
1. The Spine allows the surface to end normal
to the angular planes
2. The orientation of the surface changes to
maintain the cross-section of the sweep
perpendicular to the Spine at any point
along the guide curve.
Exercise 3A
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Exercise 3A: Recap
Sweep a profile along a guide curve.
Understand that Spine controls the
orientation and shape of the surface.
Exercise 3A
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Exercise 3B
Recap Exercise
15 min
In this exercise, you will practice the sweep sub-options to create a speaker grill of
automotive door. You will practice the sub-options of Circle and Conic type of sweep.
High level instructions for this exercise are provided.
By the end of this exercise you will be able to:
Extrude a profile in a direction.
Create a Fill surface.
Create a swept surface using the Two Guides
and Tangency surface available in Circle option.
Create a swept surface using Two Guides
available in Conic option.
Exercise 3B
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Exercise 3B (1/8)
1. Create a new part.
To create a new part file, select Part from the New
dialog box.
a. Click File > New.
b. Choose Part from the New dialog box.
c. Click OK.
d. Enter the new part name as Table Lamp
e. Click OK.
1b
1c
1d
2. Access Generative Shape Design
workbench.
1e
Exercise 3B
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Exercise 3B (2/8)
3. Create a Sketch.
Create a Circle in a sketch on XY plane.
3
4. Extrude a surface.
Create an extruded surface using the previously
created sketch.
4
Exercise 3B
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Exercise 3B (3/8)
5. Create a Sketch.
Create a Sketch on XY plane.
5
Exercise 3B
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Exercise 3B (4/8)
6. Create a Swept surface
Create a swept surface using the sub-option Two
Guide and Tangency surface available in Circle
sweep option.
Observation:
It is mandatory that the first guide curve selected
should lie on the specified Tangency surface or plane.
The swept surface generated maintains tangency with
specified surface.
6
Exercise 3B
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Exercise 3B (5/8)
7. Re-create a swept surface by changing the inputs.
Create a swept surface using the sub-option Two
Guide and Tangency surface available in Circle
sweep option.
Observation:
Sketch.1 lies on the specified tangency surface. The
surface generated will be tangent to the surface an with
In the limits of the guide curve.
7
Exercise 3B
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Exercise 3B (6/8)
8. Create a Fill surface.
Create a Plane parallel to XY plane at a distance of
5mm.
8
9. Create a Point.
Create a Point at a distance of 15mm from the
absolute coordinate system.
Point
Plane
9
Exercise 3B
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Exercise 3B (7/8)
10
10. Create a Sketch.
Create a Sketch on Plane 1.
11. Create a Fill Surface.
Create a fill surface using Sketch.2 passing
through Point.1
11
Fill Surface
Exercise 3B
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Exercise 3B (8/8)
12. Create a Swept surface
Create a swept surface using the sub-option Two
Guide curves available in Conic sweep option.
12
Exercise 3B
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Exercise 3B: Recap
Extrude a profile in a direction.
Create a Fill surface.
Create a swept surface using the Two Guides
and Tangency surface available in Circle
option.
Create a swept surface using Two Guides
available in Conic option.
Exercise 3B
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Exercise 3C
Recap Exercise
15 min
In this exercise, you will practice to create swept surface using law. You will design a
turbine blade .You will be provided with the basic curves.
High level instructions for this exercise are provided.
By the end of this exercise you will be able to create a
swept surface using law.
Exercise 3C
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Exercise 3C (1/2)
1. Open the part.
Open an existing part file. The file consists of
Section curves for blade model..
a. Browse and open part:
Exercise_3C_start.CATPart
2. Create Line Sweep.
Create blade surface using Line sweep option.
Specify the given curve as guide and YZ plane
for draft direction.
The orientation of the blade changes along the
guide curve at a constant angle. To attain this
specify a linear law for angular dimension. The
angle varies from 15 deg to 75 deg.
Exercise 3C
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Exercise 3C (2/2)
3. Define a Law
Use the law type as Linear.
Specify the start angle as 15 deg and end angle
75 deg.
4. Rotate the Surface
Rotate a surface along given axis line at an angle
of 18 deg.
Specify the object instance to 20 numbers.
Exercise 3C
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Exercise 3C: Recap
Create a sweep using law.
Exercise 3C
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Step 4: Create a Multi Section Surface
In this section, you will learn to create Multi-Section Surface.
Use the following steps to get
familiar with Surface creation.
1. Choice of Surfaces
2. Extruding or Revolving a Profile
3. Sweep a Profile
4. Create Multi-Section Surface
5. Create an Adaptive Sweep Surface
Step 4 :Creating a Multi Section Surface
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What is a Multi-Section Surface
A surface computed by passing through two or more
consecutive sections along a spine is called Multi-Section
surface. The shape of the Multi-Section surface can be
defined more precisely by specifying the sections.
During a certain design situations, you may need a shape
which varies in its cross-section along its length. In such case
you can create Multi-Section surface which passes through
the defined sections along the spine or guides.
Multi-Section surface helps you to attain a smooth transition
surface between two or more varying sections and at the
same time maintains the G1 continuity with adjacent
surfaces.
Step 4 :Creating a Multi Section Surface
Sections
curves
Guide
curves
Adjacent
Surface
Adjacent Surface
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What are Sections and Guide Curves
Section are the user defined profile. A section can be a planar
or a non-planar curve. It is an elementary input to create a
Multi-Section Surface. A Multi-Section surface passes through
the set of consecutive sections to inherit their shape.
The Guide curve defines the path for the surface to transit
between two sections. The guide curve is a point continuous
curve and intersects with each consecutive section of a Multi-
Section surface.
Section Curves
Guide Curve
Step 4 :Creating a Multi Section Surface
Guide Curve to give the correspondence
between these 2 vertices
Section
Curves
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What are Coupling Points (1/2)
Coupling Points are the connecting points used to
compute the segmentation on the surface.
When a Multi-Section Surface is created using a coupling
option, CATIA computes virtual points called as coupling
points on each section at its vertices, and discontinuities.
During the surface generation, the coupling points of one
section are automatically connected to the corresponding
coupling point of the consecutive section to attain a
guided flow between two or more sections.
You can choose for manual coupling when there are
unequal numbers of coupling points in each section.
In the illustration,
A
B
1. There are equal number of coupling points in all
the three sections. The corresponding points of
different sections couples with each other to form a
segment. A1, A2 and A3 are the corresponding
points of different sections coupled together.
2. Each section has a different number of coupling
points. You can couple the points manually
according the required segmentation. Here C1 is
coupled with the C2 and B3 points of second and
third section respectively.
A1 A1
A2
A3
B1
B2
B3
C1
C3
C2
A1
A2
A3
B1
B2
B3
C1
C2
D1
D2
E1
E2
E3
Step 4 :Creating a Multi Section Surface
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What are Coupling Points (2/2)
A. When number of coupling points in all the given sections are
equal, CATIA computes the surface using other coupling options,
1. Tangency
2. Tangency then Curvature
3. Vertices
B. When number of coupling points in all the given sections are
unequal, Points can be manually coupled (topologically) based
on desired segmentation.
A2
By default, CATIA computes the coupling points based on the
section length ratio (Curvilinear abscissa).
B
A1
A3
Step 4 :Creating a Multi Section Surface
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What are Closing Points
A. Closing point computed at different vertices for the
two given sections.
B. When the surface is generated, it follows the
orientation of sections defined by closing point.
C. Modify/Replace the Closing point in section 2 to top
vertex. You can observe the orientation of the
Multi-section surface is changed.
A
B
C
A closing point is an end point of the closed section. The
closing point is associated with the orientation of the section.
When a surface is generated, the closing point of the one
section couples with the closing point of consecutive section.
Thus decides the orientation of the surface.
CATIA automatically computes the closing point of the
closed section, either on its vertices or an extremum point.
You can change the closing point of one or more sections to
modify the orientation of the surface.
Observe the following illustration:
Step 4 :Creating a Multi Section Surface
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Replacing a Closing Point
1. Select the Multi-Section Surface icon.
2. Select the first section and second section.
3. Observe the location closing points for both section. (If
they are not at the corresponding points of each section
we need to replace them).
4. Select Replace through contextual menu on the closing
point you need to change (Right click on the closing point
to pop up the contextual menu).
5. Specify the new point for the closing point..
6. Click OK to generate the Multi-Section surface.
Use the following step to replace the closing point of a
Multi-Section Surface.
Closing Point 2
Closing Point 1
After Replacing
Closing Point
Closing Point 1
Closing Point 2
1
4
2
5
6
Step 4 :Creating a Multi Section Surface
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Creating the Multi-Section Surface
1. Select the Multi-Section Surface icon.
2. Select the first section.
3. Select the Second Section.
4. In the Coupling tab, create manual coupling (Create
points on the first section if required). Couple
between points created on first section and
corresponding vertices of second section.
5. Click OK to create a Multi- Section surface.
Use the following step to create a Multi-Section Surface using Manual coupling.
1
2
3
4
5
Step 4 :Creating a Multi Section Surface
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Exercise 3D
Recap Exercise
15 min
In this exercise, you will practice to create the Multi-Section surface. You will be given
with set of section curves of a shoe. You will create a Shoe model .You will also
understand the different coupling options of Multi-Section surface.
High level instructions for this exercise are provided.
By the end of this exercise you will be able to:
Create a multi-section surface.
Use different coupling options.
Exercise 3D
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Exercise 3D (1/5)
1. Open the part.
Open an existing part file. The file consists of
Section curves for shoe model..
a. Browse and open part:
Exercise_3D_start.CATPart
2. Create Geometrical Set.
Insert a Geometrical set and rename it as
Shape Surfaces.
Exercise 3D
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Exercise 3D (2/5)
3. Create a Multi-Section Surface.
Create a Multi-Section surface using the 3 closed
sections without guide curve.
Observation:
By default, the mode of coupling is in Ratio. The
results obtained is computed using Ratio.
Section 1
Section 2
Section 3
Closing Point 1
Closing Point 2
Closing Point 3
3
Exercise 3D
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Exercise 3D (3/5)
4. Change the Coupling Mode to Vertices.
The segmentation of the surface is changed.
Observation:
You will observe that the segmentation of the surfaces
changes. CATIA couples the surface with
corresponding vertices of different sections.
Exercise 3D
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Exercise 3D (4/5)
5. Change the Coupling Mode to tangency.
An message is shown that the tangency option of
coupling is not feasible to generate the surface due
to unequal coupling points on each sections.
Observation:
You will observe that the tangency discontinues points
which acts as a coupling point on each section are
unequal.
Exercise 3D
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Exercise 3D (5/5)
6. Couple the sections manually.
You will create the coupling between three sections
manually to obtain the desired segmentation on the
surface.
Coupling 1
Coupling 2
Coupling 3
Coupling 4
Exercise 3D
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Exercise 3D: Recap
Create a multi-section surface.
Use different coupling options.
Exercise 3D
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Step 5: Create an Adaptive Sweep Surface
In this section, you will learn to create Adaptive Sweep Surface
Use the following steps to get
familiar with Surface creation.
1. Choice of Surfaces
2. Extruding or Revolving a Profile
3. Sweep a Profile
4. Create Multi-Section Surface
5. Create an Adaptive Sweep
Surface
Step 5 :Creating an Adaptive Sweep
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How is an Adaptive sweep Calculated?
10
15 110
Adaptive Sweep Surface is a surface which can adapt to changing dimensions of the parent profile
along the defined path.
A. A constrained sketch profile is swept along the
guide curve.
B. The surface is computed along the guide curve
respecting the sketch constraints and
dimensions. The sketch is constrained with
respect to external reference in order to maintain
the associativity along the guide curve.
C. You can vary the cross-section of the sweep
along the guide curve by defining the user-
sections. The User-section inherits the
constraints of the parent sketch and allows you
to modify them independently.
D. You can specify different dimensions for the
sketch at every user section. The surface is
computed, adapting to the changing dimensions
at each consecutive user-section.
User Section .1
User Section .2
Sketch
Guide Curves
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5
100
Step 5 :Creating an Adaptive Sweep
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How is an Adaptive sweep different from a simple sweep?
Lets see some salient features of Adaptive sweep which differs it
from a simple sweep.
A. Adaptive Swept surface inherits the sketch
constraints along the surface.
B. Adaptive sweep allows you to create intermediate
sections (User-sections) on the fly along the guide
curve.
C. Adaptive sweep allows you to modify the
intermediate sections independently.
D. Adaptive sweep ensures that the profile is normal to
the guide curve or spine at the time of creation.
B
C
Step 5 :Creating an Adaptive Sweep
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Constrained Sketch
A. The sketch of an Adaptive surface has to be a constrained sketch. By default: a constraint is created
between the guide curve and the sketch originThe sketch origin is always placed on the guide
curve all the sweep long
B. To make the dimensions of the sketch vary: dimension the sketch during its creation
C. To ensure the relative positioning of the sections with reference elements (parallelism, angle, offset
...): constraint the sketch elements on the intersections of the sketch plane and the reference
elements.
D. It is recommended to use angle constraints rather than tangency or perpendicularity constraints, to
avoid changes in the sketch orientation as it is swept along the guiding curve. In some cases, with
tangency or perpendicularity constraints, the sketch may be inverted and lead to unsatisfactory
results.
While creating the Adaptive sweep remember the following key points.
No coincidence constraint, but a
geometric superimposition
Surface is not computed along the guide
curve. No associativity with the guide curve.
Sketch based on the point as the
intersection of the sketch and
the guiding curve
Surface is computed along the guide curve.
Associativity with the guide curve is
maintained.
Step 5 :Creating an Adaptive Sweep
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Creating an Adaptive Sweep (1/3)
When you create an adaptive sweep the sequence of
creation becomes important based on the reference
element you choose.
If you want to create an Adaptive swept surface which
lies on other surface, you will create the sketch in
context because you want to add some associative
constrains with the existing geometry.
For example.
Here we want that the sketch keeps its coincidence
with the surfaces (the intersection between the
surface and the sketch plane) in each section of the
sweep.
By building the sketch directly from the Adaptive
sweep sketch dialog box, you will ensure that the
sketch keeps the constraint associativity with the
guide curve (or 3D reference elements).
Sketch keeps its Coincidence
with the surfaces
Step 5 :Creating an Adaptive Sweep
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Creating an Adaptive Sweep (2/3)
1. Select the Adaptive Sweep icon.
2. Select the Guide curve (By default, Guide curve is
considered as spine and mean Plane as Reference
surface).
3. Select the reference surface.
4. Select the Sketcher icon, Sketch creation panel is open.
5. Specify the point to be a origin of the sketch. Also select
the reference elements.
a. Specify both the guide curves as constructional
element.
6. Select OK to enter the Sketcher workbench.
Use the following step to create a Adaptive Swept surface.
1
2
4
5
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5a
3
Step 5 :Creating an Adaptive Sweep
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Creating an Adaptive Sweep (3/3)
6. Create the section profile in the sketch as shown and
exit the sketch.
7. In the User-section area in the panel, create the
sections along the guide curve by selecting the
points on the guide curve.
8. Change the profile dimensions on each sections to
attain the required shape of the sweep.
9. Select OK to generate the Adaptive Sweep.
Use the following step to create a Adaptive Swept surface (continued)
6
7
8
9
Step 5 :Creating an Adaptive Sweep
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Errors that can encountered while computing the Sweep.
Step 5 :Creating an Adaptive Sweep
Choose passing points carefully or use
the create section here tool
A plane normal to the spine
and passing by a chosen
point cannot be computed
Section creation failed or
sketch not normal to the spine
Solution
Try to avoid using of 3D projections or
intersections other then reference
element .
Error/Warning
The projection of 3D
reference elements may
become meaningless along the
guide curve and produce
unexpected result or sketch
inconsistency.
Try to avoid using of 3D projections or
intersections other then reference
element .
Using reference: ensure the references
are intersected all the sweep long.
When the sketch has used
the projections/intersection
from the 3D geometry which
cannot be referred through
out the surface flow along the
guide curve CATIA gives this
error on preview.
Error occurred during
section computation. Please
check if the reference elements
or constraint of the sections are
usable at the current place.
Whenever you select the point in a 3D
space as a input for sketch center,
ensure that the plane normal to the
guide at that point intersects the guide.
When the Point specified in
the sketch creation dialog box
do not intersect with the guide
curve CATIA gives this error.
The Moving Plane
(perpendicular to the spine )and
guide do not always intersect.
When the sketch has used
the projections/intersection
from the 3D geometry which
cannot be referred through
out the surface flow along the
guide curve CATIA gives this
warning on exiting the sketch.
Description
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Exercise 3E
Recap Exercise
15 min
In this exercise, you will practice the creation of Adaptive Sweep surface. You will be
creating a base surface for Floor Rail part.
Detailed instructions for this exercise are provided.
By the end of this exercise you will be able to
create a adaptive sweep surface.
Exercise 3E
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Exercise 3E (1/6)
Exercise 3E
2. Create set of points on a curve.
You will create five points on the guide curve using
Points and Planes repetition tool.
a. Select Point and Plane Repetition icon.
b. Specify 5 point and select curve.1.
c. Click OK to create the points.
a. The Points would be used to create user-sections while
defining the sweep.
2a
2b
2c
1. Open the part.
Open an existing part file. The file consists of
Section curves for shoe model..
a. Browse and open part:
Exercise_3E_start.CATPart
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Exercise 3E (2/6)
Exercise 3E
3. Create an Adaptive swept surface.
Create an Adaptive Swept surface using the
given guide curves.
a. Click on Adaptive sweep Icon.
b. Select Curve.1 as a guide curve and
Spine.
c. Select the sketcher Icon to create a
sketch contextually.
d. Select the vertex point of curve.1 as a
reference point of the sketch.
e. Select curve.2 as Optional Construction
Element.
f. Click OK to enter the Sketcher.
3a
3b
3c
Curve 1
Curve 2
3d
3e
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Exercise 3E (3/6)
Exercise 3E
4. Create sketch profile.
You will create a cross section profile as
shown.
4.5
5.0
6.0 4.5
3
5
d
e
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110 deg
Exit the Sketcher after you completely
constrain the profile.
The Profile would look like this
after the sketch
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Exercise 3E (4/6)
Exercise 3E
5. Define the User Sections.
Select the previously created Points to
define User-Section.
a. Select Point 1 to 5 consequently as
shown to create 5 user sections.
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Exercise 3E (5/6)
Exercise 3E
6. Edit the User Sections.
You will edit the dimension of each User-Sections to
obtain the desired shape of the surface.
a. Select the Parameters Tab.
b. Select the User-Section.1.
c. Change the dimensions of the sketch as shown.
B
C
A E
F
D
35 deg 4.6 110deg 5.0 16.5 13.0 User-Section.5
35 deg 4.6 110deg 5.0 12.0 12.0 User-Section.4
35 deg 4.6 110deg 5.0 10.0 11.0 User-Section.3
35 deg 4.6 110deg 5.0 7.0 9.0 User-Section.2
35 deg 4.6 110 deg 5.0 4.5 6.0 User-Section.1
F E D C B A User Sections
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Exercise 3E (6/6)
Exercise 3E
Select Ok in Adaptive Sweep panel to generate the swept
surface.
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Exercise 3E: Recap
Create a Adaptive Swept surface.
Exercise 3E
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Case Study: Surface Creation
You will practice what you learned, by completing the case study model . In this
exercise, you will create the Door inner components.
30 min
Recall the design intent of this model:
Create a Door Substrate. The substrate profile needs to be
adaptable for design modification & changes without replacing
the original input.
Create a broad cross-section surface for an Arm rest attached to
the front door for design feasibility study.
Create a cross-section surface for Key-pad (for Electronic control
) at a measured distance from the Arm rest ankle point.
Create a single merged part by using Arm rest and the key pad
component.
Close the end of the Arm rest & Key-pad with rounded end.
Case Study: Surface Creation
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Case Study: Surface Creation
Design the door latch.
Design a Map-Pocket with the rounded edges.
Using the techniques you have learned in this lesson and previous exercises, create
the model without detailed instruction.
Case Study: Surface Creation
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Do It Yourself : Surface Creation (1/3)
1. Open the given part consisting of the
wireframes of Car Door model, in Generative
Shape Design workbench.
Browse through the files and open the model
Lesson _3_ Case Study_Start.CATPart
2. Create an Adaptive sweep surface.
Create a door substrate using the guides provided
using Adaptive swept surface.
3. Create a Sweep surface.
Create a swept surface at Arm rest and Key pad area
using profile and the guide curve.
Case Study: Surface Creation
The following steps offer hints to guide you through
the creation of door part surfaces.
2
3
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Do It Yourself : Surface Creation (2/3)
4. Create a single merged part by using Arm
rest and the key pad component.
Create a Multi-Section Surface between Arm Rest
surface and Key Pad surface.
Extract the boundary of the swept surfaces and
build a Multi-Section surface between two
boundary as shown.
5. Close the end of the Arm rest & Key-pad with
rounded end.
Revolve the boundaries of the swept surface to
attain the rounded ends as shown.
Case Study: Surface Creation
4
5
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Do It Yourself : Surface Creation (3/3)
6. Create a Door latch.
Create a Multi-Section Surface using the sections
and guide provided.
7. Create a Map pocket feature.
Using the circle sweep option create bottom half of
the pocket. Connect the edges of the resultant
surface and fill the upper part of the pocket.
Case Study: Surface Creation
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6
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Case Study: Surface Creation Recap
Create a Door Substrate. The substrate
profile needs to be adaptable for design
modification & changes without replacing
the original input.
Create a broad cross-section surface for an
Arm rest attached to the front door for
design feasibility study.
Create a cross-section surface for Key-pad
(for Electronic control ) at a measured
distance from the Arm rest ankle point.
Create a single merged part by using Arm
rest and the key pad component.
Close the end of the Arm rest & Key-pad with
rounded end.
Design the door latch.
Design a Map-Pocket with the rounded
edges.
Case Study: Surface Creation