CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Create Complex Surfaces
Student Notes:
In this lesson, you will be introduced to the functionalities available in the Generative Surface Design workbench.
Lesson content:
Copyright DASSAULT SYSTEMES
Case Study: Surface Design Design Intent Stages in the Process Create the Complex Surface Geometry Perform Fillet Operations
Duration: Approximately 0.5 day
Copyright DASSAULT SYSTEMES
8-1
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Case Study: Surface Design
Student Notes:
The case study for this lesson is a simplified B pillar. The chassis section is a part of the Cradle frame sub-assembly.
Copyright DASSAULT SYSTEMES
The case study focuses on creation of surface features and performing surface operations that incorporate the design intent of the part.
Copyright DASSAULT SYSTEMES
8-2
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Design Intent The model of the simplified B pillar must meet the following design intent requirements: The main junction surface (A) must pass through the four section curves. D
• Create a multi-sections surface passing through the four section curves.
Length of the base junction surface (B) must be 700mm. • Create an extrude of Base_Junction_Curve.
Sharp edges must not be present between the main junction surface and the base junction surface. • Trim the surfaces and create an edge fillet of radius value 100mm.
C
A
B
Copyright DASSAULT SYSTEMES
The front pillar surface (C) and the back pillar surface (D) must pass through the respective guide curves. • Create sweep surfaces passing through two guide curves.
The result must be a single surface. • Move the final surface to the “Result” geometrical set.
Copyright DASSAULT SYSTEMES
8-3
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Stages in the Process 1
Use the following steps to create the model of the simplified B pillar: Create a Multi-Section surface.
2.
Fill the surface and create a join.
3.
Create an extruded surface.
4.
Apply fillets to the sharp edges.
5.
Create a sweep.
6.
Join the surfaces to get a single result.
3
5
4
Copyright DASSAULT SYSTEMES
1.
2
Copyright DASSAULT SYSTEMES
8-4
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Create the Complex Surface Geometry
Student Notes:
In this section, you will learn some to the common tools used to create surface geometry.
Use the following steps to create the simplified B pillar: 1.
Perform Fillet Operations
Copyright DASSAULT SYSTEMES
2.
Create the Complex Surface Geometry
Copyright DASSAULT SYSTEMES
8-5
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
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,
Copyright DASSAULT SYSTEMES
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).
Surface passing through the repeated sections
Copyright DASSAULT SYSTEMES
Spine Guide Profile
Profiles repeated in the planes
8-6
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating Swept Surface – Explicit Subtype Swept Surfaces are created by sweeping a profile along a spine. The spine, by default, is the first selected guide curve.
1
Use the following steps to create a simple explicit type Swept Surface: Select the Swept Surface icon. Select the profile. Select a guide curve. Click OK to complete the feature.
Copyright DASSAULT SYSTEMES
1. 2. 3. 4.
Copyright DASSAULT SYSTEMES
3
2
4
8-7
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Creating a Swept Surface – Reference Surface Option By default, a Swept Surface uses the mean plane of the spine as the surface the profile is swept along. A user-defined surface can also be used. Use the following steps to apply a reference surface to a Swept Surface feature:
Student Notes:
1 2 3
Copyright DASSAULT SYSTEMES
1. Select the With Reference Surface option from the dialog box. 2. Select the surface. 3. Enter an angle. This angle is measured between the profile and the reference surface.
Copyright DASSAULT SYSTEMES
2
8-8
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Swept Surface – Second Guide Explicit swept surfaces can also be created using a second guide curve.
1
Use the following steps to add a second guide curve to a Swept Surface feature: 1. 2. 3.
Copyright DASSAULT SYSTEMES
4. 5.
From the Subtype menu, select the With two guide curves option. Select the profile. Select the first guide curve. This guide curve, by default, will also act as the spine. Select the second guide curve. Click OK to generate the feature.
3
Copyright DASSAULT SYSTEMES
4
5
2 8-9
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Swept Surface - Spine A Spine can control the orientation of the profile as it sweeps along the guide curve(s). By default the first guide is used as the spine for the Swept feature.
1
If required, another element can be selected to act as the Spine. Use the following steps to change the spine: Click on the Spine field. Select the new element.
Copyright DASSAULT SYSTEMES
1. 2.
2
Copyright DASSAULT SYSTEMES
8-10
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Swept Surface - Relimiters By default, the Swept Surface will be created along the total length of the spine. Using points or planes the surface can be longitudinally reduced.
1 2
Use the following steps to relimit the swept surface: 1. 2. 3. 4.
Click on the Relimiter 1 field. Select the relimiting element. In this example, a point is selected. Click on the Relimiter 2 field. Select the second relimiting element. In this example, a plane is selected.
2
Copyright DASSAULT SYSTEMES
4
Copyright DASSAULT SYSTEMES
8-11
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating an Offset Surface (1/2) Use the Offset tool to create a surface offset from an existing surface.
1
Use the following steps to create an Offset Surface: 1. 2. 3. 4.
5.
2
3
5
4
6
Copyright DASSAULT SYSTEMES
6.
Select the Offset icon. Select the reference surface. Enter offset value. If necessary, select Reverse Direction to change the direction of the offset. Use the Both sides option to create offset surfaces on either side of the reference surface. Select Repeat object after OK to create several surfaces separated by the same offset distance.
Copyright DASSAULT SYSTEMES
8-12
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating an Offset Surface (2/2) Use the following steps to create an Offset Surface (continued): 7. 8.
Click OK. When the Repeat object after OK option is selected the Object Repetition dialog box appears. Enter the number of instances to be created. 9. The new instances will be created in a new open body. To create the instances in the existing open body, clear the Create in a new Open Body option. 10. Click OK to create the surfaces. The resulting offset surface is parallel to the reference surface.
8 9 10
Copyright DASSAULT SYSTEMES
Side View
Copyright DASSAULT SYSTEMES
8-13
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Fill Surface (1/2) Use the Fill Surface tool to create a surface inside a closed boundary. The boundary can consist of wireframe elements or edges of existing surfaces.
Copyright DASSAULT SYSTEMES
Use the following steps to create a fill surface: 1. Select the Fill icon. 2. Select the edges that will form the boundary. 3. Tangency can be applied at any boundary, by selecting the boundary from the Fill Surface Definition box and selecting the support surface. In this example tangency is applied to the last boundary. 4. Specify the type of continuity between the support surface and the fill surface. In this example Tangent continuity is selected.
Copyright DASSAULT SYSTEMES
1 2b
2c
2a 2d 3a 3b
4
8-14
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Fill Surface (2/2) 5
Use the following steps to create a fill surface (continued): 5. 6.
7.
If necessary, define a point though which the surface will pass. If necessary, edit the boundary by adding additional elements to the boundary, replace or remove existing elements or support surfaces. Click OK to generate the surface.
Copyright DASSAULT SYSTEMES
5
Copyright DASSAULT SYSTEMES
7
8-15
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Blend Surface (1/4) A blend surface is used to create a surface between two wireframe elements.
1
Use the following steps to create a blended surface: 1. 2. 3.
2 4
Copyright DASSAULT SYSTEMES
4. 5.
Select the Blend icon. Select the first curve. If required, select the support for the first curve. Select the second curve. If required, select the support for the second curve.
Copyright DASSAULT SYSTEMES
8-16
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Blend Surface (2/4) Use the following steps to create a blended surface (continued): 6.
If supports are specified, define the type of continuity for each side. Continuity can be defined as: a. b. c.
7.
Point Tangency Curvature
6 7
If required, select the Trim Support options. When selected, the support surfaces are trimmed to the curve and are assembled into the blended surface.
6b
6c
Copyright DASSAULT SYSTEMES
6a
Copyright DASSAULT SYSTEMES
8-17
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Blend Surface (3/4) Use the following steps to create a blended surface (continued): 8.
If supports are specified, you can define tangency between the blended surface borders and the support surface borders. Tangency can be defined as: a. b. c. d.
Both extremities None Start Extremity only End extremity only
8a
8b
Copyright DASSAULT SYSTEMES
Seco nd
Copyright DASSAULT SYSTEMES
er rd o tb rs Fi
8c
bord er
Second support
First support
8d
8-18
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Blend Surface (4/4) Use the following steps to create a blended surface (continued): 9.
If required, specify tension at the blend surface limits. Tension can be specified as: a. b. c. d.
9
Default Constant Linear S type
10. Click OK to generate the blend surface.
Changing Tension Surface 1
Copyright DASSAULT SYSTEMES
T4
Copyright DASSAULT SYSTEMES
T3
T2 T1
T1 Constant Surface 2
8-19
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Blend Surface: Curves Orientation The curves used must be oriented in the same direction:
Copyright DASSAULT SYSTEMES
One of the curves is oriented differently (use the arrow)
You get a twist:
Beware the curves orientation
Copyright DASSAULT SYSTEMES
8-20
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Blend Surface: Coupling points Define how to get from one curve to the other using coupling points:
Vertices and points correspondence
Coupling points defined
Copyright DASSAULT SYSTEMES
Without Coupling points definition
Copyright DASSAULT SYSTEMES
8-21
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Multi-Sections Surface (1/6) A surface is 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.
Adjacent Surface Guide curves
During a certain design situation, 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.
Sections curves
Copyright DASSAULT SYSTEMES
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.
Adjacent Surface
Copyright DASSAULT SYSTEMES
8-22
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Multi-Sections Surface (2/6) Section Curves
Section are the user-defined profile. A section can be a 2D or a 3D 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 MultiSection surface.
Guide Curve
Guide Curve to give the correspondence between these 2 vertices
Copyright DASSAULT SYSTEMES
Section Curves
Copyright DASSAULT SYSTEMES
8-23
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Multi-Sections Surface (3/6) Use the following step to create a Multi-Section Surface using other options (Guides, Spine, Relimitation, Canonical elements) 1.
Select the Multi-Sections Surface icon.
2.
Select the first section, second section and third section.
3.
Select tangent surfaces for first and last section.
4.
Ensure that the orientation of all the sections at closing points is same.
3
1
3 2
2
Copyright DASSAULT SYSTEMES
3
Copyright DASSAULT SYSTEMES
8-24
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Creating a Multi-Sections Surface (4/6) 5.
In the Guides tab, select the guide curves. The resulting surface will respect these guide curves.
6.
You can Replace, Remove or Add the guides during the edition of Multi-sections surface.
Student Notes:
5
6
Copyright DASSAULT SYSTEMES
5
Copyright DASSAULT SYSTEMES
8-25
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Creating a Multi-Sections Surface (5/6) 7.
In the Spine tab, select the spine. By default the spine is calculated automatically. The spine must be tangent continuous.
8.
You can Replace, Remove or Add the spine during the edition of Multi-sections surface.
Student Notes:
7
Copyright DASSAULT SYSTEMES
8
Copyright DASSAULT SYSTEMES
8-26
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Multi-Sections Surface (6/6) 9.
In the Coupling tab, select Ratio type. Depending on the sections configuration, you can select the suitable coupling type.
Copyright DASSAULT SYSTEMES
9
10. In the relimitation tab, you can choose to limit the Multi-sections Surface only on the Start section, only on the End section, on both, or on none. By default the multi-sections surface is relimited at start and end sections.
Copyright DASSAULT SYSTEMES
10
8-27
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise: Complex Surfaces Creation
Student Notes:
Recap Exercise 20 min
In this exercise, you will open an existing model and use the tools learned in this lesson to create a surface geometry necessary for the shell of a car door panel. To save time, simple wireframe and surface elements have already been created for you. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a Swept surface Create a Connect curve Create a Projection
Copyright DASSAULT SYSTEMES
Create a Boundary Create a Multi-Sections surface
Copyright DASSAULT SYSTEMES
8-28
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (1/11) 1.
Load Ex8A.CATPart. • Load Ex8A.CATPart. This part already has some curves and surfaces created for you. a. Notice all the wireframe elements have been created in a separate geometrical set. b. Ensure that the ‘Surfaces’ geometrical set is active.
2a 2b 2c 2d 2e 2f
Copyright DASSAULT SYSTEMES
2.
Create a swept surface. • Create a swept surface from a given profile and guide curve. This surface would form the inner panel of the door. a. b. c. d. e. f.
Click the Sweep icon. Select Explicit option. Select subtype With Two Guide Curves. Select Profile as ‘Section_1’. Select Guide curve 1 as ‘Parallel.1’ Select Guide curve 2 as an edge of the ‘OUTER PANEL WITH FLANGE’.
Copyright DASSAULT SYSTEMES
8-29
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (2/11) 2.
Create a swept surface (continued). g. h.
i.
Select anchoring type as Two Point Select the first anchor point at the intersection of the profile and first guide curve. Select the second anchor point at the intersection point of the profile and second guide curve.
j.
Select Relimiter 1 as ‘Plane.4’.
k.
Select Relimiter 2 as ‘Plane.1’.
2j 2k
Profile
Relimiter 1 Anchor Point 2
Copyright DASSAULT SYSTEMES
Guide Curve 1
Guide Curve 2
Anchor Point 1
Copyright DASSAULT SYSTEMES
8-30
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (3/11) 2.
Create a swept surface (continued). l.
Click OK to create a swept surface.
Start point Sweep.1
Copyright DASSAULT SYSTEMES
End point
Copyright DASSAULT SYSTEMES
8-31
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (4/11) 3.
Create a second swept surface. • Create a swept surface from a given profile and guide curve. This surface would form inner panel of the door. a. b. c. d. e. f.
3a
Click the Sweep icon. Select Explicit option. Select subtype With Two Guide Curves Select Profile as ‘Section_2’. Select Guide curve 1 as ‘Parallel.2’. Select Guide curve 2 as an edge of the ‘OUTER PANEL WITH FLANGE’.
3b
3c 3d 3e 3f Relimiting Planes
Guide Curve 2
Copyright DASSAULT SYSTEMES
Guide Curve 1
Copyright DASSAULT SYSTEMES
Profile
8-32
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (5/11) 3.
Create a second swept surface (continued). g. Select anchoring type as ‘Two Points’ h. Select the first anchor point at the intersection of the profile and first guide curve. h. Select the second anchor point at the intersection point of the profile and second guide curve. i. Select Relimiter 1 as ‘Plane.3’. j. Select Relimiter 2 as ‘Plane.2’.
Profile
3g 3h
Guide Curve 2
Anchor Point 2
Copyright DASSAULT SYSTEMES
Guide Curve 1
Anchor Point 1
Copyright DASSAULT SYSTEMES
Relimiter 1
8-33
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (6/11) 3.
Create a second swept surface (continued). k.
Click OK to create a swept surface. Sweep.2
End point
Copyright DASSAULT SYSTEMES
Start point
Copyright DASSAULT SYSTEMES
8-34
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (7/11) 4.
Create a 3D Guide curve. • Create a connect curve between the two end sections of the swept surface created in previous steps. This curve would be later projected on the panel surface and used as a guide curve to create a Multi-Sections surface. a. b. c. d. e. f. g. h.
4a
Click the Connect Curve icon. Select the vertex of the first section (as shown). The default curve is automatically selected. Specify the tension value to 3. Select the vertex of the second section (as shown). The default curve is automatically selected. Keep the tension value as default. Click OK to create a connect curve.
4b 4c 4d
4e
First Curve
4f
Copyright DASSAULT SYSTEMES
First Point
Copyright DASSAULT SYSTEMES
4g
Second Curve
4h
Second Point
8-35
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (8/11) 5.
Project the curve • Project the connect curve on the panel surface (Blue surface). Later you would use this projection as guide curve to create MultiSections surface a. b. c. d. e.
Click the Project icon. Select the connect curve to be projected. Select the OUTER PANEL WITH FLANGE surface (Blue surface) as support. Select ZX plane as projection direction. Click OK to create projection.
5a
5b 5c 5d
Copyright DASSAULT SYSTEMES
5e
Projected Curve
Copyright DASSAULT SYSTEMES
Connect Curve
8-36
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (9/11) 6.
Create a boundary. • Create a boundary of the swept surfaces. These boundaries would be later used as section curves to create Multi-Sections surface between two swept surface.
6b 6c
a. b.
•
Click the Boundary icon. Specify the propagation type as Point continuity. c. Select the edge of the swept surface (as shown). d. Select first and second limit on the highlighted curve. e. Click OK to create a boundary curve. Repeat the step to create a boundary for Sweep.1 surface.
6a
6d 6e
Boundary Sweep.1
Copyright DASSAULT SYSTEMES
Boundary
Copyright DASSAULT SYSTEMES
Sweep.1
8-37
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (10/11) 7.
Create a Multi-Sections surface. 7a • Create a Multi-Sections surface between the two swept surfaces. a. b. c. d. e. f. g.
h.
Click the Multi-Sections surface icon. Select the boundary of the first swept surface. Select the first swept surface as Tangent. Select the boundary of the second swept surface. Select the second swept surface as Tangent. Select Project.1 as first Guide. Select an edge of the OUTER PANEL WITH FLANGE as second Guide (as shown). Click on Coupling tab , Choose coupling type as Vertices.
Copyright DASSAULT SYSTEMES
7c
7d
7h
7e
7b
Copyright DASSAULT SYSTEMES
7i
7g
7f
8-38
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (11/11) 7.
Create a Multi-Sections surface. i.
8.
Click OK to create a Multi-Sections surface.
Close the part without saving it.
Sweep.1 Multi-section Surface
Copyright DASSAULT SYSTEMES
Sweep.2
Copyright DASSAULT SYSTEMES
8-39
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise Recap: Complex Surfaces Creation
Student Notes:
Create a Swept surface Create a Connect curve Create a Projection Create a Boundary
Copyright DASSAULT SYSTEMES
Create a Multi-Sections surface
Copyright DASSAULT SYSTEMES
8-40
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise: Multi-Sections Surface
Student Notes:
Recap Exercise 10 min
In this exercise, you will open an existing model consisting of wireframe and surface inputs. You will practice how to use the Multi-Sections surface tool. High-level instructions for this exercise are provided. By the end of this exercise you will be able to:
Copyright DASSAULT SYSTEMES
Create a Multi-Sections surface.
Copyright DASSAULT SYSTEMES
8-41
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (1/2) 1.
Load Ex8B.CATPart. • Load Ex8B.CATPart. This part already has some curves and surfaces created for you. a. Observe that the two sections (flat and formed sections) are in different geometrical sets. b. Create a geometrical set called ‘MultiSection’.
Create a Multi-Sections surface. • Create a Multi-Sections surface from a given profile. Use manual coupling to guide the surface.
Copyright DASSAULT SYSTEMES
2.
Copyright DASSAULT SYSTEMES
Coupling Points
Multi-Section Surface
8-42
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (2/2) 3.
4.
Hide the Multi-Sections surface created in the previous step.
Connect Curve
Create the Guide curves. • Create the guide curves between the two sections as shown. Line
Create a Multi-Sections surface. • Create a Multi-Section surface from a given profile. Use the guide curves created in the previous step.
6.
Close the part without saving it.
Copyright DASSAULT SYSTEMES
5.
Copyright DASSAULT SYSTEMES
8-43
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise Recap: Multi-Sections Surface
Student Notes:
Create a Multi-Section Sweep using coupling points Create Multi-Section surface using guide curves
Copyright DASSAULT SYSTEMES
Create a Multi-Section Sweep using coupling points
Copyright DASSAULT SYSTEMES
Create a Multi-Section Sweep using guide curves
8-44
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise: Complex Surfaces Creation
Student Notes:
Recap Exercise 20 min
In this exercise, you will create a thermal insulation cover using simple surfaces. High-level instructions for this exercise are provided.
By the end of this exercise you will be able to: Create a Multi-Sections surface Create a Sweep surface Create an Extrude surface
Copyright DASSAULT SYSTEMES
Create a surface Trim
Copyright DASSAULT SYSTEMES
8-45
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Do it Yourself (1/4) Load Ex8C.CATPart. • Load Ex8C.CATPart. This part already has some curves created for you.
2.
Analyze the model • Study the model along with the specification tree to understand the sequence of the model construction.
Copyright DASSAULT SYSTEMES
1.
Student Notes:
Copyright DASSAULT SYSTEMES
8-46
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (2/4) 3.
Create a main surface • In Geometrical Set ‘BASE SECTIONS’, create Multi-Sections surface using section 1 and 2 as Profiles and ‘Vertices’ as the coupling option.
Multi-Section using ‘Vertices’ option
Create rounded front wall • In Geometric Set ‘Rounded Surface’, create a sweep surface as shown using Profile and Guide. • Display the Split planes in the ‘Start data’ Geometrical Set. • Specify these planes as Relimiter 1 and 2 in the Sweep dialog box.
Copyright DASSAULT SYSTEMES
4.
Copyright DASSAULT SYSTEMES
8-47
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (3/4) 5.
Create upper Split surface • In Geometric Set ‘Split upper Surface’ create an extruded surface as shown. • In Geometric Set ‘Rounded Surface’ create the split as shown.
Copyright DASSAULT SYSTEMES
Extrude
Split
Copyright DASSAULT SYSTEMES
Split Rounded Wall
8-48
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Do it Yourself (4/4) Create Final surface • Create a Geometrical Set called ‘Screen’ under the father node of the thermal screen. • Create a trim between the main surface and the front wall surface • Rename the trim surface as ‘Screen’.
7.
Close the part without saving it.
Copyright DASSAULT SYSTEMES
6.
Student Notes:
Copyright DASSAULT SYSTEMES
8-49
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise Recap: Complex Surfaces Creation
Student Notes:
Create a Multi-Sections surface Create a Sweep surface Create an Extrude surface
Copyright DASSAULT SYSTEMES
Create a surface Trim
Copyright DASSAULT SYSTEMES
8-50
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Perform Fillet Operations In this section, you will learn how manipulate the surface geometry to create the final surface model.
Use the following steps to create the simplified B pillar : 1.
Perform Fillet Operations
Copyright DASSAULT SYSTEMES
2.
Create the Complex Surface Geometry
Copyright DASSAULT SYSTEMES
8-51
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Why Are Operations on Geometry Needed? After the basic surface geometry is created, it may be composed of construction elements that do not describe the finished shape. Operations such as trim, join, extrapolate, and transform are then performed to produce the required finished geometry. While performing operations, keep in mind the following key points: A.
Surface fillet operation
Elements involved in an operation are kept in the history of the operation, but are hidden.
Copyright DASSAULT SYSTEMES
B.
Operations are used to produce the finished geometry.
Copyright DASSAULT SYSTEMES
Join Operation
8-52
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Why Do You Need Joining Elements?
Student Notes:
Join operation is used when you want to concatenate or logically group the adjacent surfaces/wireframes together into a single element that can be used for future operations. It is a mechanical assembly of curves or surfaces to form a single entity in the tree. Advantages: 1.
Only one feature to select in the tree
2.
Some CATIA tools require only one element as input, in such cases Join operation can be selected. Bottle Top
1
Copyright DASSAULT SYSTEMES
2 3
Copyright DASSAULT SYSTEMES
Bottle Body
Bottle Bottom
8-53
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Joining Elements Use the following steps to join elements: 1. Click the Join icon. 2. Select the elements to be joined. 3. Set options as necessary. a.
b.
c. d.
Copyright DASSAULT SYSTEMES
e.
When the Check tangency option is selected, the join feature will only be created if all elements to be joined are tangent. When the Check connexity option is selected, the join operation will only be performed if the elements to be joined are connected. The Simplify the result option reduces the number of resulting elements. The Ignore erroneous elements option ignores the elements that do not allow the join to be created. The Merging distance is the maximum distance below which two elements are considered as one.
1
3b
3a 3c 3e
3d 4
2a
4. Click OK to complete the feature.
Copyright DASSAULT SYSTEMES
2b
8-54
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Joining Elements – Exclude Sub-Elements While joining elements you can exclude some sub-elements from the joined surface. Use the following steps to exclude subelements: 1. 2.
3. 4.
Select the elements to be joined. Select the Sub-Elements to Remove tab to exclude sub-elements from the joined surface. Select the elements to exclude. Check the Create join with subelements option to create a second join surface with the excluded sub-elements.
2
4
1a
Copyright DASSAULT SYSTEMES
1b
Copyright DASSAULT SYSTEMES
3
8-55
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Why Use Fillets?
Student Notes:
Copyright DASSAULT SYSTEMES
Fillets are used to remove sharp edges on the parts. Fillets, along with drafts, help to easily remove the material from molds. Fillets also help in reducing stress concentration in the parts.
Copyright DASSAULT SYSTEMES
8-56
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Fillet Extremities By creating fillets using surfaces, you can have a better control on the resulting elements. For example, the connection between the fillet and the support surface(s) can be customized to create the desired geometry. There are four options available to control the extremities of a fillet:
C
B
D
Copyright DASSAULT SYSTEMES
A. The Smooth option connects the fillet surface to the support surface with a tangency constraint. B. The Straight option connects the fillet with no tangency constraints. C. The Maximum option extends the fillet to the longest selected support edge. D. The Minimum option trim the fillet to the shortest selected support edge.
A
Copyright DASSAULT SYSTEMES
8-57
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Fillet Propagation By selecting a propagation mode, the edge on which fillet has to be created can be propagated automatically. There are three options available to control the propagation of a fillet: A. B.
C.
A
The Minimal option creates the fillet only on the selected edge. The Tangency option propagates the fillet to all adjacent tangency continuous edges.
Selected edge
Fillet created on selected edge
Selected edge
Fillet propagated on adjacent tangent continuous edges
Selected edge
Fillet propagated on edges generated by intersection
B
The Intersection Edges option propagates the fillet to all the edges that have been generated by intersecting the features
Copyright DASSAULT SYSTEMES
C
Copyright DASSAULT SYSTEMES
8-58
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a BiTangent Shape Fillet Shape fillets are used to create a fillet between two surfaces.
1
Use the following steps to create a BiTangent shape fillet: 1. 2. 3. 4. 5. 6. 7. 8.
Click the Fillet icon. Select the two surfaces/faces. Enter the radius value. Ensure the red arrows point towards the concave side for the fillet. If not, select on the arrow to change its direction. Specify the Extremities conditions. Clear the Trim Support options so that the supporting elements do not assemble into the fillet feature. Click OK to create the shape fillet.
6 3 5 7
Copyright DASSAULT SYSTEMES
2
Copyright DASSAULT SYSTEMES
4
2
8-59
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating an Edge Fillet The Edge Fillet tool is used to provide a transitional surface along a sharp edge of a surface. Similar to the Edge fillets in the Part design workbench, here also you can select edges or faces to be filleted.
1
Use the following steps to create an edge fillet: 1. 2.
2
Copyright DASSAULT SYSTEMES
3. 4. 5.
Click the Edge fillet icon. Select the edge(s) of the surface to be filleted. Enter the radius value. Specify extremity conditions. Click OK to generate the edge fillet.
3
Copyright DASSAULT SYSTEMES
8-60
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Variable Radius Fillet (1/2) Use the Variable Radius Fillet tool to create a fillet on a selected edge whose radius varies at selected points.
1
Use the following steps to create a variable radius fillet: 1. 2. 3.
4.
Click the Variable Fillet icon. Select one or more internal edges of a single surface. To add additional points, click inside the Point field then select anywhere on the edge to place the point, or select a preexisting point for better accuracy. Double-click on a radius value to modify it.
2
4
Copyright DASSAULT SYSTEMES
3
Copyright DASSAULT SYSTEMES
8-61
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Variable Radius Fillet (2/2) Use the following steps to create a variable radius fillet (continued): 5.
6.
Select the Variation as Cubic. A Cubic variation helps in the smooth transition of one radius into another, while the Linear variation helps in linear transition as shown. Click OK to complete the fillet. Linear mode
Cubic mode
Copyright DASSAULT SYSTEMES
5
Copyright DASSAULT SYSTEMES
6
8-62
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Face-To-Face Fillet The Face-Face fillet is used when there is no intersection between the selected faces or when there are more than two sharp edges between the faces.
1
Use the following steps to create a face-face fillet: 1. 2. 3. 4.
2
Click the Face-Face icon. Select the two faces. The fillet is created between these faces. The selected faces must belong to the same surface. Enter a radius value. Click OK to create the fillet.
2
3
Copyright DASSAULT SYSTEMES
4
Copyright DASSAULT SYSTEMES
8-63
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating a Tritangent Fillet A Tritangent fillet creates a transitional surface by removing one of three selected surface. The fillet surface is created tangent to the three selected faces.
1
2
Use the following steps to create a Tritangent fillet: Click the Tritangent Fillet icon. Select the two faces to keep. Select the face to remove. Click OK to complete the feature.
Copyright DASSAULT SYSTEMES
1. 2. 3. 4.
Copyright DASSAULT SYSTEMES
3
4
8-64
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Boundary Curves Use the Boundary tool to create boundary curves of internal or external surface edges. While defining the boundary, only one element needs to be selected. Using the correct propagation type, the remaining boundary is automatically determined. The propagation of a selected edge can be defined by: A.
Using the Complete boundary option, the selected edge is continued about the entire surface boundary.
B.
Using the Point continuity option, the selected edge is continued about the surface boundary until a point discontinuity is met.
C.
Copyright DASSAULT SYSTEMES
D.
Using the Tangent continuity option, the selected edge is propagated about the surface boundary until a tangent discontinuity is met. Using the No propagation option only the selected edge is used to create the boundary curve.
Copyright DASSAULT SYSTEMES
A
B
C
D
8-65
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Creating Boundary Curves Use the Boundary tool to create boundary curves of internal or external surface edges. Use the following steps to create a boundary curve: 1. 2. 3. 4.
5.
1
Click the Boundary icon. Specify the propagation type. Select the surface edge. If necessary, limit the boundary curve using points or vertices.
a. b. c. d.
Select in the Limt1 field Select the first limiting element Select in the limit2 field Select the second limiting element
2 4a
4c
5
Click OK to generate the boundary curve.
4b
Copyright DASSAULT SYSTEMES
3
Copyright DASSAULT SYSTEMES
4d
8-66
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Extracting an Edge from a Surface The Extract tool is used to extract subelements from a surface. Edges and surface faces can be extracted from the original surface.
1
To extract an edge from a surface use the following steps: 1. 2. 3. 4.
2
Click the Extract icon. Select a surface edge. Specify the propagation type. In this example, Tangent continuity is selected. Click OK to complete the extraction.
3
Copyright DASSAULT SYSTEMES
4
Copyright DASSAULT SYSTEMES
8-67
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Extracting a Face from a Surface You can also use the Extract tool to extract one or several faces of a surface with or without propagation. The same operations can be performed on solids using the extract tool.
1
Use the following steps to extract a face from a surface. 1. 2. 3.
Copyright DASSAULT SYSTEMES
4.
Click the Extract icon. Select the face. Specify the propagation type. In this example Point continuity is selected. Click OK to complete the extraction.
Copyright DASSAULT SYSTEMES
2
4
8-68
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
To Sum Up
Student Notes:
Copyright DASSAULT SYSTEMES
In the following slides you will find a summary of the topics covered in this lesson.
Copyright DASSAULT SYSTEMES
8-69
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Creating the Complex Surface Geometry
Student Notes:
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. A Spine can control the orientation of the profile as it sweeps along the guide curve' s. By default the first guide is used as the spine for the Swept feature. Complex surfaces can be created by following commands: Creating an Offset Surface: The new instances will be created in a new open body. Creating a Fill Surface: Surface can be filled inside closed boundary.
Copyright DASSAULT SYSTEMES
Creating a Blend Surface: A blend surface is used to create a surface between two wireframe elements. Creating a Multi-Section Surface: A surface is computed by passing through two or more consecutive sections along a spine is called Multi-Section surface.
Copyright DASSAULT SYSTEMES
8-70
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Perform Fillet Operations
Student Notes:
After the basic surface geometry is created, it may be composed of construction elements that do not describe the finished shape. Operations such as trim, join, extrapolate, and transform are then performed to produce the required finished geometry. Join operation is used when you want to concatenate or logically group the adjacent surfaces/wireframes together into a single element that can be used for future operations. Fillets are used to remove sharp edges on the parts. The Edge Fillet tool is used to provide a
Copyright DASSAULT SYSTEMES
transitional surface along a sharp edge of a surface.
Copyright DASSAULT SYSTEMES
8-71
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Main Tools Operations 1
Join: logically fills the gap between two surfaces.
2
Boundary: creates boundary curves of internal or external surface edges.
3
Extract: creates an extract sub elements from a surface.
1
2
3
Copyright DASSAULT SYSTEMES
Surfaces 4
Offset: creates a surface offset from an existing surface.
5
Sweep: creates a surface by sweeping a profile along a spine.
4
6
Fill: creates a surface inside a close boundary.
5
7
Multi-section surface: creates a surface passing through two or more consecutive sections along spine.
8
Blend: creates a surface between two wireframe elements.
Copyright DASSAULT SYSTEMES
6 7 8
8-72
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise: Surfaces Operations
Student Notes:
Recap Exercise 20 min
In this exercise, you will create a stamp feature on the thermal insulation cover using the surface tools. During the creation, you will practice the tools learnt in the previous steps. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a Revolve surface Create a surface Boundary Create a Fill surface Create a Join between surfaces
Copyright DASSAULT SYSTEMES
Create a surface Trim Create a Fillet between surfaces Create a pre-defined Cylinder surface Create an Intersection curve Create a Split surface
Copyright DASSAULT SYSTEMES
8-73
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Do it Yourself (1/10) 1.
Student Notes:
Load Ex8D.CATPart • Load Ex8D.CATPart. This part already has some curves and surface created in the previous exercise. a. Observe that the sketches required to create the surface data are provided in the model. b. You will be creating the surface in the respective geometrical sets while performing the steps.
Copyright DASSAULT SYSTEMES
c. Study the model along with the specification tree to understand the sequence of the model construction.
Copyright DASSAULT SYSTEMES
8-74
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (2/10) 2.
Create the Stamp 2a • Define in work object the ‘Stamp’ Geometrical set. • Show the Geometrical Set ‘Stamp Balance’. • Create a Revolve surface from the sketch and stamp axis. a. b. c. d.
2c
Click the Revolve icon Select ‘Stamp_Sketch’ as profile Select ‘Stamp Axis’ as axis. Click OK to create a revolve surface.
Hide all the sketches and the Geometrical Set ‘Stamp balance’.
2d
Copyright DASSAULT SYSTEMES
•
2b
Copyright DASSAULT SYSTEMES
8-75
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (3/10) 3.
Create the upper boundary of Stamp • Create the upper boundary of stamp surface. a. b. c.
4.
Click the Boundary icon Select upper edge of the surface as shown Click OK to create a boundary.
Create the upper surface of Stamp • Create the upper surface of stamp by filling the boundary created in the previous step. a. b.
3b
3c
4a
Click the Fill icon Select the upper boundary of the surface as shown Click OK to create a fill surface. Hide the upper boundary of the stamp surface.
Copyright DASSAULT SYSTEMES
c. d.
3a
Copyright DASSAULT SYSTEMES
4b
4c
8-76
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (4/10) 5.
Assemble the surfaces • Join the Revolve and Fill surfaces. a. b. c. d.
5a
Click the Join icon Select the revolve surface Select the fill surface Click OK to join the surfaces
5b 5c
Copyright DASSAULT SYSTEMES
5d
Copyright DASSAULT SYSTEMES
8-77
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (5/10) 6.
Merge the stamp surface with Screen surface • Trim the Stamp and Screen surface. a. b. c. d. e.
6a
Click the Trim icon. Select the Stamp surface. Select the Screen surface. Select the Other side option to keep the required surface. Click OK to trim the surface.
6b 6c
6d
Copyright DASSAULT SYSTEMES
6e
Copyright DASSAULT SYSTEMES
8-78
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (6/10) 7.
Blend the sharp edges. • Create an edge fillet on the intersecting edge. Specify the parameters as follows a. b. c. d. e. f. g. h.
7a
Click the Fillet icon Select the intersecting edge. Specify the fillet radius as 10mm Click OK to create a fillet. Click the Fillet icon. Select the intersecting edge. Specify the fillet radius as 5mm Click OK to create a fillet.
7c 7b
7d
7e 7g
Copyright DASSAULT SYSTEMES
7f
Copyright DASSAULT SYSTEMES
7h
8-79
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (7/10) 8.
Rename the surface as ‘Stamp Screen’ • Rename the surface as ‘Stamp Screen’ a. Right-click the last filleted surface. b. Select Properties c. In the Feature Properties tab, specify the name as ‘Stamp Screen’. d. Click OK to rename the surface.
8a 8b
Copyright DASSAULT SYSTEMES
8c
Copyright DASSAULT SYSTEMES
8d
8-80
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (8/10) 9.
Create a pass cut for a flexible device • Show the Geometrical Set ‘stamp Balance’. • Create a Cylinder. a. b. c. d. e. f.
9a
Click the Cylinder icon Select the axis extremity as point input. Select the axis as direction Specify the radius equal to 6.5mm Specify the length equal to 100mm at both the sides Click OK to create a cylinder.
9b 9c 9d 9e
Copyright DASSAULT SYSTEMES
9f
Copyright DASSAULT SYSTEMES
8-81
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (9/10) 10. Creating an intersecting curve • Create an intersection curve between the Cylinder and Stamp Screen surface a. b. c. d.
10a
Click the Intersection icon. Select the Cylinder surface. Select the Stamp Screen surface. Click OK to create an intersecting curve.
10b 10c
10b
10d
Copyright DASSAULT SYSTEMES
10c
Copyright DASSAULT SYSTEMES
8-82
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (10/10) 11. Create a passing hole on the Stamp Screen surface • Create a split on the Stamp Screen surface using the intersection curve. a. b. c. d.
Click the Split icon. Select the Stamp Screen surface. Select the intersection curve. Click OK to split a hole on the surface.
11a 11c
11b
Copyright DASSAULT SYSTEMES
12. Prepare the final data. • Hide the Intersection curve. • Rename the Split surface as ‘Screen Finished’. • Close the part without saving it.
Copyright DASSAULT SYSTEMES
11d
8-83
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise Recap: Surfaces Operations
Student Notes:
Create a Revolve surface Create a surface Boundary Create a Fill surface Create a Join between surfaces Create a surface Trim Create a Fillet between surfaces Create a pre-defined Cylinder surface Create an Intersection curve
Copyright DASSAULT SYSTEMES
Create Split surface
Copyright DASSAULT SYSTEMES
8-84
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise: Surface Delimitation
Student Notes:
Recap Exercise 40 min
In this exercise, you will open an existing model and use the tools learned in this lesson to create a shape of a door using a surface. To save time, simple wireframe and surface elements have already been created for you. Detailed instructions for this exercise are provided for all new topics. By the end of this exercise you will be able to: Assemble the surface Define the upper/lower shape of the door
Copyright DASSAULT SYSTEMES
Finalize the door
Copyright DASSAULT SYSTEMES
8-85
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Do it Yourself (1/17) 1.
Student Notes:
Load Ex8E.CATPart. • Load Ex8E.CATPart. This part already has some curves and surfaces created for you. Study and organize the specification tree. a. Observe that all the wireframe and surface elements have been created in a separate geometrical set. b. Create a new geometrical set called ‘UPPER_DOOR_SHAPE’ c. Inside this Geometrical Set, create two geometrical sets called ‘Surface’ and ‘Wires’.
Copyright DASSAULT SYSTEMES
2.
Assemble the surfaces • Define in work object the ‘Surface’ Geometrical Set. • Join the five surface in the geometrical set ‘UPPER_INPUT_SURFACE’. a. Click the Join icon. b. Select the surfaces to be joined (Corner, Front blend, Rear blend, Upper and side). c. Click OK to create a join. d. Rename the Join surface as ‘Surf1’.
Copyright DASSAULT SYSTEMES
8-86
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (2/17) 3.
Create an offset curves • Define in work object the ‘Wires’ Geometrical Set. • Hide the “LOWER_INPUT_SURFACES” for better visualization • Create a parallel curves and Corner. a. b. c. d. e. f. g.
3a
3c
Click the Parallel icon. Select the CURVE_UPPER_TRIM. Select ‘surf1’ as the Support. Specify the offset value equal to 50mm. Select the Reverse Direction if required. Click OK to create Parallel curve. Rename Parallel curve as ‘CURVE UPPER OFFSET’.
3d
3e
Copyright DASSAULT SYSTEMES
3f
Copyright DASSAULT SYSTEMES
8-87
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (3/17) 3.
Create an Side offset curve (continued) • Create a parallel curve. h. i. j. k. l. m. n.
3h
Click the Parallel icon. Select the CURVE SIDE TRIM. Select ‘Surf1’ as the Support. Specify the offset value equal to 50mm. Select the Reverse Direction if required. Click OK to create a Parallel curve. Rename the Parallel curve as ‘CURVE SIDE OFFSET’.
3j 3k
3l
Copyright DASSAULT SYSTEMES
3m
Copyright DASSAULT SYSTEMES
8-88
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (4/17) 4.
Create a Corner on support • Create a Corner curve. a. b. c. d. e.
4a
Click the Corner icon. Select the first offset curve Select the second offset curve Select the ‘Surf1’ as Support Specify the Radius value equal to 50mm. Select Next Solution to choose the required solution. Click OK to create Corner curve. Rename Corner curve as ‘SIDE CORNER’.
f. g. h.
4d 4e 4g
Copyright DASSAULT SYSTEMES
4c
4b
Copyright DASSAULT SYSTEMES
8-89
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (5/17) 5.
Create curves • Create an intersection between Plane.1 and SIDE CORNER. Create a spline on support to connect “SIDE_CORNER” and “CURVE_FRONT”. Create a Join. a. b. c. d.
Click the Intersection icon. Select the SIDE CORNER curve. Select Plane.1. Click OK to create an intersection.
e.
Rename the point as ‘INTERSECTION 1’.
5a
5b 5c
Copyright DASSAULT SYSTEMES
5d
Copyright DASSAULT SYSTEMES
8-90
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (6/17) 5.
Create Curves (continued) f. g. h. i. j.
k. l.
Show CURVE FRONT. Click the Spline icon. Select the end point of CURVE_FRONT as the first input point Select INTERSECTION 1 Ensure that the arrow is pointing in the correct direction. If it is not, then click on the arrow to change its direction. Select Surf1 as support surface Click OK to create the spline.
5g
5h 5i
5k
Copyright DASSAULT SYSTEMES
5l
Copyright DASSAULT SYSTEMES
8-91
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (7/17) 5.
Create Curves (continued) m. n. o. p.
Click the Trim icon. Select the Spline curve. Select the SIDE CORNER. Select Other side option if required.
q.
Click OK.
5m
5p
5n
5q
Copyright DASSAULT SYSTEMES
5o
Copyright DASSAULT SYSTEMES
8-92
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (8/17) 5.
Create Curves (continued) 5r
r. s. t. u. v.
Click the Join icon. Select the trimmed curve. Select the CURVE FRONT surface. Click OK to join the surfaces. Rename the Join as INTERNAL CURVE.
5s
5u
Copyright DASSAULT SYSTEMES
5t
Copyright DASSAULT SYSTEMES
8-93
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (9/17) 6.
Create Corner on support • Create a Corner curve between CURVE UPPER TRIM and CURVE SIDE TRIM. a. b. c. d. e. f.
6a
Click the Corner icon. Select the CURVE UPPER TRIM. Select the CURVE SIDE TRIM. Select the ‘Surf1’ as support surface. Specify the Radius value equal to 50mm. Click OK to create Corner curve. 6d 6c
6e
6b
Copyright DASSAULT SYSTEMES
6f
Copyright DASSAULT SYSTEMES
8-94
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (10/17) 6.
Create Corner on support (continued) g. h. i. j. k. l. m. n. o.
Click the Boundary icon. Select the edge of the surface as shown. Click OK to create a boundary. Click the Corner icon. Select the previously created corner and boundary. Select the ‘Surf1’ as support surface. Specify the Radius value equal to 50mm. Click OK to create Corner curve. Rename the corner curve as EXTERNAL CURVE. Define in work object the ‘Surfaces’ Geometrical Set.
Copyright DASSAULT SYSTEMES
p.
6g
Copyright DASSAULT SYSTEMES
6h
6i
6j
6l
6k
6m 6n
8-95
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (11/17) 7.
Create a surface split • Split the surface surf1 using curves ‘EXTERNAL 7a CURVE’ and ‘INTERNAL CURVE’. a. b. c. d. e. f. g.
Click the Split icon. Select the Surf1 surface. Select the EXTERNAL CURVE. Select the INTERNAL CURVE. Specify the side to be kept by selecting Other side option, if required. Click OK to split the surface. Rename the split as UPPER SHAPE.
Copyright DASSAULT SYSTEMES
7c
Copyright DASSAULT SYSTEMES
7b
7e
7d
7f
8-96
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (12/17) Create the Lower Door Shape: 8.
Create the Geometrical Set • Create three geometrical sets as shown. a.
9.
b.
Create a new geometrical set called ‘LOWER_DOOR_SHAPE’ Inside this geometrical set, create two other geometrical sets called ‘Surface’ and ‘Wires’.
c.
Show the surface ‘Lower’.
Create wireframe elements • Create the four boundary elements at the shown edges of Surf1 surface in “Wires” Geometric Set.
Copyright DASSAULT SYSTEMES
a. b. c. d.
e.
Double-click the Boundary icon. Select the edge of the surface ‘Lower’. Click OK to create a first boundary. The boundary dialog box reappears, repeat the steps and create the other three boundaries as shown. Rename the boundaries as CB1, CB2, CB3 and CB4.
Copyright DASSAULT SYSTEMES
8a 8b
8c 9a CB4
CB1
9c
CB3
CB2
8-97
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (13/17) 9.
Create wireframe elements (continued) f. g. h.
Copyright DASSAULT SYSTEMES
i. j. k.
Double-click on the Point icon. Select the Curve as EXTERNAL CURVE Select the Point type as On curve option. Specify the Ratio value as 0 Click OK to create a point. Repeat the steps to create a point on the other end.
Copyright DASSAULT SYSTEMES
9f
9h 9g
9i
9j
8-98
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (14/17) 9.
Create wireframe elements (continued) l. m. n. o. p. q.
r.
9l
Double-click on the Parallel icon. Select the Curve as CB1. Select ‘Lower’ as the Support. Select Point.1 as the Point. Click OK to create a Parallel curve. Repeat the steps to create a second parallel curve from CB3 passing through the second point created in the previous step. Rename both the Parallel curves as ‘CB1_OFFSET’ and ‘CB3_OFFSET’ respectively.
9m 9n
9o
Copyright DASSAULT SYSTEMES
9p
Copyright DASSAULT SYSTEMES
8-99
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (15/17) 9.
Create wireframe elements (continued) s.
t.
Create a parallel curve at a distance of 50mm from CB2 curve on the ‘Lower’ surface. Rename the Parallel curve as ‘CB2_OFFSET’.
10. Create a Corner on support • Create a Corner curve between CB1_OFFSET, CB2_OFFSET and CB3_OFFSET curves.
Copyright DASSAULT SYSTEMES
a. b. c. d. e. f. g.
h.
Double-click on the Corner icon. Select the Element 1 as CB1_OFFSET. Select the Element 2 as CB2_OFFSET Select the ‘Lower’ surface as Support Specify the Radius value equal to 50mm. Click OK to create Corner curve. Repeat the steps to create a corner curve of 50mm radius between the resultant curve andCB3_OFFSET. Rename the resultant curve as ‘DOOR_LOWER_SHAPE_BOUNDARY’
Copyright DASSAULT SYSTEMES
10b 10c 10d 10e 10f 10h
8-100
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (16/17) 11. Create a surface split • Define in work object the ‘Surfaces’ Geometrical Set which is inside LOWER_DOOR_SHAPE. • Split the surface ‘LOWER’ using the curve ‘DOOR_LOWER_SHAPE_BOUNDARY’. a. b.
Click the Split icon. Select ‘LOWER’ as the Element to cut.
c.
Select ‘’DOOR_LOWER_SHAPE_BOUNDARY’
d.
Specify the side to be kept by selecting Other side option, if required. Click OK to split the surface. Rename the split as ‘LOWER SHAPE’.
e. f.
11a
11b 11c
as Cutting elements.
11d
Copyright DASSAULT SYSTEMES
11e
Copyright DASSAULT SYSTEMES
8-101
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (17/17) 12. Create the final door surface • Create a new Geometrical Set called ‘Door’ • Assemble the UPPER_SHAPE and LOWER_SHAPE of the door. a. b. c. d. e.
12a
Click the Join icon. Select ‘UPPER_SHAPE ’ surface as Elements to Join Select ‘‘LOWER_SHAPE’ surface as Elements to Join Click OK to join the surfaces to form a single door surface. Rename the result as ‘DOOR’.
12b 12c
Copyright DASSAULT SYSTEMES
12d
Copyright DASSAULT SYSTEMES
8-102
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise Recap: Surface Delimitation
Student Notes:
Assemble the surface Define the upper/lower shape of the door
Copyright DASSAULT SYSTEMES
Finalize the door
Copyright DASSAULT SYSTEMES
8-103
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise: Boss and Flange Creation
Student Notes:
Recap Exercise 30 min
In this exercise, you will create a flange surface of the wheel arch and add the boss. High-level instructions for this exercise are provided.
By the end of this exercise you will be able to: Create the flange surface Create the boss surface
Copyright DASSAULT SYSTEMES
Relimit the surfaces using the main surface
Copyright DASSAULT SYSTEMES
8-104
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (1/6) Load Ex8F.CATPart. • Load Ex8F.CATPart. This part already has some curves and surfaces created for you.
2.
Create construction elements for a flange surface • Define in work object the ‘Reference Elements’ Geometrical Set. • Join all the surfaces available in the ‘WING_SURFACE’ Geometrical Set. Specify the Merging distance as 0.04mm • Join the surface 8,9 and 10 available in the ‘WHEEL_ARCH_STUDY_AREA’ Geometrical Set. Specify Merging distance as 0.04mm
Copyright DASSAULT SYSTEMES
1.
Copyright DASSAULT SYSTEMES
Join 1
Join 2
8-105
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (2/6) Create a flange surface • Create a Geometrical Set called ‘Flange_Surface’ under the father node of the WHEEL_ARCH. • Create the intersection of the two join surfaces created in the previous step. • Rename the intersection as C1 • Create a parallel curve from C1 at a distance of 15mm using the first join surface as the support element. • Rename the parallel curve as C2 • Split C2 between two planes ‘Plane X=-310’ and ‘Plane 2’. • Rename the Split as C3 • Create a vertical line of length 20mm from one extremity of ‘C3’.
Copyright DASSAULT SYSTEMES
3.
Copyright DASSAULT SYSTEMES
C2
C1
Vertical Line
8-106
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (3/6) 3.
Create a flange surface (continued) • Create a line normal to surface ‘Join.2’ from the other extremity of ‘C3’ (of default length, later used for reference only) • Create an angle line from the same point with reference to the previous line at 30deg angle on the XZ plane • Project the vertical line and the angle line on the Join.1 surface • Rename these projection curves L1 and L2 respectively • Create a Corner curve of radius 4mm between L1 and C2 • Create a Corner curve of 4mm radius between the resulting curve and L2 • Rename the resulting curve as ‘CORNER’. • Project the curve “CONTOUR” on Join.1
L2
L1
CORNER
Copyright DASSAULT SYSTEMES
Project
Copyright DASSAULT SYSTEMES
8-107
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (4/6) 3.
Create a flange surface (continued) • Create a Corner of radius 4mm between this projection and the offset curve C2. Do not trim the C2 curve while creating this corner. Repeat the corner operation twice to get the corner on both the sides of the projected curve. • Hide the C2 curve. • Trim the previous corner with ‘CORNER’ curve. • Split ‘Join.1’ using the last trim and ‘C3’.
Last trim
Projected Curve
Projected curve is cornered at both end
Copyright DASSAULT SYSTEMES
C3
Copyright DASSAULT SYSTEMES
Cornered curve trimmed with ‘CORNER’ curve.
8-108
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (5/6) 4.
Copyright DASSAULT SYSTEMES
5.
Relimit the surfaces • Trim Join.2 and the last created split • Split the resultant surface between PLANE2 and Surface.7 • Trim the previous corner with ‘CORNER’ curve. • Split ‘Join.1’ using the last trim and ‘C3’.
Relimited surface after split operation
Intersect
Create a Blend cut • Intersect ‘PLANE X=-314’ and ‘PLANE.3’. • With intersection as an axis, create a cylinder (default length) and a radius of 4mm. • Split the main surface with this cylinder • Join this split with the remaining surfaces of ‘WHEEL_ARCH_STUDY_AREA’. Specify the Merging distance as 0.04mm
Cylinder
Joint surface
Copyright DASSAULT SYSTEMES
Cylinder split with main surface
8-109
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Do it Yourself (6/6)
Copyright DASSAULT SYSTEMES
6.
Create a revolved shape of the boss • Create a Geometrical Set called ‘Bosses’ under the father node of the WHEEL_ARCH. • Create revolution surfaces using ‘L3 stamp axis’ as axis and the 2 lines ‘L1 40°top’ and ‘L2 40°down’ around a full circle. • Create a 5 mm shape fillet using the two revolution surfaces and the blue surface called ‘Boss surface’. • Create a trim between the upper fillet surface and the main join. • Create a fillet of 10mm on the upper edge of the surface. • Similarly, create a trim between lower filleted surface and the main surface. • Create a fillet of 4mm on the edge that is formed (shown).
Revolved surface filleted with ‘BOSS SURFACE’
Apply 4mm fillet on this edge
Copyright DASSAULT SYSTEMES
Upper revolve surface trimmed with main surface
Fillet the upper edge of the trimmed cutout
8-110
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Exercise Recap: Boss and Flange Creation
Student Notes:
Create the flange surface Create the boss surface
Copyright DASSAULT SYSTEMES
Relimit the surfaces using the main surface
Copyright DASSAULT SYSTEMES
8-111
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces Student Notes:
Case Study: Create Complex Surfaces Recap Exercise 30 min
In this exercise, you will create a case study model. Let us recall the design intent of this model: The main junction surface (A) must pass through four section curves.
A
The length of the base junction surface (B) must be 700mm. Sharp edges must not be present between the main junction surface and base junction surface.
Copyright DASSAULT SYSTEMES
The front pillar surface (C) and the back pillar surface (D) must pass through the respective guide curves.
C
D
B
The result must be a single surface
Using the techniques you have learned so far, create the model without detailed instructions.
Copyright DASSAULT SYSTEMES
8-112
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Do It Yourself: Create the Simplified B Pillar
Student Notes:
Copyright DASSAULT SYSTEMES
Load Start_CaseStudy8.CATPart and modify the model using the information below.
Copyright DASSAULT SYSTEMES
8-113
CATIA V5 Automotive - Body Lesson 8: Create Complex Surfaces
Case Study Recap: Simplified B Pillar
Student Notes:
Create a Multi-Section surface. Fill the surface and create a join. Create an extruded surface. Apply fillets to sharp edges. Create a sweep.
Copyright DASSAULT SYSTEMES
Join the surfaces to get a single result.
Copyright DASSAULT SYSTEMES
8-114
