CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Advanced Solid Features
Student Notes:
In this lesson you will learn how to create a advanced solid features.
Lesson Contents:
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Case Study: Advanced Solid Features Design Intent Stages in the Process Transform a Body Create Ribs and Slots Create Complex Sketch-Based Features Create Advanced Drafts
Duration: Approximately 0.5 day
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Case Study: Advanced Solid Features
Student Notes:
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The case study for this lesson is the Anti-Roll Bar used in the Front Suspension and Engine assembly as shown below. The Anti-Roll Bar is a part of the Anti-Roll Bar system sub-assembly. The case study focuses on the creation of a tubular part based on a non-planar guideline and created with non-uniform sections.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Design Intent The Anti-Roll Bar must meet the following design requirements: The diameter must be 20mm. The minimum bend radius must be 20mm.
A
Link bar hole diameter (A) must be 10mm.
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Material width around the link bar hole diameter must be 7.5mm.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Stages in the Process
Student Notes:
The following steps will be used to create the Anti-Roll Bar : 1. Open an existing part. 2. Create ‘Rough’ and ‘Hole’ Bodies. 3. Create rib, pad and multi-sections solid in ‘Rough’. 4. Create a hole in ‘Hole’ body. 5. Assemble all bodies to PartBody.
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6. Save and close the document.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Transform a Body In this section, you will understand what transformations are and how to apply them to features in a part.
Use the following steps to create the Anti-Roll Bar: 1. 2. 3.
Create Ribs and Slots. Create Complex SketchBased Features Create Advanced Drafts.
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4.
Transform a Body.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Introduction to Transformations As you create a model, you may need to occasionally move the bodies. This is accomplished using transformations. These transformations enable you to move a body by translating it along an axis, rotating it round an axis, or moving it symmetrically about a plane.
A
B
C
D
A
There are four types of transformation features: A. B. C. D.
Translate Rotate Symmetry Axis To Axis {Not covered in this course}
B
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C
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Using Transformations
Student Notes:
Transformations are used in a multi-body context. Transformations are required when you have some geometry that has been created in one location and which needs to be moved or rotated into a specific position.
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A typical example would be a body representing a standard tool set which is copied into your model and then needs to be positioned with respect to your design.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Translation (1/2)
Student Notes:
The Translation tool allows you to move a body in a linear direction. You may define the translation vector in the following three ways:
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A. Direction, distance • Moves the body along a linear direction defined by a reference, such as an edge or a plane. B. Point to point • Moves the body from one point to another. The relative position of the body with respect to the endpoint is the same, as it was with respect to the start point. C. Coordinates • Moves the body with respect to a Cartesian coordinate system.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Translation (2/2) Use the following steps to perform a Direction, distance translation:
1
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1. Select the Translation icon. 2. A warning message appears. Click Yes. 3. Define a direction by selecting an axis, line, plane or planar surface. In this example, the indicated edge was selected to define the direction. 4. Specify a distance value. 5. Click OK.
2
3
4
More information is available in RecommendationsDifferences in Transformations
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Rotation An axis and an angle are required to define a Rotate transformation.
1
Use the following steps to rotate a body: 1. Select the Rotation icon. 2. A warning message appears. Click Yes. 3. Define the Axis reference by selecting a line or axis. For example, the indicated edge was selected as the rotation axis. 4. Specify the rotation angle. 5. Click OK.
2
3
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More information is available in RecommendationsDifferences in Transformations
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Symmetry (1/2) The Symmetry option enables you to mirror a body without duplicating it. Only a single reference element is required. Any of the following may be used as a reference:
A. B. C.
A
Plane or plane surface Segment Point
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B
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C
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Symmetry (2/2) Use the following steps to apply symmetry on a body: 1. Select the Symmetry icon. 2. A warning message appears. Click Yes. 3. Select a reference. In this example a plane was selected. 4. Click OK.
1
2
4
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3
More information is available in RecommendationsDifferences in Transformations
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Scaling The Scaling option allows to shrink or expand an entire body based on a single point as a reference. Use the following steps to create a Scaling feature: Select the Scaling icon. Select the reference point. Modify the scaling ratio. Click OK.
2 3
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1. 2. 3. 4.
1
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Recommendations for Transformations
Student Notes:
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You will learn about the specific methods and recommendations about Transformations.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Differences in Transformations
Student Notes:
Transforming a body can be done using the Transformations tools or using the compass. How to use the compass to move items will be discussed later in the course. When you select any transformation tool, a Question dialog box will be displayed (as shown below).
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Selecting Yes will proceed to the use of the Transformations as selected. The message in the dialog box reminds you that you can also transform a body using the Compass. This is useful since you cannot use a Transformation tool to transform sketched geometry.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Scaling the Part to Define Mold “Shrink”
Student Notes:
A part gets scaled differently depending on the type of element used as the reference. If a point is used, the scaling is done using the same scaling ratio in all three directions.
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In the design of the model for an injection molded plastic part, the design part will often be scaled up, to account for material shrinkage. Depending on the material, the part may shrink by different amounts in each direction.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Create Ribs and Slots In this section, you will learn some sketchedbased features available in the Part Design workbench.
Use the following steps to create the Anti-Roll Bar: 1.
Transform a Body.
3.
Create Complex SketchBased Features Create Advanced Drafts.
2.
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4.
Create Ribs and Slots.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
What are Ribs and Slots ?
Student Notes:
A rib is a positive (i.e., add material) solid that is generated by sweeping a profile along a center curve. A slot is a negative (i.e., subtract material) solid that is generated by sweeping a profile along a center curve. To create a rib, you must have the following: The planar profile which can be an open or closed loop sketch.
B.
The center curve which can be a planar sketch or a non-planar continuous wireframe element.
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A.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
When Should Ribs and Slots Be Used ?
Student Notes:
Consider using a rib or slot feature whenever you need to extrude a profile along a nonlinear trajectory. Both these tools enable you to create complex walls as a single feature. Without these tools you would have to create many other features (such as pads and pockets) to make the same wall.
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Ribs can be used to create a pipe feature by sweeping two closed loop profiles, created in the same sketch, along a center curve.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Creating a Rib 4
Use the following steps to create a rib feature:
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1. Click the Rib icon. 2. Select the profile to be swept. 3. Select the center curve to sweep the profile along. In this example, the center curve is a 3D curve created in the Wireframe and Surface Design workbench. 4. Select the appropriate Profile Control option. In this example, Pulling direction is selected as the profile control and the top surface of the base feature is selected as the reference. 5. Click OK to complete the rib feature.
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2
1
4
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Creating a Slot Use the following steps to create a slot feature: 1. 2. 3. 4.
5.
3
Click the Slot icon. Select the profile to be swept. Select the center curve to sweep the profile along. Select the appropriate Profile Control option. In this example, the default option, Keep Angle is selected. Click OK to complete the slot feature
2 1
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Rib and Slot Options (1/2) Profile control and Merge ends options can be used to help control the rib or slot. The profile of the feature is controlled using the options from the Profile control menu. A.
B.
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C.
The Keep Angle option maintains a constant angle between the profile sketch support and the tangent of the center curve. The Pulling Direction option causes the profile to be swept along the center curve with respect to a specified direction. The direction can be defined using a plane or an edge. The Reference Surface option causes the profile to remain at a constant angle with respect to a selected reference surface.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Rib and Slot Options (2/2) Profile control and Merge ends options can be used to help control the rib or slot (continued). The Merge slot’s ends and Merge rib’s ends options can be used to extend or shorten the feature to its proper wall. A.
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B.
When the option is cleared the feature terminates at the end of the center curve. In the example shown, the feature does not fully extend to the edge of the base feature when the option is cleared. When the option is selected, the feature is extended or shortened to blend into the existing material. In the example shown, the profile is extended to fully intersect the base feature.
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A
B
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise: Part Design Transformations
Student Notes:
Recap Exercise 15 min
In this exercise, you will use the transformation techniques learned in this lesson to manipulate a robot hand part. The PartBody will be transformed with respect to the part origin. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a part symmetry Create a part rotation Create a part scale
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Cut and paste a feature between two parts
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (1/5) 1. Load Ex8A.CATPart. Load Ex8A.CATPart.
1
2. Perform a Symmetry operation. Use the Symmetry tool to create a left hand from the existing part. Use the ZX plane as the symmetry plane.
2a
2b
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a. Click the Symmetry icon. b. Select Yes from the prompt that asks if you want to keep the transformation specifications.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (2/5) 2. Perform a Symmetry operation (continued). c. Right-click on the reference field of the Symmetry Definition window and select ZX Plane. d. Click OK to complete the symmetry.
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2c
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (3/5) 3. Perform a Rotation operation. Rotate the left hand of the robot to point the thumb upwards.
3c
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a. Click the Rotation icon. b. Click Yes from the prompt that asks if you want to keep the transformation specifications. c. Right-click the Axis field and with the contextual menu select the X Axis. d. Enter [180deg] for the rotation angle. e. Click OK to complete the rotation.
3a
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (4/5) 4. Copy and paste a feature from another model. Load Ex6Dreference.CATPart and copy the mounting pocket feature. Paste it into the current model.
4b
a. Search and load
Ex6Dreference.CATPart.
b. From the specification tree, select the Pocket.1 feature and click Copy from the contextual menu. c. Switch window and make the Ex6D.CATPart active. d. Select the mounting surface of the robot’s hand and click Paste from the contextual menu. e. Click the Update icon if necessary to see the copied feature.
4d 4d
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4e
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (5/5) 5. Perform a Scale operation. Double the size of the robot hand using the Scale tool.
5a
a. Click on the Scaling icon. b. Select the coordinate system origin as the scaling reference. c. Enter [2] as the scaling Ratio. d. Click OK to complete the Scaling.
5b
5c
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5d
6.
Close the file without saving it.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise Recap: Part Design Transformations
Student Notes:
Perform a symmetry on a part. Copy and paste a feature from another part. Perform a rotation on the part.
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Scale the part
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise: Rib and Slot
Student Notes:
Recap Exercise 15 min
In this exercise, you will create a new model and use the tools learned in the lesson to create a rib and a slot feature. High-level instruction is provided for this exercise. By the end of this exercise you will be able to: Create a Rib Feature
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Create a Slot Feature
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (1/4)
Student Notes:
1. Create a new part file. • Create a new part file called Ex8B.
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2. Create the center curve sketch. • Create a positioned sketch as shown for the center curve. • Rename the sketch to [Center Curve].
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (2/4) Create a reference plane. • Create an offset plane as shown.
4.
Create a profile sketch for the rib. • Create a positioned sketch as shown for the rib profile.
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3.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (3/4) Create the rib feature. • Use the center curve and profile sketch to create a rib feature.
7.
Create a profile sketch for the slot. • Create a positioned sketch as shown for the slot profile.
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5.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (4/4) Create a slot feature. • Create a slot feature using the sketch created in the last step as the profile and the Center Curve sketch as the trajectory.
9.
Close the file without saving it.
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8.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise Recap: Rib and Slot
Student Notes:
Create a rib
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Create a slot
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Create Multi-Section Solids In this section, you will learn some complex sketched-based features available in the Part Design workbench.
Use the following steps to create the Anti-Roll Bar: 1. 2.
Transform a Body. Create Ribs and Slots.
4.
Create Advanced Drafts.
Create Complex Sketch-Based Features
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3.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Multi-Sections Solid
Student Notes:
A multi-sections solid can be a positive (i.e., add material) or a negative (i.e., subtract material) solid that is generated by two or more planar profiles swept along a spine. A common use of multi-sections solids is to create complex solids and transition geometry between two existing solids.
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Like multi-sections solids, removed multi-sections solids are used to subtract a transitional surface from an existing solid.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Multi-Sections Solid: Closing Point and Orientation (1/4)
Student Notes:
While defining a multi-sections solid, the closing points are displayed on a vertex in each of the selected profiles. These closing points indicate how the system will connect the vertices. The directional arrow indicates the direction of the next aligned vertices. Ensure that the arrow points in the same direction for each section.
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The closing points must be aligned for proper orientation of the sections. The multi-sections solid will become twisted if the closing points are not aligned.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Multi-Sections Solid: Closing Point and Orientation (2/4) Use the following steps to replace the closing point location: 1. 2. 3. 4.
Right-click on the existing closing point. Click Replace from the pop-up menu. Select the replacing vertex. To change the direction of the arrow, click on the arrow.
2
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Multi-Sections Solid: Closing Point and Orientation (3/4) If there is no vertex in the required location for the closing point, you can create a closing point while in the feature operation. Use the following steps to create a closing point: 1. 2. 3. 4.
2
Right-click on the section. Click Remove Closing Point. Right-click again on the section Click Create Closing point.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Multi-Sections Solid: Closing Point and Orientation (4/4) Use the following steps to create a closing point (continued): 5.
5
Define the point location using the Point Definition dialog box. Click OK to generate the closing point and return to the feature definition.
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Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Creating a Simple Multi-Sections Solid Use the following steps to create a simple multi-sections solid: 1. 2.
3.
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4.
Click the Multi-Sections Solid icon. Select the sections through which the feature will pass. The order of selection is important; it defines the order of connection between the sections. Ensure that the location and direction of the closing points are correct. Click OK to generate the feature.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Multi-Sections Solid Creation: Guides Guides are used to control the shape of the multi-sections solid as it moves between the profiles. Guides must intersect all the sections of the feature. 1
From the Multi-sections Solid Definition dialog box use the following steps to add guides: Click on the Guides tab. Select the guides. One or more guides can be used to control the shape of the feature.
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1. 2.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Multi-Sections Solid Creation: Spine A spine is used to control the shape of the feature between the profiles. As the feature moves between the sections it must always remain perpendicular to the spine. A spine is automatically computed when creating the solid. If required, you can use a user-defined spine.
1
2
From the Multi-sections Solid Definition dialog box use the following steps to add a user-defined spine. Click on the Spine tab Select in the Spine field. Select the spine.
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1. 2. 3.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Multi-Sections Solid Creation: Tangent Surfaces When multi-sections solids are used as the transitional features, it is often required that they be tangent to the adjoining solid.
1
3
Use the following steps to apply tangency: 1. 2. 3.
From the Multi-sections Solid Definition dialog box select the section. Select the tangent surface. Repeat steps 1 and 2 for each section that requires tangency. In this example, tangency constraints are applied to both the first and last sections.
3
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Multi-Sections Solid Creation: Coupling (1/2)
Student Notes:
Coupling refers to the way the profiles are connected. The following coupling options are available:
A.
Using the Ratio option, the curves are coupled according to the ratio of the total length of each section
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A
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Multi-Sections Solid Creation: Coupling (2/2) B.
C.
Using the Tangency then curvature option, the curves are coupled at their tangency discontinuity points first and then their curvature discontinuity points. To use this option the same number of tangency discontinuity points and curvature discontinuity points must exist in all the sections. Using the Vertices option, the curves are coupled at their vertices. To use this option the same number of vertices must exist in all the sections.
B
C
D
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D.
Using the Tangency option, the curves are coupled at their tangency discontinuity points. To use this option the same number of tangency discontinuity points must exist in all the sections.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Coupling: Points of Continuity For a better illustration of the Points of Continuity concept see the profile shown below. This profile has several types of continuity:
Points on Profile
Point Continuity
Tangency Continuity
Curvature Continuity
P1
P1 P2 P3 P2
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P3
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Modify Coupling Use the following steps to change the coupling option: 1. 2. 3. 4.
5.
1 2
Activate the feature. In this example, a multi-sections solid will be created. Select and orient the profiles. Click the Coupling tab. Select the type of coupling required. In this example, the Ratio option is selected. Ratio is selected because the number of vertices in each section is not equal. Click OK to generate the feature.
3
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Manual Coupling: Displaying Uncoupled Points (1/2) An error will be displayed if CATIA cannot couple the profiles automatically.
Section 2
Student Notes:
Section 1
For each coupling mode, the points that could not be coupled are displayed in the geometry with specific symbols.
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For example, if a hexagon profile is transitioned to a square profile with rounded edges an error message will be displayed indicating that the current coupling mode cannot be applied for the coupling options of Tangency, Tangency then Curvature, and Vertices.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Manual Coupling: Displaying Uncoupled Points (2/2)
Student Notes:
For each coupling mode, the points that could not be coupled are displayed in the geometry with specific symbols: A. B. C.
Uncoupled Tangency discontinuities are represented by a square. Uncoupled Curvature discontinues are represented by an empty circle. Uncoupled Vertices are represented by a full circle.
B
C
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Multi-Sections Solid: Manual Coupling (1/2) If the sections in the multi-sections solid (or removed multi-sections solid) do not have the same number of vertices you can define the coupling manually.
1
From the Multi-sections Solid Definition dialog box use the following steps to manually couple the sections: 1. 2.
Click the Coupling tab. Click the Add button. If the Add button is grayed out, select inside the coupling window to activate it. Select a point on the first section. Select the corresponds point on each of the other sections. Remember to select the points in the correct order or the feature will fail.
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3. 4.
2
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Multi-Sections Solid: Manual Coupling (2/2) From the feature definition use the following steps to manually couple the sections (continued): 5.
6. 7.
Once the coupling points for each section have been defined, the Coupling dialog box automatically disappears. Select inside the coupling window to activate the Add button. Repeat steps 2 – 6 for each coupling.
6
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Multi-Sections Solid: Relimitation (1/3)
Student Notes:
By default, the multi-sections solids and the removed multi-sections solids are limited by the start and end sections. You can choose to change the limit of the feature to the length of a user-defined spine or guidelines. You can limit the start or the end section of the feature by checking the appropriate option on the Relimitation tab.
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For example, when a multi-sections solid is created through three sections and the Relimited options are selected the feature will be limited by the start and end sections.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Multi-Sections Solid: Relimitation (2/3)
Student Notes:
When the relimited options are cleared, the feature will be limited by either the spine or a guide curve, whichever is the shortest.
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For example, a multi-sections solid is created through three sections with a spine that extends past the first and last sections. If the Relimited on start section and Relimited on end section options are cleared, the feature will extend beyond the start and end sections to the start and end points of the spine.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Multi-Sections Solid: Relimitation (3/3)
Student Notes:
If a user-defined spine and guide lines are defined, the feature will be limited by the shortest curve. For example, a multi-sections solid is constructed through three sections using the spine and guide curves to control the transitions surfaces.
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If the Relimited options are cleared, the feature will be limited by the shortest curve. In this example, the shortest guideline will limit the feature.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise: Multi-Sections Feature
Student Notes:
Recap Exercise 20 min
In this exercise, you will open an existing model and use the tools learnt in this lesson to create a multi-sections solid. These solids will be created using the existing sketches and 3D wireframe and surface elements. Detailed instructions are provided for the new topics present in this exercise. By the end of this exercise you will be able to:
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Create a Multi-Section Solid Feature
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (1/12) 1. Load Ex8C.CATPart. • Load Ex8C.CATPart. a. Notice the sketches in the PartBody. These three sketches are the profiles for the multi-sections solid. b. Notice the Spline and symmetry feature in Geometrical Set.1. These features are the guides for the feature. c. Notice the extruded surface in Geometrical Set.1. The multi-sections solid has to be tangent to this surface.
1a
1c
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1b
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (2/12) 2.
Create multi-sections solid. • Create a simple multi-sections solid. a. b. c. d.
2a
Select the multi-sections solid icon. Select Sketch.1as the first profile. Select sketch.2 as the second profile. Select sketch.3 as the third profile.
2d
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2c
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2b
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (3/12) 2.
Create multi-sections solid (continued). e.
f. g.
h. i.
Right-click on the Closing Point for the first profile and click Replace from the contextual menu. Select the vertex shown. Ensure that the directional arrow for the first closing point is correct. If needed, click on the arrow to change its direction Move the closing point of the second profile to the vertex shown. Ensure that the closing point for the third profile is in the correct location and direction.
2e
2i
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2h
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (4/12) 2.
Create multi-sections solid (continued). j. k. l. m. n. o.
Click OK. An update error occurs. Read the error. Why did the feature fail? Click OK to the Update Error. Select the Coupling tab. From the Sections coupling pull-down select ‘Ratio’. Click OK to generate the feature.
2l
2m
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2n
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2o
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (5/12) 3.
Redefine the multi-sections solid. • Currently, the feature is coupled based on a ratio, change this to specific locations by manually coupling the feature. a. b.
c. d.
3c
3d 3e
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e.
Show Sketch.1, Sketch,2, and Sketch.3. Double-click the multi-sections solid from the specification tree or directly on the model to redefine the feature. Select the Coupling tab. Click inside the Coupling field to activate the Add button. Select Add.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (6/12) 3.
Student Notes:
Redefine the multi-sections solid (continued). Select the vertices shown. It is important to select the vertices in order (i.e., select the vertex from profile 1, then profile 2, then profile 3). This coupling connects the closing points of all three sections.
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f.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (7/12) 3.
Redefine the multi-sections solid (continued). g. h. i.
Click inside the coupling field to reactivate the Add button. Select the Add button. Create a second coupling as shown. Remember to select the vertices in the correct order.
3g
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3h
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (8/12) 3.
Student Notes:
Redefine the multi-sections solid (continued). Create the coupling for the second corner as shown.
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j.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (9/12) 3.
Student Notes:
Redefine the multi-sections solid (continued). k.
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l.
Couple the vertices for the last two corners using the same technique as the front corners. Click OK to confirm the changes.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (10/12) 4.
Apply Tangency. Redefine the feature to apply tangency to the third profile. a. Double-click on the multi-sections solid to edit its definition. b. Select the third profile from the profile window. c. Select the extrude surface. The feature is now tangent to this surface. d. Click OK to apply the changes.
4b
4c
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•
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (11/12) 5.
Add Guides. •
Redefine the feature and apply guides to define the shape of the multi-sections solid between the sections.
a. b. c. d.
Double-click on the multi-sections solid to edit its definition. Select in the Guides window. Select Spline.1 and Symmetry.1 as the guides. Click OK to apply the changes.
5b
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5d
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (12/12) 6.
Change the relimitation options. • Redefine the feature and change the feature so that it begins at the start of the guide lines and not the first profile. a. b. c. d.
Close the file without saving it. • Hide Geometrical Set.1 and close the file without saving it.
6c
6d
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7.
Double-click multi-sections solid to edit its definition. Select the Relimitation tab. Clear the Relimited on start section option. Click OK to apply the changes.
6b
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise Recap: Multi-Sections Feature
Student Notes:
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Create multi-sections solid feature.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise: Multi-Sections Feature and Rib
Student Notes:
Recap Exercise 20 min
In this exercise you will open an existing model. You will use the tools learned in this lesson to create a rib feature and a multi-sections solid feature. High-level instructions are provided for this exercise. By the end of this exercise you will be able to: Create a Rib Feature
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Create a Multi-Sections Solid Feature
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (1/7) Load Ex8D.CATPart.
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1.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (2/7)
Student Notes:
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2. Create a rib. • Use Sketch.13 as the Profile for a rib feature. • Extract the edge shown for center curve.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (3/7) Create a profile for the multi-sections solid. • Create a positioned profile as shown using the bottom face of the pad as the sketch support.
4.
Create a second profile for the multisections solid. • Create a reference plane at 7mm offset from the bottom surface of the pad. Create the positioned profile as shown using this reference as the sketch support.
3
4
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3.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (4/7) Create a multi-sections solid. • Use the profiles and the bottom surface of the shaft feature as the profiles for the feature.
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5.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (5/7) Create a second multi-sections solid. • Create a second multi-sections solid to complete the handle. Use appropriate surface of the shaft, sketch.4, sketch.5, and sketch.6 as the profiles. Use Spine.1 and Symmetry.1 as the guide curves for the feature.
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6.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (6/7) Create pocket features. • Create two pocket features to trim the excess material from the top of the wrench. Use the XY plane as the sketch support for the pocket feature.
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7.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (7/7) Clarify the display, save and close the model. • Hide all the wireframe and surface elements. Save and close the model.
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8.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise Recap: Multi-Sections Feature and Rib
Student Notes:
Create a rib
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Create a multi-sections solid
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Create Advanced Drafts In this section, you will learn about Advanced Drafts.
Use the following steps to create the Anti-Roll Bar: 1. 2. 3.
Create Advanced Drafts.
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4.
Transform a Body. Create Ribs and Slots. Create Complex SketchBased Features
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Introduction (1/2)
Student Notes:
The Advanced Drafts tool allows you to add complex draft angles to existing solids. Advanced Drafts can be used to create basic and reflect line drafts as well as drafts with two different angle values for complex parts.
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By default, the Advanced Dress-Up Features toolbar is not displayed in the Part Design workbench. To display the Feature on the toolbar, click Views > Toolbars > Advanced Dress-up Features.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Introduction (2/2) Using the Advanced Draft tool you can create: A. B. C. D.
1st
side draft A standard nd A standard 2 side draft A draft using a reflect line A draft using two reflect lines
A
B
C
D
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Select the appropriate button(s) at the top of the Advanced Draft definition dialog box to create a draft.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Creating an Advanced Draft (1/5) Use the 1st Side tab to define the characteristics of the draft angle for the selected faces. The following 1st side characteristics must be defined: A.
Draft angle •
B.
The draft angle is an angle that the draft faces make with the pulling direction from the neutral element. This angle may be defined for each face.
A
B
Faces to draft: •
These are the surfaces where the draft will be applied. B
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A
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Creating an Advanced Draft (2/5) The following 1st side characteristics must be defined (continued): C.
Neutral Element •
D.
C
The Neutral Element is used to define the pivot hinge for the drafted surfaces. The drafted surfaces pivot about a neutral curve, the hinge, where it intersects the Neutral Element. The Neutral Element, usually a plane or face, can be the same reference that is used to define the pulling direction.
D
C
Pulling Direction •
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•
The Pulling Direction defines the direction from which the draft angle is measured. It derives its name from the direction in which the sides of a mold are pulled to extract the molding. Using Advanced Draft, both sides of a face can be drafted to achieve different pulling directions.
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D
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Creating an Advanced Draft (3/5)
Student Notes:
While creating a two-sided draft using a reflect line, the Dependency menu becomes available. This menu enables you to define the dependency of the draft angle. With the Independent option, draft is created where both the 1st & 2nd side draft angles must be defined.
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With the Driving\driven option, the angle specified for the driving side controls the angle specified for the driven side. With the Fitted option, a draft is created on two opposite sides of the part and adjusts the resulting faces using the selected parting element.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Creating an Advanced Draft (4/5) A Parting Line represents the location where two halves of a mold meet. Use the following steps to define a Parting Element: 1. 2. 3.
1 2
Select the Parting Element tab. Select the Use parting element option from the Parting Element tab. Select the parting element from the model. 3
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The parting element can be a plane, a surface, or a face.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Creating an Advanced Draft (5/5) To define a second draft angle, select the appropriate 2nd Side option from the dialog box and from the 2nd side tab, define the second draft. Many of the options necessary to define the 2nd Side of the draft are the same as those that defined the 1st Side of the draft.
A
A. Draft Angle Value B. Neutral Element C. Pulling Direction B
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C
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Advanced Draft Angle: Draft Both Sides (1/5) In the following example, a standard two-sided draft is created.
Student Notes:
1
Use the following steps to create an Advanced Draft feature: Select the Advanced Draft icon. Activate the Standard Draft (1st Side) and Standard Draft (2nd Side) options.
2
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1. 2.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Advanced Draft Angle: Draft Both Sides (2/5) Use the following steps to create an Advanced Draft feature (continued): 3. 4. 5. 6. 7.
Click the Faces to draft selection field Select the faces to be drafted. Click the Neutral Element selection field. Select the Neutral Element(s). Enter the draft angle for the first side.
7
3
5
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4
5
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Advanced Draft Angle: Draft Both Sides (3/5) Use the following steps to create an Advanced Draft feature (continued): 8. Select the Parting Element tab. 9. Select the Use Parting Element option. 10. Select the parting element from the model.
8 9
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10
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Advanced Draft Angle: Draft Both Sides (4/5) Use the following steps to create an Advanced Draft feature (continued): 11. Select the 2nd side tab. 12. Select in the Neutral Element field. 13. Click the Neutral Element(s) for the second side. 14. Enter the draft angle for the second side.
14
12
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13
11
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Advanced Draft Angle: Draft Both Sides (5/5) Use the following steps to create an Advanced Draft feature (continued):
15
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15. Click Preview. 16. Click OK to generate the draft.
16
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
To Sum Up
Student Notes:
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In the following slides you will find a summary of the topics covered in this lesson.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Transform a Body
Student Notes:
Transformations are required when you have some geometry that has been created in one location which needs to be moved or rotated into a specific position. There are four types of transformations: Translate Rotate Symmetry Axis to axis When you select any transformation tool, a ‘Question’ dialog box opens. The message in the dialog box reminds you that you can also transform a body using the Compass. This is useful since you cannot use a transformation tool to transform a sketched geometry.
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The scaling option allows to shrink or expand an entire body based on a single reference. A part gets scaled differently depending on the type of element used as the reference.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Create Ribs and Slots
Student Notes:
Rib and slot are solids that are generated by sweeping a profile along a center curve. A rib is positive (i.e. add material). Slot is negative (i.e. remove material). The tools can be used create features with non-linear trajectory. ‘Profile control’ and ‘merge ends’ options can be used to control the ribs and slots.
Create Complex Sketch Based Features A multi-section solid can be a positive or negative solid that is generated by two or more planar profiles swept along a spine. It is mainly used to create complex solids and transition geometry between two existing solids.
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The closing points and directional arrows define the order in which vertices of the sections will be connected. If there is no vertex at the required location, you can create the closing point on the fly. Guides and Spines can be used to control the shape of the feature between profiles. Depending on the type of Coupling, the profiles are connected in different ways. By clearing the relimitation options, you can limit the feature according to shortest Spine or Guides.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Create Advanced Drafts
Student Notes:
Advanced Drafts tool allows you to add complex drafts to existing solids. Advanced Drafts can be used to create: A Standard 1st side draft A standard 2nd side draft A draft using a reflect line A draft using two reflect lines
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While specifying draft, Draft angle, Faces to draft, Neutral element, Pulling direction must be defined.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Advanced Solid Feature Creation Tools
Student Notes:
Advanced Solid Features 1
2
Rib: Creates a solid by sweeping a profile along a center curve.
Slot: Removes a solid by sweeping a profile along center curve.
1
2
3 3
4
Remove Multi-sections Solids: Removes a solid from two or more planar profiles.
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4
Multi-sections Solids: Creates a solid from two or more planar profiles.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Advanced Dress-Up Features Tools Transformation Features 1
Translation: Moves body from current location to newly specified location.
2
Rotation: Rotates body around an axis.
3
Symmetry: Mirrors a body without duplication.
1
2 3
4
Scale: Shrinks or expand entire body with reference to a point or a plane
Advanced Drafts
5
Advanced Draft: Adds complex draft angles to the existing solids.
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5
4
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise: Draft and Thickness
Student Notes:
Recap Exercise 30 min
In this exercise, you will open an existing part that contains a sketch and two points. Use these inputs to create a solid model. As a review, you will create holes and fillets. An advanced draft is then applied. To prepare the model for more advanced applications, faces are removed and thickness is applied. Detailed instructions are provided for this exercise. By the end of this exercise you will be able to: Create a pad Create a fillet
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Apply an advanced draft Create holes Remove faces Apply thickness to the model
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (1/12) 1.
Load Ex8E.CATPart. • Load Ex8E.CATPart.
2.
Create a pad. • Create a pad using sketch.1 and length as [63.5mm]. a. b. c. d. e.
Click the Pad icon. Select Sketch.1 as the profile. Enter [63.5mm] as length. Check Mirrored extent. Click OK to complete the feature.
1
2a
2c
2b
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2d
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (2/12) 3.
Create fillets. • Create [10mm] fillets on four edges. a.
Create [10 mm] fillets on the four edges shown.
3a
3a
4.
Create fillets. • Create [63.5mm] fillets on four edges. Create [63.5 mm] fillets on the four edges shown.
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a.
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3a 4a
4a
4a
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (3/12) 5.
Create an advanced draft. • Prepare the model for the manufacturing process by creating advanced drafts at the top and bottom faces of the model. a. b. c. d. e.
5a
5b
Click the Advanced Draft tool. Specify standard draft first side and second side. Select the lower horizontal faces as the faces to draft. Enter a draft angle of [5 deg]. Check the Neutral = Parting option.
5d
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5e
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5c
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (4/12) 5.
Create an advanced draft (continued). • Prepare the model for the manufacturing process by creating advanced drafts to the top face of the model. f. g.
Click the Parting Element tab. Check the Use parting element option. Select the ZX plane as the parting element.
h.
5f 5g
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5h
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (5/12) 5.
Create an advanced draft (continued). • Prepare the model for the manufacturing process by creating advanced drafts at the top face of the model. i. j. k. l.
Click the 2nd Side tab. Specify a draft angle of [4deg]. Check the Neutral = Parting option. Click OK to generate the draft.
5i
5j
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5k
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5l
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (6/12) 5.
Create an advanced draft (continued) . • Prepare the model for the manufacturing process by creating advanced drafts at the bottom face of the model. m. n. o. p. q. r. s. t.
Create a second advanced draft feature for the bottom surface. 1st side draft angle: [- 5 deg] 1st side Neutral element: Neutral = Parting. 1st side pulling direction: ZX plane Parting element: ZX plane 2nd side draft angle: [ - 4deg] 2nd side Neutral element: Neutral = Parting Leave pulling direction for the 2nd side as the default.
5n
5o
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5p
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (7/12) 6.
Deactivate the drafts. • Deactivate the two advanced drafts. a. b.
Multi-select Draft.1 and Draft.2 from the specification tree. Deactivate the drafts using the contextual menu.
6b
6a
7.
Create two counterbored holes. • Create two counter-bored holes on the model. Click the Hole icon. Select Center.1 from the InputWireframe geometrical set and select the face as shown.
7b
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a. b.
7a
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (8/12) c.
d.
7c
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e.
From the Extension tab, create the hole using a [25mm] diameter and a depth of [50mm]. From the Type tab, create the counterbore with a diameter of [50 mm] and a depth of [7.5mm]. Create another counterbored hole on the bottom horizontal surface. Use the same dimensions as the last.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (9/12) 8.
Assemble Base and Hole bodies. • Assemble Base body and Hole body to Result body. a. Multi-select Draft.1 and Draft.2 from the specification tree and activate them using contextual menu. b.
Select the Base body and with the contextual menu select Base object > Assemble.
8a
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8b
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8b
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (10/12) c.
8e
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d. e.
Select Empty Result body in the specification tree. Click OK. Similarly Assemble the Hole body to the Result body.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (11/12) 9.
Remove faces. • Remove the bottom faces of the counter-bored holes. These faces are not to be considered during the analysis process. a. b.
c.
9a
9b
Click the Remove Face icon. Select the inside faces of the two holes. Do not select the counterbored portion of the hole. Click OK to removed the faces.
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9c
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (12/12) 10. Apply thickness. • Add thickness to the counter-bored section of the holes. a. b. c. d.
Click the Thickness icon. Select the bottom faces of the two holes. Apply a [5.1mm] thickness. Click OK.
10a
10b
11. Close the file without saving it. • For clarity, hide the ZX plane and close the file without saving it.
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10c
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise Recap: Draft and Thickness
Student Notes:
Create a pad Create a pocket Apply advanced draft Create Holes Remove faces
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Apply thickness
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise: Advanced Draft
Student Notes:
Recap Exercise 20 min
In this exercise, you will open an existing part that contains sketched wireframe elements and a surface feature. To complete this model you will have to create several advanced draft features. You will also use pads, variable fillets, and the mirror operation to complete this model. High-level instruction is provided for this exercise.
By the end of this exercise you will be able to:
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Apply advanced draft features
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (1/6) 1.
Load Ex8F.CATPart.
2.
Create a pad Feature. Use Sketch.1 to create a pad feature with a depth of [20mm].
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•
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (2/6) 3.
Create a draft. • Create draft on the outside vertical wall. a. b. c.
Use a draft angle of 2 degrees. Use the positive Y direction as the pull-direction. Use the right vertical face as the neutral plane.
3a
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3c
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (3/6) Create a variable radius fillet. • Apply a variable radius fillet to the top and bottom outside edges. Create the fillet from [4mm] to [6mm] along each side.
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4.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (4/6) 5.
Create an advanced draft. • Create a two-sided reflect draft. a. b. c. d. e. f.
Use the Driving/Driven dependency option. Set the draft angle to 4 degrees. Use the XY plane as the pulling direction for the first side. Use the top fillet as the neutral element for the side one. Select the Extruded surface as the parting element. Use the bottom fillet as the neutral element for the side two.
5a
5b
5c
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5d
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5e
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features Student Notes:
Do it Yourself (5/6) 6.
Create two pad features. • Use Sketch.2 to create a pad feature with a depth of [30mm]. • Use Sketch.3 to create a pad feature with a depth of [50mm].
7.
Apply an advanced draft. • Apply an advanced draft feature to the two pads. a. b. c. d.
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e.
Create the draft with a 4 degree draft angle on the first side. Use the XY plane as the pulling direction for side one. Use a 6 degree draft angle on the second side. Use Extrude.1 as the parting element. Set the Neutral element on both sides equal to the parting element.
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6
7
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do it Yourself (6/6) Mirror the model. • Complete the model by mirroring the part body about the YZ plane.
9.
Clear the model, save and close it. • Hide all wireframe and surface elements and save the model.
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8.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Exercise Recap: Advanced Draft
Student Notes:
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Create an advanced draft
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Case Study: Advanced Solid Features
Student Notes:
Recap Exercise 10 min
In this exercise you will create the case study model. Let us recall the design intent of this model: The diameter must be 20mm. The minimum bend radius must be 25mm.
A
The link bar hole diameter (A) must be 10mm.
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The width of the material around the link bar hole diameter must be 7.5mm.
Using the techniques you have learned so far, create the model without detailed instruction.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Do It Yourself: Drawing of the Anti-Roll Bar
Student Notes:
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Load Start_CaseStudy9.CATPart and create the model using the drawing provided here.
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CATIA V5 Automotive - Chassis Lesson 9: Advanced Solid Features
Case Study Recap: Anti-Roll Bar
Student Notes:
Open an existing part Create bodies to use the multi-body method Create a rib, pad, multi-sections solid and hole Create Boolean Operations
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Close the document
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