CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Create Complex Parts
Student Notes:
In this lesson you will learn how to create a complex part.
Lesson Contents:
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Case Study: Create Complex Parts Design Intent Stages in the Process Organize a Solid Model Use the Multi-Body Method Create Solid Multi-Model Links Organize a Hybrid Model Create Dress-Up Features
Duration: Approximately 1 day
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Case Study: Create Complex Parts
Student Notes:
The case study for this lesson is the Knuckle part used in the Front Suspension and Engine assembly as shown below. The Knuckle is a part of the Knuckle sub-assembly.
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The case study focuses on the creation of a structured model using the Multi-Body Method.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Design Intent The Knuckle must meet the following design requirements: The thickness (A) must be 10mm. A
The height of the Hub (B) must be 12.5mm. The draft on the Hub (B) must be 25degrees. The height of the Hub (C) must be 5mm. The default fillet radius must be 20mm.
B
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Boolean operations must be used to get the final result. The reference geometry elements must be organized properly.
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C
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Stages in the Process
Student Notes:
The following steps will be used to create the Knuckle : Open an existing part.
2.
Create the Bodies: ‘Core’ and ‘Hub’.
3.
Create sketched geometry and pad in the ‘Hub’ body.
4.
Copy and Paste (As result with Link) the ‘Rough’ body into the ‘Core’ body.
5.
Apply the thickness and fillets on the pasted body.
6.
Perform Boolean operations and create a final result in the ‘Result’ body.
7.
Organize the reference geometry elements.
8.
Save and close the document.
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1.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Organizing a Solid Model In this section you will become familiar with the model organizational tools available in CATIA V5.
Use the following steps to create the Knuckle: 1. 2. 3.
Use the Multi-Body Method. Create Solid Multi-Model Links. Organizing a Hybrid model. Create Dress-up Features.
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4. 5.
Organizing a Solid Model.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Model Organization
Student Notes:
As you begin to create increasingly complex models, it is important to efficiently manage your model. A properly organized model has the following advantages: • • • •
Other designers can easily interpret the model The model will behave more predictably while it is modified and updated It will be easier to reorder and replace the features Problem solving becomes easier as the root cause of the problem can be easily identified.
The following tools are available in CATIA to organize your design
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• Bodies • Geometrical Sets
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Bodies
Student Notes:
Bodies are a storage location for solid features that are added to the part model. By default, all the parts contain at least one body: the PartBody Additional bodies can be added to provide a structure to a complex model. To add a body, click Insert > Body. Each body acts independently in the model until the bodies are combined using Boolean Operations.
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The image on the right-hand side demonstrates a model that was created using multiple bodies. Each body has been named according to its function. This makes the model very easy for other designers to interpret. The designer can also work on a discrete area of geometry by displaying the features within a specific body only.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Geometrical Sets Geometrical Sets are a storage location for wireframe and surface features (Image A). The features in a geometrical set behave in a nonlinear fashion. It is possible to reference a feature that resides in a later position in the tree. Multiple Geometrical Sets can be added to a model to organize the wireframe and surface geometry. For example, wireframe and construction geometry can be separated from the surface geometry that will be used to create a solid (Image B).
A
C
B
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Geometrical Sets can also be placed within a body. This allows you to group the wireframe and surface geometry and solid geometry within the same body. The body now represents all the geometries of a given area of the model providing the designer faster access to the required features (Image C).
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Part Design Recommendations (1/2)
Student Notes:
Since the design of a part corresponds to a set of functional requirements, it is strongly recommended that you organize the structure of your CATIA V5 tree in the same way. Two criteria can be considered for the respect of design intent:
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A. Use the reference elements such as parameters, geometrical wireframe and surface as the specification inputs.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Part Design Recommendations (2/2)
Student Notes:
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B. Use functional bodies aggregated with Boolean Operations.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Use the Multi-Body Method In this section you will learn how to use a multibody technique to create complex models.
Use the following steps to create the Knuckle: 1.
Organizing a Solid Model.
3.
Create Solid Multi-Model Links. Organizing a Hybrid model. Create Dress-up Features.
2.
4.
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5.
Use the Multi-Body Method.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
What is Multi-Body Method? The Multi-Body Method allows you to organize discrete areas of geometry within a complex model into different bodies. Each geometry area is created in a separate body. Each body acts independently in the model.
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In the images on the right-hand side, the Pillar model is divided into four bodies. The geometry in the bodies is modeled using positives. The bodies are then combined using Boolean Operations to create the completed model shown in the top right-hand image.
PartBody
Body.2
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Body.3
Body.4
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Using the Multi-Body Method (1/2) Use the following steps to apply the Multi-Body Method: 1.
2.
Break the model into bodies a.
Consider the areas of the model that should be contained in a separate body.
b.
These can be functional areas, for example a complex cutout or area of the model.
c.
Try to combine features that can similar design intent into the same body.
d.
Create as many bodies as required.
Define the body structure. a. b.
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3.
Click Insert > Body to add a new body to the model. Bodies should be descriptively named so that the design intent is clear.
3a
Insert features into the bodies. a.
4.
2a
To activate a body, select it from the specification tree and click Define In Work Object from the right mouse button contextual menu.
Combine the bodies using Boolean Operations.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Using the Multi-Body Method (2/2)
Student Notes:
Advantages •
Provides an organized approach to modeling complex parts.
•
Solid features within a body can be hidden independently of the rest of the model.
•
Groups of geometry can be de-activated by deactivating the body.
•
Complex geometry is easier to create within a focused area of the model.
•
Model will update faster due to the organized structure.
Disadvantages
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•
The number of operations in a multi body method is greater than the number of operations in the pure feature modeling method.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
What Are the Boolean Operations? Boolean operations enable you to use a Multi-Body approach to modeling. Using multiple bodies in a model or in different models, you can use Boolean operations to manipulate the bodies to achieve different results. For example, casting models can be developed using bodies to represent cast and machined features.
Object 2 in brown Object 1 in Green
In the images on the right-hand side, a Boolean operation is performed on the two bodies to subtract the volume of the second body from the second where they intersect. The Boolean operations are: A. Assemble B. Add C. Remove D. Intersect
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E. Union Trim F.
Remove Lump
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Assemble (1/4) In this example, Body.2 will be assembled into PartBody. When Body.2 is assembled to PartBody, the operation between the bodies is a union. An Assemble operation will respect the “nature” of features. If Body.2 contains Pocket feature (permissible) as its first node, the Assemble operation will remove material from Body.1.
Body.2
PartBody
Use the following steps to perform the Assemble operation:
2
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1. Right-click the body to be assembled. In this example, Body.2 will be assembled into the PartBody. 2. From the contextual menu click x.object > Assemble.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Assemble (2/4) Use the following steps to perform the Assemble operation (continued):
4
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3. By default, the selected body will be assembled to the active body as the last feature. If required, select another body to which the selected body will be assembled. 4. Click OK to finalize the operation. Notice that Body.2 contains a groove. As the groove features remove material, the result of the union removes material.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Assemble (3/4) To work more efficiently, a single operation can be performed on multiple bodies. Use the following steps to Assemble multiple bodies into one: 1
1.
Pre-select all the bodies using the key. In this example, Body.2, Body.3, and Body.4 are all pre-selected.
1
2.
Right-click the last selected body.
1
3.
Click Selected objects > Assemble from the contextual menu.
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3
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Assemble (4/4) Use the following steps to Assemble multiple bodies into one (continued): 4.
Select the body in which other bodies will be inserted.
5.
Click OK to complete the operation.
4
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Add (1/2) In this example, Body.2 will be added to the PartBody. The Add operation also creates a union between the two selected bodies. The difference between an Add and an Assemble is that if Body.2 contains a pocket feature as its first node, using an Add operation the pocket will be seen by PartBody as a pad.
Body.2
PartBody
Use the following steps to perform an Add operation: 1.
2
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2.
Right-click the body to be added. In this example, Body.2 will be added to the PartBody. From the contextual menu click x.object > Add.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Add (2/2) Use the following steps to perform an Add operation (continued): 3.
4
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4.
By default, the selected body will be added to the active body as the last feature. If required, select another body to which the selected body will be added. Click OK to finalize the operation. Notice that Body.2 contains a groove; however, using the add operation the feature remains as it was before the operation.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Remove (1/2) In this example, Body,2 will be removed from the PartBody. If Body2 is Removed from PartBody, the operation is PartBody minus Body2. Use the following steps to perform a remove operation: 1. 2.
Body2
PartBody
Right-click on the body to be added. In this example, body.2 will be added to the PartBody. From the contextual menu click x.object > Remove.
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2
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Remove (2/2) Use the following steps to perform a remove operation (continued): 3.
4.
By default, the selected body will be removed from the active body. If required, select another body from which the selected body will be removed. Click OK to finalize the operation.
4
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It is required to get the precise fillet value here.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Intersect (1/2) In this example, Body.2 will intersect PartBody. The resulting solid is the material common between the two intersecting bodies. Use the following steps to perform an Intersect operation: 1.
2.
Body.2
PartBody
Right-click the body to be added. In this example, body.2 will be added to the PartBody. From the contextual menu click x.object > Intersect.
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2
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Intersect (2/2) Use the following steps to perform an Intersect operation (continued): 3.
4
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4.
By default, the selected body will intersect the active body. If required, select another body to intersect. Click OK to finalize the operation.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Union Trim (1/2) In this example, Body.2 will be used to trim the PartBody using the Union Trim operation. This operation is a union of two bodies with an option to remove or keep one side. One face is selected to remove the lower section of Body.2, while keeping the outer section of the PartBody, while the other face is selected to keep only the upper section of Body.2. For the union trim operation to work, the geometry must have sides that are clearly defined.
Body.2
PartBody
Use the following steps to perform a Union Trim operation: 1.
2.
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3.
Right-click the body to be added. In this example, body.2 will be added to the PartBody. From the contextual menu click x.object > Union Trim. Select another body. This body will be trimmed by the body you have already selected. In this example, PartBody is selected.
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3
2
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Union Trim (2/2) Use the following steps to perform a Union Trim operation (continued): 4
4. 5. 6. 7. 8.
Select in the Faces to remove field. Select the faces to be removed by the operation. Select in the Faces to keep field. Select the faces to be kept by the operation. Click OK to finalize the operation.
6 8
5
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Boolean Operation: Removing Lump (1/2)
Student Notes:
Lumps and cavities may appear in the model after certain operations. These elements can be removed using the Remove Lump tool. The previous options work between two bodies. The Remove Lump option works on geometry within a specific body. A lump is a material that is completely disconnected from other parts within a single body. You can delete any lump as a single entity even if the lump is a combination of features.
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Cavity
Lumps
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Boolean Operation: Removing Lump (2/2) Use the following steps to remove Lump and cavities from a model: 1.
2. 3. 4. 5.
Right-click the body from which the Lumps and Cavities are to be removed. In the given Lump and Cavities have to be removed from the PartBody. Click x.object > Remove Lump from the contextual menu. Select in the Faces to remove field. Select the Lumps. Click OK.
2
4
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Replacing a Body (1/3) The Replace tool can replace a body used for an operation by another body. This eliminates the need to delete the operation and redo it with the correct body.
Body.3 Body.4
Use the following steps to replace the body used in an operation: 1.
Right-click the body to be replaced.
2.
Click Replace from the contextual menu.
3.
Select the replacement body.
2
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Replacing a Body (2/3) Use the following steps to replace the body used in an operation (continued): 4.
5.
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6.
In this example, additional references are required to replace the bodies. From the Replace dialog box click on the second field. A Replace Viewer dialog box displays the reference. Select the appropriate reference in the replacing body. In this example, the missing reference is the face that is to be removed during the Union Trim operation. Click OK to close the Replace Viewer dialog box.
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4
5 6
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Replacing a Body (3/3) Use the following steps to replace the body used in an operation (continued): 7.
Click OK to complete the operation.
8.
If necessary, update the part by selecting the Update All icon.
7
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Changing the Boolean Operation Type (1/2) The type of Boolean operation can be changed without deleting the operation and recreating it. Consider the following example. Three bodies are constructed: A. B. C.
PartBody Body.2 Body.3
C
B
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Currently, Body.2 and Body.3 have been assembled into the PartBody. However, Body.3 should be removed from the PartBody.
A
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Changing the Boolean Operation Type (2/2) Use the following steps to change a Boolean operation: 1.
2.
3
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3.
Right-click the operation to be replaced. In this example, the Assemble operation is to be replaced. A list of operations, which the current operation can be converted to are shown in the contextual menu. Select the appropriate operation. Here, the Change to Remove option is selected.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Recommendations for Working with Boolean
Student Notes:
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In this section, you will be given a recommendation to help during working with Boolean operations.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Maintain a Flat Specification Tree Structure (1/2)
Student Notes:
It is recommended that you maintain a flat specification tree structure while working with Boolean operations. Flat specification tree structure enables you to: 1. 2.
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3.
Easily understand the way in which the part is designed. Easily locate the failed feature, in case of feature failure. Reduce the update time.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Maintain a Flat Specification Tree Structure (2/2) In order to maintain a flat specification tree : 1. 2.
Perform the Boolean operations in an empty PartBody. Create dress-up features (Draft, Fillet, Shell, etc.) as close as possible, to the solid primitive.
Boolean operations are done in empty body
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Basic features are close to solid primitives
Empty Part Body
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Exercise: Multi-Body Work
Student Notes:
Recap Exercise 15 min
In this exercise, you will create a new part by creating multiple bodies. You will use the tools learned in the previous lessons to create a pad and a pocket. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a multi-body structure Create a pad Create a hole Create a circular pattern
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Create Boolean operations
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (1/11) 1. Create a new part. Create a new part file. a. Click File > New. b. Select Part from the list of document types. c. Click OK. d. Enter part name [Ex7A] e. Click OK.
2. Create Multi-Body structure. Create multiple bodies and rename them by changing properties.
1d
1e
2a
a. Select Insert > Body. b. Right-click on the new body and through the contextual menu, select Change Properties > Feature properties. c. Change the default name to Base. d. In the same way, create a body and rename it as Holes.
2b 2b
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2c
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (2/11) 3.
Create a sketch. Create a positioned sketch that will represent the profile for a base. a.
b. c. d.
Contextual menu on the Base Body and select Define in Work Object. This ensures that any features that are created are added to the Base body. Click the Positioned Sketch icon. Select the XY plane as the sketch support. Select origin type as Part origin and click OK to enter sketcher workbench.
3a
3b 3c
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3d
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (3/11) 3.
Create a sketch (continued). e. f.
g. h.
i. j.
Click the Rectangle icon and sketch a rectangle. Select the length of the rectangle and click the Constraint icon to specify the length dimension. Change the dimension value to [120mm]. Select the width of the rectangle and click the Constraint icon to specify length dimension. Change the dimension value to [120mm]. Dimension and constraint the sketch as shown.
3e 3f
3f
3g
3j
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3g
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (4/11) 4.
Create a pad. Add a pad feature of [5mm] thickness using Sketch.1 as the profile. a. b. c. d. e.
Select Sketch.1 Click the Pad icon. Select Dimension from the Type menu. Enter [5] for the length . Click OK to complete the feature.
4a
4b
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4d
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4c
4e
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (5/11) 5.
Create an edge fillet. Add an edge fillet of [20mm] on four edges of a pad. a. b. c. d.
Click the Edge Fillet icon. Select four edges of pad.1. Enter [20mm] as the radius. Click OK to complete the feature.
5a
5b
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5c
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5d
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (6/11) 6.
Create a point. Create a origin point to define the location of a hole. a. b.
c.
7.
Click the Point icon. Select Coordinates as a Point type and enter [0mm] as X, Y and Z coordinates. Click OK to complete the point creation.
6a 6b
6c
Create a point. Create a point to define the location of a hole. a. b.
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c.
Click the Point icon. Select Coordinates as a Point type and enter [0mm] as X and Z coordinates. Enter [36mm] as Y coordinate. Click OK to complete the point creation.
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7a 7b
7c
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (7/11) 8.
Create a hole. Create a hole in Holes body. a.
b. c. d. e. f.
Select Holes body. Using contextual menu and select Define in Work Object. This ensures that any features that are created are added to the Holes body. Click the Hole icon. Select Point.1 Select the top face of a pad. Enter [24mm] as the diameter and [10mm] as the depth. Click OK to complete the hole.
8a 8b 8c
8d
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8e
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8f
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (8/11) 9.
Create a hole. Create a hole in Holes body. a. b. c. d. e.
Click the Hole icon. Select Point.2 Select top face of pad. Enter [5mm] as the diameter and [10mm] as the depth. Click OK to complete the hole.
9a 9b
9c
9d
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9e
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (9/11) 10. Create a circular pattern. Create a circular pattern of a hole. a. b. c. d. e. f.
Click the Circular Pattern icon. Select Object to Pattern as Hole.2 Select Parameters as Complete crown. Instances [3]. Reference direction: Using contextual menu, select Z axis. Click OK to validate the pattern creation.
10a
10c 10d
10e
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10b
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (10/11) 11. Create Boolean operations. Assemble the body “Base” and body “Holes” to an empty PartBody. a. b. c.
Contextual menu on Base body > Base object > Assemble Select PartBody in the To field. In the same way, assemble Holes body to PartBody.
11a
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11b
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11c
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (11/11)
Student Notes:
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12. Close the file without saving it. For clarity, hide the Geometrical Set and close the file without saving it.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Exercise Recap: Multi-Body Work
Student Notes:
Create a multi-body structure Create a pad Create a hole Create a circular pattern
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Create Boolean Operations
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Exercise: Multi-Body Work
Student Notes:
Recap Exercise 25 min
In this exercise you will create a new part. Using the pad, groove, hole, pocket, fillets and Boolean Operations you will construct an arm. High-level instructions for this exercise are provided. By the end of this exercise you will be able to: Create a multi-body structure Create a pad Create a groove
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Create a hole Create a pocket Create Boolean Operations
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (1/7)
Student Notes:
1. Create a new part file. Create a new part file called [Ex7B.CATPart]. Rename the PartBody to Result. Insert a new body and rename it as Rough.
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2. Create a pad feature. Create a positioned profile as shown to construct a pad feature.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (2/7)
Student Notes:
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3. Create a pad feature. Create the profile shown to construct a pad feature.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (3/7)
Student Notes:
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4. Create a pad feature. Create the profile shown to construct a pad feature.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (4/7)
Student Notes:
5. Create a groove feature. Insert a new body and rename it as Machined. Create the profile as shown to construct a groove feature in a pad created in step 4.
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6. Create a hole feature. Create Tapered hole with angle 16deg fin a pad created in step 3.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (5/7)
Student Notes:
7. Create a pocket feature. Create the profile shown to construct a pocket feature.
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8. Create an edge fillet. Create an edge fillet of [12mm] on four edges of the above created pad as shown in red.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (6/7)
Student Notes:
9. Create a pocket feature. Use the sketch created in step 7 to construct a pocket feature
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10.Create an edge fillet. Create an edge fillet of [12mm] on four edges of above created pad as shown in red.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (7/7)
Student Notes:
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11. Assembly in Result body Assemble Rough to Result Assemble Machined to Result
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Exercise Recap: Multi-Body Work
Student Notes:
Create a multi-body structure Create a pad feature Create a groove feature Create a hole feature Create a pocket feature
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Create Boolean Operations
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Create Solid Multi-Model Links In this section you will learn how to create multimodel links.
Use the following steps to create the Knuckle: 1. 2.
3. 4.
Create Solid MultiModel Links.
Organizing a Hybrid model. Create Dress-up Features.
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5.
Organizing a Solid Model. Use the Multi-Body Method.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
What Are Multi-Model Links? (1/3) Using multiple bodies while designing can give the model added flexibility. Boolean Operations allow creation of complex models by adding, removing, or intersecting simple geometric shapes. Geometry can be shared between the models to quickly replicate the features in a number of parts.
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However, in order to share geometry, it is recommended that first the elements must be published. In this case the shared geometry can be restricted to the published elements only.
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Unpublished geometry is shared.
Published geometry is shared.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
What Are Multi-Model Links? (2/3) In the context of the concurrent engineering, multi-model links enable you to design a model using the elements from another model. Using multi-model links you can copy the bodies created in different files into your own part. This enables you to automatically update your part when changes are made in the source files.
Part A
Part B
2
4
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For example, 1. Part A is created by Designer A. 2. Part B is created by Designer B. 3. Designer B publishes geometry that must be shared. 4. Using multi-model links, Designer A copies Part B into Part A.
1
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
What Are Multi-Model Links? (3/3)
Student Notes:
For example (continued): 5. 6. 7.
Using a Remove operation, Part B is removed from Part A. Part B is modified by Designer B. Because of the multi-model link, Part A is automatically updated to reflect the changes in Part B.
5
6
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Establishing Multi-Model Links (1/3) Use the following steps to establish a multimodel link: 1. 2. 3. 4. 5.
3
Open the source and target files. From the source model, right-click on the body to be copied. From the contextual menu click Copy. From the target model, right-click on the PartBody. Click Paste Special from the contextual menu.
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5
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Establishing Multi-Model Links (2/3) Use the following steps to establish a multimodel link (continued): 6. 7. 8. 9.
6
From the Paste Special dialog box select As Result with Link. Click OK. The source PartBody is copied into the target model. Complete the model as necessary. In this example, the copied body is removed from the PartBody.
7
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8
9
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Establishing Multi-Model Links (3/3)
Student Notes:
Use the following steps to establish a multimodel link (continued): 10. If required, make changes in the source model. In this example, several features have been added to the source body. 11. Update the target model. The model gets updated to reflect the changes.
10
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11
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Paste Special (1/2)
Student Notes:
The different types of features in one CATIA document can be reused in another CATIA document. This reduces the need to recreate features that are commonly used and also helps in concurrent engineering. Several paste special options are available, choose the option that best meets the requirements of your design:
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A.
The As Specified in Part Document option copies the element(s) with their design specifications. Each feature is recreated in the target model and can be edited. There is no link to the source model. In this example, the PartBody from the source document is copied into the Target model. Observe that a second body is added to the model containing all the copied elements and their design specifications.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
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Paste Special (2/2) B.
The As Result with Link option copies the element(s) without their design specifications and links it to the original object(s). When changes occur in the source document they will automatically get updated in the target document. Observe that when the PartBody from the target model is copied using this option, it creates a single solid element with a green dot indicating that there is a link between the source and target documents.
C.
The As Result option copies the element(s) without their design specifications and without a link. This option is useful when you do not want the feature information to be shown or when you do not want to make changes to the copied elements in the target document. Observe that when the PartBody from the target model is copied using this option, it creates a single solid element with a red lightening bolt. This indicates that the link has been isolated.
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Student Notes:
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Managing Multi-Model links (1/4)
Student Notes:
When you use the Paste special option As result with Link you create a link between the source document and the target document. Copied links display a number of symbols depending on their status:
Icon
Icon (working with Description Publications) The pointed element is loaded and synchronized The pointed document is not loaded
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The link has been isolated. This icon will appear if the source document has been copied using the As Result paste special option.
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The source document has been modified. The target document is not up to date. The source document is not found.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Managing Multi-Model links (2/4)
Student Notes:
Using the Links, you can determine the document at which the model points.. To access the links panel click Edit > Links. The links document lists all the links referenced by the correct document and their status.
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Use the links panel to Load, Synchronize, Activate/Deactivate, Isolate, or Replace the referenced documents.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Managing Multi-Model links (3/4)
Student Notes:
Another way to determine the source document for a copied solid is to click Parents/Children. A panel displays the source document.
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If you do not want the target document to update the changes in the source, you can break the link from the solid’s contextual menu. Click Isolate to break the link between the source and target document.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Managing Multi-Model links (4/4)
Student Notes:
When changes occur in the source document, the linked document will display a red X in its icon. This indicates that the link is not up to date. You can update the link using the links panel. Another way to update a link without opening the Link panel is using the contextual menus. To update an individual link, right-click on the solid and click Solid.1 object > Synchronize from the contextual menu.
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To update all the links in a model at the same time, right-click on the part and click Part2 object > Synchronize All from the contextual menu.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Organizing a Hybrid Model In this section you will become familiar with the model organizational tools available in CATIA V5 in Hybrid environment.
Use the following steps to create the Knuckle: 1. 2. 3.
4.
Organizing a Hybrid model.
Create Dress-up Features.
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5.
Organizing a Solid Model. Use the Multi-Body Method. Create Solid Multi-Model Links.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Ordered Geometrical Sets
Student Notes:
An Ordered Geometrical Set (OGS) adds the functionality of a linear update sequence to the geometrical set. This allows the OGS to have the following additional functionalities:
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• Features can be scanned (using Edit > Scan or Define In Work Object) allowing you to see the way the features were created • Geometry that is consumed by a downstream feature (e.g. a surface that is trimmed) are not shown. • You can reorder elements. • Graphical properties for new elements are inherited from the parent elements. In order to use an OGS, it must be manually added to the model by clicking Insert > Ordered Geometrical Set.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Hybrid Design (1/2)
Student Notes:
Hybrid Design provides greater flexibility while structuring your design. The Hybrid Design method uses a special type of Hybrid body that can contain both solid geometry and wireframe and surface geometry without the need to add a geometrical set. While working within the Generative Shape Design (GSD) workbench, wireframe and surface elements will be automatically added to the active hybrid body. You can still add Geometrical Sets, and use their non-linear behavior for processes such as Conceptual Design.
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The combination of Part Design and Generative Shape Design (GSD) functionalities allow you to access the GSD features from the contextual menu while creating solid features.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Hybrid Design (2/2)
Student Notes:
The ability to combine wireframe and surface features with solid feature within the same body allows you to organize the features of the model with respect to their function. For example, the right-hand side image depicts a part model that has been created using the hybrid bodies. The geometry for a specific area of the model has been grouped beneath a hybrid body. This structure shows that the solid features are created after the wireframe and surface features that they reference.
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When the model is examined by another designer, the Scan or Define In Work Object function allows the designer to step through the entire design and view the order of creation of both Part Design and GSD features.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Create Dress-Up Features In this section you will learn the dress-up features available in the Part Design workbench.
Use the following steps to create the Knuckle : 1. 2. 3. 4.
Create Dress-up Features.
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5.
Organizing a Solid Model. Use the Multi-Body Method. Create Solid Multi-Model Links. Organizing a Hybrid model.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Introduction The following tools allow you to dress-up the existing solids.
A.
Thickness: • Use this tool to add a thickness to a face.
B.
Remove faces: • Use this tool to simplify the geometry of a part for a downstream processes. Replace a face with a surface: • Use this tool to replace a planar solid face with a surface.
B
C
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C.
A
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
What is a Thickness? (1/2)
Student Notes:
The thickness feature is often used to add or remove material before machining a part. Thickness enhances the design intent and allows rapid modifications.
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Material can be quickly added or removed from various faces of a part to accommodate machining or other manufacturing operations. For instance, you might add thickness to account for additional material necessary to cast the part.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
What is a Thickness? (2/2) A. The Thickness tool adds material to the pad while still considering the other features. Use the Thickness tool to add material quickly and efficiently.
A
B. Another common use of the Thickness tool is to apply thickness to the selected walls of a model that has been shelled.
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B
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Creating a Thickness Use the following steps to apply thickness to a model: 1. 2. 3. 4.
Click the Thickness icon from the Dressup Features toolbar. Select the faces to thicken. Enter the thickness value. Click OK.
1
2
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3
It is recommended not to have multiple thickness values in a single thickness feature.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Ignoring Faces While Creating a Thickness
Student Notes:
In some cases, when you apply a thickness an error message appears indicating that some of the bodies cannot be built properly. After closing the window, another message appears prompting you to ignore the faces that have a problem. If you click Yes, the thickness is created and the face causing the issue is removed.
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For example, if the inside face of the model shown in the image on the top right-hand side is offset, an error message will appear. CATIA is unable to offset the filleted surface. Select Yes to create the thickened body as shown in the image below.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Reset Ignored Faces Option for Thickness Tool
Student Notes:
If a thickness feature has been created ignoring some faces, the Ignored faces can be previewed when you edit the thickness from the specification tree, as shown in the image on the top right-hand side.
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The option Reset ignored faces appears in the Thickness Definition Dialog box. After selecting this option, the ignored faces are reinitialized and the ‘Ignored Face’ note is removed from the geometry.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Remove Faces (1/2)
Student Notes:
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To simplify the part for a finite element analysis, you can remove some of its faces or features using the Remove Faces tool.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Remove Faces (2/2) Use the following steps to remove faces: 1
1. 2. 3. 4. 5.
3
4
5 6
2
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6.
Click the Remove Face icon. Select the internal faces to remove. Select in the Faces to keep field. Select the faces to be kept. Check the Show all faces to remove option to preview all faces that will be removed during the operation. Click OK to complete the feature. The selected faces are removed and a new feature is added to the specification tree.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Replace Face The Replace Face tool is used to extrude a solid face up to a surface.
1
Use the following steps to extrude a solid face up to a surface: 1. 2. 3. 4.
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5.
Click the Replace Face icon. Select the replacing surface. Select the face to extrude. Ensure that the arrow points in the direction of the material to be kept. Click on the arrow to change its direction. Click OK to complete the feature.
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3 5
4
4
2
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
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 8: Create Complex Parts Student Notes:
Organizing a Solid Model When dealing with the complex models, it is important to manage your model efficiently so that it can be modified and updated easily. It also helps other designers to interpret the model easily. In CATIA, tools available for organizing the model are: Bodies Geometrical sets Bodies are a storage location for solid features added to the part model. Geometrical sets are storage locations for wireframe and surface features.
Use the Multi-Body Method
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Multi-body method allows you to organize complex models by creating each geometry area in a separate body which acts independently. The various bodies can then be manipulated to get required results by Boolean operations such as Assemble, Add, Remove, Intersect, Union Trim, and Remove Lump.
PartBody
Body.2
Body.3
Body.4
This provides an organized approach to modeling of complex parts. The models can be created and updated faster. It is recommended to maintain a flat specification tree while working with the Boolean operations.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Create Solid Multi-Model Links Multi-Model links can be used to share geometry between models. This reduces the need to recreate the features that are commonly used. It is possible to maintain the link between the source and target model, so that when the source model is updated, the target model can also be updated. If required the geometry can be isolated to remove the link.
Part 1
Using parent – children relation panel or links panel you can manage the Multi-Model links.
Part 2
Part 1 with Shared geometry from Part 2
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Organizing a Hybrid Model Hybrid design uses a special type of body that can contain both, solid geometry and wireframe and surface geometry. This allows you to organize the features of the model with respect to their function. If required, you can add Geometrical sets and use their non-linear behavior. The scan or Define in Work Object functions allow you to view the order of creation of both, Part Design and GSD feature.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Create Dress-Up Features
Student Notes:
To dress up the existing solid, following tools can be used: Thickness: add or remove material from various faces of the body. Remove faces: remove some faces to simplify the geometry.
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Replace a face with a Surface: extrude a solid face up to a surface.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Organizing Solid Model Tools Insert 1
Bodies: insert bodies in the part tree.
2
Geometrical sets: insert geometrical set in the part tree.
3
4
Ordered Geometrical Set: insert ordered geometrical set. Insert in New Body: project the existing 3D elements onto the sketch plane.
1
2 3 4
Boolean Operations
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5
Assemble: assemble selected bodies depending upon their nature.
6
Add: union of two bodies.
7
Remove: remove the selected body from part body.
8
Intersect: retain common material between selected bodies.
9
10
Union Trim: union of two bodies with an option to remove or keep one side. Remove Lump: remove material that is completely disconnected from other parts of a single body.
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5
6 7 8 9 10
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Additional Tools Reference Elements 1
Point: creates a point in 3D space
2
Line: creates a line in 3D space
1 2 3
3
Plane: creates a plane in 3D space
Dress-Up Features 4
Thickness: adds or removes material from various faces of the body
5
Remove faces: removes some faces to simplify the geometry
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Exercise: Core Removing
Student Notes:
Recap Exercise 25 min
In this exercise, you will create a simplified Camshaft Sprocket housing. You will use the tools learned in this lesson to create different bodies and combine them to create a shelled part. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a structured multi-body part
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Create a shelled part using Boolean Operations
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (1/10) 1. Load the Ex7C.CATpart. Load an existing part. a. Verify whether the PartBody is active. b. Verify whether the reference geometry Axis and Limit_Plane is in a named geometrical set. 1a 1b
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2. Insert and name a new body Insert a new body to represent the rough part. a. Click Insert > Body. b. Select the new body Body.2 and from the contextual menu select Properties. c. Select the Feature Properties tab. d. Select the Feature Name Body.2. e. Enter the name as Rough. f. Click OK.
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2c 2d
2e
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (2/10) 3. Create a positioned sketch. Create a circular profile of diameter [112 mm] on YZ plane. a. b. c. d. e. f.
3a
Click the Positioned Sketch icon. Select the yz plane to place the sketch. Click OK. Click the Circle icon and sketch a circle. Dimension the circle to [112mm] as shown. Exit the Sketcher workbench.
3b
3c 3d
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3e
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (3/10) 4. Create a pad. Create a pad from the sketch. a. Select Sketch.1 in the specification tree. b. Click on the Pad icon. c. Select the First Limit Type as Up to plane. d. Select Limit_Plane from tree as the Limit. e. Click OK to complete the feature.
4b
4c 4d
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4e
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (4/10) 5. Create a fillet. Create an edge fillet of [3.5mm]. a. b. c. d.
Click the Edge Fillet icon. Select the edge of the pad as shown. Enter a Radius value of 3.5mm. Click OK.
5a
5b
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5c
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5d
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (5/10) 6. Create a new body. Copy and paste the Rough body. The new body will represent the core and will be modified to add the thickness.
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a. Select Rough and from the contextual menu select Copy. b. Select Sprocket_Housing and from the contextual menu select Paste Special. c. Select the option As Result with Link. d. Click OK. e. Select the resulting body and from the contextual menu and select Properties. f. Select the Feature Properties tab and enter Feature Name as Core. g. Click OK.
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6a
6b
6c
6f
6d
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (6/10) 7. Add core thickness. Add a thickness feature to the Core body. This will be a negative value in order to represent the shell thickness when the core is removed from the rough part. a. b. c. d. e.
Hide the Rough part. Click the Thickness icon. Select the rear face of the Core body as shown. Enter the Default thickness as [1.5mm]. Click OK.
7b
7c
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7d
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7e
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (7/10) 8.
Add a pad feature to the Core body. Create a positioned sketch on Limit_Plane and create a pad. a. b. c.
d.
e. f.
Click the Positioned Sketch icon. Select the Limit_Plane plane to place the sketch. Check Reverse H to inverse the direction of the horizontal axis and click OK. Click the Circle icon and sketch a circle. Dimension the circle to [40mm] as shown. Click the Pad icon. Create a pad with the yz plane as the First Limit plane. Click OK to validate the pad definition.
8b
8c
8c
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8d
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8f
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (8/10) 9. Create a rough body assembly. Assemble the Rough body in the PartBody to create a separate rough feature in the final specification tree. a. Show the Rough part and verify whether its envelope is larger than the Core. b. Select the Rough part and from the contextual menu select Rough object > Assemble. c. Select the empty PartBody in the specification tree. d. Click OK.
9a
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9d
9c
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Do it Yourself (9/10) 10. Remove core body. Remove the Core body from the PartBody to create a separate core feature in the final specification tree. a. Select the Core body b. From the contextual menu select Core object > Remove.
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10a
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Do it Yourself (10/10)
Student Notes:
11. Hide geometry other than final 3D part. Hide wireframe and reference geometry. a. Hide the geometrical set Reference_Geometry. b. Hide the yz plane.
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12. Close the part without saving it.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Exercise Recap: Core Removing
Student Notes:
Create a structured multi-body part
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Create a shelled part using Boolean Operations
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Exercise: Wireframe and Multi-Body
Student Notes:
Recap Exercise 25 min
In this exercise you will modify an existing part. Using the hole, groove, pockets and Boolean Operations you will construct a Valve body. High-level instructions for this exercise are provided. By the end of this exercise you will be able to: Create a wireframe geometry Create a multi-body structure Create a groove
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Create a hole Create a pocket Create Boolean Operations
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Do it Yourself (1/11) Load Ex7D.CATPart. Set the ‘Wireframe’ Geometrical set as inwork object.
2.
Create a point. Create a point as shown and rename it as P4.
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1.
Student Notes:
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Do it Yourself (2/11) Create a line. Create a line as shown and rename it as L6.
4.
Create a circle. Enter the Generative Shape Design workbench. Create a circle as shown and rename it as CRV1.
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3.
Student Notes:
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Do it Yourself (3/11) Create a point. Create an end point of CRV1 as shown and rename it as P5.
6.
Create a point. Create an end point of CRV1 as shown and rename it as P6.
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5.
Student Notes:
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Do it Yourself (4/11) Create a pad. Insert a new body “Sensor_Plate”. Create a positioned profile as shown on PL6 and create a pad.
8.
Create an edge fillet. Create an edge fillet of [2mm] on one edge as shown.
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7.
Student Notes:
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (5/11) 9.
Student Notes:
Create a pad. Create a positioned profile as shown on PL6 and create a pad.
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10. Create an edge fillet. Create an edge fillet of [2mm] on the two edges as shown.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (6/11)
Student Notes:
11. Insert a new body “Machining_Body” and create a hole. Create a simple hole of diameter [20mm] as shown.
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12. Create a groove. Create a positioned profile as shown on the YZ plane and create a groove.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (7/11)
Student Notes:
13. Insert a new body “Machining_Top_Flange” and create a groove. Create a positioned profile as shown on the YZ plane and create a groove.
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14. Create two holes. Create simple holes of diameter [6mm] as shown.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (8/11)
Student Notes:
15. Insert a new body “Machining_Sensor” and create a groove. Create a positioned profile as shown on the YZ plane and create a groove.
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16. Create two holes. Create a simple hole of diameter [5mm] as shown.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (9/11)
Student Notes:
17. Insert a new body “Machining_Motor” and create a hole. Create a simple hole of diameter [10mm] as shown.
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18. Insert a new body “Machining_Base_Flanges” and create holes. Create a simple hole of diameter [8mm] as shown and make a pattern.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (10/11)
Student Notes:
19. Insert a new body “Machining_Top_Face” and create a pocket. Create a positioned profile as shown on PL3 plane and create a pocket.
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20. Perform Boolean Operations. Assemble ‘Sensor_Plate’ body to ‘Rough’ body.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do it Yourself (11/11)
Student Notes:
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Insert a new body ‘Machining’ and assemble the bodies as shown. Assemble ‘Rough’ and ‘Machining’ to PartBody. To see the results assemble Rough Body first.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Exercise Recap: Wireframe and Multi-Body
Student Notes:
Create a wireframe geometry Create a multi-body structure Create a groove feature Create a hole feature Create a pocket feature
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Create Boolean Operations
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts Student Notes:
Case Study: Create Complex Parts Recap Exercise 10 min
In this exercise you will create the case study model. Let us recall the design intent of this model:
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The thickness (A) must be 10mm. The height of the Hub (B) must be 12.5mm. The draft on the Hub (B) must be 25degrees. The height of the Hub (C) must be 5mm. The default fillet radius must be 20mm. Boolean Operations must be used to get the final result. The reference geometry elements must be organized into a single geometrical set.
A
B
C
Using the techniques you have learned so far, create the model without detailed instruction.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Do It Yourself: Create the Knuckle
Student Notes:
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Load Start_CaseStudy8.CATPart and create the model using the drawing provided here.
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CATIA V5 Automotive - Chassis Lesson 8: Create Complex Parts
Case Study Recap: Knuckle
Student Notes:
Open an existing part Create bodies to use the multi-body method Create pads, thickness and fillets Create Boolean Operations
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Save and close the document
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