CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Contextual Design
Student Notes:
In this lesson, you will be introduced to designing in context
Lesson Content:
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Case Study: Contextual Design Design Intent Stages in the Process Clarify the display Create Contextual Parts Create Assembly-Level Features Manipulate the Contextual Components Save the Contextual Models
Duration: Approximately 7 Hours
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Case Study: Contextual Design
Student Notes:
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The case study for this lesson is the completion of an earphone, as shown below. The focus of this case study is the creation of a cover part. The features that are used to design the cover part are created within the context of the existing components. This method ensures that the cover part will interface properly with the existing components.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Design Intent (1/2)
Student Notes:
The model of the earphone must meet the following design intent requirements: Contextual links must be used. •
This will ensure that changes to referenced parts are reflected in the contextual part.
Contextual links can only reference the housing component Using the Analyze dependencies tool you can ensure that only the Housing component is referenced.
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•
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Design Intent (2/2)
Student Notes:
The model of the earphone must meet the following design intent requirements (continued): The oval cut may need to intersect other components that have not yet been created. • Additional components may be added to this assembly depending on the model. By creating the cut at the assembly level you can control the components the cut will intersect.
The assembly must be saved to another directory in its entirety.
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• Using the Send To Directory option you can be sure that all files associated with the assembly are copied to the required directory.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Stages in the Process
Student Notes:
Use the following steps to create the model of the earphone: Clarify the display Create contextual parts Create assembly features Manipulate the contextual components Save the model
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1. 2. 3. 4. 5.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Clarify the Display In this section, you will learn how to clarify the display and improve the performance of CATIA when working with large assemblies.
Use the following steps:
1. 2. 3.
4.
Create contextual parts. Create assembly-level features. Manipulate the contextual components. Save the Contextual Models
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5.
Clarify the display.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Working with Large Assemblies
Student Notes:
In complex industrial assemblies, the root assembly contains a large number of components and instantiations, which results in a large overall assembly. This may adversely affect CATIA's performance, it can take longer to open, zoom, pan, update and save large assemblies. It can also take more time to generate and update drafting views. The following tools can be used to help improve the performance of CATIA when working with large assemblies:
Visualization mode
B.
Hiding components
C.
Deactivating representations
D.
Deactivating components
E.
Selective load
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A.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Visualization Mode
Student Notes:
By default, an assembly is loaded in design mode. The exact geometry and parameters of all components are loaded in memory. This step can involve longer time for larger assemblies. To improve the performance, you can set the option to load an assembly in visualization mode. In this mode, only a representation of the geometry is loaded. If a document is loaded in design mode, the components in the tree will be expandable because the exact geometry is loaded.
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If a document is loaded in visualization mode, the components in the tree cannot be expanded because the graphical information is being read from a CGR file.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Comparison Between Visualization and Design Mode (1/2)
Student Notes:
The following table shows a comparison between visualization and design mode:
Comparison of Design Mode and Visualization Mode Behavior
Design Mode
Visualization Mode
Memory and Performance Loaded in Memory
Fully Loaded
Load and Update Performance
Normal
Display Performance
Normal
Visibility Visible in Show
Partially Loaded Faster, which is benefit over design mode Normal
Yes
Yes
Visible in Non show
Yes
Yes
Viewable in Non Shaded Mode
Yes
Yes
Viewable in DMU and Sketcher Section
Yes
Yes
Visible in Drafting
Yes
Yes, Automatically switches to Design mode
Accessible for adding Assembly Constraints
Yes
Yes, Automatically switches to Design mode
Assembly Constraints regenerated Updated
Yes
Yes, Automatically switches to Design mode
Accessible to define translation and Notation
Yes
Yes, Automatically switches to Design mode
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Assembly Constraints and Transformation
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Comparison Between Visualization and Design Mode (2/2)
Student Notes:
The following table shows a comparison between visualization and design mode:
Comparison of Design Mode and Visualization Mode Behavior
Design Mode
Visualization Mode
Analysis Calculated in Clash,Clearance,Contact
Yes
Yes
Calculated in Mass Property Analysis
Yes
No
Accessible for Measurement
Yes
No, other than minimum distance measurement
Part Geometry Geometry features accessible in Tree
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Geometry may be edited
Yes
No
Yes
No
Geometry may be used to define sketches & features in other parts in the assembly (eg: up-to-plane)
Yes
Yes, automatically switched to Design mode
In context features re-generated/updated (eg: associativity)
Yes
Yes, automatically switched to Design mode
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
User Setting: Turning on the Cache (1/2) Turning on the cache system will automatically load the components in visualization mode. The cache is a read-write path located locally on your machine or anywhere on your network and is used to store CGR files. The first time a component is inserted, a corresponding CGR file is computed and saved in the local cache as well as displayed in the document window. The next time this component is required, the CGR file which already exists (and not the original document) is automatically loaded from the local cache.
1
Use the following steps to turn on the cache 3
1. 2.
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3. 4. 5.
Select Tools > Options. Expand the Infrastructure node and select Product Structure. Activate the Work with the cache system option. Click OK to the warning message. Click OK to confirm. Restart CATIA.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
User Setting: Turning on the Cache (2/2)
Student Notes:
Depending on whether you are in design mode or visualization mode, the ability to edit the component is different: A.
With the cache system (visualization mode), the component branches in the tree are not expandable and therefore the part bodies are not accessible. In this mode, you are working with CGR files.
A
B
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B.
Without the cache system (design mode), you can edit the components by expanding the component’s branch in the tree.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Manually Switching to Design Mode
Student Notes:
Components can be manually switched from visualization mode to design mode without having to restart CATIA. Use either of the following methods to manually switch from visualization mode to design mode: Double-click a part in the specification tree.
B.
Click Representations > Design Mode from the contextual menu of a component.
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A.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Automatic Switch to Design Mode The Automatic Switch to Design mode option allows you to add constraints between components that have been loaded in visualization mode. Use the following steps to add a constraint between two components loaded in visualization mode:
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1.
1
Ensure that the Automatic switch to Design mode option is activated under Tools > Options, Mechanical Design node, Assembly Design node, General tab.
2.
Select a constraint tool, such as coincidence constraint.
3.
The pointer will display an eye next to the arrow when it is on geometry. Select the required geometry to make the constraint.
4.
The two constrained components switch to design mode automatically.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Update Status Unknown
Student Notes:
The Compute exact update status at open option loads the minimal data needed in assembly components to determine whether or not the assembly is updated. Access the option from Tools > Options, Mechanical Design node, Assembly Design node, General tab. When the Update icon is available, select it.
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When the Update icon is not available, the status of the active model is up to date.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Hiding Components
Student Notes:
Hiding components can improve display performance and reduce clutter in the show space. Hiding a component will make it invisible in the show space and in drawing views. Its icon in the tree will be unavailable. The hide/show state of a component is stored in the CATProduct file. Hiding components is similar to deactivating components, but with the added advantages of: excluding components from drawing views
•
part elements remaining accessible to design parts and assemblies
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Comparison Between Show and Hide (1/2) The following table compares the capabilities of show and hide while in design mode:
Comparison of Show and Hide (In Design Mode) Behavior
Shown
Hidden
Fully Loaded
Fully Loaded
Memory and Performance Loaded in Memory Load and Update Performance
Normal
Display Performance
Normal
Visibility Visible in Show
Normal Faster, which is benefit over being Shown
Yes
No
Visible in Non show
Yes
Yes
Viewable in Non Shaded Mode
Yes
Yes
Viewable in DMU and Sketcher Section
Yes
Visible in Drafting
Yes
Yes No, which is benefit over being deactivated
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Assembly Constraints and Transformation Accessible for adding Assembly Constraints
Yes
Yes
Assembly Constraints regenerated Updated
Yes
Yes
Accessible to define translation and Notation
Yes
Yes
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Comparison Between Show and Hide (2/2) The following table compares the capabilities of show and hide while in design mode:
Comparison of Show and Hide (In Design Mode) Behavior
Shown
Hidden
Analysis Calculated in Clash,Clearance,Contact
Yes
No
Calculated in Mass Property Analysis
Yes
Yes
Accessible for Measurement
Yes
Yes
Geometry features accessible in Tree
Yes
Yes
Geometry may be edited
Yes
Yes
Geometry may be used to define sketches & features in other parts in the assembly (eg: up-to-plane)
Yes
Yes
In context features re-generated/updated (eg: associativity
Yes
Yes
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Part Geometry
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Hiding Components Use the following steps to hide a component: 1.
Select the component to be hidden.
2.
Select the Hide/Show icon. The component will be hidden.
1
You can use contextual menu to Hide/Show a component. 3.
Right-clickon the component to hide.
4.
Select Hide/Show to hide the component.
2
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Showing Components Use the following steps to show a component 1.
Select the component to be shown.
2.
Select the Hide/Show icon. The component will be shown.
1
You can use contextual menu to Hide/Show a component. 3.
Right-click on the component to show.
4.
Select Hide/Show to show the component.
2
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Deactivating Representations
Student Notes:
Deactivating representations can improve performance and reduce clutter in no show space. Deactivation can also be used to exclude representations from mass property analysis. A deactivated representation will have a gray axis symbol instead of a red axis symbol. The activation/deactivation state is stored in the CATProduct. The default geometric representation is activated while opening an assembly. If there is only one representation, it is the default. Deactivated representations are not visible in the show or no show space.
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The deactivation of representations is similar to hiding components, but with the added advantages of: • improving performance while opening assemblies • excluding representations from mass property analysis
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Why Deactivate Representations? (1/2)
Student Notes:
Deactivating representations provide the following benefits: Mask Active representations in the specification tree and in the geometry: Visualize the geometric representation of CATIA elements belonging to a CATProduct. With the Deactivate Node functionality, only the selected element is hidden. Whereas with the Deactivate Terminal Node functionality, the last node's elements of the selected node are masked.
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Improve Performance: Deactivating representations will prevent the components from being loaded into memory. The end result is an improvement in the performance of CATIA. It will take less time to open, pan, zoom and save large assembly documents. Hide Representations from No Show Space: By deactivating representations, the components are not represented even in the no show space. Hiding the representations will move the components into the No Show space. In this sense, deactivating representations is better than hiding representations.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Why Deactivate Representations? (2/2)
Student Notes:
Deactivating representations provide the following benefits (continued): You can activate or deactivate Shape representation in Tools -> Options, Infrastructure, select the Product Visualization tab and check the box entitled Do not activate default shapes on open. The entity representation disappears, it is a profit for memory space. You can work only on the tree.
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Analysis of Assemblies: Deactivated representations are excluded from mass property analysis. At times you are interested to evaluate mass property of partial assemblies. In order to do so, you can deactivate representations which should not be considered for mass property analysis
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Differences Between Activating and Deactivating Representations (1/2)
Student Notes:
The following table compares the capabilities of activating and deactivating representations while in design mode: Comparison of Activation and Deactivation Mode (In Design Mode) Behavior
Activated
Deactivated
Fully Loaded
Fully Loaded
Memory and Performance Loaded in Memory Load and Update Performance
Normal
Display Performance
Normal
Visibility
Normal Faster, which is an advantage over being Activated No
Visible in Show
Yes
Visible in Non show
Yes
Viewable in Non Shaded Mode
Yes
No
Viewable in DMU and Sketcher Section
Yes
No
Visible in Drafting
Yes
No, which is benefit over being Hidden
Yes, even though not visible in Assembly
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Assembly Constraints and Transformation Accessible for adding Assembly Constraints
Yes
No
Assembly Constraints regenerated Updated
Yes
Yes
Accessible to define translation and rotation
Yes
No
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Differences Between Activating and Deactivating Representations (2/2)
Student Notes:
The following table compares the capabilities of activating and deactivating representations while in design mode: Comparison of Activation and Deactivation Mode (In Design Mode) Behavior
Activated
Deactivated
Analysis Calculated in Clash,Clearance,Contact
Yes
No
Calculated in Mass Property Analysis
Yes
No, which is benefit over hiding
Accessible for Measurement
Yes
No
Geometry features accessible in Tree
Yes
No
Geometry may be edited
Yes
No
Yes
No
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Part Geometry
Geometry may be used to define sketches & features in other parts in the assembly (eg: up-to-plane) In context features re-generated/updated (eg: associativity)
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Yes
Yes, after activating and updating the associated part
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Deactivating Representations Use the following steps to deactivate a representation: 1.
Right-click on the component whose representation is to be deactivated.
2.
Select Representations > Deactivate Node from the contextual menu of the component. The geometric representation of the component is deactivated. Note that only the selected instance is deactivated. The deactivated component is represented by a gray axis in the tree symbol.
1
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Activating Representations Use the following steps to activate a representation: 1.
Right-click on the component whose representation is to be activated.
2.
Select Representations > Activate Node from the contextual menu of the component. The geometric representation of the component is activated.
1
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Saving the Activation State (1/2) In order to save the assembly with the representation of some components deactivated, the status of each needs to be stored in the CATProduct file. The Save activation state command allows you to store the activation state but you need to add the icon to a toolbar.
1
2
Use the following steps to add the Save activation state icon to a toolbar:
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1.
Select Tools > Customize. The Customize dialog box will appear.
2.
Select the Commands tab.
3.
Select All Commands.
4.
Select Save activation state from the list and drag it onto a toolbar.
5.
Click Close the dialog box.
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4
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Saving the Activation State (2/2)
Student Notes:
In the example shown, one representation, the connector shell, has been deactivated. If the Save activation state option is selected, the activation states of all the component representations will be saved in the CATProduct. The next time the product is opened, the representation of the connector shell will remain deactivated.
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If the Save activation state tool is not selected, the next time the product is opened, the model will appear as shown below.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Deactivating Components
Student Notes:
Deactivating a component removes its representations and instances. The operation is simultaneous in all the CATIA documents containing this element . This operation is shared by all the instances of this part. You can apply this functionality on CATProducts, CATParts and models. Deactivated components are not visible in the show or no show space.
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In the example shown, the connector shell is deactivated. Note the change in its icon in the tree.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Why Deactivate Components?
Student Notes:
Deactivating components has the following advantages:
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Exclude components from show and no show space: By deactivating components, these components are neither in the show nor in the no show space. This results in less cluttering of the no show space. Removing components from the bill of materials: Deactivating a component will remove the component from the bill of materials. This behavior allows for a bill of materials to be generated for various configurations of an assembly.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Differences Between Modes (1/2) The following table highlights some key reasons for using visualization mode, deactivation, and hide: Comparison of Modes Deactivated Mode
Design Mode
Visualization Mode
Fully Loaded
Partially Loaded
Loaded and Update Performance
Normal
Faster
Normal
Normal
Display Performance
Normal
Normal
Faster
Faster
Visible in Show
Yes
Yes
No
No
Visible in No-Show
Yes
Yes
No
Yes
Visible in non-shaded mode
Yes
Yes
No
Yes
Visible in DMU and sketcher sections
Yes
Yes
No
Yes
Visible in Drafting
Yes
Yes
No
No
Accessible for adding Assembly constraints
Yes
Yes
No
Yes
Assembly constraints regenerated/updated
Yes
Yes
Yes
Yes
Accessible to define translations & rotations
Yes
Yes
No
Yes
Behavior
(Design Mode)
Hidden (Design Mode)
Memory and Performance Loaded in Memory
Fully Loaded
Fully Loaded
Visibility
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Assembly Constraints and Transformations
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Differences Between Modes (2/2) The following table highlights some key reasons for using visualization mode, deactivation, and hide: Comparison of Modes Deactivated Mode
Design Mode
Visualization Mode
(Design Mode)
(Design Mode)
Calculated in Clash, Clearance, Contact
Yes
Yes
No
No
Calculated in Mass Property Analysis
Yes
No
No
Yes
Accessible for Measurements
Yes
No
No
Yes
Geometry features accessible in tree
Yes
No
No
Yes
Geometry may be edited
Yes
No
No
Yes
Geometry may be used to define sketches and features in other parts (e.g. up to plane)
Yes
Yes
No
Yes
In context features regenerated/updated (e.g. associative)
Yes
Yes
Yes
Yes
Behavior
Hidden
Analysis
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Part Geometry
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Deactivating a Component (1/2) Use the following steps to deactivate a component: 1.
Select X.X object > Activate/Deactivate Component from the contextual menu of the object to be deactivated.
2.
The object will be removed from the display, but it will remain in the tree with the deactivated icon symbol. 1
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Deactivating a Component (2/2)
Student Notes:
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In contrast to deactivating a node, deactivating a component inside a assembly will remove its representation in all the CATIA documents containing this assembly.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Effects on the Bill of Materials
Student Notes:
Depending on which operation is used to manipulate the representation, the component may or may not show in the Bill of Materials (BOM): A.
Deactivating a component will remove it from the BOM.
B.
Deactivating a node will not remove the component from being listed in the BOM.
C.
Unloading a component will remove it from the BOM.
D.
Hiding a component will not remove it from the BOM. A B
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C
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Selective Load
Student Notes:
All the documents in an assembly need not be loaded, especially when working with a large assembly. Use the Selective Load tool to manage the progressive load of a product by specifying the level of depth. This tool requires the options to be set as follows:
• The Load referenced documents option must not be checked. This option can be found in Tools > Options, General node, General tab.
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• The Work with the cache system option must be checked. This option can be found in Tools > Options, Infrastructure node, Product Structure node, Cache Management tab. • The Do not activate default shapes on open option can be checked or unchecked. This option can be found in Tools > Options, Infrastructure node, Product Structure node, Product Visualization tab.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Using the Selective Load Tool (1/2) Use the following steps to load only a portion of the components in an assembly: 1.
2.
Ensure the following options have been set: a.
Load referenced documents must be unchecked.
b.
Work with the cache system must be checked.
c.
Do not activate default shapes on open can be checked or unchecked.
Select the Selective Load icon. The Product Load Management dialog box will appear.
1a
1b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Using the Selective Load Tool (2/2) Use the following steps to load only a portion of the components in an assembly (continued): 3.
Select the components to load.
4.
Select the icon shown to add the selected components to the list.
5.
Select the depth desired. The options are 1, 2, or all. If a depth of 1 is selected, then only the components that have been directly selected will be loaded and not anything in a sub-node.
4
Click Apply or OK to load the selected components.
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6.
3
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
To Sum Up (1/2)
Student Notes:
In this section, you have learnt how to improve the performance of CATIA when working with large assemblies. The following are some key points of each method: Hiding components: Display performance can be improved by hiding components which are not being edited. Deactivate representations: Deactivated representations are not loaded in the memory and this improves the performance of CATIA, and takes less time to open, zoom, pan, and save large assemblies. Deactivate components: Deactivated components are not represented in the Bill of Materials of an assembly. This behavior allows for a Bill of Materials to be generated for various configurations of an assembly.
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Using visualization mode: With this mode components are partially loaded (only the CGR is loaded) and this improves the performance of CATIA. To edit the component, change to switch to design mode.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
To Sum Up (2/2) The following is a summary of the effects of an assembly document in various modes:
Component Status
NO SHOW (Hiding Components)
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UNLOAD (Unloading Components)
Visualization (Shape Representation)
NO
Accessibility (possibility of applying constraints) YES (you can apply constraints between the hidden object and the other components in the show space)
Improvement in Performance
NO
NO
NO
YES
Deactivating a Node
NO
YES (you can apply a constraint even if the shape is deactivated)
YES
Deactivating a Terminal Node
NO
YES
Deactivating a Component
NO
NO
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YES
NO
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Component Visualization
Student Notes:
Recap Exercise 20 min
In this exercise, you will use the skills learnt in the lesson to manipulate the display of assembly components. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Hide/Show components
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Activate/Deactivate components
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (1/9) 1. •
Open a product file.
1a
Hide and Show Parts, Sub-Assemblies, and Products
a. b.
c.
Open Brush.CATProduct. You can hide a part even if other parts are constrained to it. Select Handle from the specification tree and rightclick to Hide/Show. The Handle part is no longer visible
1b
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1c
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (2/9) 1. •
Open a product file. (Continued) Hide and Show Parts, Sub-Assemblies, and Products
d.
Select the Swap visible space icon. By
e.
View the handle part in the no-show space. Right-click to Hide/Show the Handle part, it is no longer visible in the noshow space.
f.
1d
viewing no-show space, all part level features, complete parts and assemblies that have been hidden can be seen.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (3/9) 1. •
1g
Open a product file. (Continued) Hide and Show Parts, Sub-Assemblies, and Products
g.
Now Hide the Product files: Select the Swap visible space icon.
h.
Multiple part files and/or product files can be hidden in the same operation. Select
i. j.
(Bristle.4) and (Bristle.7) while holding the key down to multi-select. Hide/Show the products. The products are hidden.
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1h
1i
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (4/9) 1. •
Open a product file. (Continued) Hide and Show Parts, Sub-Assemblies, and Products. k. Individual parts of a sub-assembly can be hidden without affecting the subassembly. Now hide the parts inside the Product files.
l. m.
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n. o.
Expand the (BristleInsert.1) node. Multi-select (Bristle.4) to (Bristle.7) inclusive. Hide/Show the selected parts. The selected Bristle parts of the BristleInsert sub-assembly are hidden.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (5/9) 1. •
Open a product file. (Continued) Hide and Show Parts, Sub-Assemblies, and Products.
p.
2. •
1p
Return all hidden components to Show. There is no method in which you can show all the components, while you are in the Assembly Design workbench.You must show hidden components manually
Deactivate a sub-assembly. By deactivating a component, the update time will be reduced.
a. b.
Select (BristleInsert.1) Right-click to Activate/Deactivate Component.
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2b
2a
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (6/9) 3.
View the model. •
A deactivated component does not appear in the display and has a different symbol in the specification tree.
a.
4.
Notice that the symbol in the specification tree has changed to indicate that this component is deactivated.
3a
Deactivate components. •
Components for deactivation cannot be multi-selected. You must deactivate them one at a time.
Deactivate (BristleInsert.2) and (BristleInsert.3)
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (7/9) 5.
Deactivated components are not in session. •
Unlike a hidden component, deactivated components are not in no-show space.
a. b.
c.
6.
Activate deactivated components. •
The process used to deactivate a component can be applied to reactive it.
6a
Activate all the deactivated components.
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a.
5a
View the no-show space. The deactivated subassemblies are not visible. Toggle the display back to visible space.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (8/9) 7.
View the data that is in session. •
When a component is active, all the design information is available.
a.
8.
Expand (Insert.1) part from the (BristleInsert.1) subassembly to view the PartBody and Geometrical Set.
Deactivate representations. •
Deactivate Terminal Node is used for assemblies, whileDeactivate Node is used for part files.
Select (BristleInsert.1), right-click and select Deactivate Terminal Node.
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a.
7a
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (9/9) 9.
View the result of deactivating representations. •
A deactivated representation is not visible in the display
a.
When component representations are deactivated, the product structure is still visible in the specification tree but the data is not available.
9a
10. Activate representations. •
Activate Terminal Node is used to reactivate representations.
a.
10a
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b.
Activate Terminal Node of (BristleInsert.1) subassembly. Save the product file.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Component Visualization Recap
Student Notes:
Hide/Show components
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Activate/Deactivate components
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Visualization Mode
Student Notes:
Recap Exercise 20 min
In this exercise, you will use the tools learned in this lesson to open the assembly with all components unloaded. You will then load selected components into the assembly. You will also activate the cache system and investigate how this option affects the product. Detailed instructions for new topics are provided. By the end of this exercise you will be able to: Load selective components
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Work with Cache system
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (1/12) 1. Set options •
The representation of product visualization can be set such that the shapes are not active while opening the file.
a. b. c.
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d.
By default, all shapes are loaded. Open Cylinder.CATProduct. Click Tools > Options > Infrastructure > Product Structure. Select the Do not activate default shapes on open option. Click File > Close.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (2/12) 1. Set options. (Continued) •
The representation of product visualization can be set to not activate shapes when opening the file.
e.
f.
Reopen Cylinder.CATProduct. All the shapes are not loaded due to the option you have just set.. The product is not visible in the display, instead, the product structure is visible but does not hold any data.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (3/12) 2.
Activate a component. •
• •
The product file will retrieve very quickly as the data is not loaded. Now choose the components which you want to load. View the Activated component. Activate Terminal Node for Assemblies
a. b. c. d.
Activate Node of the BucketGland part. View the data of BucketGland part. Activate terminal node of RodAssy View the data that has been loaded.
2a
2b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (4/12) 3.
Change settings. •
Access the Options dialog box.
a.
b. c. d. e.
f. g.
Clear the Do not activate default shapes on open option. Select the Cache Management tab. Select the Work with cache system option. Accept the Warning. While working with cache management, you must close and restart the application. Click File > Exit. Open CATIA V5.
3a
3b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (5/12) 4.
Open a product file. •
• •
Now the application uses *.cgr files to generate a representation of components. You are now working in visualization mode. Switch a component to design mode. View the component in design mode.
a. b.
c.
4a
Open Cylinder.CATProduct. The components are visible but the product structure holds limited data. Hold the pointer over any representation to see the tessellated surfaces.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (6/12) 4.
Open a product file. (Continued) •
• •
Now the application uses *.cgr files to generate a representation of components. You are now working in visualization mode. Switch a component to design mode. View the component in design mode.
d.
e. f.
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g.
If changes are required for a component that is in visualization mode, it must be switched to design mode. Right-click on BucketGland and select Design Mode from the contextual menu. Switching a component to design mode will load all the data relating to that component. All the data for the BucketGland is now available.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (7/12) 5.
Make a modification to a component. •
Now that the BucketGland is in design mode, modifications are allowed.
Activate the BucketGland part. Edit Shaft.1 Edit dimension 23. Change the value to 24. Save the part. 5d Activate the Cylinder assembly.
5c
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a. b. c. d. e. f.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (8/12) 6.
Switch a component back to visualization mode. •
Once a component is switched to visualization mode, the data is no longer available.
a.
Switch BucketGland back to visualization mode. The BucketGland is now a tessellated representation again.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (9/12) 7.
Change general settings. •
Access the Tools > Options. Clear Load reference documents option and clear work with cache system settings.
a.
b. c. d.
By clearing the Load reference documents option, the application will not load any components. Clear the Load referenced documents option. Clear the Work with cache system option. Exit and restart CATIA.
7b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (10/12) 8.
Selectively Load and Manage Components. (Continued) • • •
Use selective load to manage component loading. View the loaded component. Selectively load a subassembly. Open Cylinder.CATProduct
a. b. c. d. e. f. g.
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h.
Open Cylinder.CATProduct. The representations are not visible. View the symbols in the specification tree Load management allow you to choose the components to be loaded. Select Selective Load icon. Select BucketGland part. Select the Selective Load icon from the dialog box. Apply the selective load.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (11/12) 8.
Selectively Load and Manage Components. (Continued) • • •
Use selective load to manage component loading. View the loaded component. Selectively load a sub-assembly. Open Cylinder.CATProduct i. The selected component is loaded visually and all the data is loaded. j. All the data is available for the loaded part. k. Parts and or subassemblies can be selected for selective loading. l. Use selective load to load RodAssy.
8j
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (12/12) 8.
Selectively Load and Manage Components. (Continued) •
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• •
Use selective load to manage component loading. View the loaded component. Selectively load a subassembly. Open Cylinder.CATProduct m. Selective loading option will save your time because only the components you need will be loaded. n. The loaded components have all the data loaded. o. Change settings. Loaded referenced documents does not affect a product file that is already opened. p. Activate the Load referenced documents option. q. Save the file and close the window.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Visualization Mode Recap
Student Notes:
Load selective components
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Work with the cache system
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Create Contextual Parts In this section, you will learn how to create contextual parts.
Use the following steps:
1.
Clarify the display.
3.
Create assembly-level features. Manipulate the contextual components. Save the Contextual Models
2.
4.
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5.
Create contextual parts.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
What are Contextual Parts? An assembly is a CATProduct document containing components, such as CATParts, CATProducts, V4 models and models from external sources (IGES, STEP, VRML). The individual parts are positioned relative to each other and they are constrained with assembly constraints. In addition to this, assembly design allows you to design contextual parts.
Plane of a skeleton part
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Contextual parts are parts that have their geometry driven by another component. A change in the driving geometry of the referenced part will result in changes in the contextual part. In the example shown, the depth of housing and height of insert is contextually controlled by the plane of skeleton part. The depth of housing and height of insert are defined as up to the plane of the skeleton part. If the dimension of skeleton plane will change, then the housing depth and insert height will change consequently.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Contextual Parts Using External Parameters
Student Notes:
When a part refers to parameters defined in another part, a contextual part using external parameter is created. In the example shown, a pin support is designed contextually. The inside diameter of the support uses the radius of the pin as a reference parameter. When the pin diameter is reduced, the pin support turns red because the inside diameter of the pin support references the diameter of the pin. An update of the pin support is required.
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After updating the assembly, the inside diameter of the pin support is updated to match the diameter of the pin.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Contextual Parts Using External References
Student Notes:
When a part refers to geometrical elements defined in another part, a contextual part using external references elements is created. In the example shown, a base part is designed contextually. The hole from the pin support is used as an external reference to create the hole in the base part. When the hole diameter in the pin support is reduced, the base part turns red because the hole in the base part references the hole of the pin support. An update of the base part is required.
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After updating the assembly, the hole diameter in the base part is updated to match the hole diameter in the pin support.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Contextual Parts Using Assembly Features
Student Notes:
A contextual link is also created when an assembly remove feature is created using an existing part. In the example shown, a pin is used to create an assembly remove feature in the pin supports and housing.
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Any change in the pin, such as an increase in diameter or modification in its shape, will affect the pin supports and housing.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Why Design in Context?
Student Notes:
Designing in context is a part of concurrent engineering design. It has the following benefits: Reuses existing geometry: In order to facilitate design, you can reuse any geometrical element defined in one part to aid in the creation of another part. For instance, you can reuse an existing sketch in another part instead of re-creating it. You can also reuse a geometrical entity such as a point, line, curve, plane or a surface.
Reuses parameters: You can reuse parameters defined in one part to aid in the creation of another part.
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Automatic update of an assembly and its contextual parts: When designing in context, the contextual part is automatically updated when the geometry of the referenced part changes. It is not necessary to edit the contextual part manually to reflect the change in design because of design in context.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Contextual Part Specification Tree Symbols There are three specification tree symbols that are specifically related to contextual parts and they are as follows: A.
B.
C
A
The brown gear and red flash indicates the object is the second or subsequent instance of a part that is contextual. For example, this symbol can appear for a contextual part that was copied and pasted into a separate CATProduct. The white gear and green arrow indicates the object is the original instance of a part defined in context of an intermediate document.
A
B
C
B
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C.
The green gear and blue chain indicates the object is the original instance of a part that is contextual. The component, in other words, is driven by another part in the CATProduct.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Creating Contextual Elements Contextual elements can be created while designing sketches and features in context. External geometry is copied from driving parts to contextual parts that are being driven. The copies are organized in the External References branch of the part.
1
Use the following steps to create contextual elements: 2
Check the Keep link with selected object option.
2.
Click the Pad icon and select the sketch.
3.
Select the length type as Up to plane and select Housing_Height plane of skeleton part.
4.
Click OK to complete the pad definition. This pad is now contextually designed.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Constraining Contextual Instances of Parts (1/2) Assembly constraints are forbidden when there is a potential conflict between geometric and assembly constraints. Assembly constraints are always forbidden when any element in a sketch is associative. Two cases will be discussed: one case where the geometrical and assembly constraints are in conflict and another where they are not in conflict.
1
Case 1: Geometrical constraints and assembly constraints are in conflict. 1.
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2.
A housing component is sketched on a plane which is defined in the base plate component. Also, the sketch is constrained using the edges of the base plate component. The pad’s sketch has external links to the base plate.
2
If an offset constraint is applied between the highlighted faces, a warning message will appear as shown. The offset constraint is forbidden because it would cause a potential conflict between the sketch and assembly constraint.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Constraining Contextual Instances of Parts (2/2)
Student Notes:
Case 2: Geometrical constraints and assembly constraints are not in conflict. A sketch of the shaft is designed using the face of the housing part, but it is not concentric with respect to the housing pocket. The shaft has an external link to the housing part.
2.
An assembly coincidence constraint is allowed between the axis of the shaft and the axis of the housing part, as there is no conflict between the geometrical and assembly constraint. The sketch plane reference of the shaft was the only external link to the housing, which does not conflict with the assembly coincidence constraint.
1
2
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Constraining Non-Contextual Instances of Parts
Student Notes:
Assembly constraints can be used when there is no conflict between assembly and geometry constraints. Non-contextual parts can be constrained using assembly constraints as these parts have no conflicting geometric constraints. The right insert is a copy of the left insert. It is a non-contextual instance, which means it is not designed in context. It can be positioned using assembly constraints because none of the geometric elements of the part were contextually defined within this instance of the part.
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When constraining contextual parts, you cannot use geometrical elements that have external references to other parts as parents. Geometrical elements that have no link with external geometry or parameters can be used. Examples of such geometrical elements include XY, ZX and ZY planes, a point built with coordinates and a line defined with an angle from the Z axis.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Sketch in Context
Student Notes:
It is possible to reuse a sketch created in one part to define another part. The result is that the two parts share the same sketch. If the sketch in the original instance is modified, the geometry of the contextual part is also modified.
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In this example, the pad of the fixture cover reuses sketch.1 of the housing part. As a result, the fixture cover is contextually linked to the housing part and an external reference is added to the specification tree.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Why Use a Sketch in Context?
Student Notes:
Depending on the situation, it is better to select the same sketch to define two different parts rather than using projections of edges of one part to define the other. In the first example, edges are projected from the green part into the sketch of the other. Many external references are created which have to be synchronized every time the sketch changes.
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In the second example, the sketch of the housing part is directly used to create the pad of the fixture cover. By choosing this method, there is only one external reference to synchronize, which makes the update faster.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Using a Sketch as an External Reference (1/2) Perform the following steps to use a sketch as an external reference: 1.
Edit the part in the assembly in which the new feature is to be created.
2.
Select the icon for the feature to be created. This example will use the Pad icon.
3.
Select a sketch from another part in the assembly to be used as the profile. The Selection in Context warning box will appear.
4.
Click Yes to keep the link with the selected object.
5.
Define the limits and direction for the feature.
6.
Click OK. The new feature will be created.
1
3
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Using a Sketch as an External Reference (2/2)
Student Notes:
Perform the following steps to use a sketch as an external reference (continued): Activate the assembly and attempt to move the component.
8.
Select the Update icon. Note that the position of the component relative to the original sketch impacts its geometry. Relative positions of the pad (linked to the external reference, Sketch.1) and the reference planes of the part have changed. Sketch.1 remains an exact copy of the original sketch.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Parameters in Context During assembly design, you can have parameters of one part driven by parameters of another part in the assembly. Parameters of the assembly itself could also be used to drive a parameter of one of its components.
B
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In the example shown, the highlighted parameter relating to the fixture cover (part A) with a value of 6 needs to be made equal to the parameter in the holder (part B) with a value of 5. A formula is created to relate the two parameters. Once the link between the parameters is created, any change made to the referenced parameter in the holder will reflect in the fixture cover.
A
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Creating a Parameter in Context (1/3) Use the following steps to create a parameter in context: 1.
Edit the part in the assembly in which the formula is to be created.
2.
Select the Formula icon. The Formula dialog box will appear. Select the parameter to be driven.
3.
Select the Add Formula button. The Formula Editor dialog box will appear.
4.
Select the part that contains the driving parameter from the specification tree. The External parameter selection dialog box will appear.
1 2
3
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Creating a Parameter in Context (2/3) Use the following steps to create a parameter in context (continued): 5.
Select on the feature that contains the driving parameter. The parameters related to the feature will appear in the model. Select the driving parameter. The parameter is placed into the formula editor box.
7.
Click OK to confirm.
8.
Click OK from the Formula Editor dialog box.
9.
Click OK from the Formula dialog box to confirm.
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6
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Creating a Parameter in Context (3/3) Use the following steps to create a parameter in context (continued): 10. After the parameter is created in context, the component still has a yellow gear for its specification tree symbol indicating that it is not contextual to the assembly. Also, the Length parameter is added to the External Parameters node in the tree and the formula is added to the relations node. 11. The Parents and Children box for the external parameter, Length, in the fixture cover displays the link to the parameter in the holder.
10
10
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Using an Assembly Parameter to Design a Part (1/3) A parameter of a part in an assembly can also be driven by a parameter in the assembly itself. Perform the following steps to use an assembly parameter to design a part: 1.
Edit the part in the assembly in which the formula is to be created.
2.
Select the Formula icon. The Formula dialog box will appear. Select the parameter to be driven.
3.
Select the Add Formula button. The Formula Editor dialog box will appear.
4.
Select the assembly node from the specification tree. The External parameter selection dialog box will appear.
1
2
3
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Using an Assembly Parameter to Design a Part (2/3) Perform the following steps to use an assembly parameter to design a part (continued): Select the driving parameter from the specification tree.
6.
Click OK from the External parameter selection dialog box.
7.
Click OK from the Formula Editor dialog box.
8.
Click OK from the Formulas dialog box.
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5
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Using an Assembly Parameter to Design a Part (3/3) Perform the following steps to use an assembly parameter to design a part (continued): 9.
After the parameter is created in context, the component still has a yellow gear for its specification tree symbol indicating that it is not contextual to the assembly. Also, the FittingHeight parameter is added to the external parameters node in the tree and the formula is added to the relations node.
9
9
10. The Parents and Children box for the external parameter, FittingHeight, in the holder displays the link to the assembly parameter.
9
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
External Parameters
Student Notes:
External parameters are linked copies of parameters that exist in external documents. In order to be able to create them, the Keep link with selected object option is checked. The option is located under Tools > Options, Infrastructure, Part Infrastructure, General tab. External parameters can be created in two ways:
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A. Automatically: Refer the parameter of one part to that of another using a relation, as discussed earlier in this lesson. B. Manually: Copy the required parameter, use the Paste Special command in the destination part and then select As Result With Link from the Paste Special dialog box.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Why Use External Parameters?
Student Notes:
External parameters should be used for the following reasons: To reuse a parameter that drives a part into another Part, in order to link their geometry. To help ensure that the design of the two linked parts is consistent. To avoid manual update of all the related parameters in different parts, when a modification occurs.
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In the example shown, the hub needs to adapt to the rim’s holes. External parameters have been created in order to link the number of holes and the bolt pattern diameter of the rim to the same parameters in the hub. If the number of bolt holes in the rim is changed from 4 to 5, because of the link, the number of bolt holes in the hub will also change from 4 to 5.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Fully Constraining Contextual Parts It is important to fully constrain contextual parts to avoid unintentional distortion of geometry. In this example, the housing part is contextually designed and has external references to the geometrical elements of the base part. A.
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B.
The sketch of the pad is not fullyconstrained. 1.
The housing part is rotated.
2.
The geometry of the pad is distorted after an update is made. Upon updating the housing part, the contextual sketch is projected back onto the green part and resulting in the housing part being distorted.
The sketch of the pad is fullyconstrained. 1.
The housing part is rotated.
2.
The housing part is updated without any distortion. Fully constraining the housing part ensures that it maintains the expected location relative to the small brown pad.
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A1 A2
B1 B2
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Fixing Contextual Parts in Space Moving a component can unintentionally cause geometry to move within a contextual part. In the example shown, the slot in the brown part is fully-constrained. A.
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B.
The contextual component is not fixed in space. 1.
The brown component is unintentionally moved.
2.
Updating the small brown part projects the contextual sketch back onto the green part and the pad ends up being in the wrong location.
A1
A2
The contextual component is fixed in space. 1.
The brown component is unintentionally moved.
2.
To avoid unintentional movement of geometry in contextual parts, ensure that the components are in their assembled position before updating contextual parts. Make this process easier by: a.
Firstly fixing the contextual components in space first.
b.
Then updating the assembly to move components back into their fixed-in-space positions.
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B2
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Editing Contextually-Related Parts When contextually-related parts need to be edited, it is important to recognize that there are at least two parts that exist: the contextual part that is driven by another part and the part that drives the contextual part.
Student Notes:
B A
The two kinds of parts involved with contextually-related parts are: A.
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B.
Contextual part: The tree symbol, in this example, has a green gear indicating that it is a contextual part. Also, there is an external reference under the external references node in the tree.
A
Driving part: The tree symbol has a yellow gear and no external references exist in the tree.
If part A drives part B and is driven by part C, then the tree symbol will indicate, for example, a green gear meaning that it is a contextual part.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Editing Driving Parts
Student Notes:
Editing a part that drives a contextual part can cause changes in the contextual part.
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In the example shown, Skeleton part is the driving part. The offset distance of a plane ‘Housing_Height’ has been changed. The height of the housing part is driven by this plane. Accordingly the housing part changes.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Editing Contextual Parts Parts that are contextual to (driven by) other components can be edited within or outside the context of the assembly in which the contextual elements were defined.
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Contextual parts can be edited from the following locations:
A.
Original instance of a contextual part. Often many of the contextual elements are defined here.
B.
Instances of the part that are not the original instance. This can be useful when defining new contextual elements that are dependant on the position of an instance that is not the original instance.
C.
Contextual part on without opening the assembly. The contextual elements cannot be completely updated, however, because the context (assembly and components) in which the contextual elements were defined is not available.
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A
B
C
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Editing a Driving Part After editing driving parts, the contextual (driven) parts will need to be updated in the context of the assembly.
1
Use the following steps to edit a driving part: 1.
Double-click the driving part to be edited.
2.
Make the modification to the driving part. The offset distance of plane ‘Housing_Depth’ will be increased to 6mm.
3.
Activate the root product.
4.
Update the assembly to update the contextual part.
2
3
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Automatically Synchronizing Changes while Editing Driving Parts
Student Notes:
An option exists that synchronizes all contextual elements upon selecting Update. Use the following steps to set the automatic synchronization option and edit a driving part: 1.
Check the Synchronize all external references for update option under Tools > Options, Infrastructure, Part Infrastructure, General tab. Make the modification to the driving part. The offset distance of plane ‘Housing_Depth’ will be increased to 6mm.
3.
Activate the root product.
4.
Select the Update icon to synchronize the changes in the contextual parts.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Manually Synchronizing Changes While Editing Driving Parts (1/2)
Student Notes:
Contextual elements can be synchronized individually. Use the following steps to manually synchronize individual contextual elements when a driving part is modified: Uncheck the Synchronize all external references for update option under Tools > Options, Infrastructure, Part Infrastructure, General tab.
2.
Make the modification to the driving part. The pad offset distance in the example will be increased to 18mm.
3.
Activate the contextual part. Select Parents/Children… from the contextual menu of the feature to be updated.
2
3
3
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Manually Synchronizing Changes when Editing Driving Parts (2/2)
Student Notes:
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Use the following steps to manually synchronize individual contextual elements, when a driving part is modified (continued): 4.
Select Show All Parents from the contextual menu of the required node. All the parents of the select node will be displayed.
5.
Go to the contextual menu of the node of interest in the specification tree and Select Synchronize from the Object menu.
6.
The specification tree icon for the selected element indicates that it is updated.
6
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Replacement Of a Driving Component (1/3) When you replace a component that is used as a reference for other contextual components, the driven components need to be reconnected to the new driving geometry.
2
1
Use the following steps to replace a nonpublished component that is referenced by other components: 1. 2.
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3. 4.
Select the Replace Component icon. Select the component to be replaced. In this example the Unpublished References component is selected. Select the replacing component. A warning dialog box appears indicating that contextual data will be lost. Click OK.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Replacement Of a Driving Component (2/3) Use the following steps to replace a nonpublished component that is referenced by other components (continued): 5.
6. 7.
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8.
A second warning dialog box appears indicating the geometry that is no longer synchronized because their references are lost. Activate the failing part. Notice that the external reference has a red circle on its specification tree icon. This indicates that the element is no longer synchronized. It is not synchronized because the referencing element has been removed from the assembly. Edit the feature that is missing its references. In this example, the Profile and the limiting element have to be redefined. Select new references for both missing elements.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Replacement Of a Driving Component (3/3) Use the following steps to replace a non-published component that is referenced by other components (continued): 9.
Once the geometry has been reconnected, delete the invalid references. 9
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10. The contextual part now references only geometry of the replacing component.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Feature in Context
Student Notes:
Recap Exercise 20 min
In this exercise, you will contextually create a feature in the slide components with the tools learnt in the lesson. Detailed instructions for this exercise are provided.
By the end of this exercise you will be able to:
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Create the Feature in Context
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (1/9) 1.
Set Settings. •
Ensure that external references will maintain a link with source geometry.
a. b. c.
d.
Open Slider.CATProduct. The opened assembly only has a fix constraint for the base component. Click Tools > Options > Infrastructure > Part Infrastructure > General tab. Activate the Keep link with selected object option.
1a
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (2/9) 2.
Add assembly constraints. •
It is a good practice to use assembly constraints to position components.
a. b.
Add a Coincidence constraint between the two reference planes. Add a Coincidence constraint between the two surfaces.
2a
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (3/9) 3.
Add assembly constraints. a. b.
Add a coincidence constraint between the two surfaces. Update the assembly.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (4/9) 4.
Activate a part. •
You need to activate the part file that you want to design features in context for.
a.
5.
Activate Slide part.
4a
Select a sketching plane. •
It is good practice to select a sketching plane reference that is local to the active part.
a.
Select the surface of the Slide part.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (5/9) 6.
Use geometry from Base part. •
You will project 3D elements of the Base part to create a sketch for Slide part.
a. b. c.
7.
6b
View external references. •
External references are created by projecting 3D elements of another part.
a.
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Select Project 3D elements icon. Select the 7 edges of the Base part. Exit the sketcher workbench.
6a
Expand the External References node of the specification tree and view the 7 edges that resulted in external references.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (6/9) 8.
Create a solid feature. •
You will now create a solid feature from the sketch that is defined with external references.
a. b. c. d.
Select the sketch. Select the Pad icon. Specify Up to plane as the depth option. Select the surface as the Limit.
8c
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (7/9) 9.
View the feature created in context. •
This feature is now linked with the Base part.
a. b.
9a
Open Slide part in a new window. View the pad created from a sketch that was created from external references.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (8/9) 10. Modify the referenced geometry. •
10a
You can make any change to the referenced geometry, but keep in mind how it may affect the linked geometry.
a. b. c. d.
Open Base part in a separate window. Edit Pocket.1. Edit the 22 dimension. Change it to a value of 25.
10d
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (9/9) 11. View that affects the change. •
Since the link is stored in the product file, the product file must be loaded and updated to see the lasted geometry.
a. b.
c. d.
11b
Activate the Slider assembly. The application recognizes that the linked geometry is outdated due to the changes made in it. Update the assembly. Save the assembly and close the file.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Feature in Context Recap
Student Notes:
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Create a feature in context
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Sketch in Context
Student Notes:
Recap Exercise 20 min
In this exercise you will modify an existing product file. You will use the tools learnt in the lesson to create a sketch in context. You will also drive geometry using an external reference. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create a sketch in context
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Create a formula that is driven by an external parameter
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (1/8) 1. Open product file. • Open a product file that has a completed part and an empty part.
a. Open SlotMount.CATProduct. 1a
2. Activate part. • You must activate the part that you wish to design in context.
a. Activate SlotCover part.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (2/8) 3. Create a sketch in context. • Create a sketch on a plane that is local to the active part.
a. Use YZ plane as the sketching plane. b. Project the four edges of the slot.
3a
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (3/8) 4. Create a pad. • Create a pad from the sketch created in context. Select the face of the Mount part as the limit for the depth option. Drive the thickness of the part with an external parameter.
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a. Create a Pad. b. Select the Limit type and Limit face. c. Specify the Thick option. d. Use Neutral Fiber option. e. Click Edit formula from the Thickness1 contextual menu. f. Drive thickness with parameter from Mount part.
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4c 4e
4d
4e
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (4/8) 5. View the completed part. • The Slot part is now complete. It has been designed within the context of Mount part. The sketch plane is local to the Slot part, but the geometry is driven by external references and an external parameter of Mount part.
a. The resulting geometry of Slot part design in context.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (5/8) 6. Modify a parameter value. • Modify the value of a diving parameter.
a. Activate the Mount part. b. Modify the parameter value to [5mm]. c. The updated assembly results in changes to both parts.
6a
6b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Do it Yourself (6/8)
Student Notes:
7. View external references. • Open the part designed in context and view the resulting external references.
a. Open Slot part in a separate window. b. Any parameters that are referenced from another part will be listed under the External Parameters node of the specification tree. c. Any projected edges or selected faces will be listed under the External References node of the specification tree.
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7c
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (7/8) 8. Modify referenced geometry. • You should be careful while modifying the geometry of a referenced part as it may affect a driven part.
a. Activate Mount part. b. Edit Sketch.1 c. Modify the 105 dimension to [110deg].
8a
8b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (8/8) 9. Update the assembly. • Since the link between parts is created in the product file, the product file must be updated.
a. Activate the assembly. b. Update the assembly.
9a
10. Save and close the assembly.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Sketch in Context Recap
Student Notes:
Create a sketch in context
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Create a formula that is driven by an external parameter
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Part in Context
Student Notes:
Recap Exercise 20 min
In this exercise you will open an existing product file. You will use the tools learnt in the lesson to complete a component in context of the assembly.
By the end of this exercise you will be able to:
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Create a Part in context of an Assembly
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself 1. Open a product file. •
1a
Design a part using contextual design.
a. Open DriveCoupling.CATProduct. b. Complete the design of Output.CATPart in context of the SpiderDrive.CATPart.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Part in Context Recap
Student Notes:
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Create a part in the context of the assembly
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Create Assembly-Level Features In this section, you will learn how to create assembly-level features and understand how they interact with components in the assembly.
Use the following steps:
1. 2.
Clarify the display. Create contextual parts.
4.
Manipulate the contextual components. Save the Contextual Models
3.
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5.
Create assembly-level features.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Assembly-Level Features (1/2)
Student Notes:
Although the Assembly Design workbench deals with the component and part levels, some features can still be created in this environment.
Geometry
Icon
Description Use a plane, face, surface, or previously created split as a reference.
Hole
Create a hole based on a plane, surface, or previously created part hole.
Pocket
Create a pocket based on a previously created sketch or pocket.
Add
Add a body or an existing add feature.
Remove
Remove a body or an existing remove feature.
Symmetry
Select a plane or surface as a reference to perform symmetry on a part, product, or component.
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Split
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Assembly-Level Features (2/2)
Student Notes:
Once assembly features are created, you can specify which components they will affect. Move the parts you want the feature to affect to the Affected parts section of the Assembly Features Definition window.
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An assembly-level hole feature is created in the assembly below. By setting the parts which are affected, you can control how the feature interacts with specific components.
Through one part
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Through both parts
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
What are Assembly Features? (1/3) Assembly features are features that are applied not only to a single part (from within the part design workbench) but to a set of several parts of an assembly. The following are examples of assembly features: A.
A
Hole: This operation creates a hole passing through multiple parts with a single feature.
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B.
Split: This operation splits one or more parts with the splitting surface with a single feature.
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B
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What are Assembly Features? (2/3)
Student Notes:
The following are examples of assembly features (continued): C.
Pocket: This operation creates pockets in multiple parts in a single instance.
D.
Add: This operation adds a part body to multiple parts in a single instance. The light blue PartBody is added to the two components.
C
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
What are Assembly Features? (3/3)
Student Notes:
The following are examples of assembly features (continued):
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E. Remove: This operation removes material from all affected parts using the geometry of a part body with a single feature. The light blue part body is removed from to the two components.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
What are Affected Parts? Affected parts are parts of the assembly that will be operated on by the assembly feature.
A
When an assembly feature, such as a split, is created, changes are made in the tree: A.
Affected parts become contextually linked.
B.
The linked feature is created in the affected part.
C. Creation and edition of the assembly feature is made at the assembly level. D. Affected parts and linked features are added within the assembly feature in the tree. B
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Specifying Affected Parts Each time an assembly feature is created, the Assembly Feature Definition dialog box will appear and will allow you to specify the affected parts.
A
The Assembly Feature Definition dialog box contains the following features: B
A. Edit the Name of the assembly feature.
D
B. List of assembly parts that are not currently affected by the assembly feature.
E
F
G
C. List of assembly parts that are currently affected by the assembly feature. C
D. Button to move all parts in the upper field to be included in the lower field. E. Move selected parts to the lower field.
H
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F. Button to move all parts in the lower field to be included in the upper field. G. Move selected parts to the upper field. H. Checking this option will highlight all the affected parts in the model.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Creating an Assembly Split For an assembly split, a surface or a plane to make the split is required. The surface need not be one of the affected parts.
1
Use the following steps to create an assembly split:
2
1. Select the Split icon. 2. Select the splitting surface. 3. Specify the affected parts. 4. Select the orientation of the split by selecting the required direction of the arrow.
3
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5. Click OK to confirm. The assembly split is created.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Creating an Assembly Hole 1
For an assembly split, a sketch will be created that will belong to the part containing the reference plane.
2
Use the following steps to create an assembly hole: 1. Select the Hole icon. 2. Select the reference edges and surface for the hole.
3
3. Specify the affected parts. The Add Series button allows you to define different hole specifications for each affected part. 4. Specify hole parameter values and types.
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5. Click OK. The hole is created through the affected parts.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Using Hole Series 1
When creating an assembly hole, you can define different shapes of holes going thru parts of a product within the same assembly feature.
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Perform the following steps to use the hole series option while adding an assembly hole: 1.
From the Assembly Features Definition dialog box, select the Add Series button. A new tab named Series 1 is created.
2.
Select the parts that should be affected by the new hole specification and then select the Select button.
3.
Define the new hole specification using the Hole Definition dialog box.
4.
Add additional series as required by repeating steps 1 through 3.
5.
Click OK to confirm when finished. The assembly hole will be added into the specification tree along with each series that was added. The feature can be modified from the assembly design workbench.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Creating an Assembly Pocket An assembly pocket is a sketch-based feature that requires an existing sketch. This sketch need not belong to one of the affected parts. Use the following steps to create an assembly hole: 1.
Select the Pocket icon.
2.
Select the sketch which will be used to make the pocket.
3.
Specify the parts that will be affected.
4.
Specify the pocket parameter values and types.
5.
Click OK. The pocket is created through the affected parts.
1
2
3
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Adding a Body to an Assembly The Add tool will add a body from a part to the affected parts. The body to be added can belong to one of the assembly components on which the add is being applied.
1
2
Use the following steps to add a body to an assembly: 1.
Select the Add icon.
2.
Select the body to add.
3.
Specify the parts that will be affected.
4.
Click OK. A linked copy of the body is added to each affected part. Hide all the components, except one of the affected parts and the added body can be seen.
4
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Removing a Body from an Assembly The Remove tool will remove the space occupied by a body from the affected parts. The body being removed can belong to one of the assembly components on which the remove is being applied and it can include an entire part body.
1
2
Use the following steps to remove a body from an assembly: 1.
Select the Remove icon.
2.
Select the body to be used for the remove.
3.
Specify the parts that will be affected.
4.
Click OK. A linked copy of the body is removed from each affected part.
4
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Cautions About Designing in Context
Assembly-level features: • Cannot be patterned. • Created from information in components of the active product.
•
Assembly-level hole features: • Appear in the assembly specification tree and the part specification tree. • Hole dimensions are modified at the assembly level. • Hole position is modified at the part level.
•
When referencing components: • Be careful not to create an additional reference from the target to the source part. This can create a circular reference which can cause regeneration errors.
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•
Student Notes:
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Manipulate the Contextual Components
Student Notes:
In this section, you will learn how to manipulate contextual components.
Use the following steps:
1. 2. 3.
4.
Manipulate the contextual components.
Save the Contextual Models
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5.
Clarify the display. Create contextual parts. Create assembly-level features.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Isolating Contextual Parts If a contextual relationship between the driving and contextual part is no longer necessary, the link between the two can be severed. There are two ways to sever the contextual relationships: A.
Sever all contextual relations that exist in a part.
B.
Sever individual contextual relations while leaving others intact.
A
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Reasons for severing contextual links can include: The part is being released and inadvertent changes need to be avoided. The design is stable and there is no longer a need to drive changes between the parts. The assembly and/or components that define the context for contextual elements was inadvertently deleted.
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B
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Isolating All Elements in a Contextual Part Isolating a parts severs its contextual relationship with the driving components so that changes made to the driving parts does not cause any change in the contextual part. Use the following steps to isolate all the contextual elements in a part: Select Components > Isolate Part from the contextual menu of the part to be isolated.
2.
The external references node becomes the isolated external references node and it includes all the previous external references.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Isolating Individual Elements in a Contextual Part Individual contextual elements can be isolated while keeping others intact. Use the following steps to isolate individual elements in a part: Activate the part containing the element to be isolated.
2.
Select Parents/Children… from the contextual menu of the element to be isolated.
3.
Right-click the node of interest and select Show All Parents to see the external references.
4.
Right-click the external reference of interest and select Isolate.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Analyzing Contextual Parts To gain a better understanding about the relationships involved with a particular contextual part, use the Parents/Children and Dependencies tools. Information about the relationships between driving and driven components and elements and documents can be found with these tools.
A
The following are two ways a contextual part can be analyzed: A.
Analyze the relationships between the driving and driven components:
B
In this example, the top block component is a contextual part that is driven by the bottom block component. In turn, the top block drives the round pad component, which is another contextual part.
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B.
Analyze the relationship between driving and driven elements and documents: In this example, sketch.1 has some external references to Pad.1 in the bottom block instance of another CATPart.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Analyzing Relationships Between Driving and Driven Components
Student Notes:
Use the following steps to analyze the relationship between driving and driven components: Select the component to be analyzed.
2.
Click Analyze > Dependencies….
3.
Check the Associativity option and uncheck the Constraints option.
4.
Select Expand all from the contextual menu of the component. In this example, the top block component is a contextual part that is driven by the bottom block component. In turn, the top block drives the round pad component, which is another contextual part.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Analyzing Relationships Between Driving and Driven Components
Student Notes:
Use the following steps to analyze the relationship between the driving and driven external elements and documents: 1.
Select Parent/Children from the contextual menu of the feature to be analyzed.
2.
Right-click on the node of interest and select Show All Parents to see external reference elements and documents.
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To help you graphically see the relationship between driving and driven elements, temporarily show (unhide) the external reference elements and then select the elements to highlight them
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Deleting Contextually-Related Components (1/2)
Student Notes:
Additional options are available for managing data while deleting components that drive the contextual parts or while deleting the contextual components. The two situations that will arise are as follows: A.
Deleting a driven part:
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In the example shown, when the original instance of a contextual part is deleted a warning message appears stating that a new original instance should be established.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Deleting Contextually-Related Components (2/2)
Student Notes:
The two situations that will arise are as follows (continued): B.
Deleting a driving part:
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In the example shown, when a component that drives a contextual part is deleted, the option to delete the contextual components that are driven by the component is available.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Deleting Driving Components Use the following steps to delete driving components: 1. Select the component to be deleted. 2. Press the key.
1
3. Leave the Delete all children option unchecked and select More>>.
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4. Specify the assembly constraints and contextual components to be deleted.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Deleting Contextual Components Use the following steps to delete contextual components: 1.
Select the component to be deleted.
2.
Press the key.
3.
Select OK to the warning message.
4.
Select one of the following operations, depending on what is desired: a. Isolate Part: Use this option to remove all links between the current component and other components, except for the link with the product in which the component is instantiated. Select Components > Isolate Part from the contextual menu of the component.
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b. Change context: Use this option to make a component the first instance of a contextual part.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Save the Contextual Models In this section, you will learn how to save the various files related to a contextual part, including the contextual part itself.
Use the following steps:
1. 2. 3. 4.
Save the Contextual Models
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5.
Clarify the display. Create contextual parts. Create assembly-level features. Manipulate the contextual components.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Saving Contextually-Related Components
Student Notes:
Special attention is required while saving documents that are related to contextual parts. Contextual parts reference elements in driving CATParts and specific instances of CATPart in specific CATProducts. If you save one document with a new file name, the related document should also be saved.
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In the example shown, the Small Block part references elements in the Bottom Block instance of the Large Block part.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Saving Driving CATParts After saving a driving CATPart with a new filename, the driven CATParts and the parent CATProduct must be saved because of their reference to the CATPart. Use the following steps to save a driving CATPart: 1. Perform a Save As on the driving CATPart from within the assembly containing the driving CATPart. A warning message will appear.
1
2. Click OK to the warning message. 3. Save the contextual CATParts that are driven by CATPart that was saved. 2
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4. Save the CATProduct that is the parent of the CATPart that was saved.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Saving Contextual CATParts After saving a contextual CATPart with a new filename, the parent CATProduct will need to be saved because of its reference to the driving CATPart. Use the following steps to save a contextual CATPart: 1.
Perform a Save As on the contextual CATPart from within the assembly containing the contextual CATPart. A warning message will appear.
2.
Click OK to the warning message.
3.
Save the CATProduct that is the parent of the CATPart that was saved.
1
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Saving Parent CATProducts After saving a CATProduct with a new filename, the contextual CATParts that were defined in context of the CATProduct will have to be saved because of the CATPart’s reference to the CATProduct. Use the following steps to save a parent CATProduct: 1
1.
Perform a Save As on the CATProduct. A warning message will appear.
2.
Click OK on the warning message.
3.
Save the contextual CATParts that were defined in context of the CATProduct that was saved.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Copying CATProducts Using Send to Directory Create another copy of the CATProduct with all the related files by using the File > Send to > Directory tool. Use the following steps to create a copy of a CATProduct with all the related files: 1.
Click File > Send to > Directory.
2.
Select the files to be copied and specify the destination folder where the files are to be copied. The main features of the Send To Directory dialog box are as follows: List of available files to be copied.
b.
Buttons used to transfer files over into the list of selected files to be copied.
c.
List of files selected that will be copied.
d.
Destination folder.
Click OK.
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3.
a.
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2a
2b 2c
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Assembly Split and Hole
Student Notes:
Recap Exercise 20 min
In this exercise open an existing product file. You will use the tools learnt in the lesson to create an assembly level hole through multiple components and a split feature. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Create an assembly level hole
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Create an assembly level split feature
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (1/6) 1. Open product file. • You will open a product file that requires a hole to be drilled during the assembly process.
1a
a. Open LeverJig.CATProduct.
2. Create an assembly level feature. • All assembly level features are in the Assembly Features toolbar.
a. Find and float the Assembly Features toolbar. b. Select the Hole icon.
2a
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (2/6) 3. Define the hole. • An assembly level hole uses the standard hole dialog box.
a. Select the point in the Lever part. b. Specify Up To Last depth option. c. Enter [8mm] for the diameter.
3b 3c
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (3/6) 4. Set affected parts. • You will use the assembly level feature definition to specify affected parts.
a. Select Bar from the list of Parts possibly affected. b. Select the Add Selected down arrow. c. Select the Highlight affected parts. d. The Bar part is added to the Affected parts list.
4a
4b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (4/6) 5. View the assembly-level feature. • Any assembly-level features can be added under the Assembly features node in the specification tree.
a. The assembly hole is added and the affected parts are visible in the specification tree. b. Open Bar.CATPart in a separate window and view the resulting geometry.
5a
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (5/6) 6. Create a split assembly feature. • You will create a split that will allow clearance for the bar part to swing.
6c
a. Show the SpaceClaim geometrical set. b. Activate the LeverJig assembly. c. Select the Split icon. d. Select the surface feature. e. Move the JigBase to the Affected parts list.
6a
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (6/6) 7. View the result assembly level features. a. Hide the SpaceClaim geometrical set. b. Save the completed assembly.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Assembly Split and Hole Recap
Student Notes:
Create an assembly level hole
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Create an assembly level split feature
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Links Analysis
Student Notes:
Recap Exercise 30 min
In this exercise, you will create a new model. You will use the tools learnt in this lesson to create a rib and a slot feature. The profiles for these feature have already been constructed for you. Detailed instructions for this exercise are provided. By the end of this exercise you will be able to: Analyze dependencies Investigate contextual links Investigate external links
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Isolate parameters
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (1/15) 1.
Open product file and view the symbols • •
You will open a product file that has a contextual links already defined. By looking at the symbols in the specification tree, you can see which components have contextual links.
1a
a. Open SlotBracket.CATProduct. b. CoverSlot has contextual links. c. Holder has contextual links.
1b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (2/15) 2.
Analyze dependencies. •
Analyze dependencies is only available in the Assembly Design workbench.
a. Select CoverSlot. b. Click Analyze > Dependences.
3.
View dependencies. •
Associativity will identify external references.
a. b. c. d.
3a
2a
2b
Clear the Constraints option. Activate the Associativity option. Show the Parent node. CoverSlot is associated to AngleMount
3b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (3/15) 4.
Define contextual links. •
Contextual links can be replaced.
a.
b. c.
Right-click on CoverSlot and select Components > Define Contextual Links from the contextual menu. All the external elements as well as the pointed document are listed. Click OK.
4a
4b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (4/15) 5.
Open part file and investigate the external links • •
•
Parent/child relationships are investigated in the Part Design workbench. Investigate external links. You can use the Links dialog box to load, replace, isolate, synchronize and deactivate external links. Investigate pointed documents. Pointed documents tab will report the file name and the file path to parts and/or product files where the driving geometry is located.
a. b. c.
5d
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d.
Open CoverSlot in a separate window. Select Sketch.1. Right-click to obtain contextual menu and select Parents/Children. The external references are shown as parents to Sketch.1.
5c
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Do it Yourself (5/15) 5.
Student Notes:
Open part file and investigate the external links (Continued) • • •
Parent/child relationships are investigated in the Part Design workbench. Investigate external links. You can use the Links dialog box to load, replace, isolate, synchronize and deactivate external links. Investigate pointed documents. Pointed documents tab will report the file name and the file path to parts and/or product files where the driving geometry is located.
e. f. g.
Click Edit > Links. All the external elements as well as the pointed document are listed. External parameters are also listed.
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5e
5g
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Do it Yourself (6/15) 5.
Student Notes:
Open part file and investigate the external links (Continued) • • •
Parent/child relationships are investigated in the Part Design workbench. Investigate external links. You can use the Links dialog box to load, replace, isolate, synchronize and deactivate external links. Investigate pointed documents. Pointed documents tab will report the file name and the file path to parts and/or product files where the driving geometry is located.
h. i. j.
Select the Pointed documents tab. The CoverSlot has an external link to AngleMount.CATPart. The link was created in the SlotBracket.CATProduct.
5h 5i
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (7/15) 6.
Use save management. •
Using save management you can make a copy of the complete assembly while maintaining the associative links between parts.
a. b. c. d. e.
6b
6c
Click File > Save Management. Select SlotBracket.CATProduct. Select Save As. Create a new directory named NewProduct. Click Save.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (8/15) 6.
Use save management. (Continued) •
Using save management you can make a copy of the complete assembly while maintaining the associative links between parts.
a.
6a
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b.
Select Propagate directory. The propagate directory option will save a copy of all the components of an assembly. Double-click the New Product directory. Close the product file.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (9/15) 7.
Open product file and View Changes •
Open the Product, change the Parameter values and observe changes in the Part. All contextual links remain between relative components in the new product file and are not associated with the original product file.
a. b. c.
7a
Open SlotMount.CATProduct from the NewProduct directory. Activate AngleMount part. Change the value of the Thickness parameter to [5mm].
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (10/15) 7d
7.
Open product file and View Changes (Continued) •
Open the Product, change the Parameter values and observe changes in the Part. All contextual links remain between relative components in the new product file and are not associated with the original product file.
d.
e.
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f.
Notice how the single parameter drives three different part files. This is due to the contextual link to the external parameter named Thickness. The updated product file and components appears with changes. Open Holder part in a separate window. Notice the external parameter.
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7f
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (11/15) 8.
Isolate an external parameter and test the link. •
By isolating a contextual link, the link is severed and cannot be re-linked.
a. b.
Select the Thickness parameter. Right-click and select Isolate from the contextual menu.
8a
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (12/15) 8.
Isolate an external parameter and test the link. (Continued) •
By isolating a contextual link, the link is severed and cannot be re-linked.
c. d. e. f.
Activate SlotMount.CATProduct window. Activate AngleMount part. Change the value of Thickness parameter to [12mm]. The Holder part no longer updates.
8e
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8c
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (13/15) 9.
Isolate all external references for a part and make changes to driving geometry. •
All external geometric references can be isolated.
a. b. c. d.
Select CoverSlot part. Right-click and select Isolate Part from contextual menu. The external references are now isolated. External parameters are not affected by this command. 9b
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (14/15) 9.
Isolate all external references for a part and make changes to driving geometry. (Continued) •
All external geometric references can be isolated.
e. f.
g. h. i.
Make changes to driving geometry. Before the contextual links were isolated, the Cover Slot part used the face of the Slot Bracket part as a reference for the depth option of the pad. Edit Sketch.1 of Pad.1 of Angle Mount part. Edit the 105 dimension. Enter [115deg].
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do it Yourself (15/15) 10. View the assembly. •
Since you have isolated the contextual links of the CoverSlot part, it no longer updates to changes in pre-referenced geometry.
a.
10b
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b.
The updated assembly shows the isolated CoverSlot part. Save the file and close all files.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Exercise: Links Analysis Recap
Student Notes:
Analyze dependencies Investigate contextual links Investigate external links
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Isolate parameters
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Case Study: Contextual Design
Student Notes:
Recap Exercise 40 min
In this exercise you will create the case study model. Recall the design intent of this model: Contextual links must be used to ensure that changes to the referenced parts are reflected in the contextual part Contextual links can only reference the housing component The oval cut may need to intersect other component that have not yet been created
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Assembly must be saved to another directory in its entirety
Using the techniques you have learnt in this and previous lessons, create the model with only high-level instruction.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do It Yourself: Earphone (1/11) You must complete the following tasks: 1. Open existing product file. • Open Earphone_start.CATProduct.
1
2. Create a new part. • Create a new part named 'Cover'.
3. Constrain the new part.
2
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• Position the new part using reference elements of Housing component in order to center it on Bend_Point. • Create a coincidence between 'Bend_Point' of Housing and XY plane of Cover. • Create a coincidence between YZ plane of Housing and YZ plane of Cover. • Create a coincidence between ZX plane of Housing and ZX plane of Cover.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do It Yourself: Earphone (2/11) You must complete the following tasks (continued):
4. Unload components. • Unload the Speaker, Rubber, and Flexible components. 4
5. Show a sketch. • In Housing component show 'Sketch.3'.
6. Create a sketch. • Activate the Cover component. • In Cover component, create a new sketch lying on ZX plane.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Do It Yourself: Earphone (3/11)
Student Notes:
You must complete the following tasks (continued): 6. Create a sketch (continued).
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• Project the three outlines of 'Sketch.3' in this new sketch. Make sure the link is kept with Housing Component. • Add geometry as shown on the scheme and exit the sketcher.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do It Yourself: Earphone (4/11) You must complete the following tasks (continued): 7. Create a shaft. • Create a complete Shaft around Z Axis with the sketch previously created.
7
8. Create a plane. • Create a new plane defined with an offset of 1mm from YZ plane. Reverse its direction if necessary. This plane will be used to split the shaft feature.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do It Yourself: Earphone (5/11) You must complete the following tasks (continued): 9. Create a split. • Use this plane to split the current solid. Keep the biggest part of the solid.
10.Create a fillet.
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• Define an edge fillet of Radius 2.5mm on the two corners of the Cover.
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10
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do It Yourself: Earphone (6/11) You must complete the following tasks (continued): 11
11. Create a groove. •
Create a groove reusing 'Sketch.2' (with link) from Housing component.
12. Hide component. •
Hide the Housing component for clarity.
13. Create a fillets. •
Create two edge fillets of 5mm to smooth the edges left by the groove.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Do It Yourself: Earphone (7/11)
Student Notes:
You must complete the following tasks (continued): 14. Create a tritangent fillet. • Create a tritangent fillet to remove the planar face.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do It Yourself: Earphone (8/11) You must complete the following tasks (continued): 15
15. Create an assembly level pocket. •
Reuse Sketch.8 from the Housing component to create a Pocket at the assembly level that cuts through the Cover component. Use the Up to Last depth option.
16. Create a fillet. • •
Activate the Cover component. Fillet the inner face of the pocket (Radius = 0.2mm).
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do It Yourself: Earphone (9/11) You must complete the following tasks (continued): 17
17. Create a sketch. • Create a new sketch as shown. Use the ZX plane as the sketch support.
18. Create a pocket. • Create a pocket using the Up to Last limit type for both the first and second limits.
19
19. Create a pattern. • Create a rectangular pattern to duplicate the pocket.
20. Create fillets.
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• Fillet both pockets (Radius 0.1mm)
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Do It Yourself: Earphone (10/11) You must complete the following tasks (continued): 21. Add color to the part. •
You can apply the material of your choice (Painting for instance) on Cover component.
22. Display all components. •
Show the Housing component and Load the Speaker, Rubber, and Flexible components.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Do It Yourself: Earphone (11/11) You must complete the following tasks (continued):
Student Notes:
23
23. Verify links •
Ensure that only the Cover component has external links to the housing component.
24. Save the assembly. 25
25. Send the assembly to another directory. Create a new folder called Earphone_Complete and save the entire assembly to this directory.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
Case Study: Contextual Design Recap
Student Notes:
Unload components Create part in context Hide components Create an assembly level pocket Load components Show components
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Save the entire assembly to another directory using the Send To command
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design
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 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Clarify the Display CATIA performance can be improved for large assemblies while panning, zooming, updating and saving. The following tools are used:
1
1. Visualization mode: In this mode only a light CGR representation of the model is loaded. 2. Hide: You can hide components to clarify the display and see only desired components.
Powertrain Assembly 2
Visualization Mode 3
3. Deactivate representations: Deactivating representations improves performance by hiding the components and excluding them from Mass Property analysis. 4. Deactivate components: It will remove the component from show and no show space, bill of Material.
Hiding Components
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Deactivating Representations
5
5. Selective load: Used to load the assembly up to a required depth and manage progressive loading of assemblies.
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Deactivating Components
Selective Load
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Create Contextual Parts Contextual parts are parts that have their geometry driven by another component. There are various ways to create contextual parts:
The green gear and blue chain indicates the object is the original instance of a part that is contextual. 1 Pin
1. Using External Parameters: Contextual links are created when the part uses a reference of parameters defined in another part. 2. Using External References: Contextual links are created when the part refers to geometrical elements from another part.
Housing
The pin radius is used as an external parameter to create the hole in the housing.
Housing 2
3. Using Assembly Features: Contextual links are created when there are Assembly features (Assembly Split, Remove, Hole) in a part.
The hole from the pin support is used as an external reference to create the hole in the base part.
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The benefits of using Design in Context: 1. Reuses existing geometry. 2. Reuses parameters. 3. The contextual part is automatically updated when the geometry of the referenced part changes.
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Base
3 The pin is used to create an assembly remove feature in the pin supports and housing.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Create Assembly-Level Features Assembly features are features that are applied not only to a single part (from within the part design workbench) but to a set of several parts of an assembly.
1
2
3
The following Assembly features can be created: 1. 2. 3. 4. 5.
Split Hole Pocket Add Remove
Split: The two parts Hole: The hole feature are split by the surface. affects both the parts.
4
5
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Add: The elliptical shaped body is added to the two parts.
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Pocket: The elliptical pocket feature affects both the parts.
Remove: The central hole is the result of removing a shaft feature from the two bodies.
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Manipulate the Contextual Components Various operations can be done as follows: 1. Isolate: The contextual links are broken. You can choose to isolate individual or all elements in a contextual part. 2. Delete: If the original instance of a driven part is deleted a new original instance should be established. When a component that drives a contextual part is deleted, the option to delete the contextual components that are driven by the component is available. 3. Save: After saving a driving CATPart with a new filename, the driven CATParts and the parent CATProduct must be saved because of their reference to the CATPart. After saving a contextual CATPart with a new filename, the parent CATProduct will need to be saved because of its reference to the driving CATPart. After saving a CATProduct with a new filename, the contextual CATParts that were defined in context of the CATProduct will have to be saved because of the CATPart’s reference to the CATProduct 4. Copy: Using the Send to > Directory tool, you can create a copy of the CATProduct along with all related components.
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Student Notes:
Isolated external references appear with the broken link,
Creating a copy of CATProduct using Send to > Directory.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Main Tools (1/3) Tools > Options Settings 1
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Work with the cache system: Activates the visualization mode.
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Do not activate default shapes on Open: Prevents loading the representation of the Components in the CATProduct when it is opened.
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Keep link with selected object: The object created with this option will keep the link with the original part/reference. Representation Tools
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Design Mode: Loads the component in the design mode.
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Visualization Mode: Loads the component in the visualization mode.
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Activate Node: Activates the shape representation of the component.
Deactivate Node: Displays relationships between components and constraints. View Toolbar
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Hide/Show: Hides/Shows the selected components.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Main Tools (2/3) Activate / Deactivate Tools 9
Activate / Deactivate Component: Activates/Deactivates a selected component.
Product Structure Tools 10
Selective Load: Manages the loading of subproducts level by level.
Knowledge Toolbar 11
Formula: Creates formulae and parameters to incorporate design constraints.
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Assembly Features 12
Split: Creates an assembly split feature.
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Hole: Creates an assembly hole feature.
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Pocket: Creates an assembly pocket feature.
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12 15
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Add: Creates an assembly add feature and adds the body to the selected parts. Remove: Creates an assembly remove feature and subtracts the body from the selected parts.
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CATIA V5 Mechanical Design Expert - Lesson 7: Contextual Design Student Notes:
Main Tools (3/3) Manipulating Contextual Parts 17
Isolate: Isolates the part by removing contextual links.
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Delete: Deletes the selected component.
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Save Tools 19
Save As: Saves the component with a new name.
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Send to > Directory: Creates copy of the component in selected directory.
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