To Create an Inheritance Feature
1. Retrieve an assembly, select a part in it, right-click, and choose Activate.
2. Select a second part in the assembly as the reference model from which geometry will be copied and click Get Data > Merge/Inheritance. The Merge/Inheritance tab opens with the reference model selected by default. You can select a different part as the reference model from the Model Tree or in the graphics window.
3. Click Merge/Inheritance to toggle between Merge mode (default) and Inheritance mode.
4. Set the reference type:
In Context—Set reference type to assembly context (default).
External—Set reference type to external.
5. Use the following options to define inheritance feature properties:
Add Bodies—Bodies of the reference part are copied and added as bodies to the target part, increasing the number of bodies in the target part.
Merge—Geometry of the reference part is copied and merged with the geometry of the source part. When there are multiple bodies in the reference part, they are merged into 1 body and it is copied to the target part as a new body or to an existing body.
Cut—Geometry of the reference part is removed from the geometry of the target part.
Intersect—Geometry of the reference part is intersected with the geometry of the target part keeping the shared geometry.
When you add, remove, or intersect geometry the Body Options tab becomes available.
6. Click References to change the following options.
Copy Quilts—Toggle copying quilts from the modifying model.
Include Construction Bodies—Toggle including construction bodies from the reference part to the source part in the Inheritance feature. When you select the Include Construction Bodies check box, construction bodies are copied and added to the target part.
7. Click Options to change the following options:
Include Properties—Defines the properties of the copied references to include in the inheritance feature when you add bodies or add material. All properties in the list that follows are copied by default. You can then decide which properties you do not want to copy.
Appearance—Appearances applied to the inherited geometry.
Parameters—Parameters of the inherited entities.
Names—Names. When cleared, generic names are provided for inherited entities.
Layers—Layer assignment. Places the inherited entities on layers with the same name when they exist in the target part.
Materials—Material assignment. When the material does not exist in the target part, it is copied to the target part and assigned to the newly created body.
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Mass properties are copied along with materials.
Construction yes/no—Construction attribute of a body, whether the body is a construction body or not.
Copied Geometry Update—Sets update preferences for the Inheritance feature.
Automatic Update—Keeps the relationship between the current feature and the original geometry.
Manual Update—Temporarily suspends the relationship between the current feature and the original geometry. If the original part changes, the current feature does not change. You can update the inheritance feature at any time as long as the original geometry is in session. Click the Provide notification check box to receive a notification when the source geometry is updated.
No Dependency—Creates an independent inheritance feature.
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If an Inheritance feature is independent, you cannot externalize the feature.
Refit Datums (available when you copy datum planes)—Changes the size or reference of a copied datum plane. The Refit Datums dialog box opens. Select a datum and then choose Size to edit the width and height of the selected datum. If the Lock aspect ratio check box is selected, the original width and height ratio is maintained when one of these values change. Alternatively, choose Reference to change the reference of the selected datum.
Varied Items—Opens the Varied Items dialog box. Define varied items properties.
8. Click Body Options to determine the bodies affected by this feature.
When you add material, you can add the resulting geometry to the selected body or to one of the body options below:
A new body—Select the Create new body check box
A different body—Right-click the body in the collector and click Remove. Select a different body in the part.
When you remove material, you can remove geometry from the selected body or from all bodies in the target part.
When you intersect geometry, you can intersect with the selected body or with all bodies in the target part.
9. Click Properties to change the name of the Inheritance feature.
10. Click to complete the Inheritance feature. The new Inheritance feature identified by the visual indicator, appears in the Model Tree. An Inheritance feature with varied items defined, is identified by the visual indicator in the Model Tree.