Assembly Features

Assembly features are very similar to existing part features except they can affect multiple parts, are created in the context of an assembly/scene, and the feature definitions do not pass down to each part. Assembly features can be Extruded Cuts, Spin Cuts, or Custom Hole Shapes. Assembly Features are by definition, a machining process that is processed on the assembled component and not performed on each individual component.

How To Create An Assembly Feature:

1. To create an Assembly Feature, right-click and drag an existing H-shape catalog item onto a selected assembly or scene.
2. In the resulting pop-up dialog, select Drop as Assembly Feature.
3. Select the Assembly Feature Scope (Define the Parts that will be affected by the Assembly Feature).
4. Only the part dropped on – The Assembly Feature will only affect the Part dropped on.
5. All assemblies/parts under the selected level – This will affect all parts/assemblies at the selected level (i.e. scene or a selected assembly).
6. Empty – This will drop an Assembly Feature that will not affect any part.
   
   Note:  Select Do not show the dialog to hide the dialog and to use the last selected option. This option can be turned on under the Tools Options menu.
   
7. Select OK.
8. Resize the Assembly Feature by using the sizebox/shape intellishape handles similar to other intellishapes.
9. Assembly Features will appear in the scene browser under the Assembly Feature Group (multiple assembly features can reside on a single assembly/scene).

Note:  The Assembly Feature Scope can be modified at a later time by right-clicking on the Assembly Feature (in the scene or scene browser) and selecting Edit Assembly Feature Scope.  Select part/assemblies to add/remove and select ok. In addition, in the scene browser, drag part onto the Assembly Feature Shape to add to the feature scope (right-click on a part in the scene browser under the Assembly Feature and select Remove from Assembly Feature Scope to remove).

Assembly Features that are patterned, maintain identical Feature Scope across the master and dependant instant shapes.

Linked instances of Assembly Features can have different a Feature Scope on each instance, however the shape geometry will maintain the link.

Note:  Assembly Features are not represented on external linked part/assembly instances when opened outside of the context where the assembly feature resides. Assembly Features do not apply to individual linked parts unless converted to part features.

Convert To Part Features

Multiple Part Features are similar to Assembly Features since they affect multiple parts, however multiple part features will reflect in each individual part definition. You can convert Assembly Features into part features by right-clicking on the Assembly Feature and selecting Convert to Part Features.

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How To Add An Assembly Feature And A Part/Assembly To A Catalog As A Group

Assembly Features (set as empty) and Parts/Assemblies together can be drag & dropped into a Catalog. On drop from the Catalog, the Feature Scope Options will be displayed for the Assembly Feature and then the entire group containing the assembly feature and the parts/assemblies will be dropped. This capability will allow users the ability to drop complicated assemblies that remove material from other parts/assemblies on drop from a catalog (Example would be a window frame drop onto a wall or frame members).  

1. First, create the desired Assembly Feature Group by creating the Features with the Feature Scope set to Empty (Not cutting any shapes).
2. Select the Parts/Assemblies from within the Scene Browser.
3. Hold the Shift key and select the desired Assembly Feature Group from the Scene Browser.
4. While still holding the Shift key, Left-click and drag the selection set from the Scene Browser into the desired Catalog.
5. Drag & Drop the Group into a scene.
6. On drop, the Assembly Feature dialog will pop-up to provide options of the Feature Scope.
7. Select the desired options and select ok.
8. The Assembly Feature Group and the Part/Assembly will be dropped into the scene.

Note: The location of the components will be based on the anchor location of the first selected shape in the group when selecting to drag and drop into the catalog.