Trimming Bodies

Applying the Union Trim command on a body entails defining the elements to be kept or removed while performing the union operation.

The following rules are to be kept in mind:

Rule 1

REMOVE: Selected bodies ONLY are removed

Rule 2

KEEP: selected body is kept. All other bodies are removed

Rule 3

REMOVE is not necessary if KEEP specification exists

Concretely speaking, you need to select the required bodies and specify the faces you wish to keep or remove.

This task illustrates how to use the Union Trim capability.

When working in a CATProduct document, it is no longer necessary to copy and paste the bodies belonging to distinct parts before associating them. You can directly associate these bodies using the same steps as described in this task.

Open the UnionTrim1.CATPart document.

Select the body you wish to trim, i.e. Body.2.

Click the Union Trim icon

The Trim Definition dialog box is displayed. The faces you cannot select are displayed in red.

Click the Faces to remove field and select Body.2 's inner face.

The selected face appears in pink, meaning that the application is going to remove it.

Click the Faces to keep field and select Part Body. 's inner face.

This face becomes blue, meaning that the application is going to keep it.

Clicking the Preview button lets you check if your specifications meet your needs or not. To restore the view, you simply need to click the Undo

command .

Click OK to confirm.

The application computes the material to be removed. The operation (identified as Trim.xxx) is added to the specification tree.

You cannot re-apply the Assemble, Add, Trim, Intersect, Remove and Remove Lump commands to bodies already associated to other bodies. However, if you copy and paste the result of such operations elsewhere in the tree you can then use these commands.

Avoid using input elements that are tangent to each other since this may result in geometric instabilities in the tangency zone.