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 UnionTrim.CATPart document.

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

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

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

    The selected face is highlighted and a label, pointing it out is displayed, meaning that the application is going to remove it.

  4. Click the Faces to keep field and select Part Body. 's inner face.
    A label, pointing it out is displayed, meaning that the application is going to keep it.
  •  If you want to trim the object and create a datum feature, you must click Create Datum . Ensure that you click Create Datum only after selecting the required volumes and faces in the Trim Definition dialog box.
  • Preview is available, if no faces are selected under Faces to remove. On the selection of one or more faces under Faces to remove, preview is displayed automatically.

  1. 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.

  • As much as possible, avoid selecting faces trimmed by the operation. In some cases, defined trimmed faces have the same logical name: the application then issues a warning message requiring a better selection.
 

Interrupting Boolean Operations Computations

In case you made a mistake when performing a Boolean operation, you can interrupt the feature computation launched after clicking OK, when the computation requires a few seconds to perform.
In concrete terms, if the computation exceeds a certain amount of time, a window appears providing a Cancel option. To interrupt the operation, just click that Cancel button. This interrupts the process and then displays an Update Diagnosis dialog box enabling you to edit, deactivate, isolate or even delete the Boolean operation in progress.

This new capability is available for any types of Boolean operations you are creating or editing.