Trimming Geometry

You can trim two or more surface or wireframe elements by cutting each other mutually.

At creation, when you switch from one mode to the other, the list of selected elements is automatically reinitialized. You cannot modify the mode at edition.

This task shows you how to:

Before you begin: Create a 3D shape containing geometric elements.
Related Topics
Splitting and Trimming Geometry (common options)
Selecting Using the Multi-Selection

Trim Geometry Using the Standard Mode

With Standard mode, one portion of the selected element (surface or wire) is kept and the list of trimmed elements is ordered.

  1. Click Trim .

    The Trim Definition dialog box appears.

  2. Select the Standard Mode.



  3. Select the two surfaces or two wireframe elements to be trimmed.



    A preview of the trimmed elements appears and the list of trimmed elements is updated.

    You can change the portion to be kept by selecting that portion:



  4. Optional: Select the Result simplification check box to automatically reduce the number of faces in the resulting trim whenever possible.

    Click OK to trim the surfaces or wireframe elements.

The trimmed feature (identified as Trim.xxx) is added to the specification tree.



You can also select the portions to be kept by clicking Other side / next element or Other side / previous element .

Trim Geometry Using the Pieces Mode

With Pieces mode, all trimmed curves are split together, all selected portions are kept and the list of trimmed curves is unordered.

Warning: This mode is only available with curves.

  1. Click Trim .

    The Trim Definition dialog box appears.

  2. Select the Pieces Mode.



    Every portion of each curve is numerated and all numbers are stored. The order of numeration corresponds to the orientation of the curve.



  3. Select the elements to be trimmed, as shown below:



    A preview of the trimmed elements appears and the list of trimmed curves is updated.

    You can clear a sub-element by selecting it again.

  4. Optional: Select the Check connexity check box to find out whether the curves to be trimmed are connex. If they are not, and the option is checked, an error message is issued indicating the number of connex domains in the resulting trimmed feature.

    The resulting feature is highlighted, and help you detect where the trimmed feature is not connex.

  5. Optional: Select the Check manifold check box to find out whether the resulting trimmed feature is manifold.

  6. Optional: Use Remove and Replace to modify the elements list.

  7. Click OK to trim the curves.

    The trimmed feature (identified as Trim.xxx) is added to the specification tree.

    Warning: If you modify the portion of a curve (for instance, cutting or extrapolating), the numeration is liable to change as there may be more or less intersections. As a consequence, the result may differ.