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.

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. From the Geometry section of the action bar, click Trim .
  2. Select Standard .
  3. Select 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. You can edit the table by first selecting an element and then do either of the following:

    • Click to add a line at the end of the list in the table.

    • Click to insert a line before the selected line in the table.

    • Click to insert a line after the selected line in the table.

    • Click to remove all the lines.

  5. Optional: Select the Result simplification check box to automatically reduce the number of faces in the resulting trim whenever possible.
  6. Click Intersection computation check box to compute the intersection between the trimmed elements.
  7. Click OK.


Trim Geometry Using the Pieces Mode

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

  1. Click Trim .
  2. Select Pieces .
    Every portion of each element is numerated and all numbers are stored. The order of numeration corresponds to the orientation of the element (surface / curve).

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

    Important:
    • If the first selected element is a curve, you are allowed to select curves only.
    • If the first selected element is a surface, you are allowed to select surfaces only.



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

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

  4. Optional: Select the Keep all pieces check box to keep all the pieces and generate a non-manifold result.
  5. Optional: Select the Check connexity check box to find out whether the elements to be trimmed are connected. If they are not, and the option is checked, an error message is issued indicating the number of connected domains in the resulting trimmed feature.
    The resulting feature is highlighted, and helps you detect where the trimmed feature is not connected.
  6. Optional: Select the Check manifold check box to find out whether the resulting trimmed feature is manifold.
  7. Click OK.


    Important: If you modify the portion of an element (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.
    Warning: For the Pieces mode, trimmed elements must be selected from the 3D area. Selecting the trimmed elements from the tree might produce varied results.

Extrapolate

You can extrapolate automatically the cutting curve, surface, or volume.

  1. Select the Automatic extrapolation check box to automatically extrapolate the cutting element.

    By default, this check box is selected.

  2. Clear the Automatic extrapolation check box if you do not want the automatic extrapolation of the cutting element.
    When a splitting curve is extrapolated, the extrapolation is performed on the original curve, providing the underlying geometry (that is the curve) is long enough to be used for the extrapolation.
    Important:
    • This check box is available for a split surface / curve or surface / surface.
    • This check box is also available if the element to be cut is a volume and the splitting element is a surface. This option enables to lead the extrapolation of the splitting surface in case it does not completely cut the solid.

      The Result options, Surface and Volume are useful only when a volume is selected as an element to be cut. If a surface is selected as an element to be cut, the result is always a surface, irrespective of the selected result option.

    • In the Pieces mode, this check box is available for trimmed surfaces.
    • Select a either Volume or Surface as the result type.

If the Automatic extrapolation check box is cleared, an error message is issued when the elements to trim need to be extrapolated, and the latter are highlighted in red in the 3D geometry.

To be able to trim the two surfaces or wireframe elements, select the Automatic extrapolation check box.