Creating a Cut

The Cut capability trims the shapes of one or more features of the active body by using styling surfaces or planes. The resulting body is shaped by these cutting elements. You can have two different type of cuts.

This task shows you how to:

Related Topics
More about Cuts

Create a Cut on a Shellable Prism

You can create a cut on a shellable prism.

  1. Click Cut .

    The Cut dialog box appears.



  2. Select the shellable prism as the feature you want to cut.



    Tip: If you select several features, the box displays the number of selected elements. To act on this selection, just click the icon to display the Features to cut dialog box that allows you to:
    • View the selected elements.
    • Remove any element clicking the Remove button.
    • Replace any element using the Replace button and selecting a new one in the geometry or the specification tree.

  3. Select two extrusions and one plane as the cutting elements.

  4. Click both arrows on the surfaces to reverse the direction indicating which portion of material is to be kept. The two arrows must point toward the shellable prism as shown here:



  5. The Fillet radius option has changed to Intersection radius. The Intersection Fillet option sets the radius of fillets on the edges produced by the cutting surface. For this cut, select Intersection radius and enter 6mm in the dedicated box. The Wall option lets you set if, or how, the Cut command creates walls along the cutting surface. We can leave the default thickness here (use feature thickness), we will show this option in Create a Cut on a Pocket.

  6. Click Preview to see the result.



  7. An offset distance from the selected cutting elements can be entered as an option. Enter 10mm for Offset and click Preview.



  8. Set the offset value back to 0mm.

  9. Click OK to confirm.

    The first cut feature is created. Cut.X is added to the specification tree in the Solid Functional Set.X node. The 3D shape now looks like this:



    Just hide both cutting surfaces if you want to see the filleted edges.

Create a Cut on a Pocket

You can create a cut on a pocket to reshape the pocket.

  1. Click Cut .

  2. Select the pocket as the feature you want to cut.

  3. From the specification tree, select the extruded surface as the cutting element.



  4. To define the wall, select Enter thickness and enter 5mm in the Thickness value box.

  5. Click OK to confirm the operation and hide all extrusions.

    This cut operation has split the pocket while adding some thickness from the edge produced by the cutting surface . The resulting shape looks like this:

  6. Double-click the cut feature that you have just created to edit it.

  7. Select the Split check box.

    The Enter thickness option is selected in the drop down list with 0mm in the value box. All the options in the Wall area are disabled and dimmed. The resulting shape looks like this:

    Cut.X is added to the specification tree in the Solid Functional Set.X node.