Creating a Solid Cut

You can cut shapes into a solid using wireframe objects. PowerShape creates extruded solids from the wireframe objects and either subtracts or intersects them with the solid.

You can partially cut the solid or cut straight through:

You can keep either the outside or inside material of the cut:

To create a solid cut:

1. Select the solid and wireframe using one of the following methods:
   • Make sure you have an active solid and then select the wireframe objects.
   • Drag the cursor to select an inactive solid and the wireframe objects together.
   Note: The wireframe objects must be closed and planar.
2. Click Solid tab > Feature panel > Cut to display the Solid Cut dialog:

   

   Each wireframe object is extruded along the axis normal to the plane in which it lies to create the extruded solid.

   The extruded solid has a handle , which can be used to edit the length.

   

3. Select the Type of cut from the drop-down list:
   • Select Blind to set the depth to cut into the solid.
   • Select Through to cut all the way through the solid.
4. Click to create a copy of the original wireframe used in the construction of the cut.
5. Enter the Depth. This is the length of the extruded solid, measured from the plane of the wireframe .

   

   You can also adjust the depth using the handle. If you are creating a solid cut using more than one wireframe, dragging the handle of an extruded solid changes the lengths of all extruded solids. The value of Depth in the dialog updates to reflect the change.

   

   To cut all the way through the solid, select the Through option from the Type list.

6. Enter the Angle to define a draft angle for the extruded solid:

   

7. Click to extend the extrusion in both directions from the sketch. The button changes to to show that the extrusion is extended in both directions.
8. Click to reverse the direction of the cut.
9. Click to display the Solid Feature Relationship dialog. This allows you to specify the position of the feature relative to the solid. The status of the Relationship is indicated by one of the following:

   no relationship is currently defined.

   a valid relationship is defined.

   a relationship is defined, but there is a problem with the definition.

10. Click to add the selected sketch (arc, curve or composite curve) to the feature.
11. Click to group nested sketches. This option nests any sketches that lie on the same plane and uses them to produce an island-type extrusion.
    • Using two concentric circular sketches produces a tube with a thickness.
    • Using three concentric circular sketches, the tube produces a cylinder inside it.
12. Click or to specify if the draft angle is to go in or out.
13. Use and to remove material as required. The default setting removes material outside the sketches.
    • Click to remove material inside sketches.
    • Click to remove material outside sketches.
14. Click Apply to create the cut, leaving the dialog displayed. This lets you:
    • create another cut.
    • edit the existing cut.

    Alternatively, click OK to create the cut and close the dialog.

    A Cut feature icon appears in the solid feature tree.

Name — The drop-down list contains the names of the sketches. If the feature has more than one sketch, the Delete button is active. You can remove a sketch from the feature by selecting a profile from the Name drop down list and clicking Delete.

Remove inside material — Select this option to subtract the extruded solids from the solid . Deselect this option to intersect the extruded solids with the solid .