Remove

This task shows you how to remove a sweep from a shellable prism.

1. Click the Remove icon .
   The Remove Feature dialog box is displayed.

2. Select Pocket.1 as the feature to modify.

   If you select several features, the field displays the number of selected elements. To act on this selection, just click the icon to display the Features to modify 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.

   Shape Definition

3. Remove features can have different shapes. The prism is the default shape. If you prefer a different shape, click any of the other three shapes available. To know how to create any of them, refer to the Prism, Sweep, Revolve, Thick Surface or External Shape tasks. For the purposes of our scenario, set the Sweep option .

4. Select Profile_sketch as the Profile/Surface defining the sweep.

5. Select Center_Curve as the Center curve.

   Fillet

6. Click the Fillet tab.

7. Check the Lateral radius option and enter 1mm as the lateral radius value.

8. Click Preview to check the operation.

   The defined sweep has been removed from the shellable prism. Remove Sweep.X is added to the specification tree in the Solid Functional Set.X node.

Intersection Fillet

The Intersection Fillet provides the capability to create fillets at the intersections with the targets. Also it provides the ability to keep the wall thickness constant when modifying wall creating feature that has set the constant wall option. In this case, the fillets are added at the intersections with the shellable prism.

 

9. Select Intersection radius checkbox and enter 1mm.

10. Click OK to confirm the operation.

Wall

The Wall option lets you set if, or how, the Remove Feature command creates walls along the removing surface.


To define a wall, you can set one of the options available from the drop down list:

• Use body thickness: the feature wall thickness is that of the active shelled body thickness.

• Enter thickness: simply enter the value you want. After this option is selected, the value field becomes available. Wall thickness values can only by positive values.

• Use feature thickness: the feature wall thickness will be the same thickness as the target feature (the feature you want to modify).

However, if the target feature has no thickness parameter in its definition (for example if the target feature is an external feature), the Remove Feature capability assigns the thickness value defined in Shell Properties to the wall. If this behavior does not meet your needs, you still can:

Set the thickness value to 0mm in Shell Properties before running Remove Feature. Or: In the Remove Feature dialog box, set Enter thickness and assign the value you need.

You can control whether the wall is constructed inside or outside of the selected  profile. The default is an inside wall thickness.

Inside is the inward direction of the target wall. It means that "inward" is relative to the solid shellable volume being modified such as the Shellable feature, not the modifying volume such as the Cut/Remove/Intersect feature.

When the Wall direction is Inside, the wall will be constructed inward of the Shellable Prism.

When the Wall direction is Outside, the wall will be constructed outward of the Shellable Prism.

11. Click the Remove icon again to add another Remove feature.

12. Select Pocket.1 as the feature to modify.

13. Select RemoveSketch as Profile/Surface.

14. Click Reverse Direction button.

15. Enter 40mm for First length.

16. Click OK.

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

17. Click Remove Prism.2 to edit the feature.

18. Select Enter thickness for Wall Type and enter 0mm for Thickness.

19. Click OK.

Remove Command and Protected Volumes

After you have generated a Remove feature from protected volumes, for example from a Cutout, material is generated as illustrated below:

Cutout pointed by the cursor and sketch to be used for the remove operation	Remove operation accomplished on the cutout