Combine solid bodies

The combine command provides a means to use a join, cut, or intersect operation on selected solid bodies. You can create the bodies in place or you can import bodies using the Derived Component command.

Use the Move Bodies command to position the bodies in the correct location before using combine or create the bodies in the required location to eliminate the need to move the body.

When you use the combine command, the Base body is the solid being acted upon and the Tool body is the solid performing the action on the base. You can select more than one toolbody to use in a combine operation.

The default behavior when you combine bodies is to consume the toolbodies and modify the base. Choose the option to retain the original toolbodies as separate solids if you do not want to consume the solids. Retained solids are invisible when you finish the command. If you delete the combine operation, the original solid body is available in the Solid Bodies folder. If you delete a combine operation, enable the visibility of the original bodies in the browser.

 

Procedures

Combine solid bodies

To begin, create a multi-body part and position the bodies you want to combine in the correct location. The most efficient way to position the bodies is to create them in place using feature create commands with the New solid option. You can also use the Derived Component command to import components to use as toolbodies. Use the Move Bodies command to precisely position the toolbodies.

Note The Combine command is available in multi-body part files only.
 
  1. On the ribbon, click Model tab Modify panel Combine.
  2. Click the Base selection arrow and choose the solid body to be acted upon in the graphics window.
  3. Click the Toolbody selection arrow and then select the solid bodies to act upon the base. Multiple toolbody selections are allowed. The number of toolbodies selected is shown in parentheses next to the arrow. If Keep Toolbody is unchecked, the toolbody is consumed and is not available for further operations. If you check Keep Toolbody, the toolbody visibility is turned off after the operation, but the toolbody can be used again.
  4. Select one of the following:
    • Click Join to add the volumes together.
    • Click Cut to remove the volume of the toolbodies from the base.
    • Click Intersect to create a solid that consists of the shared volume of the toolbodies and the base.
  5. Click OK.

References

Combine solid bodies

Joins one or more solid bodies by combining their volume. A join adds the volume of the toolbodies to the base. A cut removes the volume of the toolbodies from the base. Intersect modifies the base solid from the shared volume of the selected bodies.

Access:

Ribbon: Model tab Modify panel Combine

Select

Selects two or more bodies to consolidate.

Base

Selects the solid body acted upon.

nToolbody

Selects one or more bodies to act on the base solid body. The number in parentheses displays the current number of toolbodies selected.

Keep ToolbodySelect to retain the toolbody included in the operation as an independent body. The visibility is turned off after the operation. If not selected, the toolbody is consumed and cannot be used for additional operations.
NoteDeleting a combine command restores the consumed toolbody. The visibility of a retained toolbody is off by default.

Operation

Specifies whether the combine operation joins, cuts, or intersects the selected bodies.

Join

Adds the volume of the base and the selected toolbodies together.

Cut

Subtracts the volume of the selected toolbodies from the base body.

Intersect

Modifies the base solid from the shared volume of the base body and the selected toolbodies.