To Combine, Split, or Trim Bodies and Faces

Combine Solid Bodies

Note: The Combine command is available in multi-body part files only.

1. Click 3D Model tab Modify panel Combine .
2. Using the Base selection arrow, choose the base solid body in the graphics window.
3. Using the Toolbody selection arrow, select the solid bodies to combine with the base. You can select multiple toolbodies. The number of toolbodies selected displays in parentheses next to the arrow.
4. (Optional) Select Keep Toolbody.

   Keep Toolbody retains 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 can’t be used for more operations.

   Note: Deleting a Combine command restores the consumed toolbody. The visibility of a retained toolbody is turned off by default.
5. Choose an operation for the combination:
   • 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.
6. Click OK.

Split the Face of a Solid or Surface Body

1. Click 3D Model tab Modify panel Split .
2. In the Split dialog box, click Split Face .
3. Using the Split Tool selector, select a 2D sketch, 3D sketch, work plane, or surface to use to split the face.
   Note: 3D sketches must lie on and fully intersect the faces to be split.
4. Do one of the following:
   • Under Faces, click All and in the graphics window, select the part or surface body to split all its faces.
   • Under Faces, click Select and in the graphics window select one or more faces of the part or surface body to split.
5. Click OK.
   Tip: After part faces are split, you can use Face Draft to apply draft.

Trim or Remove One Side of a Solid Body

Note: The Trim Solid method of the Split command can’t be used on surface bodies.

1. Click 3D Model tab Modify panel Split .
2. In the Split dialog box, click Trim Solid .
3. Using the Split Tool selector, click a work plane, 2D sketch, or surface body to use to trim the solid.
4. Under Remove, select which side to remove.
5. Click OK.

Split One Solid Body into Two Solid Bodies

1. Click 3D Model tab Modify panel Split .
2. In the Split dialog box, click Split Solid .
3. Using the Split Tool selector, click a work plane, 2D sketch, or surface body to use to split the solid.
4. If there is only one solid in the part file, the solid is automatically selected. If there are multiple solid bodies present, select the Solid to be split.
5. Click OK.
   Note: You can export solid bodies in a multi-body part file as individual part files by using the Make Part or Make Components (not available in Inventor LT) command. Files created using these commands are associative to the parent part file.

Create Two Parts from a Split Part

Files created with this workflow are not associative to each other, or to the original source file. If associativity is required, use the Split Solid method in a multi-body part.

1. Sketch a parting line on a part face.
2. Click File Save As Save Copy As to save the part with the parting line and both halves intact.
3. Use Split and the Trim Solid method to split the part and remove the selected half.
4. Use Save Copy As to save the first half of the part.
5. Open the original file, then use Split and the Trim Solid method to remove the other half of the part.
6. Use Save Copy As to save the second half of the part.

Both halves of the part are now saved in separate, unique files.