I want to basically make a 2mm thick "cap" for a head
I create a cube, then move the head part way into the cube.
then I Subtract the head from the cube -- leaving the cube that's inside fits perfectly onto the head.
Now I want the cube, with the inside the shape of the head, to be 2mm thick from the inside (shape of head) out. Thoughts?
PS. I know how to Shell the inside of a part to be 2mm thick. I want to "shell" the outside of the part to be 2mm thick
You can easily change the direction of the shell thickness. But I think you want something different. Can you share a screenshot for better explanation?
One way to do this is to create a solid body which fills the hole you have in your part. You could do this by extruding material to fill the hole, but as a new part. Then, subtract your original part from the new part to create a solid body which fills the hole. (There are lots of other ways to do this as well.)
Once you have your solid body which fills the hole, use the Shell command on the new part. Enter a value of -2 for the Offset, and pick the bottom face for the OpenFace. The result should be what you are looking for.
If you have the Surfacing module, there is another way to do it.
First, use the Copy command in the Cut & Paste section of the Modify 3D menu. That will create a face part.
Next, in the Surfacing menu, use the Thicken command and enter the wall thickness.
You may need to clean up the bottom, but that should be easy using the Align command.
from version 18.0 on, you don't need the Surfacing module anymore.
The Thicken command is included in the base license.
if you have version 18.0 or higher:
Use Gather Faces (3D Geometry tab) to gather the inside faces in a new surface part. After that, use the Thicken command with the desired thickness.
Hope this helps you out.