How to create solid "filled" body from hollow bodies?

[jay_tay]

I'd like to create a "shadow" gridfinity box for my fisher bullet pen. Shadow boxes are often made of foam so that one can immediately see which tool in a drawer is missing. 

Something like this:

I have found a 3d model of the pen on grabcad and tried to use that model to cut the shape of the pen out of a solid body. 
The slot for the pen should be centered inside the solid body. Something like this:

Sadly, I haven't figured out the following problems given the 3d model files from grabcad.

1. I haven't figured out a way to align the pen so that it is centered to the sides of the solid
2. The model of the pen is accurate, which means that the pen is actually hollow. I have tried to join both bodies in F360 via the "combine" command, but kept ending up with two separate bodies for the pen

3. I've tried to find a way that allows me to create a simple body that follows the outer shape of the pen so that I can cut the solid with it, but haven't figured out how this could be done in F360. 

I have been pulling my hair out on this problem for several hours now, but still haven't found a solution. 
Maybe someone in this community can help? 

Suggestions and ideas would be greatly appreciated. 
Thanks!

[davebYYPCU · Accepted solution]

Turn the Pen into a Fusion solid, Combine Cut them from the foam.

Might help...

[jhackney1972 · Accepted solution]

Here the cutout of the pen in your model box.  Pretty much the same process as @davebYYPCU just using your supplied model box.  The Pen is just invisible in the model, can be turned on.  Model attached.

[jay_tay]

Everyone, thank you for helping out and please excuse my non-responsiveness!
I had my notifications turned off, and didn't see that you responded.
After looking at each of your models history, I still don't really understand the operations required. 
Would you be able to explain how I do 1. and 2. from my initial question?
What other operations are crucial here? 
Thanks a lot!

[davebYYPCU · Accepted solution]

Best I remember, reading my timeline, Step by step along the time line (after) your original stuff, 

Your pen had a few sections, I have combined them as is, with Rigid Group.

I then Jointed that group to the File Origin.

I have a sketch and Extrude to make the receiver box.

Then I have recreated new top and bottom pen halves, by

Surface > Create Offset at zero distance, so made a copy of the outer pen shape.  

I then closed the opening with the Surface > Create > Patch command.

Surface > Modify > Stitch the Surface and Patch, makes the new body completely solid.  

Same for top as the bottom.

Solid > Modify > Combine these two new articles together with Combine - Join. (My new pen)

Create the groove in the extruded box, with

Solid > Modify > Combine - Cut.  Box is cut with the pen.

Walk along my timeline, use edit feature to see the settings used.

Happy to answer more questions.

Might help....