I'm sure it's simple...

[Vincent B]

..the solid part is still isolated, though. Too bad the shell can't be made into a solid in a parametic way. Or perhaps it's possible?

Select all faces, then use this tool (Curves WB). That make a parametric solid if all faces are closed each other.

[yclee126]

Select all faces, then use this tool (Curves WB). That make a parametric solid if all faces are closed each other.

That little tool in Curves WB blew my mind. It works like a charm now. Thank you so much for sharing!

[openBrain]

As it looks like a nice challenge, attached is my proposal 100% PartDesign.
Only 'Sketch' needs to be changed to adjust the dimensions (the lone line on top of the sketch is the height).
The magic is in the DatumPlane mapping (which I admit makes it sensitive to topological naming).

[TheMarkster]

You could pad a sketch and use the draft tool in part design.

See attached example file. The sketch would need to be constrained to desired dimensions.

[openBrain]

You could pad a sketch and use the draft tool in part design.

I doubt you can obtain the OP's shape with such a way. The top face shall be a rectangle and base octagon vertexes shall be aligned with the top face edges.

[TheMarkster]

I doubt you can obtain the OP's shape with such a way. The top face shall be a rectangle and base octagon vertexes shall be aligned with the top face edges.

Okay, I see now. I was basing it on the first screenshot he posted.

[bejant]

I'm a bit late but will offer another method, all done in Part Design. To change the size of the model, edit Constraint30 (the Constraint is named "Control") in Sketch and / or the Length of Pad. In hindsight, Sketch could have been simpler.

20190918a.png (12.47 KiB) Viewed 947 times

20190918.FCStd

(58.35 KiB) Downloaded 41 times

OS: Ubuntu 18.04.3 LTS (ubuntu:GNOME/ubuntu)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19. (dated 2019-08-21)
Build type: Release
Python version: 3.6.8
Qt version: 5.9.5
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

[chrisb]

Based on bejant's ideas i have created a version using only one pad, pockets and mirrors.

Bildschirmfoto 2019-09-19 um 21.54.04.png (21.96 KiB) Viewed 926 times

.

A small difference to bejant's is in Sketch002 the usage of references to external geometry to the first sketch instead of using expressions. The latter are even more robust against changes.

The biggest difference is the usage of a DatumPlane for last cut which isn't normal to any main plane. And here I would like to praise FreeCAD: I was surprised how easy it was to create that plane with just selecting the three points defining it:

Snip macro screenshot-8e4109.png (8.39 KiB) Viewed 926 times

I admit that I did not pay much attention on the size of the rectangle in Sketch003, but I'm sure it can be calculated as well to be always bifg enough, e.g. by taking the longest side in Sketch.

[bejant]

i have created a version

I like your version too. To me it's always interesting to see how other people model something in FreeCAD.

[chrisb]

To me it's always interesting to see how other people model something in FreeCAD.

Me too. And for newcomers it often makes it really an open choice to decide if they rather start going the PartDesign or the Part way.