SketchUp is surface modeling, and doesn’t tend to create manifold objects. Reasonably easy to use for its intended purpose, but not intended for this kind of design. It was used a lot in the early days of openbuilds and as a result there are a lot of “approximate” objects out there that basically need to be re-drawn to be used for CAM or indeed anything other than mocking up. While I haven’t used it recently, SketchUp certainly was wonderful for quick mockups and getting quickly to rendering, and I have used it for that purpose. I am not familiar with its recent capabilities.
If OpenSCAD was so intuitive that you were able to use it without learning anything, my hat’s off to you. I say this as someone who found OpenSCAD initially more accessible than FreeCAD given the OpenSCAD cheat sheet. But I would have been lost in OpenSCAD without the cheat sheet, and now I’d say both that FreeCAD has become far easier to use than it was then, and that MangoJelly’s tutorials have made it reasonably easy to understand the FreeCAD operating model. But I wouldn’t expect to just open it up and start modeling. I also wouldn’t expect that in commercial solid modelling CAD. Not F360, not SolidWorks, not CATIA…
I’m not sure what solid modelling CAD program, GUI or textual, is both intuitive and powerful. Perhaps CaDoodle - Free Offline CAD Alternative to Tinkercad would fit the bill for you? I haven’t tried it, but its target audience is non-specialist. I haven’t looked at all, not even to learn whether it offers dress-up operations like fillets and chamfers.
FreeCAD Part Design workbench added “direct manipulation” this past summer as part of the Google Summer of Code, and the upcoming 1.1 stable release (currently a release candidate with just a few blocking issues between it and release) allows you to grab objects and manipulate them directly with mouse actions, instead of typing in numbers for dimensions. I’ve almost never used it, because I have gotten so used to typing numbers that it now feels easier to me than dragging things around with a mouse. But you might find that a helpful affordance.
Oh no, I’ve been nerd-sniped!
I don’t know if it’s “better” but I’ll try to make an exact replica, relatively parsimoniously.
Sketch on YZ plane:
Revolve:
Sketch on XY plane, import the torus as construction geometry, select section view, then make a circle constrained to the Y axis (X would work too) with the center constrained to the outside of the torus, and the diameter constrained tangent to the center:
Pocket:
You can just drag it through the toroid using direct modeling, but I’d just change to “Through all”, and reverse it so that it goes up from the base plane:
At this point, I discovered and reported a bug. I expect the bug is in the OpenCASCADE library that FreeCAD uses for its geometry kernel, rather than in FreeCAD proper. I had to offset the circle slightly from the center of the torus for it to cut correctly. Moving on with that workaround!
Now a Polar pattern with five instances:
Another sketch on the XY plane with the hexagon constrained the way you did in the OpenSCAD. (Note that if I were doing this from scratch I’d be constraining it by distance across flats as measured with calipers or by specification, not by the diameter around the points.)
Now pocket that 5mm in (again reversed because I’m building up in Z):
At this point we have the same thing you uploaded originally: Knob.FCStd (871.6 KB)
Now you want some fillets for comfort, right? Hover over the face of the torus (here, light green) and click to select (here, light blue):
Then select the fillet operation:
You can either drag the arrows to change the size, or modify the radius by clicking the up/down arrows or entering a size. Here it is with a 6mm radius:
Now I click OK and get the model
It renders quickly in FreeCAD and can be exported in whatever form you like, including STEP and STL. Here’s this final version: Knob.FCStd (871.6 KB)
