Help with hollowing out a custom shape

[creitzel]

Hello all, this is my first post. I've been playing around with FreeCad for a couple months now, trying to design a case to be 3D printed for an electronics project I'm working on. I've got all of the case designed, with the exception of this last part. I am attempting to create a lower case "sigma" shape, that is hollowed out on the inside. I have tried quite a few different things, on the Part Workbench, Part Design Workbench, and even on the Drafting Workbench, with no luck as of yet.

I'm attaching a freecad file that is basically the closest I've been able to get to what I'm after. This file was created on the Part Design Workbench, using an additive tube to create the basic sigma shape. It's really close to what I want, I just can't figure out how to remove the overlapping parts in the hollowed out section, and how to put a proper end wall on the sigma (since I'd like it to follow the semi-circle profile of the sigma, and be angled along the curve at the end).

It originally seemed to me that boolean operations with a couple of primitive objects (specifically a couple toruses, and a couple cylinders) should have been able to give me the effect I'm looking for, but after several hours of playing with the boolean functions in both the Part Workbench and the Part Design Workbench, and reading/watching countless posts/videos on the internet I guess I just don't understand how the boolean operations work.

Thanks in advance for any help you guys can give,

Chris

Code: Select all

OS: Ubuntu Core 20 (ubuntu:GNOME/ubuntu)
Word size of FreeCAD: 64-bit
Version: 0.20.1.29177 +233 (Git) Snap 245
Build type: Release
Branch: tag: 0.20.1
Hash: f5d13554ecc7a456fb6e970568ae5c74ba727563
Python 3.8.10, Qt 5.15.3, Coin 4.0.0, Vtk 7.1.1, OCC 7.6.3
Locale: English/United States (en_US)
Installed mods: 
  * Curves 0.6.2

[papyblaise]

PartWb has a "Connect" tool
you have to extrude the right pipe in PartWb and use the connect tool which will make the 2 pipes open to each other

[creitzel]

Nice. I haven't used the revolution, extrusion, or connect tools yet. Definitely going to play with them now.

After I posted the question, I continued playing around, and eventually got the effect I wanted using additive primitives, and boolean operations. It turns out that the boolean operations in Part Workbench work on Bodies, and I was initially trying to combine them in a single body, which is why I was having so much trouble. I still can't seem to get the primitives to line up correctly though and they always seem a little bit off. Also, it took quite a few boolean operations to get what I was after, so way more steps involved than your method.

I've attached a file showing the primitives/boolean method, just in case someone else comes along and sees this, and wants to see it.

Thanks for the solution, I think it is definitely superior to where I ended up, using boolean operations.

Chris

[chrisb]

I see room for improvement in both of these approaches: In papyblaise's approach you have links going out of allowed scope, because you must not use a PartDesign feature in a Part tool. You should apply them to whole bodies only.

In creitzel's model at least the first booleans are completely unnecessary: Fusioning a body with just a single feature in it is as good as adding the feature directly. So here you can move "Cylinder" directly with the context menu to "Body", remove the boolean and the then empty Body001 and you are done with that.

Instead of making a boolean cut with a single feature in it, you can do the same directly with the corresponding subtractive feature. In your case you can move Sketch and Sketch001 to Body and make pockets.

Here is how it looks so far. There is no time left now, but I recommend to look at the last - admittedly more complicated - body with the same critical eye. I'm sure it can be improved as well. First thing to do is probably to add the torus as a subtractive feature to Body.

[chrisb]

Had still some time left and it was easier than expected. So here we go:
The subtractive torus works as expected.
Then there is only the cylinder left, which can now be subtracted instead of being added to the cut. Please note that it is perfectly ok to cut into plain air, so there is no need anyway to shape this cutting cylinder.

So the final thing following your ideas would look like this:

SnipScreenshot-4e27cc.png (46.05 KiB) Viewed 429 times

[chrisb]

I am extremely surprised though, that your Cylinder001 has neither Placement nor AttachmentOffset visible. Do you have any idea how it happened?

[creitzel]

Awesome, thanks a bunch for the suggestions. I'm still quite new to freecad (and 3d modeling for that matter) so I was taking each step one at a time, and using separate bodies to do different operations. And then combining the bodies using boolean operations. Clearly there are more efficient ways to do this, as you have pointed out. I'll definitely be studying your version to try and learn more.

I am extremely surprised though, that your Cylinder001 has neither Placement nor AttachmentOffset visible. Do you have any idea how it happened?

I'm not sure exactly what you are referencing with Placement, and AttachmentOffset. But I created the cylinders as additive primitives, which of course places them in the center of the workspace. I then used the transform tool to rotate and offset them into the correct position with the toruses. Maybe doing it that way makes the Placement and AttachmentOffset invisible?

Thanks again for your time investment in this

Chris

[chrisb]

I then used the transform tool

That's the culprit. Transform must currently not be used to move Features from inside of a body. I will report a bug.

[papyblaise]

@chrisb what is this weirdness

[Shalmeneser]

I would try something like this, but due to coplanarity, I cannot close the circle or intersect the forms : Additive features THEN subtractive features.