Hi everyone,
I have some prior experience with Solidworks, but I wanted to try out a FOSS alternative. I’ve been messing around in FreeCAD for a couple hours and I have the following question:
How do I polar pattern a revolved surface?
I want to accomplish something similar to what is described in this video (12:14 to 13:44).
My ideal workflow is as follows:
- Create sketch (e.g. square)
- Pad sketch to create body (e.g. cube)
- Create new sketch (e.g. line)
- Revolve sketch to create surface (e.g. disc)
- Polar pattern the surface to create multiple (e.g. 4) discs
- Slice apart cube by 4 discs to yield 9 separate bodies
I’m stuck on step 5. Is this possible in FreeCAD? If not, are there any recommended workarounds to achieve the same result?
Thanks in advance!
You must log in or register to comment.
If the surface polar pattern is referenced to a revolve line such that the disc patterns do not intersect with the cube, FreeCAD will throw an error because you can’t have multiple bodies within the same body entity.
Thank you so much for your reply! Not sure why I didn’t see it until now!
If the surface polar pattern is referenced to a revolve line such that the disc patterns do not intersect with the cube,
I don’t think this should be an issue, as the axis I’m referencing for the polar pattern should result in all patterned discs intersecting the cube.
FreeCAD will throw an error because you can’t have multiple bodies within the same body entity.
Not entirely sure I understand this part. Are surfaces considered bodies, or are only things with volume considered bodies.
I’m having difficulty creating my polar pattern in the first place. The default behaviour of the polar pattern tool seems to be to pattern my cube, rather than my disc. If I manually remove the cube from the features list and select the disc instead, the following message pops up:
None of the three options seem to result in the behaviour I expected, which would be something like this:
Any advice?
Thanks!
So you can try the realthunder/linkstage branch of freecad if it is a body problem.
FreeCAD main can’t have 4 seperate solids within the same “body” (file -> part -> body -> sketch heirarchy). Every solid that isn’t intersecting has to be a seperate body.
For this test you are doing, you will have to use the Part workbench instead of Part Design, I think. There you can make 2D and 3D shapes, but every one is a separate body. Then you can do some similar pattern cuts, but it will create new bodies based on your cuts and hide the old ones.
I would say Part workbench is the most like Solidworks where Part Design is sketch based. That means use additive design as much as possible for a single solid part in Part design, then put different solid objects together with assemblies.
Thanks! Using the “Part” workbench instead of the “Part Design” workbench, and using the “Polar array” tool from the “Draft” workbench instead of the “PolarPattern” tool from “Part Design” workbench seems to have done the trick.
I’m now having some difficulty with step 6: Slicing the cube into 9 pieces. It seems like the best tool for this is “Slice apart” from the Part workbench. Is this the correct tool?
If I set the polar array number to 2 (generating two discs), I can slice the cube into 3 pieces just fine. However, if I set the polar array number to 4 (generating four discs), the “Exploded Slice” in the tree contains only 3 pieces, not 9.
The exterior faces of the cube appear to have been sliced by all four discs, but only two discs seem to have actually sliced the solid.
What am I missing?
I think you’d be better off using the Boolean XOR tool from the same Split submenu (if you approach it from the Part menubar in the Part workbench), on your cube and your array, instead of the Slice apart tool.
Then on the resultant XOR object use the Explode compound tool from the Compound submenu.
You’ll get a folder with all your sliced parts in it.
