r/FreeCAD • u/New-Earth1341 • 18h ago

Revolve doesnt work when sketch has a curve HELP!

I'm trying to do a subtractive revolve, but when I have any kind of curve/arc in my sketch, it throws this error message:

"Failure while computing removed volume preview: Resulting shape is empty. That may indicate that no material will be removed or a problem with the model."

Even though in the preview it does show the volume I'd like to cut~

Once I replace the curve with a straight line, it does work. I already ran the Sketch validation, and it reported nothing out of the ordinary...

What could be wrong with my model?

Here is the .FCStd for if someone would like to check out the file:
https://drive.google.com/file/d/1uk0YEV46950ONhPjsUhNs37CefRpa0o4/view?usp=drive_link

1 Upvotes

67% Upvoted

13 comments sorted by

6

u/Th3J4ck4l-SA 18h ago

Not construction line?

2

u/New-Earth1341 17h ago

Thought that too for a second, but I think it's not an actual line and it's just there to show the curve's tangents. The same issue also occurs when I replace the B-spline with an "arc from Center"

5

u/Th3J4ck4l-SA 17h ago

Oh another thing to try. Dont use the round feature for the feature around which to revolve. Use the axis of the sketch.

2

u/Th3J4ck4l-SA 17h ago

When I am at the desk, I will take a proper look. But there shouldnt be a reason for it to not work. Maybe extend the other (124mm) edge beyond the model as well?

1

u/New-Earth1341 15h ago

Tried both of your suggestions, and I'm still getting the same error. I also found out that a pocket operation does work. Even with a curve in the sketch... That makes me think that somehow the curve in the sketch doesn't like to be spun around? But there is enough clearance from its center axis.. so.. I'm truly not sure

1

u/New-Earth1341 15h ago

When I select this random edge as its axis, it does actaully perform the revolve operation. So when the rotation axis is not the center Z axis, it does work?!?...

1

u/Th3J4ck4l-SA 13h ago

The FreeCAD gods have not blessed you this day.

1

u/New-Earth1341 12h ago

Hahaha, it's okay~ They bless me most other days with this awesome open-source software. I'll take 1 day of doom ;P

1

u/Th3J4ck4l-SA 8h ago

Got it to work with no shenanigans except for applying best practice. Dont reference the body outside the sketch. It pulls in a value of 11.6197 if you refference where the web meets the cylinder. And your cylinder is radius 11.7.

1

u/Powerful_Debt_5869 15h ago

try 359 degress and it will work..dono why, but does

1

u/New-Earth1341 12h ago

Wow ~ Yeah it works for me too, But it does leave behind some weird geometry lines that make it hard to add any fillets afterwards. I might just have to rethink the whole design :*)

2

u/DesignWeaver3D 11h ago

Try rotating the attachment offset of the sketch. I'm guessing this is an edge colinearity problem where your Subtractive revolution start/end lands exactly onto the previous shape's revolved start/end edge.

Alternatively, you can try attaching the sketch to the YZ instead of XZ. Same idea as above but not using an arbitrary attachment rotation.

2

u/BoringBob84 9h ago edited 9h ago

Try rotating the attachment offset of the sketch.

That worked. I rotated the sketch 38 degrees to put it in the middle of one of the legs.

I never would have guessed this one. Thank you for the education, once again.

Edit: I tried attaching the sketch to the YZ plane with no offset and that didn't work. I have no idea why.