Extrusions will not extrude turns red and nothing

kevin_daney054

I am just trying to extrude a rectangle onto a part that I have already drawn. Part of the rectangle is "floating" in space, but the other part is not.
Why will it not extrude?

It is this basic puzzle cube that the  PLTW classes use.


Here is the part
 
https://cad.onshape.com/documents/7db9d78cd79a72a09c0b4e13/w/7bd1f8dd7c59e891d6edd014/e/766bdf5f644d80d9274d010c

Mark_Cheli

Hi Kevin!

This is what is known as "non-manifold geometry".  Specifically you will have an edge that is infinitely thin between the new geometry and previously created shape.  This infinitely thin edge cannot possibly exist in the real world, so Onshape prevents you from creating it.  Here's a reference that might be useful for you:

https://www.sculpteo.com/en/3d-learning-hub/create-3d-file/fix-non-manifold-geometry/

kevin_daney054

Thanks for the quick reply. I guess I understand the issue, but it seems I should be able to still make the part on the computer and 3D print it. It has a "non-manifold" geometric corner, but the rest is solid connections.  I am a teacher and the students are designing a puzzle cube with 27 3/4" wooden cubes.  They are to design it on OnShape and then actually build it in the real world with wooden clocks.
Is there anyway to still draw this on OnShape?

Evan_Reese

@kevin_daney054
Cool project. Is there a reason these two parts have to be one body? if you cut them exactly as shown out of wood somehow, they would have been cut into two pieces anyway. You can also export them as a single stl for 3D printing with no issue.

kevin_daney054

Well in the real world they will be one part so they might as well be on OnShape. Also the students are new at OnShape and to add lots of extra steps would be hard.  I guess I still do not understand why I can not extrude the part as one part. seems weird.

Evan_Reese

Ah, I looked at your image too quickly. I understand why it's confusing that it can't be done. No CAD system can do it that I'm aware, so this could be a helpful limitation for your students to learn anyway. I don't fully understand why either, but I think it's something to do with the math behind how it defines the inside and outside of the shape. At the edge it becomes infinitely small so the inside and outside can't be determined. The real solution is just to add a slight interference or slight gap, but since you don't want to add a bunch of steps, you could use the composite part feature (check the "closed" tick box) to make onshape treat them as one part.

david_salonia

Sorry Evan but you are wrong. I was able to easily model this part with Inventor. And this part can certainly be machined or cast. This is a limitation of the Onshape modeling algorithm and it should be corrected. As long as one surface of the rectangular portion of the part is attached to a surface on the T portion, Onshape should be able to model it. But it doesn't. 

NeilCooke

@david_salonia it is true that Inventor can do this but I’d love to see that part accurately manufactured. Parasolid does not permit non-manifold geometry and this will not change. 

steve_shubin

david_salonia said:

As long as one surface of the rectangular portion of the part is attached to a surface on the T portion,

I tried to open the original document, but it looks like it’s not there anymore.

You used the word attached

Well it looks like the two parts were not attached.

Looks like these two parts were touching at the corners of each and that’s all

Evan_Reese

david_salonia said:

Sorry Evan but you are wrong. I was able to easily model this part with Inventor. And this part can certainly be machined or cast. This is a limitation of the Onshape modeling algorithm and it should be corrected. As long as one surface of the rectangular portion of the part is attached to a surface on the T portion, Onshape should be able to model it. But it doesn't. 

News to me, thanks! I've only used parametric CAD packages with Parasolid at the core, and didn't realize others were different in this regard.

leonid_raiz

Your extrusion probably made using Add and therefore makes non-manifold geometry as Onshape tries to add it to preexisting parts. It should however work okay if you switch to New and will make a separate part.