Impossible in OnShape but possible in Autodesk IPT: Boolean operation failed to return a valid part

trevor_curtis

I am a high school engineering teacher. I started out in Autodesk Inventor. In that program, files are separated as parts and assemblies, etc. In Onshape, it seems that you could build assemblies inside part studios. There is a project we do where students create puzzle pieces that form to make a larger cube. Some of the parts that my students come up with are impossible to create in OnShape as one merged solid part. It always happens when two corners or edges come together with empty space on one or both sides. I get an error stating that boolean operation failed to return a valid part. I can create these same models in Inventor as one singular part, no problem. I don't understand why OnShape cannot create these models as one solid part when they are all connected through a joining body. Is there any solution for this? I have included images of two examples as well as a link to the file being used. I have tried multiple ways to create them as well as patterning. I have tried with and without "merge with all". Here is a link to the file: https://cad.onshape.com/documents/b2ea531c88ae07fcf1e23cdd/w/168c0f64537a353b0932764d/e/878a6945c242ed3dc8eb70ca
Here are some images:

S1mon

The Parasolid kernel that’s at the heart of Onshape, Solidworks, NX, and many other CAD systems can’t handle a solid with a line intersection like that. Similarly it won’t let you have a hole which is tangent to a surface of a shape either.

tim_hess427

Just for some additional context - this isn't seen as a "problem" that needs to be fixed because Onshape is primarily a tool for designing mechanical things that can be physically built. Since you wouldn't physically be able to build a part with zero-thickness features, there's not a lot of reason for people to be modeling them in onshape. 

trevor_curtis

I do not have very much experience machining or physically building these models that I make. However, I would think that these parts could be physically built in real life. All of the models that I showed as examples have underlying material for them to be permanently joined or machined out of a solid piece of material and remain as one unifying body. I would think that if I tried to extrude just two rectangles that are only touching at the corners, that would be an impossible thing to physically build. But there is a base of material below that keeps the rectangular prisms joined together as one part.

I also tried what S1mon said and added a hole that was tangent to the surface of one of the models and it would not allow me to cut a hole, just like S1mon said. I would think that it would be possible to physically drill a hole in an object and have the edge of the hole be tangent to a surface.

I will accept that this is just the way it is in OnShape. It just seems like it should be possible to have a singular part like the ones I have demonstrated.

tim_hess427

@trevor_curtis - Regarding manufacturability - While you're right that all of the material would be connected to some other material, the issue is with the zero thickness edges and corners. In the real world, you either have material touching (thickness > 0) or you don't (gap > 0). It is very possible to manufacture things with very small thicknesses and gaps, but they'll never be exactly zero. 

Also, think about a hole tangent to a surface. If you were to physically make that, what would you expect to happen? If the outside surface is continuous, that means there is a least 1 atom of thickness between the outside surface and hole (i.e. thickness > 0) OR there are missing atoms at some point along the surface and there is a gap of at least 1 atom wide (gap > 0). 

Mathematically - I think it can also cause issues in the software because it has to keep track of where the "inside" and "outside" of a part is. A single edge that connects more than two faces throws a wrench into the works, so the parasolid kernel just says "nope! can't do that!" rather than deal with the complexity of allowing real-world impossible things to be modeled. 

bryan_lagrange

Just fudge a little. 

https://cad.onshape.com/documents/32c3355da96b467494123f9d/w/cbbafaa792be9f6fb924b59a/e/f21cf85daa244a6a8bf8fccb

trevor_curtis

tim_hess427, thanks. That makes sense. I guess I am just used to being able to do it in Inventor but I see the point behind why they do it the way they do in OnShape based on your explanation. I can deal with that issue in exchange for all the other benefits that OnShapes brings to my classroom and students. 

bryan_lagrange, I used your advice and just used 0.748 instead of 0.75  for the rectangle dimensions and it will work for those instances. Thank you everyone.

dirk_van_der_vaart

With a very good machine and tools it would still look like this.

https://cad.onshape.com/documents/7d17d14d4c7ef8b173987b1d/w/5dc2ba48cd28c392814c41d6/e/d6d1eab02d43776ae7523c19

PeteYodis

@trevor_curtisIn this case you opted to add this geometry to an existing part, and it's rejected for the non-manifold case mentioned above by others. You could choose the "New" tab on the extrude feature dialog to make a new and separate part. Part studios can have numerous separate parts, but each must be manifold to themselves.  Expecting geometry to survive in tact like this in the real world as a uniform part is unwise.  Any sort of loading on infinitely thin or near infinitely thin areas of the geometry would lead to part failures in practicality.  

Toshimichi_Oda

This is a sample with zero thickness.


When machining I make chamfers in this.
But when modeling cad data, the chmafers make us comfusing.

It is restriction of CAD, not less need of modeling.

Even so, I prefer prohibit of zero thickness in cad because such cases are rare .Zero thickness makes cad-system complex.

michael3424

dirk_van_der_vaart said:

With a very good machine and tools it would still look like this.

https://cad.onshape.com/documents/7d17d14d4c7ef8b173987b1d/w/5dc2ba48cd28c392814c41d6/e/d6d1eab02d43776ae7523c19

EDM could make a square corner in the bottom, though, couldn't it?

wayne_sauder

@michael3424

  Even with EDM, I think you would need a gap in the center, which if you draw it that way Onshape will let you extrude it. 

michael3424

@wayne_sauder - true, I was referring to the cutter fillets at the inside corner.

Toshimichi_Oda

I agree zero thickness not exist when machining or EDM,
but it is different problem to want to make a model with zero thickness.
It is not necessary for me to make a model with EDM gap.

I have heard to development member of SolidWorks that parasolid kernel can treat a zero thickness. (I do not the detail.)

The following is my thought.
Pleat see modeling will be complex if permit zero thickness.

When no zero thickness, one edge have two adjacent faces.

If zero thickness, one edge can have four adjacent faces.
When you make a fillet on the edge, you must specify one of six types.


When one edge have 6 adjacent faces, how many types?
And more?

Selection of edges in 'Draft' feature has the same problem.

I think no zero thickness is restriction of cad for kind of users.

S1mon

I've always assumed that the reason that Parasolid can't handle zero thickness is due to how the algorithms handle topology. The fact that real world manufacturing methods can't produce a zero thickness situation seems like more of an excuse than anything else. The Granite kernel of Creo can handle it, so clearly it's possible if the math is set up right.

The biggest pain for me with the lack of zero thickness in Solidworks is not that I've ever wanted to model parts with zero thickness, but that cross sections would fail on some obvious place like the centerline because I happened to have some part with a hole tangent to the centerline. Sure, you can move the cross section plane some microscopic amount, but it's always seemed stupid. Somehow in Onshape they've managed to fix this issue, which is great (graphics only section?), but seems to be at the expense of being able to measure things on cross sections. 


      

konstantin_shiriazdanov

@S1mon while it can create cross sections in graphic area it would still fail to create section views in such circumstances in drawing.

S1mon

@konstantin_shiriazdanov Good to know. I'm pretty deep into parts of Onshape, but I still have barely touched drawings. I guess I'm not surprised.

tim_hess427

@S1mon - I think you're right in that it just comes down to how the math is handled in the kernel. Sure, its possible to model zero thickness features since others have done it. However, the fact that you can't physically manufacture something with zero thickness isn't an "excuse", but more of just some context that I think explains why it isn't a high priority for onshape since it's primary usage is model things that will (or could be) built eventually. 

In my opinion, not teaching onshape to engineering students because it can't do something like zero-thickness features seems a little short sighted. It's just not something that's needed in an MCAD tool. For some, it could be a good thing and prevent an engineer from sending impossible things to the machine shop.