Reply
Solved! Go to solution

What does this warning message mean?

[ Edited ]

When I used Revolve command, I got a warning message "Zero-thickness(non-manifold) body: The resulting interseciton is not supported." (I attached the screen capture.)

 

What does it mean? And how can I fix it??

Thanks.

15 REPLIES
Solution
Solution
Accepted by topic author mutyo051026
‎08-26-2015 04:32 AM

The zero thickness error means that whatever geometry you...

The zero thickness error means that whatever geometry you are trying to create cannot be merged together with the main solid body. This is probably because you have edge-to-edge contact between the bodies, with a gap on both sides of the edge. To solve this, you need to make sure that the new geometry either has face-to-face contact, or geometrically overlaps with the existing body. Think about two cubes that touch at an edge, and only at an edge (or they could touch only at a point - say a corner). Solid Edge tries to merge the blocks into a single volume, but it can't.

 

In practical terms, the way to fix it would be to edit the sketch so it extends down into the solid slightly.

Re: The zero thickness error means that whatever geometry you...

[ Edited ]

I have been using SolidEdge since 2007 & have never liked this error message. The information it provides is inadequate. I need to know which edge/face is creating the error.

Re: The zero thickness error means that whatever geometry you...

In your screenshot0 it seems there's only the edge round the arc where the volume you're extruding and the volume of the existing solid actually could actually meet so it has to be that. If you make sure your new extrusion properly penetrates the existing solid body and not touches it at an infinitely small point e.g. edge to face or edge to edge then you should be fine.

Re: The zero thickness error means that whatever geometry you...

[ Edited ]

Greg,

 

Yeah, it's an error in general that a lot of CAD users don't like because they don't understand it, and then even when they understand it, they argue it shouldn't be an error.

 

I can't tell exactly what's going on from the picture, but it looks like the main body has double curvature, and it looks like the transparent feature they are trying to add is trying to match that curvature on the face and at the edge. Both could potentially cause problems.

 

Face-to-face matching works for prismatic faces, but the more curvature you get, the less likely it becomes that it will work. The problem is that if you try to make the exact same patch of surface twice using slightly different methods, the round-off and approximations will cause tiny gaps and/or overlaps between the surface. Like a washcloth sitting on a countertop, the washcloth never lies exactly flat, it usually has some air gaps under it. Parasolid is trying to merge this into a nice clean solid, and just can't do it (because it's not nice and clean).

 

The edge-to-edge thing causes problems too, in the same way.

 

The best thing to do, and I know this from tons of failure, is to "overbuild" features that need to merge to edges or faces. If you're making a cut, don't make it stop at the face or have a corner at an edge. Make a cut extend out of the solid. If you're adding material, don't try to be super exact and make the new feature stop exactly at the face of existing solid. This drives people with OCD a little nuts. Extend the sketch or feature slightly into the existing solid, and it will have a better chance of being able to merge. Even though it might seem painfully

approximate, you wind up getting a cleaner model with fewer zero-thickness or merging errors.

 

In the first image, the cut out is exact, but it works because the surfaces are planar, and the math doesn't have big approximations/roundoff. On more complex shapes, this kind of face-to-face

and edge-to-edge stuff won't work.

 

This second one uses a bigger cut, so there is no near miss or approximation problem. This kind of over-cut or whatever you want to call it usually gets rid of the zero thickness and merge problem errors.

Re: The zero thickness error means that whatever geometry you...

As I said, the problem is not the error, it is lack of information. If I have a complex sketch, it is hard to pin down the particular problem segment. Overbuilding is fine, but it is a work-around.

Re: The zero thickness error means that whatever geometry you...

"Yeah, it's an error in general that a lot of CAD users don't like because they don't understand it, and then even when they understand it, they argue it shouldn't be an error.''

 

What a answer! Wrong and ...!!!

Solid Edge lets us define the body of two (or more) paralell cylinders:

- Overlaping or

- Far away from each other and is happy to accept it and save the part.

 

So why there is the problem if there is the line contact of those bodies.

FEA will calculate contact of the pin in the hole, stresses and deflections.

 

Parasolid problem is in "Not Fininshed" math and coding, which could cost perhaps less then 5000 dollars.

Or is there problem in somebody having patent on that missing code?

 

It reminds me how Solid Edge in year 2015, after all of those Hollywood announcement of the software versions, does not still let me in assembly to click on any components of this assembly of any assembly level, list the part features and edit the feature right there, without opening to edit part and closing it afterwards etc.

And configurations. I still can not show simply on one live draft hydraulic cylinder in two ar many positions acting on mechanism etc.

It has to be somebody having the patent on it or what.

Please check and make sure please to give me the real answer why you can not get that coded.

 

Those Cad users are absolutely right.

 

Milan WEndl, MEngSc, P.Eng.

AAA Engineering

ST8, SolidWorks 2015 Premium (waiting for 2016 SP1 coming in a few days).

Re: The zero thickness error means that whatever geometry you...

[ Edited ]

It reminds me how Solid Edge in year 2015, after all of those Hollywood announcement of the software versions, does not still let me in assembly to click on any components of this assembly of any assembly level, list the part features and edit the feature right there, without opening to edit part and closing it afterwards etc.


I can't speak to all your issues but this one I'm glad it is the way it is. Who would want the capability to randomly and very possibly mistakenly edit any old file in an assembly any old time. Or why would he want that power in the hands of others?

Is it really so hard to click "edit" first after all? Can't think of a time I ever thought, "**bleep**!", while doing so.

Bruce Shand
ST9 MP3 - Insight - Win10 - K4200

Re: The zero thickness error means that whatever geometry you...

Non-manifold geometry simply means non-manufacturable.

If you are not going to make a real world edge-connected object out of it, why model ?

Of course, analysis could be one area.

Pointing out and highlighting the problem region could be a good enhancement though.

Re: The zero thickness error means that whatever geometry you...

Of course creating Zero Thickness Non-manifold bodies is completely possible in a part file when using multiple bodies, so as Tushar pointed out, if they aren't manufacturable they cannot be modeled, however if needed for a different purpose they can still be created as multibody.

 

And of editing a part from the context of an assembly... you can double click on any part to see the feature tree and edit it (note, that it is not opened as the assembly is still there) but this also allows new features (Ordered or Synch), you can click on any feature in a part and dynamically edit those features (Ordered), and if a Synch part you can edit anything as if the part is opened or in edit mode, and you can also add all the Synch features you want to a part from Assembly.

Ken Grundey
Production: ST6 MP14
Testing: ST9 MP1