I am trying to section a model through a normal plane to the model but it says what is in the title up there. Any clues?
Make sure there is no zero geometry at the particular point. Try moving the plane back or forth to see if you get the results OK.
I don't see any zero results. Weird and I don't know how to make it right. ughhh
If you upload the model it will be easier for us to diagnose the problem.
I wish I could upload the model. IP issues though.
Do you want to perform a section in the model or in a drawing view.
In the model environment, you can use a Graphics-only Section. In this case SW does not check for zero-thickness geometry conditions.
Also, it appears that I can't do any useful work if I'm looking at a Graphics-only section. I'm still annoyed.
Belay that! Apparently I can edit parts, measure, etc. Sorry, false alarm.
It works, thanks.
I've had this problem many times, and it's very annoying. It's good to see an answer (thank you, Alin Vargatu), but going back a step what do you all mean by "zero geometry"?
That is zero thickness geometry. Imagine a cube that has inside a spherical cavity that is tangent to one or more of the faces of the cube.
You cannot really have a solid body like that in real life.
So: if I get this error message when I'm trying to view a section, it means that there is perhaps a sphere or cylinder in my model tangent to the plane that I'm using to create the section view?
I'm not convinced that this explains every circumstance in which I get the error. Yesterday it came up, so I entered a small offset from the plane. The error message repeated.
Are there any other conditions that can produce the error?
I've known this error for a very long time and I'm disappointed that it still exists (2017 version). If you have an assembly with hundreds or thousands of parts, the chances of this happening are actually quite high.
I'm working with a lot of imported parts. The assembly failed sectioning in model - and in drawing view. The "graphic only" option works, but the cut surfaces fail to show their outline. In the drawing I had no choice. I really needed this section. Fortunately SW tells which part failed, but this is still far from a solution.
By disabling parts I found out that the error occurred with a combination of two parts, both containing more than one solid. Opening these parts separately and sectioning them in the same way did not cause the error.
I ended up reversed-engineering one of the parts, that was the real culprit and now it seems to be solved.
It makes no sense that SW checks for zero thicknesses. When I make a section, I'm not really physically trying to make this part. It's just for showing internals and dimensions, so the graphic only option should always be effective. I can imagine that there are mathematical reasons why you can't show a zero thickness, but find another solution than failing the section.
Please Solidworks, do something about it!
Vote for Zero thickness geometry in the Top Ten List.
Go to this link and vote for Allow ZTG zero thickness geometry.
I see that there is a lot of opposition, because some hardliners don't want to allow things you cant make.
What I want is different. It's not a new feature, it's simply solving a program bug.
It's not really a zero thickness geometry that i'm trying to make, but probably the same internal check causing this problem. I'm importing multi body parts. The conversion is fine until I try to make a cut view. Moving or rotating the cut plane may solve it, but creates an undesired view.
Left picture error message, mid: graphics only, right section plane rotated 1deg.
Sectioning an assy containing this part fails in the same way.
I figured this out.
If you have a hollow cylinder, say with 1mm ID and 2mm OD, and you try to section it at 1mm off the center, then there is this little sliver that the SW 3D engine can't reconcile. I changed the 1mm ID to a 0.999 ID, and then the problem went away. Not a perfect fix but that's what worked for me. I consider this a bug and lost about 45 minutes trying to figure out what was going on.
How does one identify which part is causing the "invalid body"? A quick fix is to suppress that part.
Zero Thickness Issues is a limitation within SW. No way around it.SW drawing views are in essence assemblies!!! You can search forthe issue in the Assembly instead. You can use section or cut extrude to dig into the issue. The nice part is that troubleshooting in the assembly is much faster.That is if you do need the section at a specified spot and moving your section planea fraction of a thousands left or right is not possible.Working with imported geometry that is used in assemblies require some preparation.Checking the model for faults or import diagnostics is often neglected but helps avoid many issues.Including performance drag and section troubles.
can you show a "shaded left view" and "shaded right view", with front plane visible ? with no cut-view of course.
just to see your 3d model… and investigate a little, like Columbo should do...
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