Can create section view in assembly but not drawing

[HDS]

I have a top level assembly with many parts and sub assemblies. I would like to put a section view of it on the drawing. I created a section view in the assembly model it works fine. When I do the same thing in the drawing half of the parts and sub assemblies do not cut. Nothing I have tried has worked.

I am not using a Graphics-only section in the assembly.

I have tired both saving the section as a view in the assembly and creating it in the drawing.

I have moved the section plane 0.001 off center.

same display states in assembly and drawing. So the same parts are shown and hidden.

What other options are there?

I am on 2020SP5.

[Glenn Schroeder]

Just to clarify, you have a drawing view of the Assembly in the Drawing, and when you create a section view from this drawing view is when you have the problems? Or is it when you display the Assembly section view in the Drawing?

[HDS]

Both ways of creating the section in the drawing have the same problem.

[TTevolve]

If you want to do a section view in a drawing all you have to do is put a regular view down, and then section it (Either drawing a line and sectioning it, or using the section view tool).

when you say "I created a section view in the assembly model it works fine." what are you doing to do this? Are you doing a cut extrude in the assembly by chance?

[HDS]

TTevole

I use the Section View command in the toolbar at the top of the screen. Everything is sectioned with no errors.

I would give up and create a cut in the assembly except that I do not want to create the configurations to turn suppress it for the other drawing views.

Sorry, I can not show a screen shot of the actual files. I did it just like in this article.
https://hawkridgesys.com/blog/how-to-ex ... solidworks

Parts that will not section are usually tangent or point contacts creating geometry errors. Moving the section plane a little usually avoids the bad geometry and solves the problem. That is not working for this model. So I need some other tricks.

[Ben]

ya, the section view at the top of the assembly window is just so you can check if features are lining up and seeing something better or easily to work with. It has nothing to do with a drawing at all.

use the section tool on a view that you have in the drawing and then go through the steps. then place the view somewhere. after that on the section view you can right click and go to properties. look through that window at everything you can change, but go to the last two tabs and you can pick what parts/bodies you want to have in the view etc.

[HDS]

So what can I do when the section view tool in the drawing only sections 20 of 100 parts?

[Dwight]

HDS

Per Ben's reply, is the "Hide/Show Components" tab empty, as shown here?

[HDS]

Dwight

All of the show hide tabs are empty. Settings on Section Scope or View properties do not fix the problem. There are still parts and entire subassemblies that are entirely visible and cut in half by the section.

[Dwight]

Sorry, I have no idea what to suggest. I'd be calling our VAR.

[DanPihlaja]

Question:

Are the parts that are NOT sectioning made up of solid bodies? Or are they made up of surface bodies?

If they are surface bodies, you may get some traction from this selection:

[DanPihlaja]

So what can I do when the section view tool in the drawing only sections 20 of 100 parts?

When you say this....are the other 80 parts not showing up at all in the section view? .....or are they showing up, just not being sectioned?

[HDS]

Dan

The parts that are not sectioned are solid bodies, not surfaces.

Good question. They are showing up unsectioned as full parts.

[DanPihlaja]

Dan

The parts that are not sectioned are solid bodies, not surfaces.

Good question. They are showing up unsectioned as full parts.

OK then here is what you need to do.

Take each of the parts that are not sectioning and open them separately, then run a check on them:

image.png (9.11 KiB) Viewed 4834 times

Use the Stringent check, and make sure invalid faces and edges are checked as well.

If you don't get any errors, it should look like this:

But if you DO have errors, they will look like this:

If you have any faults, this might be your issue.
Even if the fault is in one part, it may be the cause of your entire issue.

[DanPihlaja]

If you end up getting errors, then there are things that can be done. The model can be repaired and rebuilt if needed.

If you modeled those parts yourself, then I would suggest running with this option checked at all times:

With this option checked, then it essentially does a stringent check with every rebuild.