Anybody else getting this message randomly in model view? The thing is, I just try it again one or 2 times without making ANY changes to the model, and it successfully sections. It's totally flaky.
I assume you're trying to section in a part or an assembly and not in a drawing. This error typically happens when the resulting section ends up with a point, edge, or face that has zero thickness so the section cut fails. It's odd that you are doing the same section and sometimes it works and sometimes it doesn't. It should be an all or nothing situation. If you are using SOLIDWORKS 2014 or newer, you can enable the Graphics-only option in the Section View PropertyManager. This creates a graphical cut (basically we hide pixels) of the model and not a physical cut so there isn't a possibility of zero thickness. If you are using SOLIDWORKS 2015 we added a helper dialog which informs you that you can use Graphics-only or choose to shift the section planes by a small amount to resolve the zero thickness issue. Shifting the planes will obviously change the actual cut edges/faces you get so it's good if you're simply reviewing the model or creating a rendering but not good if you want to take accurate measurements from where the original section planes would have been.
I'd be interested to see the model that is intermittently failing if you can share it.
Right, I totally agree and I understand the geometry (zero-thickness) will cause the failure. I've found it's helixes and such that will do it sometimes. In this part, coincidentally, I have a swept cut for threads. However, it's super glitchy. Like I said, I will just try the section a couple of times without doing a thing and it successfully sections... Super weird.
Thanks for the tip on the graphics-only option. I'm on SW 2014 btw.
Here is the file that I'm having the issue with.
Thanks Devin. Can you upload a screen shot of the Section View PM settings you are using?
I cannot get it to fail. I tried 20 or more times with a couple different sessions of 2014 and it worked each time. It's likely the thread if anything since the rest is pretty standard geometry. Unfortunately I don't know if there is anything that can be done but I'll ask our QA team to look at the file to see if something is going on.
Hi Jody, thanks for taking a look at it. It's not doing it to me today either... Maybe SW was just acting up! Strange.
QA looked at it as well and couldn't get it to fail. If you can get it to happen again, please try to capture it using SOLIDWORKS Rx and submit it to your VAR for testing.
I have run into this exact same problem several times with the most recent being a few days ago. I would send the file in for testing but I can't its a military part.
Can you reproduce the geometry surrounding the sectioned area and upload that as long as it doesn't reveal any classified information?
I have made threads the same way for many years using a helix/spiral curve. I went to make a part today using SW 2016 SP 1.0 and I got this same sectioning error.
After some investigating I found a solution for my particular case...maybe it will help others. See the attached image.
The key was that my profile sketch could not be collinear to the body OD. This seems to be creating the 0-thickness geometry with how the tool is working on the back-end causing the section tool to fail.
The strange thing is that all of my legacy parts that I now open in SW2016 section just fine, even though they use a profile sketch that is collinear to the body OD.
OK, quick update.
I went to make the opposite part to the one above [internal threads this time]...I followed my new "rule" on the profile sketch and I am getting the section error again [There are not zero thickness areas in the part]
Note I am not using the new "thread" tool because I am using non-stock thread pitch...If I manually adjust the pitch using this tool it fails. It appears that the profile the tool is creating does not scale properly in all cases.
Note that the Graphics-Only section is not an option since I need make a section view of this part in a drawing [I get the same failure in the drawing file as well].
Jody, do you have any thoughts?
Sorry for the delay in my response.
Swept helixes are notorious for merging issues. One workaround is to make the profile extend like you did. There are tolerances associated with the sweep and body surface and what can happen is the sweep will make little slivers of geometry that you can't see but the solver can so it throws an error because it can't merge them. If you are extruding the thread on the cylinder (rather than cutting into it) the reverse can happen where very small gaps form between the sweep and the cylinder face. Again the workaround is to make the profile interfere with the cylinder so there are no gaps created.
As far as the new Thread tool, you can make your own profiles (start with ours or from scratch) and add them to the Thread Profiles folder. Check out the Help section on Thread to find out best practices for creating your profile. By making your own, you can tailor it to your needs. The profiles we supplied are meant to give you a starting point for you to work from. The profile does not change size when adjusting the pitch or diameter, it simply adjust the size of the underlying helix. To get a new profile size, you'll need to add it.
Hope this helps,
No problem at all, I hope you had a nice Holiday.
Thank you for the reply. The problem is I still get errors even when the profile interferes with the cylinder geometry, some of the time. It must be related to the solver tolerances as you mentioned. My workaround so far has been to modify the geometry of the profile until the solver executes...knowing that the geometry of the part is technically incorrect.
Thanks for the info on the thread tool, I did not realize you could customize the profile sketch as well. I will try this approach next.
i just had this problem myself and I knew I didn't have 0 thickness, no matter where I moved the section on the plane it continued to give me this error. When I simply closed the assembly and opened it back up the problem went away... weird.
If you have a surface body in the solid part, delete that body. If you prefer to not delete it, select 'Partial section'.
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