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Twice today I was working in an assembly with 236 components and attempted to move a component and SolidWorks completely froze. Both times I let it set for close to 15 min. with no results. So I finally gave up and went into the task manager and killed it both times.
Is this a software issue or computer issue? Has anyone else had this issue?

I am running SolidWorks 2021 SP01 with a Dell 5820, Intel(R) Xeon(R) W-2123 CPU @ 3.6 GHZ, 64 GB RAM.
Could the graphics card be causing it? I know my graphics card is not certified by SolidWorks.

Jaylin Hochstetler wrote: ↑Thu Mar 18, 2021 5:19 pm Twice today I was working in an assembly with 236 components and attempted to move a component and SolidWorks completely froze. Both times I let it set for close to 15 min. with no results. So I finally gave up and went into the task manager and killed it both times.
Is this a software issue or computer issue? Has anyone else had this issue?

I am running SolidWorks 2021 SP01 with a Dell 5820, Intel(R) Xeon(R) W-2123 CPU @ 3.6 GHZ, 64 GB RAM.
Could the graphics card be causing it? I know my graphics card is not certified by SolidWorks.

Knowing Solidworks, 99% chance it's a solidworks issue.

When this kind of stuff happens to me 9 times out of 10 it's because there's something in the assembly that SW doesn't like. See any number of posts where SW let's you do something but you shouldn't.

If I have an assembly that is doing it regularly and I have enough additional work to do on it that it makes sense I will go thru all the parts and look for "Weirdness". Could be something like it blows up on a rebuild, a feature used a bit out of typical, wierdness/Leftovers in a sketch and on and on.

Also my first suspect is almost always imported parts. It has been my experience that SW is not stellar at importing things and will do weirdness like this some times.

If you can't find anything there try to simplify the assembly, re-mate by planes instead of features, look for mates that might fight each other, nuked configurations and so on.

Probably not what you want to hear but what you're experiencing is normal SW reaction to any "Hiccup" in my experience.

MJuric wrote: ↑Thu Mar 18, 2021 5:29 pm

Jaylin Hochstetler wrote: ↑Thu Mar 18, 2021 5:19 pm Twice today I was working in an assembly with 236 components and attempted to move a component and SolidWorks completely froze. Both times I let it set for close to 15 min. with no results. So I finally gave up and went into the task manager and killed it both times.
Is this a software issue or computer issue? Has anyone else had this issue?

I am running SolidWorks 2021 SP01 with a Dell 5820, Intel(R) Xeon(R) W-2123 CPU @ 3.6 GHZ, 64 GB RAM.
Could the graphics card be causing it? I know my graphics card is not certified by SolidWorks.

Knowing Solidworks, 99% chance it's a solidworks issue.

When this kind of stuff happens to me 9 times out of 10 it's because there's something in the assembly that SW doesn't like. See any number of posts where SW let's you do something but you shouldn't.

If I have an assembly that is doing it regularly and I have enough additional work to do on it that it makes sense I will go thru all the parts and look for "Weirdness". Could be something like it blows up on a rebuild, a feature used a bit out of typical, wierdness/Leftovers in a sketch and on and on.

Also my first suspect is almost always imported parts. It has been my experience that SW is not stellar at importing things and will do weirdness like this some times.

If you can't find anything there try to simplify the assembly, re-mate by planes instead of features, look for mates that might fight each other, nuked configurations and so on.

Probably not what you want to hear but what you're experiencing is normal SW reaction to any "Hiccup" in my experience.

A circular reference is a possibility I don't think you mentioned.

I did notice that randomly the feature tree becomes a forest fire. Then I'll do a forced rebuild and it'll fix itself. What would that point to? a circular reference...?

Jaylin Hochstetler wrote: ↑Thu Mar 18, 2021 5:19 pm Twice today I was working in an assembly with 236 components and attempted to move a component and SolidWorks completely froze. Both times I let it set for close to 15 min. with no results. So I finally gave up and went into the task manager and killed it both times.
Is this a software issue or computer issue? Has anyone else had this issue?

Graphics card is a common cause of issues like this. Try a newer or even older driver and see if it repeats. We've had assemblies that would have issues with a specific driver. One time I had a user swapping between two drivers just to work on two different assemblies. Multiple monitors can cause weirdness too, especially if you start SolidWorks in one monitor and move it to the other.

Your "forest fire" comment is interesting and suggests possible mate issues, perhaps a binding issue or mate order solving issue.

1. Do you have any assembly component patterns?
2. Do you have any assembly features (cuts, etc.)

Quite a few questions on this one....

Is the assembly Top Down or Bottom Up design?
Are there Sub-Assemblies?
If not, why not?
Do you have any sketches/geometry at the bottom of your feature tree driving any part?
Do you have a part lower in your feature tree that drives any part above it?
Where does your Forest Fire initiate from, a Sketch, a Feature or a Mate?
How often do you save? (I find that the more I save the Less SW Crashes)
As Mentioned - Do you have imported models?

Like @Glenn Schroeder mentioned - Circular Rebuild is the issue and you need to figure out which part is giving you the issue.
What I would recommend is to suppress every part in the feature tree and one by one un-suppress each part, rebuild and save every time, eventually you get to the issue.

Can you zip the file and upload it or email it?

My rule is if I have to restart solidworks, I reboot. I don't know if it makes a difference or not, but it makes me feel better.

I'm working in one of my older assemblies today which hasn't been optimized. (That doesn't mean there are circular references, just not enough sub assemblies, and too many mates for SW tiny little brain to deal with.) It is having all kinds of issues. History tree full of yellow and red until a rebuild, then everything is fine. I'm trying to work with a flexible part and it is really not happy in this environment.

So your answer is two-fold. Yes, SW has serious issues the bigger your assembly gets. But this issues can be well managed with proper assembly layout.

This is what works for me (and doesn't require top down assembly)
1. Make assemblies as granular as possible. (i.e. break them down into as small of pieces as makes sense.)
2. Use patters, mirrors, etc. as much as possible. This minimizes the number of constraints SW has to solve simultaneously.
3. As much as possible, mate to construction geometry. SW has real issues solving for things it thinks can be ambiguous. (Whether they really are ambiguous is another discussion.) Plane to plane is extremely stable.

Hey Jaylin,

Do you use external references? Have you tried locking them prior to doing the move?

Maybe something is linked to whatever it is you are moving, and after moving it the external reference keeps on rebuilding which is what makes you freeze?
Just a guess!