Speed up system 3

[designmr]

Ok, I am running 2016 Solidworks 64k, my computer is (BOXX) Window 10, I7-7700CPU @4.20GHz, 64GB Ram, 64 bit system. Some files I am loading may have over 10,000+ parts. What is the BEST way to always load these Assemblies without waiting 30+ minutes or more?

Someone say SPEEDPAK certain assemblies, BUT, with SPEEDPAK, when I need to create a drawing and make sections view, you know, YOU can't do it.

I am thinking the setting on my computer are NOT right.

ANY thoughts? Other then looking for a new icon to view instead of that spinning wheel while Solidworks is waiting.

Thank you,

 

[SBaugh]

I am working on an APEX 4 BOXX desktop and I have large assembly issues as well. I am using Speedpak for some sub-assemblies. If you have make a drawing of that sub-assembly then you're going to have to use the default configuration, not the speedpak. If you are making a drawing of the entire assembly, then you need to open it in large assembly mode and pray.

However, there are some things you can due to reduce your stress:
[ul]
[li]Don't make more than 300 mates within a single assembly. if you have more parts in the main assembly you either need to make more sub-assemblies and suppress all your mates.(I personally locate a part or sub-assembly and fix it. If I have to move it later I will worry about it then.)[/li]
[/ul]
[ul]
[li] Load everything in large assembly mode and only resolve it when needed.[/li]
[/ul]
[ul]
[li]Turn off highlighted edges[/li]
[/ul]
[ul]
[li]To much detail on your parts (If you don't design it or make it, remove it and make it simple. I had a part in my current assembly that was an imported model, but it had hundreds if not thousands of fillets on the inside of the component. The imported model opened at 200+ MB. I removed all that and got the file down to 10mb. The main assembly ran much better after removing the detail.)[/li]
[/ul]
[ul]
[li]Use assembly visualization to find which files are slowing you down, then see what you can do to fix it. Surface models will kill your performance. You may need to repair the model to get it back to a solid. Any surface models or imported models that have general faults will also be a hinderance for the assembly until you remove it and repair the model. (usually requires knowledge of using surfacing)[/li]
[/ul]
[ul]
[li]Turn your image quality down low as you can.[/li]
[/ul]
[ul]
[li]Use the Freeze bar in all your parts.[/li]
[/ul]
[ul]
[li]Don't use complex mates, for example, a Slot mate.[/li]
[/ul]

Here are some more pointers from Tom Cote of the New Mexico Solidworks Usergroup see attached

 

[designmr]

Thank you...

 

[SBaugh]

I don't know why, but the link was not attached. Just noticed that.

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376

 

[designmr]

Thank for the link SBaugh...

 

[SBaugh]

I just added 16GB of memory to my APEX4 giving myself 32GB and it runs better than it ever has. No more notifications about memory issues, crashing has slowed down dramatically. It's so much better at 32GB.

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376

 

[designmr]

SBaugh, thank you for your reply. I have 64GB installed, but I STILL get crashing, or notifications of memory issues....

 

[SBaugh]

Have you checked your Event log to see what might be causing the crashing? Filter out for error, warnings and critical and see if you have a lot happening and what is crashing. It might be something is crashing in the background like .NET and its taking SW with it. If the .NET is crashing or there is something wrong with it, then you will see problems with SW. The only solution to resolve that if you are in Windows 10 is to reformat and reinstall windows. If you are using an older release of windows you might be able to repair it using the Microsoft tool. I would recommend contacting your VAR.

Also is the crashing happening with just one assembly or any large assembly you open? It could be file specific as well. If it is, then you can send the files to your VAR to rule out your PC.

Scott Baugh, CSWP
CAD Systems Manager
Evapar

http://www.evapar.com

"If it's not broke, Don't fix it!"

faq731-376