Need Advice for Optimizing Large Assembly Performance in SolidWorks

SOLIDWORKS SW General
1

Hello there,

As you can imagine; managing and working with such a large assembly is becoming increasingly challenging. I am facing issues with performance, including slow load times; sluggish response during model manipulation; and occasional crashes; which are starting to impact my productivity.

I have already tried a few strategies; such as simplifying parts and using lightweight mode, but I am still encountering performance issues. I have read about other techniques like using SpeedPak; but I am not entirely sure how to implement it effectively, or whether it is the best solution for my scenario.

Could anyone share their experiences or tips on how to best optimize large assembly performance in SolidWorks?

Best practices for structuring and organizing large assemblies to minimize performance lag.

Effective techniques for simplifying models without losing essential details that are crucial for the design.

Any recommendations on hardware upgrades that could significantly improve performance.

Any lesser-known settings or tweaks in SolidWorks that could help improve performance with large assemblies.

Also, I have gone through this post; https://www.cadforum-net.dezignstuff.com/viewtopic.php?t=3597& which definitely helped me out a lot.

Any third party tools or add ins that might assist in managing large assemblies more efficiently.

Thanks in advance for your help and assistance.

2

Don’t be afraid to break partThe best thing I have learned to do is use sub-assemblies

Sub assemblies make it easier to turn things off (either hide/show or suppress/un-suppress) to make working on a large assembly more manageable to work on.

3

Not sure the link you posted is the correct one, it goes to a sheet metal topic, not assembly related.

Are all of the component files at the current solidworks version? I’ve heard that opening/loading files from older versions takes longer. This may be mute point for files loaded light weight.

Have you looked at the Performance Evaluation in the Evaluate tab? This might point to some low hanging fruit or files that are responsible for huge chunks of the load times.

Hope all of your files are opening from local drive.

4

https://www.youtube.com/watch?v=m_XHG4GWja4

5

[quote=Frederick_Law post_id=36746 time=1724687164 user_id=51]
https://www.youtube.com/watch?v=m_XHG4GWja4
[/quote]

Thanks very much for publishing that old video, Frederick. [mention]Padrickk[/mention] I can tell you right now, there is no magic pill to make your assembly faster. You just need to think a bit differently than a typical user: Match the Task with the Tool.



I hope [mention]matt[/mention] would not mind if I state that the fastest and easiest way to become a master of large assembly (and drawing) management is by joining me for 4 sessions of the Large Assembly and Drawing Workshop <LINK_TEXT text=“https://trimech.com/solidworks-large-as … -workshop/”>https://trimech.com/solidworks-large-assembly-and-drawing-workshop/</LINK_TEXT>.



Of course, I am more than happy to meet with you for an initial discussion to take a look at one of your assemblies and discuss the type of slowdowns you experience and your definition of success (e.g. reduce opening time by 60% in resolved mode, eliminate lag, etc.).



Let me know if interested. alin.vargatu@trimech.com

6

I am experimenting right now with one assy. Not so big, but it took about 90 seconds to save, with SW freezing all the time and other performance issues.
It now saves in 5 seconds and its file size is HALF it used to be, it opens 50% faster, the drawing takes one third of the time to generate the views.

I started with the biggest parts:
our machinery uses a lot of imported data for sensors and standard parts like valves etc.and often the engineer just import them without fixing all the topology errors running the import diagnostic.

this is the first step: no currupted faces, no gaps, no faulty edges.
no surfaces, make the body solid and fill all the internal gaps if you do not need them. no springs, no real threads, avoid patterned holes and grill like shapes.
I am able to reduce by ten folds the file size in this way and the top assy becomes lighter as well.

I do pack and go of the whole assy structure and fix one part at time. then I have a macro that open the assy, make a drawing with 4 views and give me the operation times for both.

Every corrupted component is going to bloat the top assy size. If the corrupted- unoptimized component is inside a sub assy, you need to rebuild and save the subassy as well.

There was a main culprit, a big part around 67MB full of BS geometry: it is now around 5MB without any noticeable difference, but NO grips and no threads anymore, and the faulty surfaces are now sewed into a solid.

I did not stop with this big guy and I went to fix other 5 smaller components and I gained another 50% in performance. Drawing is the part that gains more from a good and clean 3D.

Another huge performance killer are the patterns and they must be used correctly.

  1. use “feature pattern” ONLY for holes and cuts, avoid multiple features like extrusions, blends etc, use a solid pattern+separate boolean operation instead for those

  2. avoid pattern of a pattern

  3. for holes and cut use the “geometry pattern” option (10x faster)

If you do not need parameters import a parasolid dummy data. (we do it for all catalog parts) remember to run import diagnostic!

7

I’m not convinced the OP is legitimate. His first post had a janky URL with another site embedded in it. I could see having a bad URL, I struggle with that feature when I try and use it on this site. But I don’t see how you could accidentally include a link to a 3rd site unintentionally.

8

AI?

9

Hi,

From experience working SW resellers and doing support for many years this is what I found:

-Reduce file size by reducing image quality
-Fix imported geometry with import diagnostics, it matters, 2 lines trying to meet close to infinite, kills SW. SW kernel takes too long to give up.
-Be strategic, plan your designs, use large design review, if you have SW task scheduler use it to update large top assemblies
-Choose not to have Many of Many on what you can choose. If you can’t choose not to have many components in your product, you can choose not to have many configurations, many mates, gigantic feature trees, many sheets on the same drawing

Cheers
Pedro

10

I would be happy if it were to come back and prove me wrong.