After attending the Lynkoa Tour webinar some time ago about "Performance Optimization in SolidWorks" I have a few questions :)
The main problem I encounter is the opening time for large assemblies on SolidWorks (2018 SP3 + PDM).... So I wanted to follow the mentioned webinar in order to optimize my use of SolidWorks for assemblies but I was already applying a good part of the advice: reduce the image quality, use the blocking bar, disable dynamic highlighting, etc...
One of the points caught my attention, however: the use of subassemblies because according to the person in the webinar, SolidWorks does not recalculate the constraints of the sublevels! (See attached screenshot). So I modified the assembly in question, which takes a long time to open, by composing it to as many sub-assemblies as possible and thus reducing the number of first-level constraints, hoping to have a real difference in terms of opening time. But nothing, no visible difference :/
My questions are as follows :
Is the fact that SW does not recalculate the sublevel stresses valid only after the 1st opening of the assembly ? If not, do you need a newer version of SW for it to work?!
Do you have any tips/tricks to improve the performance of SolidWorks for assemblies?
I don't answer your question directly but I can tell you that it is especially in the 2019 and a little also in the following ones that they have made great progress
watch this video between 4:01 and 4:22 you will see the difference between the 2018 and the 2019 https://www.javelin-tech.com/blog/fr/tag/solidworks-2019/
This may partly answer your question should you opt for a version higher than the 2018.
In solved mode, not sure that it is really noticeable effectively because it opens everything up and rebuilds everything. (SW2020 for me)
As for the light mode, for my part, I don't like at all the time you save when opening, I find that it is lost 15 times when modifying any part in a sub-assembly... And with the way we work, that's still the case.
Otherwise for the Windows architecture (limit the number of folders) not sure that it changes much either, we had done tests with Visiative a few years ago and can import in flat folder or with lots of subfolders scattered, it didn't change anything the only modification that had significantly improved the speed of opening had been made on file storage and by on the way or the architecture of our files. (which according to Visiative was of rather good quality)
On the other hand It would be better to switch to the sp5 version for SW2018 (if you have access to it of course)
For our part, big, big assembly for implementations with several machines. The main assembly of several machines with sub-backrest sometimes contains more than 60,000 parts (120,000 for the largest to date) and indeed to modify something in the assembly it is not always fast but it works. (as for the MEP it's even slower)
For opening times, our assembly of 60,000 pieces solved 15 to 20 minutes. We have allocated an additional PC for the 10 designers in order to be able to work on our layouts in hidden time and not remain stuck waiting for a reconstruction or opening.
@Zozo_mpthe tests had been done under SW2018 since then they have transformed the assembly into SW2020 and the opening time is the same on this small assembly of about 5000 parts. (30s on SSD without network and 47s with network depending on its occupancy)
From experience, the only real point of improvement is the network and storage, unless you have a very very good architecture!
On the other hand, another point of improvement that comes back to me is on the model files (assembly parts and MEP), you have to look if they are not from one or more old versions of SW, especially on the assembly models.
For us SW2004, 206,2008,2012,2014,2016,2018 and 2020.
We went back to Visiative's advice on the model file of the 2020 version re-modified in our way and since then the assemblies and MEP are much faster in my opinion.
In fact, the purpose of reducing the number of folders is not so much to increase the speed of opening as to avoid potential errors, which can occur when the path of a file contains more than 255 characters.
There is a way to remove the 255-character limitation on Windows 10. It remains to be seen if Solidworks takes this into account or if it has its own limitation.
Solidworks now contains tools to analyze the calculation time of an assembly / drawing (TOOLS/Evaluate/performance evaluation and Visualization of the assembly with the number of total graphic triangles, opening times and reconstruction times)
This kind of feedback sometimes makes it possible to realize that the problem comes from an overly detailed screws (spokes, chamfers...) or imported commercial parts that present greedy and useless details (thank you suppliers who 3D engrave their logos on their downloadable files....). It's the kind of 'detail' that can bring any machine to its knees if the component is repeated hundreds of times in the assembly...
On MEPs, pay attention to the type of hatching and their scale depending on the materials (you need a low scale (not 32 but 1 or 2 max) and simple hatching (steel type rather than "houndstooth"): since a fairly recent update, SW is buggy and handles complicated hatching very badly (a lot of lines) (NB can be corrected since but the bug exists in V2020).
The use of sub-assembly makes life easier for the user (fewer constraints to manage at the first level, fewer worries about red constraints because of hyperstatism, less waiting time if you move a part that is already constrained). Logically it should not change the opening time too much. At best, it will limit the time it takes to recalculate the assembly after opening (if we are in resolved mode).
