Do you have one or more miracle tricks to optimize the performance of Solidworks? Because indeed we manage large assemblies so light modes, complex assembly, low level of detail... but we spend a lot of time waiting in front of the PC (at the opening, at the reconstruction, at the recording...) I think that our network must have nothing to do with it. as well as the status of certain assemblies with over-detailed files from external suppliers or to imported files.
Do you know this setting, what do you think?youComputer\HKEY_LOCAL_MACHINE\SOFTWARE\Microsoft\Windows NT\CurrentVersion\Windows GDIProcessHandleQuota set it to 20000
Do you have an opinion on the letter K at the end of the processor reference?
To check if it comes from the network you take a fairly large assembly, and you copy it entirely locally. If the opening time is x2 or more = network not great. If x1.2 to 1.5 = correct network. Several years ago, I had a long fight with the IT department, we had an opening time of x7... Following the visit of a network expert from Visiativ we now have an opening time of about 1.2-1.3. For complex assemblies, I find that this is worse than solved assemblies (faster to open but very slow with each reconstruction (so -Solved systematically) The opening time (in resolved) is certainly a bit longer but we gain a lot later for the modifications. For ideas, an assembly of + 50,000 parts can be opened in 10 minutes (with a much less powerful PC of + 8 years!) and a library with too many imports, not optimized as well. But the biggest win for us was the optimization of the network.
Edit: The letter K indicates the possibility of overclocking the processor. For the unknown parameter (for me) Edit 2: The high frequency of the processor is to be greatly preferred compared to the number of cores that SW uses very little. For me Intel Xeon at 3.6 Ghz on my old bouzin:
Hello; I agree with @sbadenis , the " Light " modes are not really interesting in terms of resource consumption compared to the " Resolved " mode. By the way, if you don't work on the assembly in question and you just want to " show " it to someone, I advise you to use Edrawing instead.
The points on which the impact has been significant on our assemblies at our company have been:
better management of antivirus (limit the scanning of the comings and goings of local files/servers and vice-versa)... if possible on all *.sld files *
Removal of Solidworks automatic backup options. (replaced by a warning after 20min).
all our templates are up to date with the Solidworks version used (document templates AND all our Solidworks files). …
Hi @Rems51 Simple: if Solidworks offers you to save it in the new version, it is because it was not already converted.
We are working on small assemblies but we have a PDM: the network is therefore much less useful since we work mainly locally. It must help a little on loading times (but the local view must be on a good SSD and not an old HDD in IDE...).
To have a few files donated by suppliers, my advice would be to do systematic analysis of all external files and simplify them (especially if they are files that are likely to be reused regularly on your designs). Casting parts with thousands of small leaves for example: if we repeat this kind of file 10x in our simple assemblies we end up with crazy latencies.
If you use BeneInox (and probably the same with others): hunt for their material extrusions with logo: the complexity of the part goes from 1 to 20 or 50 because of this kind of details (totally useless and which don't even exist in real life on the parts):
For the version of the template files, I use VersionHistory from the MyCadTools tools:
There is also a macro (not found) or a manual method with an editor it seems to me but not found either! And ideally, you shouldn't transform the old models by saving to the new version but start from the model provided by Sw and modify it to make it the new default model, which is longer but more efficient with much less bugs and latency.
From experience, working within a network is not viable. Problems come from this one. It doesn't matter how good it is. In addition 1 cartoonist ok, several this poses a problem. Antivirus, the IT underlay of companies or IT departments, are the few cases among others that pose a problem.
The only viable method is by PLM, Vault or PDM, it doesn't matter. Indeed, it allows you to extract the models you need locally. And update your cache of non-extracted parts locally. You can disconnect from your network or not, without any problem.
This does not solve everything, but the modeling is also a guarantee of the speed of your SolidWorks. Remember, it's the updates that slow down your PC. Constraints in assemblies, configurations (especially in assemblies). The simplicity of a design is to be preferred.
I forgot about a proper PC with SolidWorks, not a standard PC that your company sells you as a CAD PC
To find out the version of the files, it is also possible to add the column " Last SW recording with " in the file explorer:
To complete the remarks of @FRED78 , on the assemblies:
try to make sure that you have as many degrees of freedom as possible on your constraints in the head assemblies (even if it means " fixing " everything).
Avoid the use of flexible components as much as possible.
Don't hesitate to make sub-assemblies... and to paraphrase @froussel , yes suppliers (like Bene inox) are annoying with their logos, we sometimes spend hours removing them but it's worth it in use...
Also remember to regularly delete the content of your " Temporary " directories, the best is to do it by hand, but it is also possible to go through SolidworksRx (included in the Solidworks installation), and restart Solidworks regularly. As you are a mobile phone user, check if the " quick start" option is activated on your computer (if so, then I advise you to remove it)... Also make sure to turn off your PC from time to time (laptop users tend to never do this...)
I know it's more delicate with a laptop, but you should also favor the high or optimal power mode, at least when you are on the mains, rather than the normal mode, or worse the power saving mode. The CPU will run at full capacity instead of going back and forth between a slow state and a fast state.
Hello @Rems51 ! Like you, we have very large assemblies and significant slowness! I push the rework of some assemblies which allows you to see the part / the function that poses pb for example. Rework the steps as well and remove as much as possible unnecessary details. Sometimes the swap file is badly sized, but some of the community are more specialists than me on the subject! Otherwise disable unnecessary add-ins, real view or instant 3D. Good luck!
For WWTPs to break ties The parts I remodeled so badly designed with doubled or tripled functions, simplified the design. The result is clear: the weight is divided by 2 or 3. The assemblies I don't talk about it's crazy, we get there by being rigorous, removing redundant constraints (parallelism, etc) we arrive at an impressive slimming cure.
@Sylk, I agree with you on the optimization of the parameters. But when we do CAD, on SolidWorks or on large assemblies, we size the stations
A removed state of features and constraints reduces rebuild, but does it reduce load times?
From memory, when I put a text logo in a deleted state (without completely removing it from the mode), everything was faster. Or was it just an impression?
It seems to me that yes during the recording the assembly weighs less, but it is not necessarily faster. SW rebuilds when opening the configurations, but you can tell it not to. At one time or another, the elements you design weigh heavier and heavier when opened.
The ideal is to delete before and re-export to re-import clean (not always easy). Or better to redraw with simple functions when possible. Otherwise, another point is to lower the quality of the image for recurring objects (screws, nuts...) And also that of the models if too high. This had greatly contributed to the reduction of our problems on large assemblies. Edit: @sylk the part is heavier (longer network time, on the other hand graphically faster to load (minus detail)
Hello Get Version History Example (VBA) - 2024 - SOLIDWORKS Design Help This macro lists all successive versions of the template used in a file. For the rest, I also recommend being in performance mode in terms of power options so that the station never goes into low clock frequencies (I had a bug on my computer that made the station not exceed 1Ghz it was hell on SW). Another thing, if you ever have electronic boards from software exports like Altium, remove as many components as possible and check that the electronics engineers have not downloaded models that contain for example all the winding for a motor driver (it greatly weighs down the SW calculation when displaying even if the element is not visible). Like the others, deactivating auto saves for years. As far as CPU or RAM usage is concerned, Windows displays an average of all active cores (hence a " misleading" display), for RAM at home, we were flirting with 32GB with large assemblies (don't forget that W11 pumps a maximum of base already) since the switch to 64GB no problems with limited resources in some cases.
Another thing that hasn't been mentioned so far is the use of the blocking bar. Putting it at the bottom will allow SW to never rebuild the part (small padlocks on the functions).
Wow! Be careful with the blocking bar, it blocks everything (no more updates possible. On a part or when you are working. After that, she gets out. Again on a piece ok, applied on the fly or on a set of parts . Following the unconstrained sketch bug on the skeletons integrated in a room, we had been offered it, at the time I found the trick interesting, after unlocking 100 parts because the updates were not done... Lastuche seemed less good to me. I prefer to wait a few minutes at the opening.
I was thinking of another trick to relieve the openings or updates of your big assemblies, have you tried to create a lighter configuration by putting screws and other in deletion? And see if when switching to the other (complete) configuration it is not faster.
On the drawings, when I work on heavy shots, I hide the unnecessary views.
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to me.