Hi Guys,
I do have an assembly (20,445 KB) which was given by the client and, it has a lot of component inside. Were when I open it in Solidworks prompts a warning saying that, due to so many components in the assembly It may affect the performance.
How do I reduce the file size without affecting the scale of the components inside.
Hi Dave,
Thank you for the quick response to my query.
HP Z440 Workstation
16GB RAM
NVIDIA Quadro K2200
Your hardware is fine, you just need to learn some techniques for working with larger assemblies. There's a whole lot you can do here but the most simple is learning the proper meanings of hidden, supressed and lightweight. Then after that start reading about speedpak: https://hawkridgesys.com/blog/solidworks-improving-assembly-performance-speedpak
Google will help a lot with this once you know the terms to look for.
Also I should have linked to the swx page on this first:
The first thing I'd do is to open in Large Design Review and look at assembly. Is there something you can suppress that you don't really need when opening? That'll help a little. If you can update parts in the assembly that might be graphically intensive, I'd look at doing that too.
Steve C
20MB doesn't seem to big:) in our standards:)
Also please check on the graphics settings:
and not just in the assembly file but parts also.
you could to it through assembly by assembly visualization:
A very good point, 20Mb really isn't that big in the grand scheme of things. Graphics intensity or just one particularly intensive model is possibly the root cause rather than the absolute file size.
The top one of these assemblies opened in 80 seconds (see below). Does the open stats box give any clues as to what may be slowing down the assembly in question?
few bigger one from us:)
that first one is faulty as every time it was saved was growing in size:)
There are two points I'd suggest looking at, first fasteners nuts bolts washers o-rings do they have too much detail like threads, do you really need them? Then if it was a file from somewhere else like a .step, they could have modeled using things solidworks cant do like zero thickness geom or bad fillets. You can run import diagnostics on those things but bring a few cups of coffee. Those are the two performance killers I find often.
Hi guys,
Good day to all. :-)
I really appreciate the feedback and suggestions I am getting here. I would give a try all of it. I am not too sure on which 3D software tool the client uses to create the assembly as this is what I am seeing in the assembly "Surface Bodies (2572)". When I open it roughly it took around 10 secs. The slowdown I am experiencing was when I do insert this into another assembly. When I do rotate or zoom or rebuild etc...
Oh dear, I completely understand the slowdown now. I could be wrong but I have a theory that solidworks performs better with solid bodies rather than surfaces.
I don't have much experience with imported (PLC's?) but I can tell you I would have a little of kittens if I opened a file that had 2500 surface bodies.
A few questions: how do you plan to interact with this model? is it simple like you only need to mount it and have a stay out area or do you need to be much more involved? The goal here is brute force removal of a significant amount of surface bodies or making a speed pack configuration. Speed pack will make the file effectively weightless in another assembly.
In the assembly that contains this part, have you tried changing the component display to shaded (no edges)?
Can you ask your customer for a Parasolid (x_t) or binary (x_b)? Either would import better than a .step or especially IGS and you make be able to import diagnostics repair the assembly but that is a huge time sink. Assuming you got 250 solid bodies that could take a day or two to repair for solidworks. Warning, I would not recommend running Import Diagnostics on the part shown, it would likely hang your computer for 5 or so hours.
I assume this was an IGS file, have you fiddled around with import options to see if you can extract a better result?
Hi Justine,
This assembly will serve as a guide to the machine that we are designing, mechanically and electrically. There will be no direct interaction rather than just a guide.
I did change few setting's following the suggestions that were shared on the above feedback's. Now, it's faster than the previous attempts I did on working on my designs. And if I do not need that assembly I hide it. :-)
I would like to thank's all who had given feedback's. Salute to your unselfish sharing of knowledge.
If there are any hidden parts in the assembly you can select "Do not load hidden components" from the File > Open window.
You could also work in Large Assembly Mode or Large Design Review depending on what you need to do with the assembly.
Another option may be to open the assembly, suppress the parts you don't need active all the time and then save again, so the next time you open it there will be less to load.
Finally, a hardware upgrade may be in order - what are your computer specs?