Improving Performance - VTAstrobotics/Documentation GitHub Wiki
The two computer things that SOLIDWORKS uses the most are RAM and your graphics card. Generally RAM is used for understanding what the file is (rebuilding, calculating mates, finding references) while graphics is used for showing you what the part looks like calculating lighting stuff and drawing the edges of models.By far the thing that will slow loading files and cause crashes the most is RAM usage. Fortunately this is the easier usage to cut down on significantly.
Not a CS or CE
I'm a MechE. I don't know how computers work. This could all be wildly inaccurate, but the following tips do work.For an example here is the 2022-2023 chassis before and after using these tricks.
Before: (6+ min open time)
After: (4 second open time)
These images use the assembly visualization function in SOLIDWORKS and show the relative rebuild time not the open time as we will see there are easy ways to reduce open time. Rebuild time is the best indicator of how much a file will slow you down while working with it.
note that the two visualizations are relative to themselves not each other. The longest rebuild time before is 173 seconds and after is 15 seconds
Assembly visualization can be used to view lots of properties like mass.
Lightweight mode is a very easy way to speed up loading big assemblies. Lightweight mode changes how SOLIDWORKS loads component parts and assemblies. Subassemblies loaded this way don't load their components and parts don't load their features. Taking components out of light weight mode for measuring, mating, or editing is as easy as clicking on them or opening their drop down in the feature tree.
The best way to open things in lightweight mode is to change the large assembly settings. Set the lightweight cutoff based on your computer performance. For reference each subsystem will be about 100 components.
You can also specify the mode in which you want to open an assembly in the open dialogue.
Reducing the number of mates SOLIDWORKS has to solve in an assembly is a good way to improve performance. The two best ways to do this are subassemblies and lock rotation. Using subassemblies reduces the number of mates SOLIDWORKS has to solve in the top level assembly.
Lock Rotation:
When making a concentric mate you can check the "lock rotation" option. This locks the current rotation of the faces relative to each other. If the parts aren't currently in the correct orientation you can us a parallel mate to alight them then delete that mate and change the the concentric mate to lock rotation.
Locked rotation concentric mates show up with a filled in middle and rotation lock can be applied by right clicking
Don't remove mates at the expense of functionality or leave assemblies under defined. Under defined assemblies are worse for performance than adding more mates to fully define them. (see Configurations for how to make movable and fully defined assemblies)
Parts with lots of features can be simplified by saving them as Parasolids then saving those Parasolids back to parts. This creates what I call a PARA file (not a Parasolid the actual file type is still .prt).
Original: (179 second rebuild time)
PARA: (.13 second rebuild time)
As you can see this improves the RAM performance of the part although it does not improve the graphics performance as SOLIDWORKS still has to draw all the edges the same. In doing this you loose the ability to change the features that created the model. Always keep the original model! When doing this always use an index number (see File Naming) and include "PARA" in the description. The new PARA file is not linked to the original file so if you make changes to the original you need to repeat the process to update the PARA file. You can also make new features in the PARA file just like any part file.
Save as dialogue:
