Large Assembly Performance (or the lack thereof…)

Solidworks has added some tools over the last few years to help with large assembly performance. There are quite a few so I wanted to also take the time to discuss their differences and when you may want to use them.

Lightweight Mode

First, is lightweight mode… Basically, this will open the assembly and all of the parts into RAM but not load the part’s feature data. This opens the assembly faster but still loads all the graphic data. When the user needs the parts features you simply right-click and set part to resolved or edit part. This will load the individual parts data into RAM. You can access Lightweight Mode in the System Options > Performance tool.

System Options - Performance

I also recommend setting the Check out-of-date lightweight components to Indicate. This will show in the tree as a red feather instead of the up-to-date blue feather. To “update” the file, simply resolve it.

Beyond Lightweight is Large Assembly Mode

This functionality in Solidworks allows the user to set a threshold and what options apply when that threshold is reached. I stress some caution with the “do not save auto recovery file” option, for obvious reasons. One that is very useful is the “turn off edges in shaded mode” option. This turns off all the little black edges on the parts. HUGE savings on your graphics card with many parts or even a few complicated castings etc.

System Options - Assemblies

Large assembly mode can also be turned on during file open and after by going to tools, Large Assembly mode, as a toggle switch to turn it on and off. The default threshold is 500 parts but you can adjust that depending on your needs based on computer/graphic card performance.


One of the most powerful, yet under-utilized tools for performance is SpeedPak.

SpeedPakSpeedPak basically allows the user to create their own customized lightweight sub-assemblies. It functions as a special derived configuration. To create a speed pak of an assembly, right-click on the configuration and click add speed pak. This dialog will appear on the left side of the screen.

The top boxes are for selecting individual faces or bodies to include in the SpeedPak. Essentially, you would select the faces of the sub-assembly that you would use when mating the assembly into place. Alternatively, you can select the “Enable Quick Include” option which allows for a slider bar to grab faces based on complexity. Use this method when your only goal is performance and not mating.

The ‘Remove ghost’ checkbox option refers to the graphic card ghost that occurs when hovering over the sub-assembly at the top level. While it is a pretty cool effect, it does take extra memory and graphics card processing.

Once the sub-assembly has been saved with a SpeedPak, you can access it by right-clicking the sub in the top level assembly and going to component properties. Then simply select the SpeedPak version.

If many of your subs have SpeedPaks, you can check the box “Use SpeedPak” on the file open dialog to reference them.

The end output is a very light assembly that shows all the detail with almost none of the math data. Great for presentations, design review, and I even work in this mode regularly on extremely large assemblies. The best part is the BOM still generates with all the parts!

Large Design Review Mode

Lastly, I wanted to touch base on 2012’s new functionality called Large Design Review Mode.

SolidWorks just introduced this new tool, and it allows a user to open extremely large assemblies with no prep work. It allows for many great features while in this mode as well.

Large Design Review

This mode is best used for presentations and reviews. One cool function unique to this tool is snapshots. You can create snapshots (saved in the display tab) that you can jump back to during presentations. This way you can quickly make bullet points for discussions without having to open a massive assembly to create views or walk-throughs. The default threshold for Large Design Review is 5,000 parts, but that can be changed as well in Tools > Options > Assemblies. You can also choose this mode during the ‘File open’ dialog.

Hopefully some or all of these tools will help you gain more performance out of your assemblies so you can design better and faster with SolidWorks!

John MacArthurJohn MacArthur
DASI Solutions

This entry was posted in Tips & Tricks. Bookmark the permalink.

Leave a Reply

Your email address will not be published.