Optimizing Your Workstation
If you are working on large assemblies in excess of 2,000 parts (especially if your parts are very detailed), you will need a workstation to meet the demands that SOLIDWORKS will place on your CPU, GPU, RAM, and Hard drive.
To get started, take a look at this list of hardware recommendations from basic to advanced workstations for SOLIDWORKS.
Make sure you are using a SOLIDWORKS certified graphics card and driver. You may have a certified graphics card but if your driver isn’t tested and certified by SOLIDWORKS it can dramatically affect performance. For this step, you can check and update your GPU driver here, SOLIDWORKS RX Diagnostic.
Large Assembly/Drawing Performance
Now that your system is optimized for SOLIDWORKS, let’s take a look at some things you can do to make your large assemblies and drawings perform better.
Evaluate Your Large Assembly.
SOLIDWORKS has a tool called performance evaluation that comes in handy for analyzing your large assemblies or drawings and can lead you to some ways to improve their performance. Check out this link which covers all the aspects of this tool.
Unnecessary detail in the part models of your assembly can also impact performance. A good practice to follow is to have simplified configurations of highly detailed parts that are only needed for placement in your assemblies. Features such as text, patterns, fillets, drafts, and thread can be suppressed in the simplified configuration. Every unnecessary face that SOLIDWORKS has to calculate just adds to the problem.
- You can use the Performance Evaluation Tool on your parts to see which features are taking the most time to rebuild. Suppress any features in the simplified configuration (that won’t affect its fit, form, or function) to be used in your assemblies.
Cache Files Locally.
Having all the referenced files cached to your local hard drive and placed in one folder can improve speed as well. Files coming from network drives tend to take longer to load and it can slow down performance. If you are working from project folders where others have access, once the assembly is finalized and no one else needs to make changes, cache it locally to make the drawing.
Don’t Load All Sheets.
One thing that you could do to improve performance is select only certain sheets to load. In large assembly drawings many times the first few pages contain views of the whole assembly, and the trailing pages are for detailing individual parts or sub-assemblies. You can load just the detail pages and leave the other ones as quick view. This can save a lot of processing power so that it doesn’t have to load every component.
- To do this select, or highlight, the drawing in the open dialog box. It will then allow you to choose which sheets to load.
Use Lightweight Components, or Large Assembly Mode.
- Lightweight Components have only a subset of their model data loaded into memory. The remaining model data is loaded on an as-needed basis. Assemblies with lightweight components rebuild faster because less data is evaluated. You can manually set single components, subassemblies, or entire assemblies to lightweight mode, or automatically load components lightweight as part of Large Assembly Mode.
- Large Assembly Mode is a collection of system settings that improves the performance of assemblies. You can turn on Large Assembly Mode at any time, or you can set a threshold for the number of components, and have Large Assembly Mode turn on automatically when that threshold is reached. Large Assembly Mode usually includes using lightweight components.
To have Large Assembly Mode or Lightwieght Components automatically turned on go to Tools, Options, System Options, Assemblies, and check each box.
SpeedPak creates a simplified configuration of an assembly without losing references. If you work with very large and complex assemblies, using a SpeedPak configuration can significantly improve performance while working in the assembly and its drawing.
When you dimension SpeedPak configurations in drawings, you can only dimension to edges included in the SpeedPak, which are shown in black. Edges not included in the SpeedPak are shown in gray. Learn how to create a SpeedPak here.
Adjust Image Quality Settings.
- Shaded and Draft Quality HLR/HLV resolution controls the tessellation of curved surfaces for shaded rendering output. A higher resolution setting results in slower model rebuilding but more accurate curves.
The option to “Apply to all reference documents” is available for assemblies only. This applies the settings to all the part documents referenced by the active document.
- Wireframe and High-quality HLR/HLV resolution control the image quality of model edges in drawings. A higher resolution setting results in a slower screen redraw but a higher display quality.
To change these settings go to Tools, Options, Document Properties, Image Quality.Note: For better performance, while still maintaining a good display output, set the slider somewhere in the middle of the bar.
I would love to hear back from you once you have tried out one or more of the above suggestions. Let me know which of them worked best in your case to help improve performance for your design project.