Set Up CAD to Work Faster

A less then pleasant aspect of working with a resource-hungry application such as CAD is waiting on the app to complete a task. Although the waiting can never be completely eliminated, especially with large, complex assemblies and assembly drawings, a bit of tweaking can significantly improve performance.

The first thing that needs to be defined is expectations. That 2 GB assembly is not likely to perform blazingly fast, unless you have an endless amount of money to spend. On the other hand, don’t expect your 4-year-old system with 8 GB of RAM and an obsolete video card to perform well, even with relatively small assemblies. Tempering your expectations to accommodate a balance of performance and budget is, for most of us, a reality that can’t be avoided.

In this article, we will look at system settings and SOLIDWORKS settings to increase SOLIDWORKS performance. Any article about performance must make mention of hardware, so I will provide an overview of the four hardware components that have a very direct impact on performance.


The CPU, for the most part, is going to be the workhorse of your SOLIDWORKS system. Likely this is where you want to spend your money. Although most SOLIDWORKS applications rarely use more then one core, add-ins such as PhotoView 360 and Simulation can take advantage of up to eight cores. When choosing the number of cores, you should also consider other applications that will be running on your system in conjunction with SOLIDWORKS. Can they run on additional cores that SOLIDWORKS is not accessing?

Because the SOLIDWORKScore does not benefit significantly and/or directly from multicores, overclocking can provide better performance gains. Care must be taken, as overclocking can cause your system to overheat, which in turn can cause serious damage to your system. If you’re not familiar with overclocking, you should avoid setting this or have an expert do this for you. Better still, some computer vendors sell systems that are overclocked and these systems come with full warranties.


RAM or random access memory is the location where the data you are working on is temporarily stored — and the more the better. Data is stored and retrieved from RAM many times faster then it can be accessed from a hard drive, including modern SSDs (solid-state drives).

When you start your computer, the operating system is loaded into RAM. Any application that you launch will try to load into RAM, as will any files you open. When you run out of RAM, apps or files that cannot be loaded into RAM will be loaded in a temporary folder on your hard drive. Hard drives are much slower then RAM. Any files loaded to this temporary file will suffer from decreased performance and can lead to instability. If your RAM usage is consistently above 75 percent, you can expect poorer performance and more crashing.

Hard Drive

An SSD is much faster then a HDD (hard disk drive). If you can’t afford a large SSD drive to accommodate all your data files, then get one at least for the operating system and all your installed programs.

GPU (Graphics Processing Unit aka Video Card)

Choosing an adequate video card can be more difficult then choosing other hardware components. If the level of detail in parts is low and your assemblies are small, then a middle-of-the-road card is likely sufficient. But if your components are highly detailed and/or your assemblies are large, a higher end card should be considered. Many system and GPU manufacturers provide guides for choosing the appropriate GPU. Regardless of how much you plan to spend on a card, be sure you choose a certified card.


SOLIDWORKS provides a tool to help validate the hardware on your system and compare it to similar systems.

The Diagnostics tab will show whether your GPU and GPU driver are certified and provides a link to access the certified drivers.

GPU information in SOLIDWORKS Rx —Diagnostics tab.

The Diagnostics tab also provides information about system memory, including a general statement on how large of an assembly can be opened with the amount of system RAM.

Diagnostics tab displaying system resources.

The SOLIDWORKS Rx Benchmark tab compares your computer to those of other SOLIDWORKS users.

Running the Benchmark test.

Now that we have reviewed hardware, lets look at some Window settings that can be tweaked to increase performance.

Windows Visual Effects

Windows Visual Effects are just that, visual effects. Although they can enhance the appearance of Windows, they can also reduce performance. Many of these can be disabled without reducing the usability of Windows or SOLIDWORKS.

Visual Effects can be accessed through the Windows Control Panel by selecting System and Security>System>System Properties> Performance Options.

Accessing Visual Effects from Windows Control Panel.

Visual Effects can also be accessed by pressing Win-R on your keyboard, to start the Windows Run command, and entering “SystemPropertiesPerformance.exe.”

Accessing Visual Effects from Windows Run.

By default, Visual Effects are set to have Windows decide which ones to use based on your system. Disabling some of these can increase performance. Below are some common settings that strike a balance between performance and the Windows “experience.”

Common Visual Effects settings.

Some settings can also be controlled from the Microsoft Ease of Access Center by selecting “Turn off all unnecessary animations (when possible).” Make computer easier to see. And make it easier to focus on tasks.

Use the computer display.

Make the computer easier to see.

Make it easier to focus on tasks.

You can also change these settings from the Windows Registry. The settings that need to be made can be found online. Setting these through the registry allows you to copy these settings to other computers by copying the registry settings.


SOLIDWORKS offers settings in Tools>Options>System Options that can help with performance. The first group of options we will look at is in the General tab.


These options offer minor performance gains. If you find yourself having to change these settings in order to make SOLIDWORKS workable, you should consider a more capable system.

Also in the General tab, there are the following, which can have a greater impact on performance improvements:

  • Enable FeatureXpert attempts to repairs errors automatically so components load successfully. This option may impact performance, but it can also capture and repair errors that would have to be fixed manually. Although we are speaking about rebuild errors, it should be noted that they can have a significant effect on performance. Rebuild errors should be addresses as they occur.
  • Enable Freeze bar can be used to exclude features from rebuilds, which in turn can improve performance.

When rebuild errors occur, SOLIDWORKS:

  • Stops the rebuild, allowing the user to correct the errors;
  • Prompts the user to stop and rebuild so the error can be addressed or
  • Continues the rebuild without prompting the user.

As noted earlier, rebuild errors can significantly impact performance. A good option is to have SOLIDWORKS prompt you. This allows you to decide whether to fix the error or continue on to the next error.

Drawings can tax a GPU as well as consume RAM. In Drawings>Performance under System Options, these options can be disabled to improve performance.

  • Unselecting “Show contents while dragging drawing view” will reduce the load on the GPU by only showing the view bounding box when a view is dragged.
  • “Allow auto-update when opening drawings” updates the drawing as it is opened. Unselecting this option will make the drawing open faster, but a subsequent rebuild will be required to update the drawing.
  • Unselecting “Save tessellated data for drawings with shaded and draft quality views” will reduce the file size by not saving tessellated data in shaded and draft-quality views. A word of caution: This may prevent drawings from being viewed in eDrawings.

Performance options for drawings.

In Drawings>Display Style, you can select “Draft quality” to increase performance when working with complex drawing views, such as those of large assemblies. On the negative side, this option can degrade print quality and make it difficult to select drawing edges.

Draft quality option in System Options.

“Assembly transparency in Tools>Options>System Options>Assembly transparency for in context edit” under Display, can have a significant impact on performance. This option only affects the components that are not being edited. Setting the transparency to opaque will offer the best performance.

Setting the “Assembly transparency for in context edit” option.

As the name implies, the Performance tab is where many of SOLIDWORKS performance settings can be found.

  • “Verification on rebuild” offers another level of error checking. Turning this option off can increase performance, but the extra level of checking can catch errors in complex models that otherwise may not appear until later in the design process. This can lead to time-consuming edits in order to address these errors.
  • Transparency is normally set to low quality and results in a display that is similar to looking through a mesh. When a component is not being moved, the display does not need to refresh, so less resources are being used. Selecting “High quality for normal view mode” allows a cleaner display of transparent parts, while minimizing resource use. Low-quality transparency will offer better performance, but not using transparency at all will increase performance even more.
  • Keeping “Curvature generation” at the lowest level that you can work with will offer the best performance. This level can be tweaked until a happy medium is reached.
  • Lightweight components load the bare-minimum model information required when loading an assembly. Because there is no real downside to loading components lightweight, you should always select the “Automatically load components lightweight” option.
  • “Always resolve subassemblies” will resolve the assembly while setting the subassemblies components to lightweight. This may be a happy compromise for those who want to minimize delays while editing subassemblies.
  • “Check out-of-date lightweight components” will check if assembly components have changed since the assembly was last opened. The options are:
    • “Don’t Check” will not check if components have changed. This offers the best performance, but changes to the components will not be reflected in the assembly.
    • “Indicate” will label which components have changed with this icon  in the FeatureManager. Although this option uses more resources then “Don’t Check”, it makes it apparent which components have changed.
    • “Always Resolve” will load all components that have changed.
  • Turning off “Mate animation speed” can also increase performance, but seeing how components come together can be useful in confirming that the right mates are added.

Performance options.

Other performance options include the following:

  • “Purge cached configuration data” will reduce the file size and can reduce open times, but loading configurations once the component is open will be slower.
  • “Update mass properties while saving document” can reduce open times since the mass properties do not need to be calculated the next time the file is opened unless the component has changed. However, save times may be longer.
  • “Use software OpenGL” should only be used if the system has a GPU that is not certified or if you are troubleshooting graphics issues.
  • “No preview during open (faster)” can increase performance when opening a document by removing the graphical preview.

Additional Performance options.

In the Assemblies tab of System options, the following options can be changed, to increase performance:

  • Large AssemblyMode can be triggered when an assembly exceeds a user-defined number of components. The following can be disabled when an assembly is loaded in Large Assembly Mode:
    • If you are diligent at saving regularly, checking “Do not save auto recover info” will eliminate performance delays, while components are automatically saved. Auto recover is set in Tools>Options>System Options Backup/Recover.
    • Rebuilds take time and system resources, enabling “Do not rebuild when switching to assembly window” will prevent these rebuilds, but any changes will not be shown until a manual rebuild is performed.
    • Items in the View menu may not be required when working in an assembly. Selecting “Hide all planes, axes, sketches, curves, annotations, etc.” will turn these off. Note: Some of these may be required when working with tools such as SOLIDWORKS Routing.
    • Edges in shaded mode may not be needed for most assembly operations, but for some, such as mating, they may be required. Also, it can be difficult to distinguish between components when edges are turned off.
    • “Do not preview hidden components” will turn off the preview when you select a component in the FeatureManager.
    • As mention earlier, “Disable verification on rebuild” can increase performance, but it reduces the level of error checking.
    • “Optimize image quality for better performance” will downgrade image quality to increase performance.
    • “Suspend automatic rebuild” will defer the automatic rebuild of assembly-level features. In order to show changes that affect these features, a manual rebuild will be required. The rebuild icon will appear next to these features until they are rebuilt.
  • Large Design Review will open large assemblies quickly and still allow for some capabilities such as Measure, Hide/Show, Section and Create Walkthroughs. As the name implies, this is a review tool only.
  • When working with envelopes, these components can be automatically loaded as lightweight.

Assembly options.

Additional system options that can impact performance include:

  • External References>Load referenced documents: Loading external references takes time and consumes resources. Not loading these documents may increase performance, but features dependent on these external references will not update. A good choice would be the “Prompt” option.

Load referenced documents.

The “Load documents in memory only” option prevents external references from opening in separate windows.

  • Deselecting the FeatureManager options “Scroll selected item into view”, “Dynamic highlight” and “Use transparent flyout FeatureManager tree in parts/assemblies” can improve performance by reducing the load on the systems GPU.

FeatureManager options.

  • In the View tab, deselecting “Zoom to fit when changing to standard views” and lowering or turning off transitions can also increase performance.

View Options

Additional Performance Considerations

The display settings in the heads-up display also contain some options that can affect performance.

Although “RealView Graphics” and “Shadows in Shaded Mode” can add to the visual impact of a component, these options consume GPU resources and are not normally needed when creating and editing components.

Where SOLIDWORKS documents are saved can also impact performance. Networks will almost always be slower then a hard drive. If a centralized location of SOLIDWORKS files is required, then a data management solution, such as SOLIDWORKS PDM, should be considered. These data management solutions generally store files centrally but also cache files to users’ computers.

We have looked at many options and settings in this article. Which ones make meaningful performance gains depends on your system, your workflow and the types of components you work with. To experience the best performance, choose a system that meets your needs and budget. Then tweak your system and SOLIDWORKS so that you maximize performance, without overly sacrificing usability.


Joe Medeiros is a senior applications engineer at Javelin Technologies, a SOLIDWORKS reseller servicing customers throughout Canada. He has been involved with SOLIDWORKS since 1996. An award-winning blogger, he regularly writes about SOLIDWORKS products.

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