Open SOLIDWORKS on two different machines, and it can feel like two completely different programs. It’s the same version, the same hardware, but a completely different experience.
On one system everything feels slow, unstable, inconsistent and frustrating, while on the other system everything feels fast, stable and a generally smooth experience.
Most users assume the difference is hardware, or that the software just hates them.
However, for the most part the hardware is fine, and the software does not feel hate (for the moment, but neither did Skynet).
It is with 99% certainty that I tell you the settings are the problem.
Your Settings Are Probably Working Against You
SOLIDWORKS is not a fixed environment. It is a configurable system, and its behaviour depends heavily on how it is set up. The problem is that most users never change these settings. They learn commands and workflows, but rarely question how the system itself is configured.
This means they adapt to SOLIDWORKS — instead of making SOLIDWORKS adapt to them.
The settings in SOLIDWORKS control different aspects of a model: how it is rebuilt, how it is loaded, how the sketches behave, how effectively your hardware is used and how to ensure stable models over time.
One thing I’ve learned is that small changes to your settings your templates can reduce the rebuild time, improve stability, prevent fragile model behaviour and even make large assemblies more manageable.
Where These Settings Live
SOLIDWORKS settings exist in two main places:
First, we have the System Options. These are local settings on your machine, saved in your registry. In order to successfully alter these settings, you may need to run the program as administrator.
Next there is the Document Properties, which control many aspects of your model or your drawing, and are individual from file to file.
If you want a brief introduction to these settings, please see my previous article.
Today’s article will give you the tools to navigate through the first 5 of 10 essential settings and behaviours that directly affect how SOLIDWORKS works and behaves, as well as how to use them intentionally.
1. Verification on Rebuild
Trust is good, control is better.
Found under: System Options → Performance.
What it does
Verification on Rebuild forces SOLIDWORKS to perform a deeper geometric validation every time the model rebuilds.
Normally, SOLIDWORKS prioritizes speed. It assumes that most geometry is valid and only performs basic checks during rebuild. With Verification on Rebuild enabled, SOLIDWORKS takes a more cautious and thorough approach. During the rebuild it will verify multiple things, such as:
- Are the faces valid?
- Are all the edges properly connected?
- Do the features resolve without hidden geometric errors?
It will make the rebuild slower; how much will depend on the complexity of the model, but this process will also ensure that the model is more reliable.
Why it matters
Some model errors don’t show up immediately.
A feature can sometimes rebuild without errors and seem correct but still contain invalid or instable geometry.
Often these invisible errors will later show up as errors in the feature tree and cause a general downstream rebuild problems.
Verification on Rebuild will help you catch these issues at the source of the problem, instead of trying to fix it several features later, which is a lot of work.
Use it wisely
While Verification on Rebuild is very useful when trying to figure out what is wrong with your model, it also uses a lot of power to rebuild the model (hence the “Verification” part).
In the below example, I had a fairly simple model, which without verification on rebuild took just below 1 second to rebuild.
However, after adding the checkmark the rebuild time is more than doubled.
As you can imagine, this is not a “Leave it on at all times” setting, as it will greatly increase the rebuild time of the model.
When should you use it? If your model starts to behave unpredictably and rebuild errors appear further down the tree, it is a great tool to help you when debugging your model. And that is all it is: A debugging tool that will help reveal the problems with your model. It will not help you fix them.
And it should be turned off when you’re modeling, otherwise you will experience a lagging in your performance.
Common mistake
A common mistake is leaving Verification on Rebuild enabled all the time. While it improves model reliability, it significantly increases rebuild time, especially in larger or more complex models.
This often leads users to believe that SOLIDWORKS is slow, when in reality it is doing exactly what it was told to do.
Takeaway
Verification on Rebuild is a debugging tool — not a default setting.
Use it when something feels wrong in your model, and turn it off when you return to normal modeling to maintain performance.
2. Image Quality
If looks could kill, this would kill performance.
Found under: Document Properties → Image Quality.
What it does
The official explanation is as follows (from SOLIDWORKS Help page): “Controls the tessellation of curved surfaces for shaded rendering output.”
A high setting will of course give you smoother visuals and accurate curves, but it will affect your model performance and as well as the general rebuild time.
In the below image, I have a knight from a chess game. In the left Performance Evaluation window, the image quality setting is set to 30% and the number of graphical triangles is 9,350. On the right Performance Evaluation window, the image quality is set to 100% and the number of graphical triangles has been increased to 448,650.
You will of course notice that the rebuild time difference is “only” 0.07 seconds. While that may not sound like much, imagine instead this model is a bolt, and it has been used more than 100 times in an assembly.
Always keep in mind that neither the model accuracy nor your drawings are affected by the image quality; the only difference is how you see it on your screen.
Common mistake
A common mistake is increasing Image Quality to improve model accuracy. Image Quality only affects how the model is displayed — not the actual geometry or drawing precision.
This means you can significantly reduce performance without gaining any real modeling benefit.
Takeaway
Image Quality is a visual setting — not a modeling setting. Lower it to improve performance while working, and only increase it when you need better visual representation. Most of the time, you are not limited by accuracy, you are limited by performance.
3. Large Assembly Mode
Performance is a strategy — not a reaction.
Found under: System Options → Assemblies.
What it does
Large Assembly Mode is a collection of performance settings that SOLIDWORKS automatically activates when an assembly reaches a defined size. Instead of manually adjusting multiple options, SOLIDWORKS applies a predefined strategy to improve performance.
These settings include:
- Loading components as lightweight — something we will take a closer look at in the next section.
- Reducing visual detail.
- Simplifying evaluation during rebuild.
In short, SOLIDWORKS changes how it handles your assembly when it detects that it is getting “too large.”
Why it matters
No matter how good you are at using design intent and obeying all the rules of good modeling, an assembly will start to act slow simply because of the amount of data that is being processed at once.
Without Large Assembly Mode, every component is treated the same and it is fully loaded by default. This will result in performance drop as the file increases.
When using Large Assembly Mode, SOLIDWORKS will prioritize speed over detail and leave out unnecessary calculations, which will result in more manageable large assemblies. This is especially important in real-world projects where assemblies can contain hundreds or thousands of components.
Typical symptoms of the need for Large Assembly Mode include when opening an assembly takes noticeably longer than expected, rotating the assembly starts to feel “laggy” or rebuild time increases significantly after adding just a few components.
How to use it
Go to System Options → Assemblies. Enable Use Lightweight Mode and Large Assembly Settings when number of components exceeds.
Set a starting threshold. A good starting point is 300–500 components, then adjust based on your hardware and typical assemblies. Click into Large Assembly Settings.
Review what is enabled and remove unnecessary options. Disable visual features you don’t need while working, and focus on performance-related settings.
Lastly, test the result. Open a large assembly, and compare performance before and after.
Start simple — you can always refine the setup as you learn what impacts your workflow the most.
Common mistake
A common mistake is setting the threshold too high. If Large Assembly Mode only activates at 2,000 components, you are likely to already be experiencing performance issues long before it helps you.
Takeaway
Large Assembly Mode is not about sacrificing detail — it is about controlling when detail matters. Used correctly, it allows you to work efficiently with complex assemblies instead of constantly fighting performance.
4. Lightweight Components
Detail on demand — not by default.
Found under: System Options → Performance.
What it does
Lightweight Components settings control how SOLIDWORKS loads parts into an assembly. Instead of loading the full feature definition of every component, SOLIDWORKS loads a simplified version which focuses on graphics data and positioning information. The feature tree and parametric data are only loaded when needed.
This is one of the key mechanisms behind Large Assembly Mode — but it can also be used independently.
Think of Lightweight Components as opening a “visual version” of your assembly. You can see the geometry, position components and navigate the model,
but the heavy feature data stays unloaded until you actually need it.
Why it matters
Most assemblies are not slow because of what you see, but because of what is loaded in the background. If every component is fully loaded (fully resolved), all the features are loaded and all dependencies are active. Every rebuild will become heavier.
With lightweight components, the load times are reduced and the navigation in the assembly becomes significantly smoother.
Once you move beyond the small assemblies, you will notice the difference.
How to use it
Set components to load as Lightweight instead of Resolved when opening assemblies.
Once the entire assembly is loaded, you can choose what to resolve (no longer lightweight mode).
Make sure that you only do this when it is needed.
For instance, when you want to edit a component, if you are troubleshooting a rebuild error or if you need a full model for analysis.
For everything else, keep it set to lightweight.
Recommended workflow
A practical way to work with large assemblies is:
- Open the assembly in Lightweight mode.
- Navigate, inspect and position components.
- Resolve only the parts you actively work on.
- Keep the rest lightweight.
This approach keeps performance high while still giving you full control when needed.
Common mistake
Many users immediately resolve the entire assembly out of habit.
This removes all performance benefits — and often results in slow rebuilds and laggy performance.
Takeaway
Lightweight Components are not a limitation — they are a strategy. The goal is not to load everything, but to load exactly what you need.
5. Add-ins
If you don’t use it — don’t load it.
Found under: Tools → Add-ins.
What it does
Add-ins are additional modules that extend SOLIDWORKS with extra functionality. For examples, SOLIDWORKS has add-ins for Simulation, PDM, Toolbox and Routing, among others.
Each add-in runs as part of SOLIDWORKS and loads functionality into your session. Some are only active when needed, while others load automatically at startup.
Why it matters
Most users focus on geometry and hardware when SOLIDWORKS feels slow.
But one of the most common causes is much simpler: Too many add-ins running in the background.
Each active add-in consumes memory, increases startup time, and adds overhead to your session. And the key issue is that you often don’t notice they’re there.
Over time, systems accumulate enabled add-ins — especially in shared environments — and performance gradually degrades because everything you load has a cost.
How to use it
Review your active add-ins. Go to Tools → Add-ins and look at what is currently enabled.
Disable what you don’t use. If you are not actively using an add-in, turn it off.
Be careful with Startup Add-ins. There are two columns, Active Add-ins (current session) marked with 1 on the image, and Start Up add-ins (loaded every time SOLIDWORKS opens), marked with 2 on the image.
Focus on minimizing the startup column, as this is often where you will see the biggest performance improvement.
Load on demand instead, and enable add-ins only when needed, not by default.
Common mistake
A common mistake is enabling all add-ins “just in case.” This is especially common in shared environments or after installing SOLIDWORKS, where multiple add-ins are enabled by default. Over time, this creates a heavier and slower system — even if you are not actively using those tools.
If you don’t use an add-in daily, it should not be loaded at startup. Load it when you need it — not before.
Even disabling just a few unnecessary startup add-ins can noticeably reduce startup time and improve overall responsiveness.
Takeaway
Managing add-ins is one of the easiest performance wins in SOLIDWORKS. They run silently in the background, and while each one may seem insignificant, together they can have a major impact on performance.
Control what loads at startup — and you control how SOLIDWORKS feels.
More Settings to Come
So far, we have looked at how SOLIDWORKS rebuilds your models, displays your geometry, handles large assemblies, manages add-ins, and loads data into memory. These settings alone can completely change how SOLIDWORKS feels to work in.
But performance is not just about how models are opened and handled. It is also about:
- What happens when you save.
- How your hardware is used.
- How you identify what is actually slowing you down.
Once your models are under control, the next step is making SOLIDWORKS work with you, not against you. In the second part, we will look at the settings and tools that give you control over these processes.
Stay tuned for part 2!