What was the last time that you worked on a SOLIDWORKS file that was slooooow?
Are you killing ten minutes while a slow drawing is loading right now? What a coincidence. Did you get a freshly brewed caffeinated drink already? Good.
We have made a list of things you can try to speed up your drawing performance dramatically. Sometimes load times go from tens of minutes to a few seconds!
SOLIDWORKS released a handy new tool in 2016 that’s appropriately named Performance Evaluation.
It already worked for parts and assemblies, but from then on it could analyze drawings as well.
Javelin wrote a nice blog post on the topic and the following images are taken from that post.
I have also learned a lot from their ‘Elite Problem Hunter’ Alin Vargatu, he is the Canadian VAR’s large assembly specialist.
When analyzing a drawing, it will generate a report like this. A different kind of report gets generated for parts and assemblies.
This should give you a few pointers to find which sheet, feature or view is the main reason for your PC’s headache.
You have probably seen the window below a gazillion times.
But have you ever even noticed the extra options? I only learned about those recently.
There are no fewer than six settings here that can help you speed up your work:
In case you were wondering what the References button does: it lets you edit the list of all referenced files. It does not change the loading process itself.
More info on the file open menu can be found on this page of the official SOLIDWORKS help.
Did I tell you there were six? Yeah I did. I gave the sixth one its own section because it’s such a big deal for massive drawings. Here it is:
This one is incredibly useful when you work with a complex and slow drawing with multiple sheets.
Apparently you don’t need to load them all! Awesome.
You can choose to load a single sheet or only a few of the 50 sheets that your monstrosity of a drawing has somehow turned into.
Detailing mode prevents the referenced part or assembly to be loaded, just like a detached drawing.
But detached drawings need to be saved like one first. Detailing mode is just a different way of opening a normal drawing.
What you can do: You can add all kinds of annotations: dimensions, notes, balloons etc. You can also move views and add revision tables.
What you cannot do: You cannot create drawing views, create other kinds of tables, add center lines or center marks, or select model faces. The undo function also doesn’t work (yet).
Read all the details about this welcome improvement in this article by Canadian reseller Javelin.
SOLIDWORKS always shows you a crude preview while the file loads. It sure looks nice, but it makes the loading take longer.
You can disable the preview in the SOLIDWORKS System Options > Performance > No preview during open (faster).
This is a big one for assemblies. By default, SOLIDWORKS rebuilds the assembly every time you switch between opened models. This might take minutes for huge assemblies though.
You can disable this behavior by going to System Options > Assemblies > When Large Assembly Mode is active > Suspend automatic rebuild
For more tips on assemblies, check out our blog post on Best Practices for Assemblies.
When a model is overly complex, the respective drawing will be as well. Try suppressing parts (for assemblies) or features (for parts) and see if you notice a 2x or even 10x speed improvement. Helices (yup, that’s proper spelling) can cause major slowdowns for example.
The performance of any SOLIDWORKS document can come to a grinding halt when a single imported part has troubles. I’ve heard stories where a massive assembly opened ten times faster after a single faulty imported part was suppressed.
Do you have views in a slow drawing that show up with a very low quality or parts that completely go missing in a drawing? Imported parts can cause this as well.
Find out more in this blog post by TriMech.
I have no idea how to determine if a corrupt template bogs down your drawing performance. But by now I have heard of a few occurrences where this was the case.
When upgrading SOLIDWORKS versions, most companies tend to import their old templates and save them in the new version. This however also saves all kinds of legacy crap and hidden errors into your brand spanking new template.
The official advice is therefore to use the default templates that came with the new version and manually copy all settings that you need. It takes a little more work but might save you many headaches in the coming year.
You can create new templates in a few seconds.
Drawing views are created in draft (low) quality or high quality.
Draft quality only loads the information that is absolutely necessary. High quality loads everything.
SOLIDWORKS creates drawing views in high quality by default. More info here.
SOLIDWORKS somehow has difficulty showing edges.
When I was working on a ship with thousands of beams and other parts, the model went from extremely sluggish to extremely usable when I switched the display style from Shaded With Edges to Shaded. It probably speeds up drawings as well.
Update: Since writing this, I have learned why this works. A model consists of a graphical representation plus a parametric model. When you turn off edges, only the graphical data is used. Turn on edges and the parametric model has to be loaded as well.
This was a surprising one for me. SOLIDWORKS forum user Peter Medina did a test and found out that the Windows power settings have a big influence on the speed of your model.
He was able to obtain a factor two increase in speed by changing the power setting to “High performance”. When you’re not working on a laptop, this is a no-brainer.
You can find these settings by going to Start > Control Panel >Power Options.
Many tasks in SOLIDWORKS have to be done in a well-defined sequence. When you open an assembly, the program goes through five distinct phases:
Most of these tasks can only be executed on a single core of your processor.
This means SOLIDWORKS really benefits from processors with a high clock frequency. Multicore processors are only really useful for rendering, where the task can be split up in many tiny tasks that can be executed in parallel.
So make sure your pc isn’t very busy with something else (Windows Update is notorious for slowing down your pc and hiding its activity) on every core by checking Windows Task Manager with the shortcut Ctrl-Shift-Escape.
Also, get an SSD if you haven’t already. It’s awesome. Or if you are in the market for a real CAD pc: get an overclocked (yet stable) one from Boxx.
You shouldn’t work with files from a network when you want great performance.
It’s that simple.
Create a local copy (preferably using a PDM system) and you’ll notice dramatic speed increases compared to network storage. Even gigabit network speeds (max 1 Gbps) don’t come close to the speed of local SSD’s, which go from 3 or 6 Gbps for simple SATA drives to over 10 Gbps for M.2 or PCI-e SSDs.
When you work with a PDM system, check out files that you are working on so others can work on their parts. You’ll really appreciate version control after a colleague accidentally throws away your work.
Drivers that went haywire can cause all kinds of weird behaviors. A faulty or corrupt driver can show parts that were deleted weeks ago. I have seen it happen. That’s not something that really points directly to the driver.
Unfortunately, this still is an issue that pops up semi-randomly once in a while.
SOLIDWORKS maintains a list of verified graphics card drivers, so if you suspect a driver that site is a good starting point. Your VAR should also be able to help you with this.
There you have it.
Twelve Fourteen ways to speed up your drawing, part and assembly models. I surely hope you identified at least one culprit. Did you increase the performance by a factor of two?
Twenty? Nice 😄