Slow drawing in SOLIDWORKS? Here are 12 possible reasons

What was the last time that you worked on a SOLIDWORKS file that was slooooow? Probably right now.

But you can make them faster. Sometimes you can make the load time go from tens of minutes to a few seconds!

Here’s how to do that.

Maurice Moss still works with SOLIDWORKS 2012 SP0

Is this you?

Table of contents

  1. Related blog posts
  2. Measure the performance of a slow drawing first
  3. File open settings
    1. File open mode
    2. Select sheets to open
    3. Detailing mode, new in SOLIDWORKS 2020
    4. Disable preview while loading
  4. Model issues
    1. Complex features
    2. Imported parts
    3. Corrupt templates
  5. Display style influences
    1. Draft quality vs high quality
    2. Turn off edges
  6. Hardware issues
    1. PC power settings (2x faster!)
    2. Processor speed
    3. Network drives
    4. Driver issues
  7. Slow drawing be gone!
  8. An ebook about SOLIDWORKS performance

2: Measure the performance of a slow drawing first

The Performance Evaluation tool is available for all models types, even for drawings.

Javelin wrote a nice blog post about it. The next few images are taken from that post.

I have also learned a lot from their Elite Problem Hunter Alin Vargatu, who is the Canadian VAR’s large assembly specialist.

Performance Evaluation

The tool generates a report like this. A different kind of report gets generated for parts and assemblies.

Performance Evaluation Report

This should give you a few pointers to find which sheet, feature or view is the main reason for your PC’s headache.

3: File open settings

3a: File open mode

You have probably seen the open window a gazillion times. But do you use the extra options to the fullest?

These are the available options for drawings:

drawing open modes

  1. Mode:
    • These are ordered from fastest (Quick View) to slowest (Resolved).
    • Quick View is a read-only mode that is blazingly fast because it only read the drawing file itself, not the referenced files.
    • Lightweight loads about half of all data for components and it loads about 50% faster.
    • Resolved loads everything and is the slowest (and default) mode.
  2. Select Sheets: see the next section
  3. References:
    1. Lets you edit the list of referenced files. It does not change the loading process itself.

More info on this window in the SOLIDWORKS Help here.

3b: Select sheets to open

You don’t need to load all sheets! Just hit the Select Sheets button.

drawing open modes

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.

Solidworks speed up slow drawing

3c: Detailing Mode, available from SOLIDWORKS 2020

Detailing Mode does not load the underlying part or assembly, just like a detached drawing does. Detailing mode is actually built to replace detached drawings in the long term.

SOLIDWORKS does this by saving extra data to the drawing when you are in release mode. That means saving in release mode will be a little slower (sometimes a lot slower) but you can quickly edit the drawing in Detailing Mode later.

solidworks slow drawing detailing mode

SOLIDWORKS is still actively building Detailing mode, so its capabilities grow stronger each year. Here is the official help page for detailing mode in SW2022.

What you can do: You can add all kinds of annotations: dimensions, notes, balloons and symbols. 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. These actions all require the underlying model, which isn’t loaded. The undo function also doesn’t work (yet).

Read all the details about this welcome improvement in this article by Canadian reseller Javelin.

3d: Disable preview while loading

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).

4: Model issues

4a: Complex features

When a model is overly complex, its 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. Helix features can cause major slowdowns, for example.

Secrets to SOLIDWORKS Performance

A complete guide to making your models fast by learning what makes them slow.


4b: Imported parts

SOLIDWORKS documents 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.

Then you need to fix the gaps or broken faces. Find out more in this blog post by TriMech.

Low quality solidworks drawing view

Before and after fixing imported model issues

4c: Corrupt templates

I have no idea how to determine if a corrupt template causes your poor 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 new template.

The official advice is therefore to always create fresh templates from the default templates when you switch to a new SOLIDWORKS version. It takes a little more work to copy all your settings but it will save you many headaches in the coming year.

SOLIDWORKS can create new templates for you in a few seconds.

5: Display style influences

5a: Draft quality vs high quality

You can show drawing views in draft (low) quality or high quality. I find the names misleading, because draft quality actually only shows the graphical approximation of the model, whereas high quality also adds geometrically correct lines and edges.

Draft quality only loads the information that is absolutely necessary. It’s very similar to Lightweight mode. High-quality views require all model data.

SOLIDWORKS creates drawing views in high quality by default. More info here.

5b: Turn off edges

SOLIDWORKS draws your model in two layers: graphical + parametric (see the previous section).  So displaying a model as Shaded is way faster than Shaded With Edges. When you turn on edges, the parametric model has to be loaded as well.

Solidworks speed up slow model

Not displaying edges will greatly speed up your model

6: Hardware issues

6a: PC power settings: 2x faster

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.

solidworks slow power settings

Go twice as fast by selecting High performance

You can find these settings by going to Start > Settings > search for “power” > Power and sleep settings > find a way to enable High Performance.

6b: Processor speed

When you open an assembly (and we know that drawings are secretly assemblies), the program goes through five distinct phases:

  1. Locating files (single-threaded)
  2. Loading files into memory (single-threaded)
  3. Locate each model in space / solving mates (multi-threaded)
  4. Resolving assembly and in-context features (single-threaded)
  5. Generating graphics (multi-threaded)

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.

6c: Network drives

You shouldn’t work with files from a network when you want great performance. It’s that simple.

Working with a local copy (preferably using a PDM system) is dramatically faster compared to network storage. Even a gigabit network (max 1 Gbps) doesn’t come close to the speed of local M.2 SSDs that reach over 50 Gbps.

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.

6d: Driver issues

Rogue drivers 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 and you can run SOLIDWORKS Rx to see if you are currently using a verified driver. Your VAR should also be able to help you with this.

Slow drawing be gone!

I surely hope you identified at least one culprit. Did you increase the performance by a factor of two, or ten?

An ebook about SOLIDWORKS performance

This post has been read over 100,000 times over the past years, so I know that performance is still a big issue.

That is why I have written down everything I know about SOLIDWORKS performance in a 127-page ebook. I read every article, watched every video and collected the best bits. The complete package even includes three handy cheat sheets, plus models and macros to improve performance with.

You can check it out here.

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