Assembly Model Performance in SOLIDWORKS 2018

Tobias Richard | Comments | December 15, 2017

As we create more and more complex assemblies in SOLIDWORKS, we find that our computer performance begins to slow down. This slowdown is frequently caused by certain parts in the assembly.Most commonly, the slowdowns occur for the following reasons:

  • Parts have too much detail or too many features
  • Parts have “Level of detail” slider set too high—found in Document Properties
  • Parts have rebuild errors
  • Parts are coming from a directory that is slow to access—due to network location
  • Parts are opening in an older version format of SOLIDWORKS

This checklist provides items to examine and correct whenever working with a slower assembly. The challenge faced is determining which parts are slowing down the assembly so that we can open these specific parts and address the issues listed above.

SOLIDWORKS 2018 introduces two great new tools to address this challenge: Assembly Performance Evaluation and Assembly Visualization. Before examining these latest tools, we will take a look at the new SOLIDWORKS 2018 Assembly Open Progress Indicator, which will help answer one of the most common questions when opening a larger assembly in SOLIDWORKS: “Is my SOLIDWORKS still actually opening my assembly? Or is it hanging?”

The Assembly Open Progress Indicator in SOLIDWORKS 2018

Figure 1. The Assembly Open Progress Indicator in SOLIDWORKS 2018.

Figure 1 shows an example of the Assembly Open Progress Indicator in SOLIDWORKS 2018. This enhancement appears whenever we open an assembly in SOLIDWORKS 2018, allowing us to see the progression of files being opened in the software.

Figure 2. A breakdown of The Assembly Open Progress Indicator.

In Figure 2, key areas of the Assembly Open Progress indicator can be seen. First is a progression of how long each component is taking to open in SOLIDWORKS. This feedback is incredibly valuable. When we opened a large assembly in previous versions of SOLIDWORKS it was difficult to answer the question “Is SOLIDWORKS actually doing anything?” because there were few indicators as to the status of the open process. Now we can answer this question with a definitive “yes,” as we can see how long each component takes to open. This feedback can help determine whether we have a bottleneck in our FILE>OPEN procedure.

A common example of a large assembly FILE>OPEN bottleneck would be seen when opening files from a slow network drive. By utilizing the Assembly Open Progress Indicator, we could determine whether the assembly opens significantly faster from a local drive as opposed to a network drive. We could use this feedback to justify the costs involved in improving network speed or as justification to change the FILE>OPEN procedure—possibly moving files to a local drive before opening them.

The Assembly Open Progress Indicator also shows us how long the assembly is taking to open and how long it took the last time to open. This is great feedback as it can help us plan our morning. If we know that it will take 7 minutes and 37 seconds to open our assembly, then that might be just enough time to go grab a cup of coffee and discuss the project with a co-worker.

Now that we have the assembly open, let’s take a look at the new tools to help us determine which parts are causing the highest demand on our system.

SOLIDWORKS 2018 Assembly Performance Evaluation

Figure 3. The Performance Evaluation Icon on the Evaluate toolbar.

The Performance Evaluation tool has been significantly improved in SOLIDWORKS 2018. This tool always has shown the number of sub-assemblies in an assembly, mates and resolved components, and other great assembly information. In SOLIDWORKS 2018 we are presented with new information to help troubleshoot slower assembly performance.

Figure 4. The new assembly Performance Evaluation window in SOLIDWORKS 2018.

In Figure 4 we can see that the assembly Performance Evaluation window now includes feedback to help identify parts that may be causing our assembly to underperform. The Performance Evaluation window distinguishes between files that may be causing the assembly to be slow to open and files that may be causing the assembly to be slow to work with.

The upper section of the Performance evaluation window shows files that are slow to open. Although it might be hard to see, the slowest file being opened is only taking .90 seconds to open. In my opinion this is a perfectly acceptable amount of time and is likely occurring because we are opening the files from a local hard drive.

Figure 5. The Performance Evaluation tool shows slower opening times when accessing files from a network drive.

Figure 5 shows much slower opening times when working with files from a network drive. The top three components are opening much slower than the fourth component at 32.82 sec, 21.94 sec, 11.51 sec and 0.51 sec respectively.Since these files are coming from different network locations we could use this information to justify relocating the slower files, possibly to a local drive, or use this information to justify investing in network architecture to speed up the process of opening and saving SOLIDWORKS projects.

Figure 6. The Performance Evaluation tool shows components that are causing a high taxation on our graphics card.

Figure 6 shows the lower half of the Performance Evaluation tool. As described back in Figure 4, this section of the performance evaluation tool tells us which components are going to be slow to work with.Some common symptoms of an assembly being “slow to work with” are:

  • Slow when switching between windows
  • Screen randomly goes all white for several seconds
  • Slow when going from EDIT PART mode back into EDIT ASSEMBLY mode
  • Slow when making/working with drawings

All of these symptoms can be caused by certain parts in our assembly having too much detail and generating too many graphics triangles. As we can see in Figure 6, my top component has 310,704 graphics triangles and has a quantity of 8 instances. In the Performance Evaluation tool the triangles are represented as a result of the number of triangles in each instance multiplied by the quantity of parts, thus each instance of this component has 310,704/8 = 38,838 graphics triangles.

This number is far too high for a single part file. I like to separate my parts into three categories when working with large assemblies and dealing with graphics triangles:

MOST PARTS – 0 to 999 graphics triangles per instance
SOME PARTS – 1,000 to 4,999 graphics triangles per instance
FEW PARTS – 5,000 to 30,000 graphics triangles per instance
NO PARTS – Greater than 30,000 graphics triangles

By sticking to these goals we are able to ensure that our large assemblies and drawings of large assemblies can maintain an acceptable level of performance.

SOLIDWORKS 2018 Assembly Visualization

Figure 7. The SOLIDWORKS Assembly Visualization icon.

As discussed above the most common culprits in assembly performance degradation are parts slow to open and ones that have a high number of graphics triangles. Using the assembly Performance evaluation toolbar we can see this information in bar graph format. Using SOLIDWORKS Assembly Visualization provides this information as a color representation overlaid on our assembly.

Figure 8. Using Assembly Visualization to sort by time to open – RED = longer to open.

Figure 8 is an example of sorting the assembly into colors based on how long each part takes to open. This can be helpful when working with an assembly that is slow to open or slow to save, as described in the section above on assembly Performance Evaluation.

Figure 9. Using Assembly Visualization to sort by number of graphics triangles – RED = higher number of triangles.

Figure 9 features a similar example of sorting, but time sorting by number of graphics triangles. As we can see, some of the parts taking the longest to open are the parts with the highest number of graphics triangles. This knowledge can be valuable when trying to determine why our assembly is slow to work with, as described above.


Figure 10. After launching Assembly Visualization click the REBUILD icon, shown on the left.

One of the coolest enhancements to SOLIDWORKS 2018 is the ability to launch the Assembly Visualization tool and then click on the rebuild icon, shown on the left in Figure 10.This icon automatically adds columns to sort by Graphics Triangle, SW-Open Time and SW-Rebuild Time. These three categories are the most common culprits when working with slowdowns in larger assemblies. The ability to identify which specific part files are causing the slowdowns is the first step in resolving them.

Now That We Have Identified the Problematic Files, How Can We Address These Issues?

There are two primary types of slowness when working with large assemblies: the assembly is slow to open and save, or the assembly is slow to work with.When the assembly is slow to open or save, we can identify which parts are taking the longest to open and attempt to determine why they are taking so long to open. Most commonly the files in question are coming from a slow network, and the solution is to move the files to a local hard drive to get faster read/write times. Occasionally these files are of an unusually high file size, so the solution is to open and work with the file to reduce overall file size.

When files are slow to work with, the most common culprit is that the number of graphics triangles is too high. When this occurs it indicates that our part files have too much detail. One method commonly used to address this is to open the part files and examine the setting for DOCUMENT PROPERTIES>IMAGE QUALITY.

Figure 11. After launching Assembly Visualization click the REBUILD icon, shown on the left.

If this setting is in the “red zone” on the far right, it will lead to a high number of graphics triangles. Opening a part file with a high number of graphics triangles and reducing this setting will help the overall performance of a larger assembly by reducing the number of graphics triangles your graphics card needs to process.

Once this setting has been set to about 1/4 of the way from the left, we are ready to move on to the final step: creating a simplified configuration of an overly detailed part file.

Figure 12. Taking a part with a lot of detail and creating a SIMPLIFIED configuration.

When it comes to reducing the overall number of graphics triangles in an assembly that has slow performance, the single best action is to create SIMPLIFIED configurations of the parts that have the highest number of graphics triangles. This SIMPLIFIED configuration can remove hundreds, and sometimes thousands, of graphics triangles from the overall assembly.

When you have extruded text, suppress it. When you have helical threads, replace them with a cylindrical boss.When you have features that you aren’t going to be able to see at the top level assembly, suppress them. Everything you do to reduce the number of graphics triangles in your top level assembly will help with your overall assembly performance. Creating a simplified configuration to reduce the overall number of graphics triangles in our assembly is one of the most effective tools we have to help speed up larger assemblies that begin performing poorly.


SOLIDWORKS 2018 has introduced some terrific tools to help us work with our larger assemblies. When we first open an assembly, we are now presented with a progress bar to ensure that the assembly is opening as efficiently as possible. After the assembly is open, we can click on the assembly Performance Evaluation tool to examine whether any one set of files opening particularly slower than the remaining files. We also can use this tool to examine which files are requiring the highest amount of graphical processing resources by yielding the highest number of graphics triangles.

If we find that parts are opening unusually slowly, we can move them to a faster read/write location, such as our local hard drive. If we find that parts have an unusually high number of graphics triangles, we can open these parts and create a new simplified configuration to reduce the overhead on our graphics card, making the assembly much faster and easier to work with.

About the Author


Tobias Richard is a SOLIDWORKS elite applications engineer from Philadelphia. He has been working with SOLIDWORKS software since 1998 and has been providing training, technical support and tips and tricks since 2001.

Recommended News