How to improve large assembly performance?

[phil]

Hi, 

We deal with very large assemblies (11k+ occurences) and over 2600 different parts.  We manage to work with them ok, but it lags sometimes and some functions take time to load (constraints, hiding or making some sub-asssembly visible, etc.)  Any suggestions on what could be improved?  We are still on 2019 version, we will move to 2020 soon which was told help on this.

CPU : Intel i7-6700K 4Ghz

32Go RAM

Nvidia Quadro K2200

Thanks

[KKizildemir]

Hi,

Use Shrinkwrap Substitute command to reduce your sub assembly loads of your project.

Here is more info about this command:

Regards,

[johnsonshiue · Accepted solution]

Hi! Based on your hardware profile and the assembly size, it should not be considered a large assembly in 2019. The overall performance should be good. A few things to check.

1) Please make sure 2019.4 update is installed.

2) All critical Windows updates are installed and graphics driver is up-to-date.

3) Clean up %temp% folder.

4) If Material and Appearance Libraries are installed in a shared network drive, you may want to consider install them and access them locally.

Does the assembly contain any large derived assembly part or imported part? It means a part actually represents an assembly. Inventor was designed to work with distributed model (parts aggregate to an assembly). If you have parts with concentrated geometry (many bodies, faces, and edges), the performance may not be good. One thing you can try is to go to File Explorer and find the folder with the files, Sort by size. If you see ipt files with 50+MB, you do have large parts. These parts more than likely represent assemblies. Make them invisible and see if you get better performance.

Another thing to try is to disable Express mode (Close all docs -> Tools -> App Options -> Assembly -> uncheck "Enable Express mode"). Does it work better now?

Many thanks!

[johnsonshiue]

Hi! Actually whether or not substitute helps boost performance is not an easy question to answer. Based on my experience and my understanding of how things work, I will say it depends. Let me use extreme cases to explain my point.

Let's say you have an assembly with 10K boxes stacked up. All these boxes are the same. When you make a substitute of the assembly, you may get interesting behavior. 1) Derive each box as a separate solid. Now you will get a 10K bodies in the substitute part. I am sure the performance of such substitute will be much worse than the original assembly due to the large number of solid bodies. 2) Derive them all in one body. Now you have a giant body but the geometry is very simple. The performance of such substitute will be much better than original 10K assembly.

Let's look at it from a different extreme. Let's say you also have an assembly with 10K boxes stacked up. But, each box is a different file. Essentially, you have 10K components with 10K definitions. This kind of assembly will perform worse than the 10K boxes assembly with one definition. 1) Derive each box as a separate solid. You get 10K bodies in the substitute part. The performance of such large part may be on par with the original 10K unique boxes assembly. But, either way the performance will not be as good as 10K boxes with one definition.  2) Derive them all in one body. Again the giant substitute box part will out perform the original assembly.

Certainly, these are extreme cases but you can see that it is not a straight forward question to answer.

Many thanks!

[KKizildemir]

Hi @johnsonshiue ,

Shrinkwrap command has also simplify options for small parts or unnecessary features. It perfectly eliminates i.e. thousands of bolts, fills pockets and holes etc. without breaking the link between this simplified model and the original assembly. This is perfect.

By the way, I agree with you about your thought.