Autodesk Inventor Pattern Optimisation with Optimized Compute.

A patterned panel modeled in Autodesk Inventor.

How to speed up pattern generation in Autodesk Inventor and reduce file sizes!

Large patterns in Inventor models can take time to generate and increase file size. Did you ever see this dialogue?

A warning dialog from Autodesk Inventor, suggesting the use of Optimzed compute. — Have you seen this warning? Do you know what ‘Optimized compute’ is?

‘This pattern will result in a large number of occurrences. Consider using Optimized compute to increase pattern performance.’

What does that even mean?

This post was first published on the Graitec Blog.

A feature being patterned across a flat panel modelled in Autodesk Inventor. A message warns that the inputs will result in a large number of patterns, and suggests use of Optimized compute. — A large number of occurrences can promote a warning to use Optimized compute.

Autodesk Inventor Optimized compute

When creating patterns in Autodesk Inventor, Inventor checks every new instance of your pattern to see if it must create new faces.

In the image below, we can see that Inventor will need to calculate new faces where the patterned feature integrates with the body of the part, and it won’t need to create new faces where the patterned feature interacts with a cutout.

A feature being patterned across a flat panel modelled in Autodesk Inventor — Calculating a feature pattern across a body with voids.

Turning on ‘Optimized compute’ tells Inventor that there are no additional features that the pattern needs to interact with, so it can get on and build the pattern.

To turn on Optimized compute, expand the part feature pattern dialogue by clicking on the ‘>>’ arrow button and select the radial button next to ‘Optimized.’

Here is an Article on the Autodesk Knowledge network with more details.

A feature is being patterned across a panel in Autodesk Inventor. The panel has no cut outs - Optimze compute is an option. The image shows which options to select in the pattern dialog for optimised compute. — Using the ‘Optimized’ option for patterns in Autodesk Inventor.

Warning!

This option will fail if you are patterning over the top of an existing feature. It will work out OK if you create any additional cuts after your pattern.

TIP: If you see an error, In the warning dialog, expand the nodes until you see a node with red text and a red cross beside it. Click on the red text and the problem feature will highlight.

A features is being patterned across a panel in Autodesk Inventor. The pattern has failed. Clicking on the red text in the warning dialoge can indicate where the failure is. — Tip: Click on the red text in the warning dialog for a visual clue on where the feature is failing to compute. In this case, it’s where the feature pattern hits a void.

An alternative method

You may get a better result if you create a cut feature as a body, and then pattern the body instead of patterning the cut.

A feature is being patterned in Autodesk Inventor — An alternative is to model the feature, and then pattern it as a feature or body.

Using this method, Inventor only has to copy the body rather than analyzing the interactions between faces.

Examples

Workflow	Part file size on disk	Pattern generation time
Cut first then pattern	700 KB	415ms
Pattern with optimized compute then cut	750 KB	150ms
Pattern body then cut	800 KB	1430ms

Your results may vary depending on the version of Inventor you are running and your hardware specs.

Conclusion

If you are having trouble with large feature patterns In Inventor taking a long time to compute, giving you large, unwieldy file sizes, or even crashing Inventor entirely, consider changing the order of your features and patterns and try the ‘Optimized compute’ option!

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