reducing big STEP files

[johan.degreef]

From time to time we receive really big (400-600 Mb) STEP files we need to use in our assemblies. It makes our projects slow. What are our options? Can I easely reduce the STEP file to something less detailed?

[andrewiv]

Are you referencing the step file or converting it to Inventor files?  Is it an assembly or a multi body solid?

[johnsonshiue]

Hi! There is indeed a way to reduce the STEP file size at the expense of tolerance. Go to Save Copy As -> STEP -> Options -> change Split fit tolerance to something bigger (default to 0.01mm). Are you already using 0.01mm?

The looser the tolerance, the smaller the STEP file. However, this may reduce model precision and also increase the risk of generating bad bodies.

Many thanks!

[imajar]

There is alot you can do to speed things up - but these optimizations would have to be made each time you receive a new file.  Here is a full support article about optimizing large assemblies.

The first thing is using "level of detail" to manage what is loaded and unloaded.  By suppressing stuff you don't need, you can make a massive assembly load and run very fast.

Usually, the first thing I do is right click, change selection filter to parts, then Shift + right click and click "component size", then you can select components by size and suppress them.  This is a great way to quickly remove small stuff that is usually less important like bolts, nuts and washers.  For very large assemblies, it can take a minute to select, I suggest learning the workflow on something small.

After that you can also use shrinkwrap to have the software automatically remove holes, pockets, fillets, chamfers, internal voids, hidden parts, etc.   This can also be time consuming for complex geometry, but well worth the gain in performance.

If all you need is to view the step file and your model together, Give Navisworks a try (if it is part of your subscription).  It took me a bit to learn how to use it (and like it), but now that I know, I actually link my Inventor assemblies into a master Navisworks assembly.  When done right, it loads and navigates very fast.  

[johnsonshiue]

Hi Johan,

I am sorry I got it reversed. I thought you were talking about exported file size. But, you are asking importing. I would say you need a lot of RAM. You will need at least 32GB RAM. Also, you may want to leverage Task Scheduler to import the files automatically (TS runs graphics-less Inventor so it may reduce member foot print).

In terms of the detail, there isn't much you can do before bringing it to Inventor. The detail reduction should have been done on the Export end. After the geometry is imported, you can remove the unnecessary geometry or components. Use Simplification workflow to trim down the unneeded detail.

Many thanks!