Assembly File Verses Part File

[isocam]

Can anybody help?

I have an extremely large assembly made up of many sub-assemblies. This is taking many hours to open!!!

If I converted all the sub-assemblies to part files (ipt) using derived part, will each sub-assembly be a lot smaller than the original "iam" file?

Basically, is it worth me doing this?

Many thanks in advance!

Darren

[JDMather]

Does Manage>Rebuild All return any errors?

Are all sketches fully defined in each and every part?

Are logical assembly constraints used for each and every assembly constraint?

Nearly every assembly I examine has foundational issues that were not resolved.

Oops, never mind - I see that you are an experienced user.

[isocam]

Hi,

Every sub-assembly is perfect (no issues)!

I can open the assembly with no problems.

The issue is the actual file size for every sub-assembly.

I thought that, if I could save the sub-assemblies as IPT files (using derived part) that the actual size of the main assembly would be a lot smaller and quicker to load.

Is this the case, or am I wasting my time doing this?

Kind Regards

Darren

[mcgyvr]

Have you looked into the shrinkwrap/simplify workflows?

What version of Inventor do you have?

[SharkDesign]

You could shrink-wrap them and then put them in. You could fill voids and holes to simplify it. The only thing I've never known is whether parts made from parameters take up less or more memory than a converted file, which is basically what shrink-wrap is. They both get cached so it might be the same. 

[JDMather]

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@isocam wrote:

Can anybody help?

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Is this Inventor 2022?

If yes, have you installed Update 1?

[A.Acheson]

Yes deriving assemblies into parts should lower the file size overall. You can do this easily in the assembly with level of detail derive into part.

If your parts in the assembly have any sort of perforations or repetitive features consider removing these detail if they are not needed for manufacturing/detailing.

One example for me would be a filter with mesh screen. The mesh screen was not  needed in our modelling so I derived the filter and remove the mesh screen solid.

Also surface bodies imported from steps can take up a lot of memory so consider a simplified solid body. 

[johnsonshiue]

Hi! This question has been brought up multiple times. There isn't right or wrong answer here. It really depends on your workflows and what you really want to do.

Inventor is a distributed design CAD. It works the most efficiently if a model is built by sub components. And, reuse components whenever possible.

When you say you want to aggregate component geometry to a part in order to boost performance. Sometimes it does help. But, in other cases, it may not.

The example I like to use the most is think about an assembly with 10K identical boxes. Inventor works the best when these boxes are instances of the part box. You simply have 10K instances of the part in the assembly.

Now, think about if each box is an unique part (different file), you will end up with a very large dataset.

If you derive the assembly into a part with 10K solid bodies. I bet the part is not even editable.

Like I mentioned, there isn't one-size-fit-all answer here. Please feel free to share an example so we can comment further. In the meantime, you may want to turn off Express mode (Tools -> App Options -> Assembly -> uncheck "Enable Express mode"). This option helps you open the assembly fast. But, the graphics objects from all components are cached at the top-level assembly, which makes the iam file relatively big. In some cases, turning it off may help make the workflows more streamline.

Many thanks!