Best Practices for Large Assembly Performance

[Anonymous]

Inventor 2016

All service packs and hot-fixes installed

I am trying to define a  workflow for producing the lightest possible assemblies and have done a lot of research but i still have 3 questions to which i can't seem to find a definitive answer:

1.  Is there a difference in the size of the file produced by Derived/Shrink-Wrap/Simplified Part? if so which is the best?

     Most of the research i have done seems to point to Shrink-wrap but i just read this thread:

     https://forums.autodesk.com/t5/inventor-forum/large-assembly-performance/m-p/6666018#M619203

     in which smokes2998 says not to use Shrink-wrap because it slows Inventor down?

2.  When using any of the above techniques, i.e. Shrink-Wrap, do you save more memory by creating a SW of each and every assembly and

     sub-assembly or is it negligible when compared to creating a few SWs of the higher level assemblies in the Top-Level assembly?

3.  This one is hard to explain.

     I have two assemblies that represent the same object in different ways:

     Assembly 1 contains 4 sub-assembly components and each has a substitute LOD that is a SW part.  i created an LOD in Assembly 1 that selects the        substitute LOD in each of the 4 sub-assemblies, leaving me with 4 substitute parts in Assembly 1.  in the status bar i show 8 occurrences and 9                documents open.

     Assembly 2 is identical to Assembly 1 except that it contains the SW parts of the 4 sub-assembly components in Assembly 1.  So instead of 4

     sub-assemblies, it contains 4 parts.  This shows 4 occurrences and 5 documents in the status bar.

     My question is:  is assembly 2 less memory intensive than Assembly 1 because those numbers are lower?  do those numbers affect assembly

     performance or am i splitting hairs?

Just you think i am crazy for trying to reduce the memory of a 4 component assembly, i created these assemblies for experimenting with this so i can apply it to the MUCH larger assemblies i normally work with.

I am interested in any answers, comments, suggestions, examples of workflows, etc.  even if it's just a comment that i am wasting my time and none of this will increase my performance by a significant margin.

[Mark.Lancaster]

@Anonymous

Just throwing a few thoughts out...

Clean out your C:\Temp, C:\Windows\temp, and your C:\Users\[username]\Appdata\Local\Temp folder. Appdata is a hidden folder and you may need to adjust your viewing settings.

Turn off Windows Bells & Whistles, use classic theme, and disable desktop gadgets and unused (Windows) services..

Also configure Inventor and Windows per the recommended performance options link #1 and link #2

If possible keep Inventor Design Data locally. Having it on the network can lead to performance issues.

Work locally on your models if possible. If you have to store your models on the network. Leave the common files on the network and move your models back and forth using a file management tool. May want to consider implement Vault basic..

Keep your sketches simple and only project the necessary geometry.

Resolve issue via the Design Dr. Don't ignore them. Every so often on your model, perform a rebuild all. Other things to consider, limit adaptivity and use modeling functions over sketching commands. If you need to use the adaptive method.. Use it and then turn it off when done.

I know this is common sense, but keep your workspace, hard drive, or share network location organized and clean.
Properly configure a project file. Define the workspace and etc.

Don't put your eggs all in one basket when it comes to assemblies. Demote, simplify or break your model up into smaller chucks, Use the BOM structure (https://synergiscadblog.com/2015/02/06/inventor-bill-of-materials-structures/ ) to your advantage.

Simplify, Simplify, Simplify. Determine if the exact details are really necessary. If it is, create a simplified version (iPart, derived, shrinkwrap and etc) of the part. Think about using appearance over detail

Review the Autodesk Inventor 2014 working with large assembly performance guide (http://beinginventive.typepad.com/files/inventor-deep-dive---large-assembly-instructions.pdf)

Unload unnecessary Inventor add-ins

Invoke defer update and manually update when you're ready.

Look at creating View Reps, Level of Details (LODs), or working with Express Mode with your models.

Think about the parent to child relationship. Do you have these options turned on in Application Options (Relationship redundancy analysis and features are initially adaptive) ?

Constraints consume memory. Simplify them as much as possible. Maybe you want to ground your components or consider using skeleton modeling techniques. Or suppress constraints to limit them if you have numerous ones.

IF you're using bolted connections, this can impact performance. Create LODS and turn them off when not needed.

Set your Windows Virtual Memory to the recommend settings.

Make sure your graphics card driver is up to date. Don't rely on Windows telling you it is. Go directly to the Vendor web-site.

If you're using the 3D Connexion device.. Make sure its driver is up to date and you have calibrated it.

Limit the number of other Windows application that are currently running.

Use the "Disable Refinement" option if you're using Inventor 2016 or newer. (This option is located under Tools/Application Options/Display tab)

In Tools/Application Options/Display tab, you may want to consider setting Min Frame rate (Hz) to zero. Thus allowing faster rotation/spinning/orbit of your model.

Yes there's a lot of info here and not everything I pointed out will work for you or for others who may review this information.

[jtylerbc]

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@Anonymous wrote:

Inventor 2016

All service packs and hot-fixes installed

I am trying to define a  workflow for producing the lightest possible assemblies and have done a lot of research but i still have 3 questions to which i can't seem to find a definitive answer:

1.  Is there a difference in the size of the file produced by Derived/Shrink-Wrap/Simplified Part? if so which is the best?

---

Shrink-Wrap and Simplify are both really just the Derive tool, presented differently with focus on different options.  You end up with the same type of feature in the browser regardless of which one you use.

I'm pretty sure that everything that can be achieved by the Shrinkwrap and Simplify tools can be done using just the Derive tool if you know what options to select, and the results (file size, browser features, etc.) will be identical.

[Curtis_Waguespack]

Hi Bg45,

I didn't read all of this very well (just skimmed) but here is one key to using Shrink Wrap that many overlook:

Do not just shrink wrap what you have and expect a smaller file, you'll actually get a slightly larger file.

Shrink wrap is intended to be used with Level of Detail (LOD) .  So create your LOD and remove internal parts, etc. and then shrink wrap using that LOD, this will result in a smaller file, how small depends on how much detail was removed.

If you do this for your subassemblies, and then use the shrinkwraps as a substitute LOD for your subassemblies in your upper level assembly(s) you should be able to achieve some performance gains.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com