Large assembly very slow...is it the program or computer?

[Anonymous]

I'm working in a very large assembly (over 100k parts) and am wondering which side of the system is bogging.  Currently it takes several hours to open the model and at this point you cant really utilize it at all anyways.  We are being fed .stp files from the prime and have to assemble them into a large model before we can start removing what we dont need...so having a complete assembly is needed for now.  I found a PDF on this site "Large Assembly Performance" and matched the settings suggested within and I cant say that its helped much.

I've also tried to create derived components to see if we can make dummy files and even the subassemblies are just too big for that it seems.  Yesterday I let one subassembly of approximately 10k parts run and it either crashes or goes into a seemingly infinite loop of "processing".

Have i met the max capabilities of the program, or is my computer system not up to snuff?  I am running Inventor 2016 Professional.

[Anonymous]

@swalton are you referring to the "Inventor PC Index" as the final value for speed?

Mine showing 1-4.45?

[kgilham]

@Anonymous

Unfortunately without seeing the dataset it is very difficult to say why something is being slow.  If your manager has any concerns feel free to have them email me at kyle.gilham@autodesk.com and we can talk about any concerns you may have be it security or IP protection.

Thanks,

[Anonymous]

I forwarded your message/email to him, I suspect he will shoot you an email.

Thanks.

[Anonymous]

For those curious, the master has 27,115 unique files and 124,243 total parts SO FAR.  

[Mark.Lancaster]

@Anonymous

That large you made want to consider the following:

Is Design Data local or on the network.  Having it on the network can also lead to performance issues when loading models.

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

Unload unnecessary Inventor add-ins

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

Look at creating View Reps, Level of Details (LODs) as @Fouad-l pointed out, or working with Express Mode with your models.

Thinking about using the drawing open options to defer updates/fast open

Switch drawing view preview to partial or boundary box (Tools/Application Options/Drawing tab)

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)

If you are using shaded views in your drawing, try to limit them because they too will impact performance. In Document Settings/Drawing tab, make sure the Shaded View/Use Bitmap option is set to Always.

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.

Also how are you connected to your network?  WIFI, hard wired or through a VoIP phone?  If WIFI, get hard wired.  If through a phone connection for a test unplug the workstation from the phone and plug directly into a wall outlet.  Although this is rare, I've seen cases where VoIP phones causing performance issues.  One more thing...  For a test disable you Anti-Virus and load your assembly.  If that helps the load time you will need to put in the exceptions (https://knowledge.autodesk.com/search-result/caas/sfdcarticles/sfdcarticles/Are-there-antivirus-exclusions-I-can-implement-to-make-programs-run-better.html)

[Anonymous]

Responses in BOLD below

Is Design Data local or on the network.  Having it on the network can also lead to performance issues when loading models. (On network...should be using Vault in next day or so)

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. (We are required to use the file structure sent from the prime so the assembly trees properly)

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 (This is part of what we are trying to do.  We are given data, but dont know what it is until its assembled into the model.  Once we have the model created, we can start removing the unnecessary components and areas.  It is backwards, but thats what we have to work with. I cannot get Derived to work except in very small assemblies.  Shrinkwrap seems to lose alot of detail according to a coworker?)

Unload unnecessary Inventor add-ins (Done already)

Invoke defer update and manually update when you're ready. (Done already)

Look at creating View Reps, Level of Details (LODs) as @latrach.fouad pointed out, or working with Express Mode with your models. (We are working with Express)

Thinking about using the drawing open options to defer updates/fast open (I will look into this)

Switch drawing view preview to partial or boundary box (Tools/Application Options/Drawing tab) (we are still in design phase, this is all in 3d models not drawings yet)

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) ? (I will look into this)

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. (all components are constrained plane to plane from the origin and modeled "in space" to fall into the correct location)

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.  (What is the recommended setting?)

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. (Will check for update)

If you're using the 3D Connexion device.. Make sure its driver is up to date and you have calibrated it. (Will check for update)

Limit the number of other Windows application that are currently running. (I only ever have Inventor and Outlook open)

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

If you are using shaded views in your drawing, try to limit them because they too will impact performance. In Document Settings/Drawing tab, make sure the Shaded View/Use Bitmap option is set to Always. (not to drawings yet)

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. (I will change that, the settings I found suggested was 10 but it was at 0)

Also how are you connected to your network?  WIFI, hard wired or through a VoIP phone?  If WIFI, get hard wired.  If through a phone connection for a test unplug the workstation from the phone and plug directly into a wall outlet.  Although this is rare, I've seen cases where VoIP phones causing performance issues.  One more thing...  For a test disable you Anti-Virus and load your assembly.  If that helps the load time you will need to put in the exceptions (https://knowledge.autodesk.com/search-result/caas/sfdcarticles/sfdcarticles/Are-there-antivirus-excl...) (Hard Wired)

[johnsonshiue]

Hi! You might consider trying a few things here.

1) Close Inventor and go to %temp% and remove files there.

2) Start Inventor -> go to Tools -> Application Options -> Files -> uncheck Quick File Open option.

3) Instead of opening the file in Express mode, open it in Full mode with Level of Detail set to All Components Suppressed.

The assembly should open immediately since there will be no other files to load.

4) Now activate LOD:Master.

How long does it take?

[Anonymous]

@johnsonshiue I will give those a try.  Thanks for the suggestions.

[Anonymous]

Load full, all items suppressed it took 8 minutes to "load" the screen...will try to turn everything on now and see what happens.

[Anonymous]

Or not...Inventor just crashed when I selected "Options" from the Open tab.  🙂

[johnsonshiue]

Hi! That is not what I wanted you to do. Could you try this instead?

1) Close Inventor and restart it.

2) Open -> find the assembly -> Options -> uncheck Open Express and set Level of Detail to All Components Suppressed -> Ok.

It should open instantaneously.

3) Activate LOD:Master.

How long does it take?

Many thanks!

[Anonymous]

That is what I did, steps 1 and 2.  It took 8 minutes for the cursor to stop spinning and become the normal arrow.

Once I clicked "Options" to try to LOD: Master, the program crashed.

[Anonymous]

Ah, I selected "all Parts suppressed" not "all components suppressed"

Doing COMPONENTS, it did in fact open instantly.

[Anonymous]

I'm giving this another go...I gave it a little over an hour last night and it was still loading so will run it through completion today to see how long it takes.

[Anonymous]

3 hours in and its still loading using the instructions above.  

[johnsonshiue]

Hi! Could you tell me how much memory is used by Inventor.exe after the whole assembly is loaded (Task Manager -> Processes)?

Many thanks!

[Anonymous]

If I can get it to open, sure.  

I'm at hour 9 right now and its just churning.  

[johnsonshiue]

Hi! What about now? How much RAM is used by Inventor.exe?

Many thanks!

[Anonymous]

Currently...

[ChrisMitchell01]

To correct one of the bullet points below, for better graphics performance you should set Min Frame Rate to 20 not zero. To quote:

"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. (I will change that, the settings I found suggested was 10 but it was at 0)"

Also change to the Medium or Rough setting for Display Quality.

From the Hardware tab of Application Options ensure you're on Performance mode & then open a part & run the diagnostics; cut/paste the data into a text file & attach here.

As Kyle mentions we really need to see the data to better understand your problem(s) - hopefully that will be possible; we often work with customers under NDA where securely protecting customer IP is paramount. Your benchmark results suggest that your PC is generally under-powered for the size of assembly you're working with too.

Thanks,
Chris