topic Re: Inventor Large Assembly Drawing Performance TOO SLOW in Inventor Forum

Inventor Large Assembly Drawing Performance TOO SLOW

Anonymous — Thu, 10 Aug 2017 13:16:48 GMT

I'm DYING! I'm trying to make a drawing of a large assembly but my computer is STRUGGLING to function... This can't be normal. I have a BOXX computer that is only about a year old. There's no way I can live with it taking so long to open and do any normal/typical commands.

I've searched for this issue but it doesn't seem like anything truly works... I could really use some help with this.

Please and thank you!

~Shawn

Re: Inventor Large Assembly Drawing Performance TOO SLOW

dgorsman — Thu, 10 Aug 2017 14:49:09 GMT

Welcome to the forums.

I can get a computer that's less than a year old which would barely be useful for our receptionist, let alone 3D work. So actual specs would be a good start, including Inventor version, OS version, input devices (3D mouse, for example). Some idea on part counts/complexity would also help.

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Mark.Lancaster — Thu, 10 Aug 2017 14:59:00 GMT

@Anonymous

In addition to @dgorsman request for additional information here are some other things to consider

Disable your anti-virus application on 1 machine and see if that changes the performance. If it does, apply the necessary exceptions

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.

Perform a disk defrag (unless you have a SSD drive). It may be necessary for you to clean up your hard drive and repair registry. Use a tool like CCLEANER (but at your own risk).

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 (Review this and that)

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 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

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.

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) ?

Are you putting too much details in your drawing.. Like trying to jam 20lb worth of stuff in a 5 lb bag.. Break up your drawings into smaller chunks.

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.

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. But its another way of looking at boosting performance in your model

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Anonymous — Thu, 10 Aug 2017 17:10:40 GMT

Inventor 17

I was mistaken...I just got this laptop last February.

It's a BOXX

Intel Core I7-6700 4.0Ghz Quad Core

32 GB DDR4-2133 (2 - 16GB SODIMMS)

NVIDIA Quadro M3000M 4GB

1.0 TB SSD M.2 PCLE Drive

Windows 10

Just using a simple standard Logitech bluetooth mouse and keyboard. Nothing fancy...

I'll need to double check those numbers shown in the bottom lefthand side of the screen, but I think I remember them showing over 25,000 and the other as almost 7,000...

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Anonymous — Thu, 10 Aug 2017 17:16:11 GMT

WOW!!! That's a lot of info.... Wonder where to start.

Re: Inventor Large Assembly Drawing Performance TOO SLOW

blair — Thu, 10 Aug 2017 17:21:27 GMT

I've attached one file that may help, I'll try and track down a couple of other documents.

Have you also looked at using "Express View"?

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Mark.Lancaster — Thu, 10 Aug 2017 17:22:24 GMT

@Anonymous

Yes it is.. That's why I always finish with "Yes there's a lot of info here and not everything I pointed out will work for you"

Actually I'm presenting a class at AU2017 regarding this very same topic... "Boosting Inventor Performance" if anybody is interested in learning more about this topic and attending AU..

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Anonymous — Thu, 10 Aug 2017 18:35:18 GMT

"Express View"? In the drawing?? Not sure what you mean...

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Anonymous — Thu, 10 Aug 2017 18:35:50 GMT

I'd definitely be interested in learning more.

Re: Inventor Large Assembly Drawing Performance TOO SLOW

johnsonshiue — Fri, 11 Aug 2017 16:01:50 GMT

Hi! The hardware spec looks fine to me. How large is the assembly? Could you share the files with us to understand the behavior better? Do you have access to Inventor 2018?

Many thanks1

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Anonymous — Fri, 11 Aug 2017 16:16:04 GMT

I'm assuming I can update to 2018.

The drawing file size is 30,424kb

The assembly file size is 303,347

Someone told me I should do a test and try to store files locally versus out on our network server. I'm not super computer savvy so I'm not sure the best way to go about my daily business if that would be the case. We don't currently have Vault either.

Another co-worker thought maybe I should be using Plant 3D to build my assembly...???

Re: Inventor Large Assembly Drawing Performance TOO SLOW

johnsonshiue — Fri, 11 Aug 2017 17:08:39 GMT

Hi! Purely based on the file size, it does sound large. But, we have customers working on drawing and assembly equivalent or larger than the one you have with good performance. Something does not make sense to me. You mentioned that you have files stored in network drive. Is this a network drive on your domain? How far is it from your machine to the server?

Many thanks!

Re: Inventor Large Assembly Drawing Performance TOO SLOW

dgorsman — Fri, 11 Aug 2017 17:49:22 GMT

@Anonymous wrote:

Another co-worker thought maybe I should be using Plant 3D to build my assembly...???

That depends on a number of factors. It doesn't handle detailed work as well as Inventor, it's much more "macro" in scale using simplified components and specification-driven selection. If you need to follow "piping specs", require "piping iso's", and care more about pipes and valves rather than individual nuts'n'bolt types and locations, Plant3D may indeed be a better choice. If you are doing primarily mechanical design, with piping components only part of the model, and parametric controls are necessary, you'll want to stay with Inventor.

Re: Inventor Large Assembly Drawing Performance TOO SLOW

blair — Sat, 12 Aug 2017 18:37:50 GMT

Here's a document on Express View.

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Anonymous — Tue, 15 Aug 2017 12:14:06 GMT

Trying to work "Local". It seems to be MUCH faster. I'm trying to figure our the "Pack and Go". I'm assuming this is the best method for doing this type of work... Pack and Go to my computer then when done move it back? Does this sound like the best way? We don't have Vault (not sure if that's good or bad). Would you happen to have a good tutorial on "Pack and Go"?

Thanks!

Re: Inventor Large Assembly Drawing Performance TOO SLOW

blair — Tue, 15 Aug 2017 17:10:27 GMT

Not really unless you are the only person using Inventor. Generally Pack and Go is used to get a copy of files of a specific assembly to send to someone and not an everyday work process.

With the improved results by bypassing the network, it shows where your issues are, in this case your network. It's a good indication that you have issues with your network, either server(s) or switch/router(s).

Re: Inventor Large Assembly Drawing Performance TOO SLOW

kelly.young — Tue, 15 Aug 2017 19:37:47 GMT

@Anonymous I see that you are visiting as a new member to the Inventor Forum.

Welcome to the Autodesk Community!

About Packaging Files with Pack and Go

Using Pack and Go with Autodesk Inventor

Please select the Accept as Solution button if a post solves your issue or answers your question.

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Anonymous — Wed, 16 Aug 2017 13:08:58 GMT

Working Local seemed to be better however I seemed to still have several "Not Responding" issues yesterday... Both, inside drawings and inside assemblies. I couldn't find or figure out a common reason for this happening. Only option felt was to hard crash the program and start over from last save.

Betreff: Inventor Large Assembly Drawing Performance TOO SLOW

S_May — Wed, 16 Aug 2017 14:49:54 GMT

Hello together,

Please work with LOD and replacement objects for assamblies.

Only this works, we work with assemblies up to 80,000 parts, with replacement objects and LOD, it is 2500 parts.

Please see the Video.

Please the computer test >>> Test <<<

Re: Inventor Large Assembly Drawing Performance TOO SLOW

Anonymous — Wed, 16 Aug 2017 17:46:17 GMT

Now that I've pulled some info onto my laptop using Pack and Go and made some changes, how can I push back onto my server and not lose any relationships or intelligence that was there before I pulled off? I have to assume this is possible?? Or, am I screwed??