Inventor General Discussion

Inventor General Discussion

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Distinguished Contributor
BrettCaldeira
Posts: 160
Registered: ‎10-27-2008
Message 1 of 11 (3,991 Views)

Very LARGE Inventor Files

3991 Views, 10 Replies
04-14-2011 12:16 AM

Hi All

 

Was wondering if you can help.

I am having an issue with some Inventor files. We are busy with large and fairly complex models of well over 1000 parts. When I derive these assemblies I often get ipt files larger then 100MB in size. I do include the reduced memory mode when creating these derived components but still get massive files. The assemblies then get very heavy with this sort of file inserted. I have gone through a lot of white papers on "working with Large assemblies" which have helped in some aspects. Do any of you have any comments or suggestions on working on large assemblies, or reducing the file size of some of my derived assemblies?

 

Our workstations are more then recommended spec with 12GB RAM, 2.8GHz Quad Core processors and have Quadro Cards.

 

Regards,

 

*Expert Elite*
mcgyvr
Posts: 7,101
Registered: ‎12-01-2004
Message 2 of 11 (3,970 Views)

Re: Very LARGE Inventor Files

04-14-2011 05:16 AM in reply to: BrettCaldeira

Welcome to the world of large files.. its normal.

#1-Hard drive space is cheap.

#2-Remove any unnecessary parts if you can (fasteners,etc..)

 

What is your purpose of deriving the assemblies?

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Distinguished Mentor
pauldoubet
Posts: 703
Registered: ‎10-11-2006
Message 3 of 11 (3,946 Views)

Re: Very LARGE Inventor Files

04-14-2011 07:23 AM in reply to: BrettCaldeira

Can you clarify if you have an assembly with 1000 files open or 1000 instances of parts?

 

I have worked with assemblies much larger than this and really don't see any noticable performance issues. Recently I worked with a site model containing over 7000 instances of parts and covering an area about 63 feet x 82 feet. None of the assemblies in this site model were derived into ipt files, etc.

 

Paul

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mcgyvr
Posts: 7,101
Registered: ‎12-01-2004
Message 4 of 11 (3,940 Views)

Re: Very LARGE Inventor Files

04-14-2011 07:38 AM in reply to: pauldoubet

The actual number of files is irrelevant.. The size/complexity of the files makes a world of difference.

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MariaManuela
Posts: 870
Registered: ‎12-04-2003
Message 5 of 11 (3,923 Views)

Re: Very LARGE Inventor Files

04-14-2011 08:16 AM in reply to: BrettCaldeira

Hi,

Use Level Of Detail representations. Makes all the difference.

 

Help says:

"Level of Detail representations improve capacity and performance. They suppress unneeded components or replace many parts with a single part representation to reduce memory consumption and to simplify the modeling environment. Save the representation with a name and activate it for modeling tasks or select it for creating drawings, presentations, and derived assemblies. A derived part created from an assembly that uses an LOD with a reduced number of parts can be used in the same assembly it was created from as a Substitute LOD. A simplified substitute provides greater memory savings than suppression alone. When a Substitute Level of Detail is active, all components are suppressed and hidden in the browser. "

 

Manuela

Maria Manuela Pinho
Application Specialist
Cadtech / Asidek - Autodesk Gold Partner
Autodesk Inventor Professional 2015 | Lenovo W520
Valued Contributor
Loren_J
Posts: 90
Registered: ‎09-10-2010
Message 6 of 11 (3,902 Views)

Re: Very LARGE Inventor Files

04-14-2011 09:15 AM in reply to: BrettCaldeira

Our major sub-assemblies have 10,000-20,000 instances, and the top level assemblies have 50k-60k instances of 3k-4k files. Whether or not you use derived parts, the key to performance is using Levels of Detail. For example, you rarely need to show fasteners in the top level assembly. You can suppress internal components and small components that don't add value. If you want to use a different LOD, it can be faster to close the model and reopen with a different LOD than switch LODs with the model open. I don't know why it takes 2-3x more time to switch, but it does make a difference in my quality of life.

 

You need to be careful with LODs in drawings. When you create a view of an assembly using a different LOD it brings the entire model in. You can have a 10 sheet drawing and it will only load the model once if all of the views use the same LOD. If you use a different LOD for the base view on each sheet, the drawing will load the model 10 times.

 

The other way to improve performance at the top level is to use View Representations. Once the model is loaded, graphics become the main performance hit. On a large assembly, you are usually only working with 10-20% of the model. Y can dynamically turn the visibility on and off for components without a huge time hit, and you will see a big performance improvement.

 

Although it is tempting to use Derived parts, I am not seeing a big improvement in loading the top level assembly model. It is a big performance hit working with the model because I can't turn off visibility of sub-assemblies. If you do use derived parts, select the Maintain Each Solid as a Solid Body option. This is new in 2011, and Inventor doesn't have to analyze every model face to determine if it is on the inside or outside. I haven't seen a performance impact while using the derived part with all of the solids, but it makes a huge difference creating or updating it.

 

My basic process is:

  1. Create a few LODs that match the required drawings for the model. For example, create a general assembly LOD that is used for putting the model together and creating the GA drawing. If there is a separate field installation drawing, I would create an LOD for that. A GA might have internal details that are used in section view, while the FI usually only needs the external components.
  2. If a subassembly is complex, I would also make a reduced detail LOD that is only used for building the parent assembly. It isn't used for drawings because of the file loading issue noted above.
  3. When working in one of the large assemblies, create view reps as needed to hide the components you don't need. Make sure you create a new view rep instead of using Default. It 's annoying to place a base view of a model and only get a fraction of the components because they are turned off in Default. You then get to open the model, and play with visibility to get everything back for Default. The Default view rep should always be the same as Master. 
  4. Use View Reps to clean up drawing views. Unlike LODs, they don't require loading extra versions of the model in the drawing, DO NOT turn off component visibility in the browser. It is a little extra work to create a new view rep, but it makes life a lot easier if you have to change visibility of some components. I really don't want to dig into a 50,000 instance assembly in the drawing browser to find the sub-assembly I need to turn back on.

Of course, performance is dependent on the model size. Our models are huge, so there is an ROI to spend the time creating LODs and View Reps. You have to experiment to see how much performance improvement you get with LODs. Graphics cards make a huge difference in large assembly performance. Once the model data is loaded, the graphics have to be generated and then analyzed when you rotate, zoom in and out, etc. I haven't looked at hard drives yet, but people are reporting a big performance improvement using solid state drives. This makes sense because the data is pulled off disk more quickly.

 

Graphics settings are also important. In Application Options>Display tab, set the View Transition Time as low as you can. It helps to have some delay so you can watch the model view rotate, but every update takes time. Set the Minimum Frame Rate as low as you can. This impacts how much of the model disappears as you change the view, especially while panning. The recommended performance setting is 10, but don't believe it. You can see a big performance difference when you try the different settings. Reducing the Display Quality causes the model to display as faceted during view manipulation. Lower settings display fewer facets. Of course, these settings don't impact performance as much as you turn component visibility off.

 

As I mentioned, you should experiment with your models so you can optimize the different settings. It would also be nice if you would report back with your findings. I am sharing the results of several weeks of performance testing spread out over 3-4 months. Another data point will help other users achieve their performance improvements more quickly.

LorenJ

Inventor 2011 Pro
Win7 64 SP1
Xeon W3550 @3.07 GHz
ATI FirePro V5700, 8.773.0.0
12 GB RAM
Distinguished Mentor
pauldoubet
Posts: 703
Registered: ‎10-11-2006
Message 7 of 11 (3,887 Views)

Re: Very LARGE Inventor Files

04-14-2011 09:59 AM in reply to: mcgyvr

The number of files is relevant, less files open more instances requires less computing power than more files open with fewer instances of each file.

 

Paul

Employee
chucksavatsky
Posts: 13
Registered: ‎10-22-2007
Message 8 of 11 (3,882 Views)

Re: Very LARGE Inventor Files

04-14-2011 10:22 AM in reply to: BrettCaldeira

Hi Loren,

 

Inventor 2012 has addressed the issue in Drawings where when using a partslist it pulls in the entire assembly instead of only the components that are part of the LOD.  It has also been addressed in the Assembly BOM.

 

Regards,

 

Chuck Savatsky

Senior Dev Manager

Inventor

Regards,

Chuck Savatsky
Director Software Development Inventor
Autodesk
Valued Contributor
Loren_J
Posts: 90
Registered: ‎09-10-2010
Message 9 of 11 (3,836 Views)

Re: Very LARGE Inventor Files

04-14-2011 02:38 PM in reply to: chucksavatsky

Hi Chuck,

 

I saw the number of components double when I created a base view with a new LOD. I was testing drawing creation performance with different LODs, and it caught my attention. I don't recall if I had a parts list for the first LOD, but I closed without doing anything with the new LOD.

 

It would be nice if the the model loading issue was resolved for drawings in general. For our very large assemblies, I would still create a specific LOD for each drawing type and use view reps to control what is displayed in a view. There are enough performance issues creating and switching between LODs that it isn't worth the effort creating extra LODs.

 

We recently moved to 2011, and I need to evaluate 2012 so we can determine when to schedule the transition. Since we have unusual requirements, I need to do a pretty rigorous evaluation.

LorenJ

Inventor 2011 Pro
Win7 64 SP1
Xeon W3550 @3.07 GHz
ATI FirePro V5700, 8.773.0.0
12 GB RAM
Contributor
rfaussete
Posts: 21
Registered: ‎05-23-2008
Message 10 of 11 (3,671 Views)

Re: Very LARGE Inventor Files

05-05-2011 07:23 AM in reply to: Loren_J

I'm in the 60k + range as well... very frustrating at times.  LOD's definately help.  Just started shrinkwrapping some of the lower iam's.  Hopefully that will help a little as well as using a LOD with All Hardware Off.  Hopefully getting a new workstation soon too.

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