Unknown Performance Issues with Inventor

Technical Inventor
1

Just to start things off, I’ll say this might be a fairly long post as I’d like to get as much information that I know out there as possible. You have been warned.

OK. Well to start things off I’m a four year alumni of FIRST and this is my first year back with my old team as a CAD Mentor. Skip ahead to about two weeks ago, and everything had been going fine with Inventor with the exception that the computers provided by the school were having some real problems properly running Inventor. Now these are old machines. Pentium D’s, 3GB of RAM, 32bit Windows XP and an ATi Firepro who’s model I can not remember off the top of my head. Needless to say, they’re barely capable of running large models, much less an entire assembly of the robot.

However we had managed to get around that issue thanks to the other mentor and myself bringing in our laptops and letting the students use those to finish the final assembly. Well on Monday of this week I decided to leave work a few hours early to check-up on the final preparations of our Robot and see what (if any) help my CAD team still needed. I come to find out that the laptop the other mentor lent to them to work the assembly on, was running Inventor so slowly that it would take literally 2 minutes for a single tick of the mouse wheel to show that it zoomed in.

Needless to say, that is completely unusable in that state. Something I hadn’t seen before. To be fair, it is a consumer laptop without workstation graphics cards, but that’s never stopped any laptop in the past from properly running Inventor. In a fit of desperation I relented and decided to bring in my custom built desktop from home. Now before I go on, let me just say I’m fairly well versed when it comes to computer hardware and my desktop reflects that - running quite high-end hardware. An i7 950, 6GB of RAM and two Geforce 470’s in SLI. I’ve even got an SSD drive to boot.

I recognize the hardware components are for the most part all consumer. Especially the graphics cards. However with 1.3GB of vRAM I figured that would still be more than enough (seeing as the average workstation card usually has about 2GB of vRAM) and for the first 4-5 hours it was running about as fast as you or I would think it should. Then nearing the end of the day on Monday it began really slowing down. Not quite as bad as it was on the laptop and still leagues better than on the school computers but running far slower than the hardware should have ever permitted it.

Come Tuesday I decided to take off work and bring my desktop in to let the students work on it all day. Yesterday was incredibly slow. Nearly a minute just to apply a simple Aligned constraint (please forgive me - I forget the name of the constraint in Inventor because I work with Unigraphics for a living) of a bolt into a hole. It took nearly an hour to get 8 washers, onto 8 bolts, into 8 holes.

Now I’m not one to brag, and I certainly don’t want to come off that way, but everything I’ve read tells me my hardware should be OVERKILL for what we need. And yet it’s almost as slow as it was on the laptop they were using previously. I can not explain what is going on. I have searched through autodesk forums and found a “feature” (more like a designed bug) that records every single movement you make of the model into memory so you can use the rewind feature to go back to a previous view. Frankly it sounds useless to me, and I wouldn’t care except there’s no way to shut it off and even worse the only way to make Inventor free the memory being used is to restart the computer.

Now unless I’ve missed a forum post somewhere on this site, I haven’t seen anybody else encounter this issue. I had just assumed the school computers as well as the laptop were simply underspecc’d to handle such a large assembly. However the hardware in my desktop should breeze through such trivial assemblies and models without even breaking a sweat - even if it is using consumer cards and non-Xeon/Opteron processors.

So - after this long and drawn out explanation, I ask if anyone has encountered anything like this before? Could it really just be that “rewind feature” that is causing this? Even if it does load up everything into RAM, I would think 6GB is enough (though I have seen a few people on autodesk forums recommend at least 8). I have tried uninstalling and re-installing - again to no avail. We have the professional edition on the school computers as well as the other mentor’s laptop, and the student edition that came in the KOP on my desktop. 32bit and 64bit versions. Non and student editions. All encountering the same problem.

The only other commonality between them is that both the laptop and my desktop use an SSD. However on my desktop Inventor is installed on the mechanical hard drive with the files installed on the SSD as I assumed it would decrease load times. Does Inventor have some issue with SSDs and the way it caches to the page file?

I am sorry for all of these questions (especially so soon before the March 3rd deadline) however I am really at a loss here. I’ve even turned down the detail as far as possible for the models and we’re still having issues. Short of renting out a server to do all of our modeling on, what can I do? I have never had a performance issue in all of my years this badly before. Is there some issue with the kit of parts files? Some issue with mixing them with the FTC files because they converted from Pro-E files?

ANY assistance ANYBODY can give me would be greatly, GREATLY appreciated. Help me Chief Delphi - you are my only hope.

2

I’m not an Inventor expert, but take a look into “Level of Detail”. I’ve never used it, but I think it can simplify sub-assemblies to make larger assemblies more manageable.

Here’s a good article on managing large assemblies:

Sorry that’s all I can suggest, good luck!

3

Thanks for the post. From what it sounds like, the Level of Detail acts just like Reference Sets in Unigraphics - which although we weren’t using them we were suppressing unused sub assemblies and the like, so I don’t think that will help matters.

I’ll look through the other 30 pages or so though and see if there’s anything else in there that can help me out. Thanks for the help.

4

So, try the Level of Detail, but I think you have a much bigger issue here. First of all, are you running the most up to date sevice pack of inventor (at work this seemed to fix most issues)?

Bear in mind that inventor 2011 is written for gaming cards instead of CAD graphics cards, so your hardware should be WAY more than enough.

5

Yes, I downloaded all of the latest updates for Inventor during the installation process.

And yes, I agree. There is something is seriously wrong here, I’m just at a loss as to what it could possibly be (obvious with this forum post here). I’ll look back into the Level of Detail, but from what I understand it’s no different than just manually suppressing parts in an assembly. However there does seem to be a few tricks in there as well to reduce strain on the system.

I just don’t know WHY it’s producing SO much strain on such high-end hardware.

6

might be a bit of a silly question, but are you using sub assemblies?

7

Yes.

Why, is there an issue with Inventor and Sub Assemblies?

8

That is very interesting. Try running Inventor with only one GTX470 and see what happens. Is your i7/GTX470 overclocked?

I’m running Inventor on a 9600GT and it runs fine… :confused:

9

You know, as embarrassing as that is, I haven’t though of running only one 470. I should go disable SLI and see what happens. That still doesn’t explain why it worked fine for the first 5 hours on Monday, then began lagging.

I also haven’t overclocked my i7, and I brought my 470’s back to stock clock levels because I know the clock frequencies don’t really give that much of a boost to 3D Modeling Programs.

And before you ask, I have tried running Inventor with Hyper Threading enabled and without. I haven’t noticed a positive or negative difference with either setting.

10

I agree your hardware should be more than enough to run Inventor, but is it possible you’re overdrawing still? What color is the RAM bar in the bottom right hand corner? The less full it is the better.

In order to figure out if this is a hardware or software issue, I’d check your performance monitor equivalent. If the CPU load is low, and the RAM is under 50% usage, the problem is with Inventor.

Hope this helps.

11

The highest I’ve ever seen my memory usage spike is about 2.5GB. Which seeing as I have 6GB should still be more than enough.

I’ll have to get back to you about my CPU usage though.

12

The most common problem I see in a situation like this is a conflicting assembly constraint. Impossible to diagnose without sitting in front of the machine - but I would make a substantial wager that is the problem. You might be able to isolate it by removing parts or subs one-by-one. When I sit down to find a problem like this I can usually find the suspect part or assembly fairly quickly.

I would rate almost everything I see done in Inventor as garbage. Garbage in - garbage out. There is a real problem with professional level training.

If you can pack and go the assembly and send it to me I’ll take a look. (be sure to preserve file/folder structure) jmather_at_pct_dot_edu

13

There are several constraints I’ve seen with errors on them. And as you said, they don’t seem to be uncommon. I never realized that conflicting constraints could cause such severe performance issues.

I can take a look at them myself over the weekend since I finally have some time and I’ll report back my findings. I’m used to having to deal with broken and conflicting constraints with the Unigraphics models I work with at my job.

Thank you for that insight though. I really had no idea that conflicting constraints could do anything to the performance of Inventor except just make it error prone in terms of getting proper movement and proper association.

14

no, I was thinking that if you did not use sub assemblies, that inventor might be trying to update to many constraints which will kill performance.

15

That’s a bit strange.

I run Inventor on my Dell Dimension E520 (Intel Core 2 Duo CPU, 3GB DDR2 RAM, running at 2.13GHz on Windows XP Media Center) and I can have several parts and assemblies running at once as well as a few tabs open in Firefox at the same time with no lag, but when I play Garry’s Mod, if I spawn too many props (>25) it lags like crazy.

I think it’s probably the computer’s reaction to continued use, possibly heat?

16

I’ll admit it, I also want a solution to how to get around it, and although when I encountered it, it wasn’t so painfully slow (only about 5-10 second delay time), it was indeed very annoying and frustrating. So, it’s for that reason, or a similar one anyway why I would rate Inventor 2010 better than 2011 (although I would say it is pretty close, 2011 improved on 2010 a lot in getting around to what needed to get done).

/rant

But anyway, you mentioned that you constrain every bolt and washer you can. Part of the problem might be because Inventor tries to render every single part before moving. While I doubt it is the major factor as to the slowing of your computer, it might help a little bit and get things done more efficiently.

Otherwise, try to do everything you possibly can in sub-assemblies to make the chunks you have to work with as small as possible, thus the least amount of rendering that has to be done.

17

I am starting to come to the realization that we perhaps somehow used too few sub assemblies. We’ve done exactly what we’ve done in years past, however I guess with the increased complexity of Inventor 2011, we had to re-adjust how we put our assemblies together. Adjusting the Level of Detail did nothing, and previous years assemblies open just fine.

It must be some combination of incorrect/conflicting constraints and the sheer number of them. I just didn’t think that even with that it could bring hardware like mine to its knees.

I’ll have to keep a closer eye on this kind of issue next year, so hopefully we can catch it before it ever even becomes an issue.

Thank you to everyone who assisted me.

18

If you are at the Championship in St Louis, drop by the Autodesk booth and we can have a longer discussion on this topic.

19

I’m sorry to say that I won’t be able to make it to St. Louis with the rest of my team due to my job.

20

A couple thoughts come to mind:

  • Try suppressing all constraints (easy to do if you change to Model view at the top of the browser), to see if indeed conflicting constraints are the culprit. If you already have a mix of suppressed constraints and do not want that lost, then either close and do not save once you have investigated, or Undo.

  • LODs should help, but if you are seeing such dramatic performance issues, I do not suspect the memory is a problem.

Also, LODs are designed to respect constraints, even if the component is suppressed, so if the issue is indeed constraints, the LODs will not help.

  • Assembly Features can cause performance issues if used too liberally. Generally I recommend keeping them in subassemblies as best possible, instead of high up in top assemblies.

  • Are you using a Space Mouse? We have seen driver issues in the past, causing just this kind of multi-minute delays.

Regards,
Pete
Autodesk