Does size matter? - Drawing/Assembly limitations

[David_L]

Hi All!l



I have heard from users within this company and others, stating that they are unable to work with DRAWINGS of assemblies that exceed 3000 parts and that to work around this problem they have been exporting the drawing to AutoCAD for detailing. They indicated that they are running IV7 on current dual processor machines with a Gb of RAM and a decent video card. I have also heard from companies creating assemblies with greater than 3000 parts, without issues at all.


Because the large assembly performance issue has come up on multiple occasions and is now becoming an major issue within our organization, I’m looking to sponsor a thread that will help myself and others learn more about the capability of the Inventor and it’s limitations or lack thereof. The following list of questions is meant as a seed for conversation in hopes to get a dialog started. Please feel free to add new items for consideration or suggest additional ways in which to review large assembly performance. Without question, suggestions on how to improve performace are always welcome!


One tip that was shared with me that I thought useful was that on large assemblies it may be worth considering enabling the DEFER UPDATES option beneath the drawing environment's document settings.




Questions to start with:


What version of Inventor (and what service pack) are you using to create drawings of large assemblies?




What operating system are you running and at what service pack?




How large is the largest assembly that you have created drawings from, both in MB of the overall assembly and quantity of parts?




How large is too large?




If you are regularly working with large assemblies are you creating derived parts of the sub-assemblies and then breaking the links? Does breaking the link cause problems down the road when wanting to change the derived assembly? Does it significanlty improve performance?




Are you working with complex shapes (fillets, curves, splines, surfaces, etc.) or is it pretty much just dumb steel?




What is your hardware makeup (CPU type and size, duals?, RAM, video card, etc.),




Are you working off of a network drive?




Are you working in a shared, semi-shared or isolated user environment?





Anything else?






Thanks for your input!!!


David

[Anonymous]

Don't mean to burst your bubble, but this may not turn into a huge thread. Mostly because a lot of your issues and questions have been addressed in detail on this newsgroup with a fair amount of frequency.

I'd recommend doing some searching through the newsgroup with various search topics.

I'll try to sum up what I expect you'll learn....

I don't think versioning and service packs will have very much impact on drawing performance. I've heard there are some improvements to drawing performance in the next release (8), but that remains to be seen.

As you've probably surmised, "large" in the assembly environment and "large" in drawing manager are different. I've been able to create a several-thousand part assy, but IV choked on the drawing view. This is mostly a RAM issue. Search on 3 MB switch in this newsgroup and on the internet in general for some tips on utilizing more RAM. And yes, you'll probably find that you need to buy more.

Breaking the link basically means you're abandoning the parent, and edits will become problematic. I believe that this process does increase capacity slightly, but not significantly enough to give up the editing capability.

The problems I've described above were with relatively simple shapes. Complex shapes will contribute to the problem though.

I think you'll find that the root of your problem is RAM and your OS's ability to leverage all of that RAM that you have. Processor and Video card are important factors, however.

Working across a network will also contribute to this problem. You might want to try working in semi-isolated mode, running a pack-and-go to get everything local, or install and try the vault and see if that helps any.

My blanket recommendation is get 3 GB ram, Windows XP and create your drawing views with all of your non-library part and assembly files local.

Hope that helps.
-Allen

[Anonymous]

>I don't think versioning and service packs will have very much impact
>on drawing performance.

This is not the case.

Bugs have and do exist that directly and adversely affect idw performance.
These bugs have: existed from the start; surfaced over time as other
features have been added (in new releases); or surfaced over time as other
bugs have been fixed (in service packs). It's a house of cards really.

Some users encounter these bugs and others don't because: the bugs have
triggers and unless certain steps are traced the trigger isn't pulled; the
performance degredation is proportional to the model size being documented.

The best idw performance I can recall was in 5.3 but that release was
inflicted by another crippling bug in the assembly environment rendering the
release useless. This assembly environment bug was fixed in 6 but a new bug
was introduced in 6 (or 6sp1, I'm not sure which) that adversely affects the
idw environment. This bug has existed since.

There will be those who disagree with my statements and to those I say....
ignorance is bliss.

Dave

[Anonymous]

Yeah, you're right. I didn't mean to gloss over that aspect. I agree that drawing performance was excellent in 5.3, but reverting back to a release that's 2 (almost 3) versions old isn't a viable option.

Basically, just stay up-to-date with service packs.

[Anonymous]

>Basically, just stay up-to-date with service packs.

I'm not sure this advice should always apply. Rather, (on a case-by-case
basis) if a particular release or service pack works for you then don't "fix
it". However, never have I been satisfied and never has the product (in our
case) not been in need of "fixin'" at any release level.

With respect to downgrading, even if it made technical sense the EULA
prevents one from doing so.

Dave

[Anonymous]

The latest EULA allows you to keep the previous version. 5.3 was light years ahead of 6 in drawing performance. 7 is much better than 6. What surprised me is that a video card upgrade has a very very very drastic impact in drawings for me. Not in view generation, in annotation. Upgrading my video card made selection and dragging tolerable, which it wasn't even on a brick with my Wildcat 4110.



I think you've gotten some good advice here. Keep in mind drafted filleted arrayed parts are nasty critters. A 1000 piece assembly of molded parts can be much worse than 5000 sheetmetal and machined parts. Also keep in mind, if you hard drive is spinning during an operation you need more ram. If all is quiet and you have the hour glass you need more processor. For that, Intel w/ 800 FSB bus rules. Until the Sledgehammer is ready for primetime anyway.

[David_L]

No bubbles here, just looking for information! Your reply was great and provided much useful information.



It would be helpful to know how many parts was "several thousand"?

When IV choked on the IDW, were you able to work past it? If not, what was the solution? Where you running with 3gb at the time?



I'll jump up to 3Gb and apply the /3Gb switch, however I have heard of network issues when doing so. I've done several searches looking for this information with varying results, thanks for your input. I would love to hear more!


David

[Anonymous]

Hard to say on the total part count. I'd guess that it was 4000+ including hardware.

At the time (5 months ago), I was on Win2000 w/ 1.5 GB and simply COULD NOT make a drawing view with R7 (that was with all parts local as well).

My work-around to get my top-level drawing created wasn't pretty, but let me just say it involved a much-less sophisticated Autodesk product.

Depending on what your timeline is and if you're on subscription, I would certainly be interested in how R8 improves drrawing view creation. Other than that, you're on the right track.

[Anonymous]

Hi,

I spoke to David in a private email.

The bug he is referring to was actually introduced in R6SP2. This bug
caused terrible open performance issues in idw files. We have supplied a
patch for this that fixes this problem for R7 SP1.

If you encounter open performance issues with idw files, please download
this patch. Some users are not seeing a noticeable improvement, but many
are.

Regards,

--
Chuck Savatsky
Inventor Drawing Manager Software Development Manager
Chuck.Savatsky@Autodesk.com
"David Radlin" wrote in message
news:EA034BEB98F202CB9442EF391A7A3BD2@in.WebX.maYIadrTaRb...
> >I don't think versioning and service packs will have very much impact
> >on drawing performance.
>
> This is not the case.
>
> Bugs have and do exist that directly and adversely affect idw performance.
> These bugs have: existed from the start; surfaced over time as other
> features have been added (in new releases); or surfaced over time as other
> bugs have been fixed (in service packs). It's a house of cards really.
>
> Some users encounter these bugs and others don't because: the bugs have
> triggers and unless certain steps are traced the trigger isn't pulled; the
> performance degredation is proportional to the model size being
documented.
>
> The best idw performance I can recall was in 5.3 but that release was
> inflicted by another crippling bug in the assembly environment rendering
the
> release useless. This assembly environment bug was fixed in 6 but a new
bug
> was introduced in 6 (or 6sp1, I'm not sure which) that adversely affects
the
> idw environment. This bug has existed since.
>
> There will be those who disagree with my statements and to those I say....
> ignorance is bliss.
>
> Dave
>
>

[David_L]

I really appreciate your input, Thank You.


You aren't the only one that has used the solution you elude to, I have heard of others as well. Which is why I addressed the problem with our Autodesk AE. I'm looking forward to IV8, there's lots of hype about it and I'm anxious to see how it will resolve our current needs.


Our Autodesk AE suggested that we utilize Design Views throughout the assembly process to prevent hidden and non-essential content from being presented and calculated in the next assembly up (visibility off). If components won’t be visible, why tax the computer with it? Sounds simple, but it got me wondering if everyone/anyone is using this technique, and what their success has been. By developing assemblies using this technique IV users should benefit from increased hardware performance on ALL assemblies, not just large ones. It was stated that 40,000+ part assemblies, with 5,000 unique parts have been opened on a notebook. Yow! I question the many IV users in this forum that are working with large assemblies, and are concerned with their hardware performance; have you tried this…does it work for you? I have been trained to derive sub-assemblies and use the derived parts in upper assemblies, how do these two techniques compare in large assembly management?


When would I use derived sub-assemblies vs. Design View controlled sub-assemblies?

Which is the better solution?

Has everyone been using these techniques? Anyone?....Buhler?……..





Thanks Again!
David

[Anonymous]

Design views are the only way to go with real large assemblies. PTC used something called simplified reps to do this. Well I think thats what they called it, been a long time. It took it one step further in that you could control part feature supression, not just part features but PTC users got used to managing large assemblies this way. I think IV users need to start using these new tools more as well.

[Anonymous]

Definately a commanding use of design views is
required in any attempt to document a modestly complex assembly.  We use
design views extensively however in spite of this they provide only limited
remedy.

There are just WAY TOO MANY HIDDEN
LINES generated on a view of any assembly of even modest complexity. 
It is impractical in most cases to ever turn them on and thus it is
impossible or impractical to create proper
(coherent) documention.

There is a DIRE NEED for some means of
controlling hidden edge display in idw views.  As of current it is
basically display all or none.  This is a high priority need if we are ever
going to work with modest efficiency in documenting assemblies.

Bite, my tounge but I like the way
SOLIDWORKS DOES IT - there you can suppress hidden line generation in
drawing views on a BY-PART or BY-FEATURE basis.

A solution is LONG OVERDUE from
Autodesk.

Dave

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"rllthomas" <
href="mailto:rllthomas@attbi.com">rllthomas@attbi.com> wrote in message

href="news:f190a5e.9@WebX.maYIadrTaRb">news:f190a5e.9@WebX.maYIadrTaRb...

Design
views are the only way to go with real large assemblies. PTC used something
called simplified reps to do this. Well I think thats what they called it,
been a long time. It took it one step further in that you could control part
feature supression, not just part features but PTC users got used to managing
large assemblies this way. I think IV users need to start using these new
tools more as well.