2013 crash/extremely slow performance with patterns

[Anonymous]

Hi all,

I have a mech/mfg-necessary pattern set on several parts, to the tune of about 90 slots and 500 holes each. Inventor is absolutely sucking it up handling these parts, and the assembly of these parts together is just a complete nightmare.

I have half-hour load times, constant crashes, and to top it off, they're iparts (used in an iassembly), which means I am constantly having to regenerate the whole part family with every change, a process that can take literally hours. 

What do? 

Are there substitute tricks, or display setting shenanigans I can pull?  All of the features are individually needed somewhere, but no mgf machine needs all of them present at once.

Thanks in advance,

Nate

[Yijiang.Cai]

Could you attach the image or dataset? So that we could have more details for further investigation.

[Anonymous]

It's a ~20GA sheet metal part; bent in a 2ft wide flattened "U" shape like this: |____________|

The shape is about two feet deep. For almost the entire length of the up-bent walls of the "U" there is a 0.060 X 1 IN slot pattern; 2u x 45u on each side:  

_______________________________________

||     ||     ||      ||     ||     ||     ||     ||      ||     ||     ||     |

||     ||     ||      ||     ||     ||     ||     ||      ||     ||     ||     |

------------------------------------------------------------------

This pattern alone is a hassle and considerably delays every operation that requires thier regeneration.  This pattern and the rest of the features are built on the RHS of the part and then mirrored to produce the other side.

After the mirror, there is a set of two hole patterns (i need it staggered) in the floor of the U; 500 holes (22u x 21u) @ approx .2 IN dia.  I can't put the hole patterns ahead of the mirror because they are slightly asymmetrical.

These three patterns together took the part from ~500K to almost 10MB in size and my load/working times from seconds to half-hours. That green bar alternates between frantically moving or just stopping, and Inventor hangs hard for 5-30 minutes. The rest of the system seems only slightly slowed if I windows+D out of inventor.

I'm working off a network drive, no vault.  Machine specs attached.  Side question: in these moments of intense calculation, why does Inventor peak at only 25% CPU usage? 

[Yijiang.Cai]

Based on the details you provided, I created this sheet metal from scratch, and it works fine. No hang or crash is seen. Please see the attached part, and you could try it in your environment. If the part is not the exactly right with your ideas, please update it and send it back to me for further investigation.

I also attach the details about my hardware.

[Anonymous]

That file process super-quickly on my system with no issues, indeed. 

But... I tweaked the file you attached to add a particular proprietary feature, and I got it to blow up again immediately.  The file size shot up to 7+ MB, and inventor chugs for at least five minutes just to compute the interaction of the slot pattern and the proprietary feature I added.  I can't attach anything real, but the bottom line is this: the sides of the "U" are actually wavy, and the slot pattern has to cut through this wavy countour flange.  That's the killer.  I'm not sure if it's the cut distance having to be something other than "thickness", or what. ugh.

I'll attach something crudely representative.

So I'm redrawring the part, with just these two problem-children features.  Inventor built that proprietary-representative counter flange in seconds.  Now I'm starting the initial slot-pattern calculation... it's 9:05.30...

Heh, I'm trying to build even this super-simplified example, and it's taking FOREVER to generate.  To work with these files, I usually end supressing the slot feature until I need it, but it is such a nightmare to supress, and then a much larger nightmare to unsupress.  Also, when I'm working with it supressed, I never know whether or not Inventor is breaking references and things like that along the way; I'll only find out when I try to unsupress the feature later, which is a huge hassle. 

Ok, finished at 9:07.39. That wasn't too bad.  Starting the mirror at 9:08.18...

The real test, and the cause of my initial gripe, is going to be making a change to the part that forces it to recalculate the slot pattern.  which is practically any change at all, since I put the slot pattern at the END, where it is affected by everything, rather than at the beginning where it might now have to be recacluated so frequently.

9:13.30, still calculating.  Here's another question: why does it take so much longer for the mirror than it does for the cut?  would I be better off just manually cutting the opposing side and using parameters to link the cuts together?  The whole point of a mirror is to save time, right?

Ok, done at 9:14 on the dot.  Creating a few simple, random flanges @ 9:15.22 (these are lower in the feature tree than the slot pattern!  why does this take so long?)... 9:16... man, next I'm going to move these flanges ahead of the slot pattern and what this thing just die in a fire... 9:17... 9:21.20, and we're done.  6 minutes, just to flange the part a few times, BENEATH the slots in the tree.  whew. 

Ok, here comes the killer:  Moving the flange ahead of the slott pattern.  Let's do the move...

Oops, before I did that I decided to delete this random work plane left over from the original example part.  clicked "delete" @ 9:22.57...  and Inventor hangs.  This is a great example of the frustration I am feeling: that plane had ZERO effect or relationship to the slots oir to anything else on the part; it was just a random vestigial bit taking up space in the browser.  WHAT IS HAPPENING?  it's 9:25...

"Executing Delete Selections"... no green bar... we're in full, grayed-out screen, (Not Responding) "hang" mode now. 9:27...  I don't know why, but I think Inventor is completely rebuilding the entire part now, basically accomplishing what I wanted to do with moving the flange ahead of the slots.  Done! 9:28.45.  6 minues, again.  Interesting.  

Saving the file to check the filesize... save takes five seconds, filesize 4.4 MB.  I'm going to attach the file in this state because at this level it is still managable and super simple: 

- One wonky U-shaped countour flange

- With a slot pattern on it

- The slot pattern is mirrored across the part

- And a few random flanges. 

The actual part I am working with includes the floor 500-hole pattern and about twice the number of other cuts, faces, and features and is much more precicely interally referenced.  It is also linked to an excel parameter file, and is an iPart using table replace in an iAssembly; you can imagine the pain I am in here, working with this thing.

What I think we should try is to modify the initial contour sketch in some completely minor way to force a rebuild.  If that doesn't work, or if your system blazes through that, then move the flange ahead of the slots, report how long that takes, and then try changing the flange dimensions and see how long THAT takes. 

EDIT: can't attach the file.  too large, and don't want to risk anything anyway.  try the operation I just went through, instead: build a wavy countour flange, and slice it completely with a cut pattern, and manipulate.  shenanigans ensue.

[dgorsman]

On the side issue, I take it you have a quad-core processor and viewing processor use as a single graph?

[Anonymous]

I believe so, yes.

[Anonymous]

does inventor not take advantage of multiple processor cores?

[Anonymous]

Ok, very crude MSPAINT example attached.

[LT.Rusty]

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@Anonymous wrote:
does inventor not take advantage of multiple processor cores?

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Only in a few areas.  Rendering & FEA, most notably.  I hear something about drawing view updates as well, but I've never actually watched the task manager when I'm updating a drawing.

None of the major engineering software packages are completely multithreaded, so it's not just Inventor.

[innovatenate]

Nate,

There are a lot of 'tricks' that you may be able to use to improve Inventor 2013's performance.

Sheet Metal parts require an additional unfoldability check over standard parts for the flat pattern. Unfortunately, slower feature pattern performance can become apparent in a sheet metal part with patterns. However, there are built in options to speed up patterns. For example, faster feature pattern computation is possible with the use Optimize or Identical termination instead of Adjust to Model. Using the 'Cut Across Bend' option in a sheet metal cut can be a resource intensive. How the features are being model and the options in the pattern dialogue can make a big difference.


A sample file would go a long way here to determine which shortcuts may be a good fit.

If the purpose of the part is visual, you may consider using bmp textures with cutouts and overriding the appearance of individual faces instead of modeling the all the geometry. This link is dated, but the concept is still there.
http://inventortrenches.blogspot.co.uk/2011/04/textures-bump-files-and-ral-colors-for.html

Another option is to create the Sheet Metal part as Standard Part. You can then use the derive feature in a sheet metal part to quickly get a flat pattern, as needed at a later time. This may allow you to get around using some of the slower sheet metal features like cut the 'across bend' feature enabled and bypass the flat pattern check. I'm not sure how this would play with a factory table, but thought it was worth mentioning.

Hope this helps.

[Yijiang.Cai]

I recreated this sheet metal using wavy contour flange, please see the attached model. And no hang even crash is seen. Maybe there is a key step missing in the model. Could you update the model and send it back to me for further investigation if you are available?

If you think the size of model is too large to upload, you could move EOP to top to reduce the file size and upload it.