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speeding up constrain execution

43 REPLIES 43
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Message 1 of 44
eleblanc
1228 Views, 43 Replies

speeding up constrain execution

SO what is everyone say, trick about speeding up constrain execution. I have started working on this new project with 2013. And i'm finding myself losing alot of time. Basicly what i do is insert part from our database or content center and assemble them. So 80% of my activities on inventor are constraints. Right now i have this assemblies 175 / 156(small to me). And executing a constraint is minimum 4 seconds each time. If you consider that about 3 contraint is needed for each piece and final total part will probably be around 1000. i'm losing alot of time here

 

Yeah, i am not using preview. Why is inventor recalculating that much each time? Is it doing a rebuilt after each constraint?

 

What have you done that really increase the excution time of constraints?

 

Workstaion is

Windows 7 64bit

Intel Extreme i7cpu  I975 @ 3,33

12bg ram

4 ssd in Raid stripping.Nvidia FX3800

Inventor 2013 SP1

43 REPLIES 43
Message 21 of 44
SteveMDennis
in reply to: stevec781

So 20% of 400 between 1 and 3 constraints per occurrence... maybe 200 constraints? Seem a good guesstimate?

 

That is actually a lot from my point of view and I see a lot of customer data sets.  Compartmenting into sub assemblies is what most seem to do.

 

"I understand that associaive sketches will impact rebuild time when parts are edited, I just dont get why dragging parts and adding mates are causing rebuilds in unrelated parts"

  Sometimes we have issues but dragging a part that is constrained is a solve. If that solve causes the adaptive sketch to solve that part will become dirty.  Just guessing here since I don't hav ethe data.

 

"Complete rebuild means rebuild all, then save, then save again just be sure 100% sure everything is up to date and saved.  Then rotate the wheel and press save to get supplied screen shot.  The rotate is affecting the other parts."

 

In your original post you didn't mention the saves. Is the wheel constrained?  Then rotating it is a solve and w/o the dataset I can't say whether you have found an issue or not.

 

Can you supply the data?

 

 



Steve Dennis
Sr. Principal Engineer
Inventor
Autodesk, Inc.

Message 22 of 44
stevec781
in reply to: SteveMDennis

Hi Steve

 

Whenever I use derive or associativity I always ground so mates and dragging are not an issue with regard to associativity.

 

So if I understand correctly, when a change is made that affects any mate in assembly A, the the solver will solve every mate in Assembly A.  Is that right?

 

My business is expaning and my boats will be up to 10x longer  so for future projects 200 might be a low estimate so I need to decide if Inv can do the job or not.  I would prefer if it did so I dont have to learn a new program but I must select software that can handle the task.  How do people with assemblies of say 20,000 parts keep the number of mates significantly lower than 200?  What do you consider to be a reasonable number?

 

The wheel has just an insert mate., so it is free to rotate.

 

Post 18, which I thought you were responding to said  "After a complete rebuild and save I rotate the wheel by dragging it"  Perhaps you were replying to the OP and I misinterpreted.

 

I cant send the data but Autodesk is welcome to send someone on site to have a look at it.

 

Message 23 of 44
stevec781
in reply to: stevec781

I just tried supressing every mate in the top level except the steering wheel.  When I rotate the wheel the problem is still the same.

Message 24 of 44
SteveMDennis
in reply to: stevec781

Not every mate will be solved every time...  w/o the dataset I cannot be specific.



Steve Dennis
Sr. Principal Engineer
Inventor
Autodesk, Inc.

Message 25 of 44
eleblanc
in reply to: SteveMDennis

Please spare my thread! Smiley Happy

 

Steve,

 

How can i send you my files?

Message 26 of 44
johnsonshiue
in reply to: SteveMDennis

Hi! Please send me an email so I can set up a secure account for you to upload the files. Or, you can send them directly to me via email if less than 20MB.

Could you try the following for me in the meantime? Go to Tools -> Add-In -> unload Frame Generator. After that, does it become faster?

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 27 of 44
stevec781
in reply to: eleblanc


@eleblanc wrote:

Please spare my thread! Smiley Happy

 


Your thread has been answered by Autodesk in post 21.  You want to mate 1000 parts, so well over 200 mates required which is apparently a problem for their variational solver.  Sadly they wont say how many mates per sub assembly it can handle so just use trial and error.  Good luck with that.

 

Message 28 of 44
johnsonshiue
in reply to: stevec781

Hi! I need a bit clarification here. Could you tell me where you got the information saying 200 mates would siginificantly slow down constraint solving process due to the solver?

I have never heard of a statement like this. Do you have an example showing the behavior?

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 29 of 44
SteveMDennis
in reply to: stevec781


@stevec781 wrote:

@eleblanc wrote:

Please spare my thread! Smiley Happy

 


Your thread has been answered by Autodesk in post 21.  You want to mate 1000 parts, so well over 200 mates required which is apparently a problem for their variational solver.  Sadly they wont say how many mates per sub assembly it can handle so just use trial and error.  Good luck with that.

 


Steve, that is NOT what I said, since you were not forthcoming with an exact number I tried to extrapolate. I do not generally see customer files (and I've seen thousands) have 200 or more at the top level.  It might be a problem, it might be imported data, it might be the way you modeled it, it might be any of dozens of things. Without your dataset I can't solve your issue or even speak to specifics.  I'm sorry if that upsets you. There are no hard and fast rules in any software package this large, ours or the competitors.

 

We are here to help but can't do it based on text in a message board all the time.



Steve Dennis
Sr. Principal Engineer
Inventor
Autodesk, Inc.

Message 30 of 44
stevec781
in reply to: SteveMDennis

Steve I'm not upset.  Here's what you said in post 21.

 

So 20% of 400 between 1 and 3 constraints per occurrence... maybe 200 constraints? Seem a good guesstimate? 

That is actually a lot from my point of view and I see a lot of customer data sets.  Compartmenting into sub assemblies is what most seem to do.

 

So I read that you think 200 mates is a lot for Inventor to handle regardless of anything else.

 

My top level has 104 mates, clearly too many for the type of parts I create, but I am surprised that a 380 part model that has already been broken down into 44 subassemblies still needs to to be broken down ever further. 

 

I dont need to send you the data - I know the answer - for the type of geometry I create and the relationships I need I have to use more sub assemblies with less mates.  But without any knowledge of how inventor thinks I have to use trial and error to see how far I have to break it down, and so will the OP.

Message 31 of 44
machiel.veldkamp
in reply to: eleblanc

So, I see that are working on R:/. Is that a network server or a local disk?


Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.

___________________________
Message 32 of 44

Local SSD

Message 33 of 44

Could you perhaps do a pack and go into a Zip and upload it here?
I'm very curious if I (or someone else) could experience the same issue. 

Did you find this reply helpful ? If so please use the Accept as Solution or Kudos button below.

___________________________
Message 34 of 44

Steve,

 

You said about my comment:

 

     So I read that you think 200 mates is a lot for Inventor to handle regardless of anything else.

 

I think it is more than what I normally see, that is all my statement was directed at. I do not think that is "too many" for Inventor to handle, it is simply more than I see from MOST customers.

 

We have actually found the cause of the original poster's slowdown after he sent the data to Johnson. He had many adaptive sheet metal parts, by turning off the adaptivity the speed increased.  Adaptive parts do not need to be adaptive for eternity as a lot of customers know.  Remember that was one of my first questions for him.

 

You may have a diffferent reason, So if we have the dataset we can make better analysis and help most users.  This is what we do.

 

Steve, I have great pride in Inventor, I have been working on Inventor since before R1, over 14 years now. I have worked in almost every area of Inventor short of the AddIns. It is millions, and millions of lines of code that sometimes interact in unknown ways.  I think I am a very good software engineer and we have a team of people that can address 99% of issues we ever receive, but we can't do it anecdotally.

 

If you can ever send the data (or choose to) please let me know.

 

 

 

 



Steve Dennis
Sr. Principal Engineer
Inventor
Autodesk, Inc.

Message 35 of 44
eleblanc
in reply to: eleblanc

Autodesk look up my assembly and there are 7 parts that uses adaptivity, once adaptivity of those parts disable the executing constraint was instant again.

 

Only 7 adaptive parts!, i think i used to be able to have alot more adaptive parts in a assembly without that much slow down!

 

a assembly wide setting to enable/disable temporarly adaptive parts would probably be a good idea.!

Message 36 of 44
SteveMDennis
in reply to: eleblanc

Eleblanc,

 

 Thanks for sending Johnson your data.  Adaptivity is a powerful feature but as you just discovered it can sometimes affect performance adversely.  I usually use adaptivity in the early stages to get the size/shape correct and then turn it off. You are right that maybe some kind of "valve" command that negates all adaptive instances in one shot would be a nice addition!

 

Adaptivity means the part recomputes once or more to try to satisfy the constraints in the assembly, so the performance of adaptivity at the assembly level is directly related to the complexity of your part(s).  Johnson told me that your parts were sheet metal parts as well, I wonder if when they adaptively recomputed if they were then being unfolded again?

That would also greatly affect the performance.

 

Thanks again for helping us help you.



Steve Dennis
Sr. Principal Engineer
Inventor
Autodesk, Inc.

Message 37 of 44
mrattray
in reply to: SteveMDennis

I don't use adaptivity at all, personally. There's no need for dealing with it when I can do everything I ever need to do by linking parameters and with iLogic.

Mike (not Matt) Rattray

Message 38 of 44
eleblanc
in reply to: SteveMDennis


@SteveMDennis wrote:

Johnson told me that your parts were sheet metal parts as well, I wonder if when they adaptively recomputed if they were then being unfolded again?

That would also greatly affect the performance.

 

Thanks again for helping us help you.



You might be up to something here, yes they are sheet metal. I wonder if they weren't. Would i have the same issue?. for the unfolded again during recompute, i dont now, i guess you would have to go ask the correct person at autodesk in the inventor team?

 

 

Message 39 of 44
eleblanc
in reply to: eleblanc


@eleblanc wrote:
You might be up to something here, yes they are sheet metal. I wonder if they weren't. Would i have the same issue?. for the unfolded again during recompute, i dont now, i guess you would have to go ask the correct person at autodesk in the inventor team?

 

 



I just converted my adaptive parts to solid and it did not change anything.

Message 40 of 44
mrattray
in reply to: eleblanc

You could just delete the flat patterns (don't save so you don't screw up your drawings) as a test.

Mike (not Matt) Rattray

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