inventor 2013- single user
working with an assembly of about 100 parts
file was working fine until about the last large componet i am working on.
when I edit a part and then hit return the ("excuting end edit componet " in lower left hand ) it seems to take some time to compute. This part i have a lot of sketches that are tide to other componets to create the postion of those. so i think this is the reason. i supressed this compent and the file got about 75% better so I am thinking that this is my issue.
for example when i need to make a cut out in one compent that is overlaying another I create a construction projection of the componet and then use this to off set or create a feature from that so that if I change the other one it changes the cut out. I am thinking the computer is having to figure out what is changing everytime.
out side of this the files are fast. no issue with zoom in out or turning files on off. i tried it in wire frame same issue.
Dale
Maybe someone experienced with very large assemblies could commment on the ponts below.
1. Would reducing the undo size improve preformance for assemblies like this. (reducing undo ability of course)
2. App Options, there are a few check boxes for analizing constraints, etc... Does unchecking them help with large complex assemblies. (see Screenshot)
Always wondered about those settings and preformance.
T.S.
Knowing your systems specs might offer some clues as well, just in case it's a hardware issue and not Inventor.
Chris Benner
Inventor Tube & Pipe, Vault Professional
Cad Tips Tricks & Workarounds | Twitter | LinkedIn
Autodesk University Classes:
Going With The Flow with Inventor Tube and Pipe | Increasing The Volume with Inventor Tube and Pipe | Power of the Autodesk Community | Getting to Know You | Inventor Styles & Standards |Managing Properties with Vault Professional | Vault Configuration | Vault - What is it & Why Do I Need It? | A Little Less Talk - Tube & Pipe Demo | Change Orders & Revisions - Vault, Inventor & AutoCAD | Authoring & Publishing Custom Content
see the attached specs.
when i surpress the 2 larger componets that have alot of of rectangle pattern and projected geometry the file is snappy and quick.
dale
UPDATE
tried to suppress features one at for about 20 and this did not work.
so I started to break the links on each feature. Found one set of 12 cut outs that were link to 12 individual componets. basically a 12 clearance holes for 12 should bolts. I broke these links and the computing time from making an edit or contrainting went from 48 second to about 6 seconds.
it was taking 45 seconds every contraint I try to put on any new componet.. ugh.
not sure why this created such a big deal for inventor but I won't do that again.
not sure this is the fix as it will break more work if i need to go back and move something but for now I can finish
What type of graphics card do you have, and are the drivers all up to date?
Chris Benner
Inventor Tube & Pipe, Vault Professional
Cad Tips Tricks & Workarounds | Twitter | LinkedIn
Autodesk University Classes:
Going With The Flow with Inventor Tube and Pipe | Increasing The Volume with Inventor Tube and Pipe | Power of the Autodesk Community | Getting to Know You | Inventor Styles & Standards |Managing Properties with Vault Professional | Vault Configuration | Vault - What is it & Why Do I Need It? | A Little Less Talk - Tube & Pipe Demo | Change Orders & Revisions - Vault, Inventor & AutoCAD | Authoring & Publishing Custom Content
Hi! The behavior you describe here does not sound right. Have you applied R2013 SP2 to the machine? If not, please apply it and see there is a difference. If it still does not help, could you share the files with me? You can either email me directly (less than 20MB) or I can set up a secure account for you to upload.
Thanks!
How big are the files? If less than or equal to 20MB, please zip up and send it to johnson.shiue@autodesk.com. If larger than 20MB, please send an email to me so I can set up a secure account for you.
Thanks!
Depending on the complexity of shapes, it may take awhile. Also are you using bolted connections in your model?
update:
I think i have narrowed it down.
when I surpress the 2 componets the file is not slow.
Both componets I has as adaptive and have some drive contraints to becaue these are compoents i like to move and see the fit etc.
I turned the apative feature off and the file is back to normal so I think this is my issue in that the adaptive feature combined with all the proecte germerty just needs time to compute where everything is at etc.
I dont' have alot of experience with this and large assemblies but I think i am on to something.
feel free to weigh in on if the adaptive feature hog memory and processing time.
Dale
Mike,
It is not true that adaptive always has to be slower and regular solve. It largely depends on what type of geometry transformation is required to fulfill the assembly constraint solve. I am in the process of understanding this particular case. Once I find some conclusion, I will update this thread.
Many thanks!
Yes, adaptivity can affect performance, especially if it controls the placement of features. Everytime you do an edit, it must check to see if the adaptive part would change, and therefore open up it as well and check through all its constraints as well. Simple adaptivity won't affect it, you just might have a situation where it is difficult for the computer to solve it in this one case. The next assembly with adaptivity may not affect performance at all.
Well, Johnson below was awesome helping me figure this out.
Johnson Shiue (johnson.shiue@autodesk.com)
Principal SQA Engineer, Inventor
Manufacturing Group
Autodesk, Inc
The issue was as follows which came from Johnson
I am finishing my investigation here. The poor performance is probably due to the following reasons.
1) There are 42 adaptive components on the first level. It is a bit extreme in my opinion. I personally do not think these 42 components need to stay adaptive all the time. As long as the driving geometry does not change, there is no need to turn adaptive on.
2) Quite a few adaptive components have more than 10 active adaptive features.
3) Among the 42 adaptive components, only two of them (“lower 3rd form outer.ipt” and “lower 1st form inner.ipt”) have dependency on non-adaptive components. It means the remaining 40 adaptive components have mutually adaptive relationship.
4) Most of Component Patterns depend on adaptive feature pattern.
Indeed, the poor performance seems to be directly related to Adaptive in this particular case. When there are adaptive components, Inventor Assembly Solver is allowed to tweak adaptive geometry in order to fulfill the requested constraints. Adaptive is best suited when there is clear “driver-follower” relationship. When multiple adaptive components have mutually adaptive relationship, the Solver will need to do extra work in order to obtain the result. I personally think the mutually adaptive relationship is the main cause leading to the poor performance. Component Patterns depending on adaptive feature pattern just adds to the complexity but it should not be the main cause.
My suggestion is that you may want to turn off adaptive on the components that will not likely be changed from now on. Leaving them adaptive does not help. Avoid establishing mutually adaptive relationship if possible.
Thanks!
Johnson
I turned them off and i am able to work on this file with out coffee breaks.!
Can't find what you're looking for? Ask the community or share your knowledge.