Need advice on managing large assemblies

[cadcoke5]

I am dealing with a very large assembly, which has run into some memory limits in the version of Windows we are using.

I know I can freeze components, such as fasteners by setting a filter in the Hireachy window, and filtering for "screw*" and "washer*", etc, and then freezing them. but, this still leaves a model file that is quite large, since all the components are still there.

I am thinking that one way to deal with this is to first check out a large assembly from the library, and then make all of it a local copy. This is so that I can not just freeze the small fasteners, but delete them entirely from the model file. However, I don't know an easy way to make the entire assembly and all its sub-assemblies a local copy. I know I can manually make a local copy of each one, and rename them as I go. But, since there are so many, I am hoping there is a way to do all of this at once.

Then, the 2nd phase would be to somehow erase all the unused components from the model file.

SolidWorks and Inventor both have a way to make a copy and rename all its components by adding a prefix or suffix automatically. This is all done as one operation. After editing the copy of the assembly another step that can be done is to export that new assembly so that you leave all the orphan components behind.

My main goal is to end up with a smaller assemly. Am I overlooking an easy way to do the same thing in I-Deas?

Thank You,
Joe Dunfee

 

[SDETERS]

Have you looked at using "prune"??

 

[SDETERS]

So before you bring your assembly out of I-deas TDM and or teamcenter you "prune" the parts you do not need. Or Prune all the parts. Then when you bring in you assembly into I-Deas you can unprune the parts you need to work on or with. I also do believe you can view JT representation of the pruned parts. Sorry For double post I hit submit way to soon.

 

[cadcoke5]

Thank you SDETERS, I had looked at pruning a while back, but had eventually dismissed it as a solution, since I thought it required me to choose the items to prune before I get it from the library. Also, since we don't save with facets, I didn't think I could get a visual representation. I was wrong.

I re-evaluated after reading your recommendation, and see that you can prune objects after you have them in your model, and it will show faceted display. I imagine the model file itself is still large, but perhaps it improves other performance issues.

Thanks,
Joe Dunfee

 

[cadcoke5]

I just realized an issue with Pruning. When you create a drawing view, I had read that pruned objects would not display. However, pruned objects see to have to be re-loaded from the library. I just created a drawing, intended to check on some test assembly objects. I just created one view, and am waiting right now as over 1,000 fasteners are re-read from the library. Early lunch break?

I have a theory that CAD systems have a special service intended to benefit the end user. Back when we had to wait for a pen-plotter to view a drawing in detail, we would take long coffee breaks during that waiting period.

Computers are now a few orders of magnatude faster then they were then. So, the programmers put stuf like this in the program, just to restore the coffee breaks!

Joe Dunfee

 

[marcmata]

Hello,
Maybe if you create a JT file from the parts that you aren't working with it will be easier. Add the JT in your assembly with the geometry that you don't really need. If you want to create a Drawing once you have the view create a symbol so you may need it later.
Regards,

 

[IdeasNative]

Try changing your Memory.AutoSetting to 2 in your param file. There is a full explanation of this in the help docs.
You could probably add this to your user param file rather than updating the site param for all users.


! AUTOMATED MEMORY TUNING SWITCH
! ----New in Master Series 7----
! ----Modified in I-deas 8----
! ----Modified in I-deas 12m1----
! If set to 0, turns on Custom Memory Tuning of I-deas.
! If set to 1, turns on Automated Memory Tuning of I-deas.
! If set to 2, turns on Large Address Aware TVM for I-deas.
!
! Automated Memory Tuning was OFF in MS7, but is ON by default since MS8.
!
! Valid settings:
! LAA TVM: 2
! Auto TVM: 1
! Custom TVM: 0
! Default: 1
!
Memory.AutoSetting: 2

 

[cadcoke5]

Thank you IdeasNative... it looks like you are a great source of info. In my case, the limitations of performance dictated by my local machine are only a small part of the problem. Much of it relates to the fact that our data is stored in Europe, and I am in the U.S. And though a local cache exists for stuff I have accessed before, any new large assemblies can take hours to obtain over the network.

I am unclear how pruning effects performance in regards to obtaining parts over the network. The time necessary to un-prune suggests that it is obtaining the parts from Europe. But, it could be that our local network is not ideal for dealing with these large assemblies.

I think the main thing I should focus on is the pruning, since it really takes a bite out of the problem directly. Also, pruning is something I can control, whereas any user parameter changes have to go through someone above my pay scale.

The manual says that pruned parts to not diplay in drawings. In the section labeled, "Pruning and Unpruning Assemblies", it says, "Pruned instances don't appear in the drawing."

I know I can suppress parts in a view buy using the View's advanced properties and the "Suppress Instances" feature. Is this the same as pruning? Might the phrase in the prior paragraph, "Pruned instances don't appear in the drawing." only apply to this "Suppressed instances" sort of suppression?

Thank You,
Joe Dunfee

 

[marcmata]

Hello,

If you prune an object when you unprune it the info needd to be downloaded from the TDM again. So unprune a part will take as if you download it from the library again, maybe only a little less time.

Supress an instance from a drawing is as using supress in a assembly, and the pruned parts are counted also as supressed in a drawing but is not the same. The part supressed is all in the model file, if pruned it needs to be downloaded again from library with unprune.

So, in you case prune will not be a valid solution because you are in US and your server in Europe. I suggest you to download all the assembly and then suppres the parts that you don't really need or create a JT like I suggested before.

Regards,