STAR doesnt finish 2

[ZillionM]

09.22 Dordrecht, The Netherlands

Hi everyone,

Im fairly new to SW (+/-2 years) and am just starting with CW. (v.2008)
After alot of product modeling, im now trying to put them to the test in order to obtain some certificates.
So I invested the necessary loads of hours to prepare my model (21 parts) for the calcs (linear static). Connectors, Mesh controllers, Soft spring, no penetration where set. And after some re-re-re-meshing I was ready for the job.
Im running STAR for 16.5 hours now (over night) and its on 50% of Solving contact constraints..
When I pause and check for warning messages it says there arent any. PC = HP xw4400, Intel Core 2 CPU 6300 @ 1.86 GHz
2 G's RAM

What to do??

thanks in advance,

regards

 

[ZillionM]

btw. my cpu is running on 80% constantly (not that it stopped or anything) Mem usage= 1,3G's

 

[cbrn]

Hi,
what to do? Just wait...
... you don't tell anything about how many DOFs your model has, and how many contact pairs and how many contact elements...
btw, the contact calculation is perhaps the worst thing in CosmosWorks...

Regards

 

[ZillionM]

hi cbrn

thx for the quick reply.
My model has 114640 nodes, 82237 elements and 375192 DOF's
Have one restraint, one force, 13 connectors. Contact is set on global no penetration.
Now, there is some rubber involved coz its a vibration damper. But I created the rubber in state of max displacement, so im avoiding the Large Displacement flag thing. (I want to see behaviour when limiters going to work)
When I stop at 50%, it saves all calculated data.
When I show stress result, it seems like star doing its job.
However, with no penetration set on, a steel limiter plate is penetrating the rubber. Can I avoid that with an extra Contact set? (no penetration » surface-surface)

Another question: Is GeoSTAR same as the STAR.exe which is started when running my study? And if, are the settings in GeoSTAR manager the one of COSMOS STAR?

thx

greets Zillionm

 

[jte]

Zillion-

ROFL... Ok, getting serious... wait... ok... I'm better now.

You are just starting to use FEA and are jumping straight to nonlinear (contact and rubber) problems of multipart assemblies? Quite ambitious.

The problem you are faced with is that you need to keep the number of nodes down around the 25,000 range to get an answer within a few hours. If you can get it down to 10,000, that will be significantly faster still. Otherwise, as you are experiencing, it is quite a chalenging problem for the 'puter to solve. Try a much coarser mesh first, just to see if it gives you an answer. Then start to fine tune the mesh as required and be ready for a long run once you add mesh density. Try to find a mentor to help you out. You are dealing with something which requires years of experience in addition to the courses you may have taken.

I'd guess that what you are seeing as far as the plate penetrating the rubber is a result of not finishing the iterations.

No, GeoStar is not the same as Star. GeoStar is the original pre/post processor for Cosmos. I still use it on occasion when I cannot get SW to do what I need for it to do since GeoStar gives the user the ability to deal with models on a node by node basis when necessary. SW has some huge advantages, but at times I revert back 15 years and just get the job done. Not sure what settings GeoStar manager has but don't think they would directly affect Star. Are you sure you're not running NStar?

jt

 

[cbrn]

Hi,
yes, I think your problem is in the Contacts. You must ensure that the number of system Degrees-of-Freedom is zero. If some bodies are hold in place only by contacts, you must ensure that these contacts effectively restrain the bodies in all the directions. I don't remember the implications of "no penetration" in CosmosWorks, but most probably it won't apply any contact friction and so it won't restrain a body "in-plane" (or tangentially). A surf-to-surf contact will most probably resolve that (the global setting will have to be set to "free").
Star.exe is the executable of one of the solvers CosmosWorks has. It must not be confused with GeoStar, which is an entire FE environment with much more powerful capabilities. Afaik, Cosmos-M also uses Star.exe, but not GeoStar (BUT I'M NOT SURE !!!).

Regards

 

[jte]

cbrn-

Our Cosmos/M package used GeoStar as its pre/post processor at least a couple of years before I started using it in the early 1990's. Star is the basic linear statics solver, NStar is the nonlinear solver, HStar is the thermal solver, etc...

jt

 

[cbrn]

Hi,
thanks Jte for the info. I stopped using Cosmos*** family of products when CosmosWorks was on release 2004, so my memory sometimes plays tricks on me...
In v.2004, CosmosWorks treated the contacts with a VERY DANGEROUS - in my opinion - simplification: it computed contact stiffness at start, then never updated it during the solution. This resulted in the linearization of the problem, alas with materials like rubber I suspect there might be serious problems... I don't know if the algorythms are still behaving like that (which would explain why the linear solver starts...): in this case, final results would have to be examined with EXTREME care and suspicion, but only Zillion will be able to judge if the results make sense or not.
25000 nodes for a solution in a few HOURS seems tremendously unefficient, but as I remember that contacts were a disaster in v.2004, you may be right... Right now I'm running a loadcase of a non-linear analysis with 15 contact pairs and 115200 total elements, and the solution takes about 15 mn on a HP xw4400 PC... OK, the software is not the same...

Regards

 

[ZillionM]

thx for reply guys

Ok, so if im right, I need to glue every single part so that they are restrained in all 3 axis. Big(ger) mesh with big flat surfaces and parts with low priority. Same mesh with parts that matter?
Im running my model overnight, so I've got 15 hours between shifts

I didnt took any course of any kind at all.. so yes, ambitious sounds about right.
Let me put it this way; I find it quite simpel to learn my way through all products of Solid. Much easier that 3DSM for example, yet much more powerfull than AutoCAD.(alltough my colleague disputes it )
I think I can solve this problem in matter of days (have other work 2)
I'll keep you posted

greets Zillionm

 

[ZillionM]

Oh wait.. something is seriously wrong here..

I did a study with 103380 nodes, 68347 elements and 324386 DOF's and it finished in just over an hour.

Ofcourse, after I used 12 pin- and 12 rigid connectors. I need some sort of freedom, so I think the DOF's are necessay (I connected all bonded components in all directions)
Also used 'no penetration' surf-to-surf
The rubber didnt get penetrated at all
The stress results look very good and realistic. The chief confirmed my results and was pleased with them.

But how in the world did my comp accel 15 times in mathematics???

greets Zillionm
(if any want some pics displayed, please let me know)

 

[jte]

ZillionM-

Are you running this in a linear or nonlinear mode?

jt

 

[ZillionM]

jt,

Im running my study in linear mode.

 

[jte]

That explains why its running so quickly. Just keep in mind that rubber is not a linear material nor is contact a linear boundary condition...

jt

 

[ZillionM]

What I've figured out is that it doesnt realy matter how much nodes, elements or dof's I have in a static study. Only thing what matters is how I connect my assembly.
Im running static study cuz I only can run static study (for now) and because I only need static study.
As I explained earlier, I want to see stress in metal parts.
As a matter of fact, I realy dont need the rubber to prove a safety factor of 2 toward my product.
And the displacement hasnt the extent to enable 'large deisplacement'
So for the future months im running static study's on almost all our products.
And after that is accomplished, Im requesting COSMOS professional or advanced professional.
Because it has the ability to replace our expensive vibration/shock damper prototypes.
Anyway, to long way out of topic I guess.
My problems are solved for the moment.
thx guys!

greets ZillionM