×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Questions for the experts!!

Questions for the experts!!

Questions for the experts!!

(OP)
Hi all you expert Ansys users,

I was hoping to get some feedback on one of my models that I am running.  I have a working model, and I am confident in the results.  However, I have many models to run and the run times are quite long (in my opinion).  I was looking for some thoughts, comments, and advice.

I have a very Large Deformation, nonlinear analysis with about a dozen contact pairs.  I have a high level model for rubber (Ogden 3rd order).  There are metalic parts encased in a large rubber boot (as a cable bend stiffener).  The model has about 200,000 elements.  My model takes approximately 2 weeks to solve.  This is my hardware configuration:
2x quad core Xeon 3.2Ghz
32GB RAM (fastest available)
15,000rpm SAS drives in RAID 10 (is that a problem?)

I have the full blown Ansys license.  Available is the HPC license, VT accelerator, SMP, DANSYS, etc.

I currently am using shared memory parallel with 6 processors (I found that 6 is better than using all 8).

Even thought the model *should* fit incore, the pivoting option keeps activating which (I believe) is causing an out of core solution.  For the shared memory Sparse Solver I use the BCSOPTION,,incore.  For DANSYS and the distributed solver I issue the DSPOPTION,,incore command. However this always fails in solution because of the pivoting and exceeding the amount of predicted memory!

Does anyone have input, comments, suggestions, quetions?

Thanks!!!!!!!!!

RE: Questions for the experts!!

(OP)
I also forgot to mention, I keep seeing all the LN files being written, read, etc.  Is it correct that this means it definitely is running out of core?  Those files should never be written to the HDD if it is incore, correct?
Thanks

RE: Questions for the experts!!

Hmmm... strange...
It's not useful to mention that you're using a 64-bits architecture, but which Operating System? Are you sure there isn't some setting of the OS which prevents ANSYS from using a sufficiently large contiguous block of memory?
Try adding the ",performance" key in the BCSOPTION command, this will give you a really verbose output and perhaps it will help you finding your way out...
Also, before launching the solution, exit from Ansys and re-enter by manually setting a "database size" as small as possible, just enough to keep your database file into memory, and a "total workspace memory size" as large as possible.
I know the latest versions of ANSYS generally do a better job than the user in managing mem sizes dynamically, but I found that in some cases it does not.
If it doesn't become unstable because of too strong a non-linearity of the model and because of the materials' constitutive laws, you could also try to solve with one of the most evolved iterative solvers (most obvious is PCG): their memory management is globally far better.
As a "last chance", due to the huge memory you have, you could set up (from the Operating System) a "virtual drive" completely into RAM and run the whole ANSYS from there. I know, it's tremendously uneffective, in normal cases (as the whitepaper from Ansys Inc. correctly explains), but it seems to me that for some reason yours is all but "normal"... winky smile

Hope this helps in some way...

Regards

RE: Questions for the experts!!

(OP)
I was reading through the many papers Ansys has available.  It says that ALL models in which the pivoting option activates are forced to run out-of-core.  It would appear that it has something to do with Ansys not being able to properly estimate the needed memory so it goes to the HD just in case...

Also, i have done the performance option; no useful info really.  I have also set my memory as high as I can and it still goes out of core...

Also, I am running Vista x64 (I know, I know... but according to some benchmarks and stuff I have read, it is no different than XPx64).  I am also using v11.0sp1.

I think I may try that virtual drive thing...

RE: Questions for the experts!!

What type of "pivoting" is going on exactly?  I would consider the following:

1) Do you have an overly constrained model?
2) Can you substructure part of the model?
3) Perhaps the AMG solver is faster in this case?

I would look at the NLDIAG command and see if any of the outputs can be of help to you.  Also, posting a snippet of your output would allow forum users to make better suggestions as well.

RE: Questions for the experts!!

(OP)
Thanks for the response.  I am near certain that I do not have an over constrained model.  
Also, I am unfamiliar with substructuring.  
I forgot to enable file output this time, so i had to take a screenshot of the output window.  Please check that to see if there is anything strange going on.   

RE: Questions for the experts!!

Without seeing the entire output file it's hard to say what you could do to speed things up.  Are you truly utilizing your HPC capabilities.  Your output indicates that your stiffness matrix is unsymmetric.  I don't think the unsymmetric solver within Ansys is multi-threaded.  Is your problem ill conditioned?  Do you get element shape warnings?

RE: Questions for the experts!!

(OP)
I do get some element shape warnings.  88 of about 250,000 elements violate SWL... I didnt think it was a problem since its so few.  Yes, my system matrix is unsymmetric (which i set for the contact).  I have found that unsymmetric yields better convergence... Does it really matter? If my problem is ill-conditioned, I dont know how to make it better.  I really thought about the simulation and how to define boundaries and loads.  I do have a decent amount of contact pairs though and a few different hyperelastic materials.  


For this analysis, i am using the sparse direct solver (not the distributed).  I am running in a SMP mode also.  I do not seem to have the parallel performance module installed (or the license is MIA... I have to check).   

RE: Questions for the experts!!

(OP)
Stupid question... I have the mechhpc license.. do I need something else to use the AMG solver?  It isnt even listed as a solver in the solution controls area.  I have distributed sparse, but not AMG or any of the others...

RE: Questions for the experts!!

(OP)
And how do I change the matrix to symmetric?  Sorry for the simple questions...  

RE: Questions for the experts!!

You need to have Distributed Ansys installed.

Issue the following:

/SOLU
EQSLV,AMG
NROPT,FULL

I don't know why you would need to use an unsymmetric solver.  I don't see your problem as being highly path dependent...but I could be wrong.

RE: Questions for the experts!!

(OP)
I got the AMG solver (I actually am a moron because I did know how to activate it I just forgot...) Anyways though, how do I make the problem symmetric?  When i initialize the solution, it says
   GLOBALLY ASSEMBLED MATRIX . . . . . . . . . . .UNSYMMETRIC
which I assume needs to be symmetric.  I have the friction stiffness matrix set as symmetric (is this what I am looking for?) Thanks
 

RE: Questions for the experts!!

(OP)
OK, i got that symmetric thing fixed.  However it turns out i cant use AMG anyways... i get an error that it cant be used with 180 series elements with mixed u-p formulations so it switches to the distributed sparse instead.  I can can post my output later if need be.  I will cross my fingers with this analysis! Thanks

RE: Questions for the experts!!

Friction is not always a symmetric phenomenon.  Do you REALLY need friction in this model?  Friction typically takes 1.5X the number of iterations to converge vs. without.  Another option you may want to consider if needed is the "rough" contact behavior if you want no slippage to occur between two parts.  I would be skeptical of the stress at the surface where this behavior occurs if used however. Beware of that.

Have you been to an Ansys nonlinear or contact class?  If not and you feel it'd be beneficial I'm sure you could make a case to your manager based on this experience alone and the # of hours it could have potentially save you.

RE: Questions for the experts!!

(OP)
Well i decided that i didnt REALLY need friction so I removed it.  However its worse converging now!  I dont understand really.  I get good convergence with my old model which ran on the sparse solver out of core.  It took forever, but it always converged fast.  Now I get very fast iterations, but terrible convergence.  

I wish I could just "submit" my problem and have someone look at it..

RE: Questions for the experts!!

If there is no IP constraints from allowing you to do so then upload it here.  I'd be more than willing to take a look at it over lunch sometime.  If posting for the public IS a problem then I'd recommend consulting your ASD.  To obtain maximum file compression I would do the following:

CDWRITE,DB,,,          ! Write database information only

Zip CDB file and post to site

RE: Questions for the experts!!

(OP)
Thank you so much.  I am modifying a few parameters right now.  I believe my problems have to do with my cotnact, specifically the stiffness factors.  I am running a solution now with low (0.01) factors and I am achieving quick convergence.  When it is done I will check the results and adjust the factor.

Also, as a result of these modifications i am sucessfully running incore with the DSPARSE solver.

RE: Questions for the experts!!

Be careful when adjusting contact stiffness.  You may see excessive contact penetration with such a low normal stiffness.  If you feel excessive contact stiffness may be your problem in the first load step set keyopt 9 = 2 or 4 for the contact elements.  This ramps stiffness and aids in convergence.

RE: Questions for the experts!!

Hi,
in addition, if problem is convergence and not calculation speed "per-iteration", then you'd better check that you do have "adjust contact stiffness -> at each equilibrium iteration" set.
If not, then the contact stiffness is evaluated at the beginning of the substep's solution and never updated through the equilibrium iterations, which can easily be a severe problem with hyperelastic materials.

In addition to Stringmaker's comment, sometimes I've achieved good results with low initial stiffness factor, strict penetration tolerance, and update at each equilibrium iteration. In this case, however, you may check that you don't spend too many iterations in order to respect the penetration tolerance ( = warning "XXX elements have too much penetration" in the solver output file, after the equilibrium iteration).

Regards

RE: Questions for the experts!!

(OP)
Thanks, I actually am having convergence difficulties.  (I said I got convergence yesterday but I lied b/c I forgot to apply my load haha).. anyways, what keeps happening is the solution oscillates.  My criterion and forced convergence value seem to move in unison.  I will try the update at each equlibrium iteration.  I have really simplified my model, and glued many volumes together (which i origonally had as bonded contact).  I am using solid 186 elements (alot of memory requirments) so I am going to change to solid 185.  

I also have a low level neo-hookean model for polyethelene.  It is not very critical and I do not need a complex model.  however I know neohookean can become unstable in certain situations.  My data is just uniaxial tension.
Thanks guys!

RE: Questions for the experts!!

Hi qwicker,

to get back to your initial question i.e.
'why did the Sparse solver not solve in-core'.

I did check your output1.jpg:

at least at that attempt to run the job
you got less RAM available then required for in-core
(excerpt reported in attachment).

Why your box started out at "only" 24 o/o 32GB RAM
at that instant is another matter. Appears as if other apps
occupied (32GB - 24GB avail - 2GB say_for_OS) say 6GB of
your RAM. 24GB were just low to fit the model in-core.

Free some additional RAM.

Hope that helps.

Frank Exius
IFE Deutschland
www.ife-ansys.de
Germany
 

RE: Questions for the experts!!

(OP)
IfeGermany,
That was the issue I was getting with the pivoting option.  The initial memory requirement was only 22GB but then it would change every step varying as much as 3GB so I could never properly predict the memory.  It always went out of core.

However though, I have rebuilt my model and glued many volumes instead of using contact pairs.  I also am now using the symmetric solver instead of unsymm.  My issue is no longer incore as I have achieved that with the DSPARSE.  I am now playing with the contact parameters (stiffness).  I also have the update each iteration (PAIR based) as well as the augmented lagrange formulation.  My model is much smaller now and more efficient.  However the tradeoff seems to be that the contact parameters have to be properly adjusted.  I always get the below warning.  I have the stiffness factor set at 0.05

*** WARNING ***                         CP =      44.928   TIME= 12:06:22
 The default contact stiffness used for contact pair identified by real
 constant set 16 is affected by defined inelastic material properties,  
 even if the material properties are inactive.  You shoud confirm that  
 the appropriate contact stiffness was used.
 

RE: Questions for the experts!!

qwicker,

"..affected by defined inelastic material properties.."
ANSYS reduces the stiffness to a factor of 1/100 if
plasticity is present, if I recall ok.

Check with Contact Guide - if this applies only if plasticity is actually present,
or if the sole definition of the plasticity law is sufficient to trigger this.


P.S. wrt xSPARSE I'd leave BCSOPTION resp. DSPOPTION to default parameter values.
At times I used manual memory setup -m -db instead of automatic RAM allocation.

Frank Exius
IFE Deutschland

RE: Questions for the experts!!

(OP)
Hi Stringmaker et al,

I have uploaded my database as you suggested.  I have really troubleshooted this to death.  I have removed components and gotten convergence, I just cannot get it when the entire model is assembled.  I really appreciate you taking a look when you have a moment.
Unfortunately I was having issues uploading the file as 1 piece so I had to break it up into 4 RAR files.  Please just save them all in the same location and unzip the first part to remake the .cdb file.

Thanks so much!

http://my.engineering.com/pg/file/Qwicker/read/173994/ansys1
http://my.engineering.com/pg/file/Qwicker/read/173995/ansys2
http://my.engineering.com/pg/file/Qwicker/read/173996/ansys3
http://my.engineering.com/pg/file/Qwicker/read/173997/ansys4

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources