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!!!!!!!!!
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!!
Thanks
RE: Questions for the experts!!
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"...
Hope this helps in some way...
Regards
RE: Questions for the experts!!
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!!
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!!
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!!
RE: Questions for the experts!!
RE: Questions for the experts!!
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!!
RE: Questions for the experts!!
RE: Questions for the experts!!
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!!
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!!
RE: Questions for the experts!!
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!!
I wish I could just "submit" my problem and have someone look at it..
RE: Questions for the experts!!
CDWRITE,DB,,, ! Write database information only
Zip CDB file and post to site
RE: Questions for the experts!!
Also, as a result of these modifications i am sucessfully running incore with the DSPARSE solver.
RE: Questions for the experts!!
RE: Questions for the experts!!
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!!
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!!
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!!
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!!
"..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!!
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.
http://my.
http://my.
http://my.
RE: Questions for the experts!!