sol 401 and EMA memory 2

[tstanley320]

I have decided to use sol 401 because of the cohesive elements. It is a model using composites, for studying delamination. I have successfully modelled many 4 bar tests without the cohesive elements and get consistent results that match reality. To run cohesive elements sol 401 is required and the 4 bar test model with cohesive elements, with and without delamination in the model, runs successfully. Now I have made a model of a real part using the same materials and types of elements as used in the 4 bar test. However there are orders of magnitude more elements and nodes, approximately 2 million nodes. My computer has 64 GB of ram and and three solid state drives each with about 1.5 TB of free space. C drive is used for the program and the model, D drive is the scratch directory, and E drive is for the output. I have set aside quite a bit of virtual memory and increased the memory in the preferences. Under the "Nastran Esecutive and Solution Options" there is a place to set the solver memory. Normally I leave this at "0" for "auto" but it gives a fatal error with the large model so I tried entering several values for the memory. Typically there is an information message that reads
"USER INFORMATION MESSAGE 6573 (EMA)
EMA IS USED. INSUFFICIENT MEMORY SPECIFIED FOR EMAINC. INCREASE
THE MEMORY LIMIT BY 16025 MB FOR BETTER PERFORMANCE."
Help doesn't show that particular information message.

My question is what is meant by EMA and EMAINC? If I new this I might be able to allocate the memory so that the model solves. I am not so much concerned about the time it takes, as long as it solves.

 

[tstanley320]

On the advice of Support, I did add the command "system(166)=128" and that helped a bit but didn't solve the problem of lack of memory. I asked about only having 64GB of RAM and they thought it would be OK. I have tried several things to re allocate memory; to no avail. Last night I placed an order for a set of ram sticks with 128 GB with the idea of trying something even if it is wrong. Luckily the price didn't go up until this morning.

I have been hoping Blas Molero, our guru, would reply to this post. I would still like to know what is meant by EMA and what memory it uses. One of the error messages that I get is "if system(166)=128" doesn't resolve the problem call support; which I have done of course.

 

[ThomasH]

Hi
I got a bit curios since I have a vague memory of something similar.

I am looking in the manuals for Simcenter Nastran. You'll find a reference to EMA (Element Matrix Assembler)in the User Guide. And regarding System Cell 166 you'll find some info in the Quick Reference Guide. If the issue is an insufficient core setting 1 may be worth trying. You can also check in the Numerical Methods Guide.

I think your questing more relates to Nastran then to Femap and since your issue relates to SOL401 my reference from Simcenter (NX) Nastran may be completely irrelevant . Perhaps you should repost in the Nastran forum instead.

I my memory is correct, when I had this type of problem some years ago. I had to explicitly define the memory for the solver, it was not enough that is existed on the computer.

Good Luck

Thomas

 

[tstanley320]

Thank you. I will check on the guides you mentioned. If the problem persists I will try reposting in the Nastran Forum.

Tom

 

[nlgyro]

not sure if the OP is still following this thread... but if the OP can post the f04 and the log files from the failed run, it could be of help to debug.

 

[BlasMolero]

Dear TSTANLEY,
A nonlinear model with 2 Million nodes requires more than 64 GB of RAM, I suggest to upgrade your hardware to 128 GB of RAM.
Please note SOL401 supports the sparse direct solver (default), but also the element iterative solver, the PARDISO solver, and the MUMPS solver:

• The DIRECT SPARCE solver is my favourite, is a robust and reliable option, but requires a lot of RAM.

• The ELEMITER solver performs well with solid element-dominated models. It may be a faster choice if lower accuracy is acceptable. For problems involving contact and 3D solid elements, the element iterative solver is generally faster as compared to the sparse direct solver, and you can solve the the 2 M problem with 64 GB RAM sure!!.

• The PARDISO solver is a hybrid direct-iterative solver, potentially faster with larger numbers of cores than the sparse solver but with slightly lower accuracy.

• And the MUMPS solver require less memory than the Pardiso solver.

Also, go to <femap-install-dir>\nastran\conf (in my case C:\Program Files\Siemens\Femap 2021.2\nastran\conf) and edit the file nastran.rcf and make sure to enter the following according the 64 GB RAM available in your computer:

buffsize=65537
$Buffsize=8193 if DOF=100000
$Buffsize=16385 if 100000 < DOF = 100000
$Buffsize=65537 if DOF>400000
memory = 0.55*physical
smem = 20.0X

Test the above settings and let us know how things progress.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[tstanley320]

Thanks

I did install 128 GB ram and that seemed to solve the problem of the memory. My scratch drive has 2 TB. Looking at Blas Molero's post there is still more for me to improve. It looks like I can increase my buffer size and memory in the rcf file. My rcf file looks like this:

Sdir=D:\Scratch
scr=yes
buffsize = 32769
memory = 0.45*physical
smem = 40.0X
buffpool = 20.0X
ishellpath = %NXN_BASE%\bin
msgbell = no
fpe = no
diag = 8
program=FEMAP
SSCR=400GB
SDBALL=400GB

Thanks also for the listing of the available solvers. I have a similar but smaller model with about 335000 nodes and 100000 elements that I can experiment with. Also there is physical testing on that model to judge the accuracy of the results and can try out the various solvers to judge the speed and accuracy.

Currently I am having a problem with my cohesive elements as the load increases. This is the error message:
USER FATAL MESSAGE 4658 (NHEXCZ)
DIFFICULT GEOMETRY PREVENTS FURTHER COMPUTATIONS FOR ELEMENT WITH ID =

The elements seem to be random cohesive elements. The cohesive elements are 8 noded hex elements that have hex elements on each side that have mid side nodes. I suspect that the mid side nodes on these elements may be passing right through the cohesive elements under load. I wanted the mid side nodes to avoid shear locking, but my next step is to eliminate the mid side nodes and see what happens.

Sol 401 with cohesive elements is a steep learning curve.

Thanks for your help.

Tom