Unable to recover NX Nastran result file

[adnanh]

Hi,

I am running a static linear analysis witgh something I imported from Pro/E as .stp file. The model involves pressure loads and simple contraints such as fixation of a surface by method: model -> constraint -> nodal and then a I choose the surfaces which I want to fix.

The pressure load I applied by: model -> load -> on surface and then choosing the surfaces on which I want the pressuro to act.

Nastran runs fine en no errors occur during anaysis, but it does not load the result file. By choosing view -> select I am not able to open any binary result file.

Any suggestions?

Thanx in advance.
Adnan

 

[adnanh]

I forgot to mention that I am using Nx Nastran with FEMAP.

 

[Ronald62]

Is there F06 or OP2 files at all? Those are result files of NX.

Have you tried to analyze a simple cantilever beam case (modeled using beam elements)?

 

[adnanh]

Hi Ronald,

There is a f06 and op2 file. However the results should automatically be loaded after the analysis is completed. I also noticed that the Nastran message window does not say "Boundary conditions applied/Linear static analysis started and completed" Here, obviously something goes wrong. Despite of this, the op2 and f06 are generated but are probably empty as I can not access the binary result file.

I have tried other models (incl. a simple beam) and it workt all fine: after the analysis is completed the results are automatically loaded. Only thing I have to do is go to VIEW menu and click on SELECT and view the results. In these cases I can see in the messages "Boundary conditions applied/Linear static analysis started and completed"

 

[Ronald62]

Hi,

Have you built up the analysis set properly? I especially mean Nastran Output Requests. (Model -> Analysis)

 

[adnanh]

Usually I don't set up anything in Output Requests. I leave it as it is. It usually worked but that's now a different story. I will have a look at the Output Requests, maybe I can adjust something there properly.

Thanks a lot Ronald.

 

[adnanh]

Hi,

The problem I had disapearred when I removed some of the features which do not make a big difference for the structural analysis. This resulted in a reduction from approximately 160000 tetrahedral elements to a rough 90000 elements.

I run Windows XP 32-bit on a machine with following specs:
- CPU: Intel Core 2 Duo E4400
- RAM: 2GB DDR2 667 Mhz
- Swap space enabled: 4000 MB

This is the info I found in the .log file:

Current resource limits:
Physical memory: 2046 MB
Physical memory available: 1627 MB
Paging file size: 4095 MB
Paging file size available: 4095 MB
Virtual memory: 2047 MB
Virtual memory available: 2038 MB

So, 2gb of physical memory a+ an additional 4 gb of swap space seems to be not enough for the analysis of a model with 160000 tets. The number of degrees of freedom for the smaller model is 330000. For the initial model this must have been around 0.6 mln.

What is the limitation on the magnitude of the model NX Nastran can take with these hardware resources combined with a 32-bits OS? Is there a way to tweak around this limit?

I also found that my results are not quite realistic. The thing is that I imported a .stp file in FEMAP with dimensions newtons and mm's while the default in FEMAP is pounds and inches. In order to convert units in FEMAP I specified a multification factor of 25.4 for length and 4.45 for force (1 inch = 25.4mm and 1 pound = 4.45N). But do I also need to specify a factor for pressure or is this autamicalle taken care of with the two other factors (length and force)?????

Many thanks in advance,

Adnan

 

[adnanh]

Correction:

The number of degrees of freedom for the smaller model is 890000 instead of 330000.

So the model that woukd not run must have contained 2 or 3 mln DOF's.

 

[Ronald62]

Hi adnanh,

NX has a poor memory management and this is the reason why you are not able to run big models with your desktop computer. It's interesting to see how 64 bit version works.

You can try to control the memory management by vary the 'memory' value in NAST70 file. The default is 'mem=estimate'.

You can also try to use the iterative solver. Model -> Analysis. In 'NASTRAN Executive and Solution Options' you can select the iterative solver by select Iterative Solver: ON. If you use the iterative solver, you should be careful because it may give wrong results... It's safer to use direct solver instead of iterative but a big model may demand the iterative solver.


About the units: I use SI units. Dimensions are meters, forces are newtons so the stress results are Pascals.

 

[ThomasH]

Hi adnanh

Try the following:

INIT MASTER(S)
$NASTRAN SYSTEM (151)=1
INIT SCRATCH LOGICAL=(SCR(70GB)), SCR300=(SCR300(70GB))
INIT DBALL LOGICAL=(DBALL(70GB))
ASSIGN SCR = './tmp.scr',TEMP
ASSIGN SCR300 = './tmp.scr300',TEMP
ASSIGN DBALL = './tmp.DBALL',TEMP
$DIAG = 44

NASTRAN OP2NEW=0

It is the very beginning of the dat-file that might benefit from some changes.
The 70 GB statement is dependant on yor disk but don't be afraid to set it high. These settings are from one of my old MSC-files but it might work since NX is MSC-based.

Good luck

Thomas

 

[adnanh]

OK, I will try to keep my models small enough to avoid problems with memory menagement. Usually these large models are even not necessary. I may try to change settings which you described, when get a little bit more familiar with the structure of the .dat file and other Nastran files.

About the units:

I don't know how to choose a certain unit system (either SI or English), the only thing I can do is apply multification factors in order to switcch form one system of units to the other. How can choose between systems of units (if possible)?

 

[wvillers]

If you're running NX Nastran 32-bit, you should be able to assign about 1.3GB of RAM on Windows, and maybe 1.5GB on Linux, but not more... With NX Nastran 64-bit, things get much better since you can assign 8GB-10GB easily...

For a model like this, I would definitely use the elemental iterative solver (nastran iter=yes, elemiter=yes). This solver runs in RAM and doesn't need the stiffness matrix to fit in memory (it's a PCG solver), but you will need to assign more memory than estimate thinks you need (mem=1.25GB for instance).

As far as the accuracy of this solver, as it is an iterative solver, it is approaching the solution within a prescribed tolerance (as opposed to the "exact" solution of a sparse matrix solver). The default convergence threshold should be 0.1% on stress IIRC, so I wouldn't worry much about it being "inaccurate". The only thing to remember with iterative solvers is the need for a "well defined" problem, i.e. AUTOSPC,YES will not be active, all rigid body modes need to be constrained or the solver will kick you out.