Urgent help needed! - how to speed up SOL 106 analysis in Nastran 2018? 1

[alan.s]

I am trying to find a way that can significantly reduce analysis time.

Currently it takes about 56s to complete one anlaysis. However, i have over 40,000 bdf files. Each bdf is 16.5mb big. What can i do? It seems that command options like smp and gpuid are not applicable here.

The attached file is one of the bdf file.

Thank you so much in advance

 

[dfreire]

Hello,

Sorry but I could not find the attached file so, without reviewing the model, I can´t say very much. The following ideas maybe could help you:

1.- I am aware that in version 2017, by default, Nastran assigns low amount of memory to the solver. You can check this by searching for 'hicore' in the *.f04 file. It is interesting to increase as much as possible the memory assigned to 'Buffer pool area', so the solver will use less scratch.

2.- Is it possible to reduce the amount of models or to simplify them? I mean, maybe it is interesting to run all the 40,000 (or less) models in linear statics and then apply nonlinearities to these models that seems the worst. For example, if the goal of this analysis is to get the model which presents the higher stress magnitude, you will only need one nonlinear model, so the computacional time should decrease.

I don´t know if this will help you, but if you upload the model I can take a look.

 

[alan.s]

Thank you very much for your reply. Sorry i forgot to paste the file link. Here it is:

https://files.engineering.com/getfi...e=implant_rho_2.000000e-01_element_113292.bdf

The runtime output says that estimated memory is 8g and bpool is 2gb.

i am not sure if i can run only one analysis. The difference between these 40,000 bdf files is in MAT1 card. I assign a specific MAT1 and PSOLID to each element. In this case, i can modify each element's material properties. For example, starting from line 388374, i gradually change each mat1's properties until line 399496.

Another issue that i am facing is large f06 output. Each output is almost 500mb. I am also running out of space.

 

[karachun]

There is no silver bullet but I can give couple of advices.
1) Remesh model with regular hexahedral elements, this should reduce nodes count, but not drammaticaly because you already use linear tetra elements.
2) Try to reduce number of models, first run models with large step in mat properties, analyse results and run detailed steps only in region of interest, if it is possible.
3) Try to include coule of models in one .bdf file. Maybe running many mofels in one large modell will be faster than run many small models sequentially.
4) AFAIK SOL106 dont support parallel computing and can use only one core. If you have acces then try to run this model using SOL400.

 

[dfreire]

I took a look of the bdf file.

For reducing the amount of f06 output data you can set all your outputs as 'plot' instead of 'print', e.g., DISPLACEMENT(PLOT) = ALL. So all the output will be sent only to the results file (xdb, op2, etc).

In order to simplify the model we can do many approaches. In my opinion, change that amount of properties is not worth the effort. It isbetter to define some regions, and then you can define an optimisation analysis which will vary the properties automatically. I mean, it is important to focus in the main objective. In this analysis:
Is any magnitude of stress or displacement limited by some value? This can give you a hint about where it is better to modify the material.
Is it needed a nonlinear analysis for all the models? I ask this because I didn´t find any nonlinear material.

My advice is to simplify the problem, because with a small number of analysis you can get a good result. I hope it helps.

 

[cohoman]

I did a quick scan of your bdf file and I didn't see any obvious non-linear input lines. So, can you explain why you are running SOL106 instead of linear static SOL101?

As mentioned previously, using the PLOT keyword in your output request will definitely speed up the run (since Nastran won't need to write so much data to the f06 file). However, if you need to view your results in the f06 file try to limit it to whatever nodes/elements that you are interested in only (using the SET card).

Finally, if SOL106 is required but your structure isn't deforming much, you might try using an NINC value of 2 instead of the default 10 on the NLPARAM card as such:

NLPARM 1 2 AUTO 5 25 NO

Good Luck!

 

[nlgyro]

I ran your input file (as-is) and the max deflection of your model is 0.00691 units. You ONLY use LGDISP,1 in your SOL 106 analysis so the source of assumed non-linearity is purely geometric. I ran the same file as a SOL 101, and I get the exact same max. deflection of 0.00691 units. The location of the max. deflection being identical.

The question then becomes why SOL106 for your model when it essentially behaves linear?

The linear run on my dinky laptop takes 40sec, but you're screwed either ways as it would still take 40000x40/(3600x24) = ~19 days to run all your files!

If afraid but a change in MAT1 per file as you claim in one of your earlier posts does warrant a separate run per file. So it is the shear number of files that you have to run that is your problem not the run time per file.

 

[ESPcomposites]

If the problem is linear, you might also be able to use MYSTRAN (

http://www.mystran.com

) since the input decks are often interchangeable (depends on what cards you use). Since MYSTRAN is free, you could use it on multiple computers (it may be too expensive to do that with a commercial version of Nastran).

Brian

http://www.structuralfea.com

 

[Payaroshd]

Hi,
You can speed up by several methodes one methode added core proseccore of the system of computer seconde by adedd bufer size of fem in patran analyis soultion options.