Cluster utilization - Patching in a combustion model
I am running a series of combustion simulation using Ansys Fluent for which I have been granted access to a cluster to help things along slightly. (Thank god) This is great but I have come up against an issue which I cant seem to find the answer to.
The cluster does not utilise the graphical interface, I interact with it via PuTTy (I believe this is called Fluent in batch mode). I have the commands to load different cases and to examine the data written to the out file. This is grand for cold simulations however for combustion simulations in order to obtain reasonable convergence I have to use the two step process. First iterating the cold solution to convergence and then restarting the case after patching in the premixed model and once again iterating to convergence.
As I see it i have two options, the first is something like:
; Read case file
; Initialize the solution
; Calculate 5000 iterations
;Write a data file
;PATCH IN COMBUSTION MODEL HERE
; Calculate another 50 iterations
; Write another data file
; Exit FLUENT
But I can't work out how the patch command, some sources say you cant do it, some say you can.
Do the cold element on a workstation and then patch in the combustion model using the GUI. What I don't know how to do there is tell Fluent to look at the produced data set for the initial value to start the combustion elements of the simulation. Do I just remove the initialize instructions from my command VI file, does that data carry within the case file I load or do I need to load the data file as well? If so does anyone know how to do that?
Hopefully someone can point me in the right direction
I can help with this ! when you get your coldflow data, say example5000.dat
download it to you workstation, open that data, patch, then save it. put it back to the cluster.
now read the case file, then read that data, of course you have to cancel the line that say initialize !!!
Was I clear ??
It is also possible to patch via TUI COMMAND:
/solve/patch "cellzoneidname" "variable" "value"
Thank you very much for your help, can I just clarify the command for reading the .dat file
I know the command to read the case file is:
I assume that the read .dat file is different?
I managed to get the patch option to work nicely but this would save me a bunch of time re-running the cold element when I'm just trying to fine tune the combustion model!
Thank you very much
read case and data ! I saw your post yesterday. I answered on the bus, guess I lost internet while answering ! Good for you, enjoy
Could I maybe pose one more question on the same theme:
The commonly accepted practice for using a first order upwind scheme seems to be that you should run a second order scheme from the converged results. I tried doing this in batch mode within my journal file and got this:
> ;2nd order scheme
Convective discretization scheme for Momentum (0 1 2 4 6) 
Error: eval: unbound variable
Error Object: /solve/iterate
;Third stage of interations
/solve/iterate 10000 Invalid integer.
The requested scheme is unavailable
It seems to happily switch to the second order scheme (my commands in bold) but then get distinctly unhappy. Would either of you have any thoughts on this? Do I have to reload the old data file even if its in the same journal file and the same run?
It does not switch the scheme. As Fluent says it is expecting an integer. This number sets your discretization scheme. You can find the correct number for 2nd order upwind in the manuals, I don't have it mind now. I think it is one. The correct line should be:
> ;2nd order scheme
Ah, that would do it!
|All times are GMT -4. The time now is 08:33.|