CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Cluster utilization - Patching in a combustion model

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 8, 2014, 09:26
Default Cluster utilization - Patching in a combustion model
  #1
Member
 
Mark
Join Date: Feb 2013
Location: London
Posts: 33
Rep Power: 3
M_Tidswell is on a distinguished road
Dear All

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
rc example.cas
; Initialize the solution
/solve/initialize/initialize-flow
; Calculate 5000 iterations
it 5000
;Write a data file
wd example5000.dat
;PATCH IN COMBUSTION MODEL HERE
??????????

; Calculate another 50 iterations
it 5000
; Write another data file
wd example10000.dat
; Exit FLUENT
exit
yes

But I can't work out how the patch command, some sources say you cant do it, some say you can.

Or:

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

Thank you!

Last edited by M_Tidswell; January 8, 2014 at 10:00. Reason: Added clarity
M_Tidswell is offline   Reply With Quote

Old   January 10, 2014, 13:04
Default
  #2
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,218
Blog Entries: 22
Rep Power: 18
diamondx will become famous soon enough
Send a message via MSN to diamondx
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 ??
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   January 10, 2014, 13:07
Default
  #3
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,218
Blog Entries: 22
Rep Power: 18
diamondx will become famous soon enough
Send a message via MSN to diamondx
It is also possible to patch via TUI COMMAND:

/solve/patch "cellzoneidname" "variable" "value"
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   January 11, 2014, 13:41
Default
  #4
Member
 
Mark
Join Date: Feb 2013
Location: London
Posts: 33
Rep Power: 3
M_Tidswell is on a distinguished road
Hi

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:

rc /home/k0955535/ANSYS/Mark/Fluent-HPC-Test-1-7.cas

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

Mark
M_Tidswell is offline   Reply With Quote

Old   January 12, 2014, 21:12
Default
  #5
kad
Senior Member
 
Join Date: Feb 2013
Location: Germany
Posts: 152
Rep Power: 12
kad will become famous soon enoughkad will become famous soon enough
Quote:
Originally Posted by M_Tidswell View Post
Hi

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:

rc /home/k0955535/ANSYS/Mark/Fluent-HPC-Test-1-7.cas

I assume that the read .dat file is different?

Mark
Suprisingly it is "rd". Now guess what "rcd" does.
kad is offline   Reply With Quote

Old   January 12, 2014, 21:39
Default
  #6
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,218
Blog Entries: 22
Rep Power: 18
diamondx will become famous soon enough
Send a message via MSN to diamondx
read case and data ! I saw your post yesterday. I answered on the bus, guess I lost internet while answering ! Good for you, enjoy
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   January 14, 2014, 08:18
Default
  #7
Member
 
Mark
Join Date: Feb 2013
Location: London
Posts: 33
Rep Power: 3
M_Tidswell is on a distinguished road
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
/solve/set/discretization-scheme/mom
Convective discretization scheme for Momentum (0 1 2 4 6) [0]
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?

Many thanks

Mark
M_Tidswell is offline   Reply With Quote

Old   January 14, 2014, 09:04
Default
  #8
kad
Senior Member
 
Join Date: Feb 2013
Location: Germany
Posts: 152
Rep Power: 12
kad will become famous soon enoughkad will become famous soon enough
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
/solve/set/discretization-scheme/mom 1
kad is offline   Reply With Quote

Old   January 14, 2014, 09:52
Default
  #9
Member
 
Mark
Join Date: Feb 2013
Location: London
Posts: 33
Rep Power: 3
M_Tidswell is on a distinguished road
Ah, that would do it!

Many thanks
M_Tidswell is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Liquid rocket engine non-premixed combustion model Erik FLUENT 2 November 28, 2013 14:09
eddy dissipation model: combustion doesn't occur roukaia FLUENT 0 December 25, 2011 13:50
eddy dissipation model: combustion doesn't occur roukaia FLUENT 0 December 24, 2011 09:10
Combustion Model for CAI/HCCI - AVL FIRE Patryk Main CFD Forum 0 July 24, 2009 16:43
combustion model Hennie van der Westhuizen CD-adapco 7 February 27, 2002 02:10


All times are GMT -4. The time now is 01:25.