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

Help using FLUENT in batch mode: script in the Journal file

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 14, 2012, 09:27
Default Help using FLUENT in batch mode: script in the Journal file
  #1
New Member
 
Daniele Obiso
Join Date: Apr 2012
Location: Torino
Posts: 6
Rep Power: 5
danobis is on a distinguished road
Good morning,
i'm starting to use Fluent 12 in batch mode, and i have some problems.
I use an interactive window to submit the batch command, so i think that is right working; anyway i post it here:

bsub -n (number of cores) -q (queue name) -R (resource name) -R rusage[aa_r=1:aa_r_hpc=1:duration=1] -e ./errorfile_%J -o ./outputfile_%J fluent12.sh -ar 3ddp -g -i script_input_jou.txt

I think the problem could be with the journal file; i wrote this command lines:

file read-case-data name_of_case.cas
solve iterate 1500
exit

Is this script right? Another doubt i have is about the journal file extension: .jou or .txt?

Thank you very much!
danobis is offline   Reply With Quote

Old   April 14, 2012, 10:36
Default
  #2
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
danobis, here is a working example of a journal files (.jou), when you see a ";", it means i'm asking fluent to skip that command:

/file/read-case-data /home/maghazlani/Analysis/intake_test_3-1-23000.cas
;/define/operating-conditions/operating-pressure 0
;/define/models/solver/density-based yes
;/define/models/energy yes
;/define/models/viscous/kw yes
;/define/boundary-conditions/modify-zones/zone-type 11 pressure-inlet
;/define/materials/change-create air air yes ideal-gas no no no no no no
;/define/boundary-conditions/pressure-inlet inlet yes no 101325 no 27357 no 300 no yes no no no yes 01 0.05268
;/define/boundary-conditions/modify-zones/zone-type 10 pressure-outlet
;/define/operating-conditions/operating-pressure 0
;/adapt/adapt-to-gradients pressure curvature 0 0.7 0.3 yes 100
;/adapt/set/max-number-cells 2000
;/solve/initialize/compute-defaults/pressure-inlet 11
;/solve/initialize/repair-wall-distance yes
;/solve/initialize/initialize-flow
;/adapt/mark-inout-hex yes no 0.000515079 0.205496 0.0156082 0.0451296 -0.000208354 -0.0265887
;/file/auto-save/data-frequency 20000
;/mesh/polyhedra/convert-domain yes yes
;/solve/set/under-relaxation/k 0.5
;/solve/set/under-relaxation/epsilon 0.5
;/solve/set/under-relaxation/turb-viscosity 0.7
;/solve/set/under-relaxation/solid 0.7
;/solve/set/limits 1 5e10 1 5000 1e-14 1e-20 100000 0.05
/solve/iterate 24000
;/display/set/contours/surfaces 0 ()
;/display/set/picture/color-mode color
;/display/set/picture/driver jpeg
;/display/set/contours/n-contour 99
;/display/set/contours/filled-contours yes
;/display/contour mach-number
;/solve/monitors/surface/set-monitor mass-flow "Mass Flow Rate" 0 () no no yes massf 1000
;/display/views/restore-view left
;/display/views/auto-scale
;/display/views/camera/zoom-camera 2
;/display/save-picture /home/maghazlani/Analysis/screenshot-mach-extended_5-4000.jpeg
/file/write-case-data /home/maghazlani/Analysis/intake_test_3-1-47000.cas
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   April 14, 2012, 10:50
Default
  #3
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
If this doesn't work, problem is from that script that you're using to submit the job. come back to me later to let me know if it works or not
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   April 15, 2012, 04:03
Default
  #4
New Member
 
Daniele Obiso
Join Date: Apr 2012
Location: Torino
Posts: 6
Rep Power: 5
danobis is on a distinguished road
Thanks very much, Ali.
I tried that script you send me, but it doesn't work.
The script i used is:

/file/read-case-data /afs/private/k120mixDDA_SG0lambda21.cas
/solve/iterate 1500
/file/write-case-data /afs/private/k120mixDDA_SG0lambda21.cas
exit

and it gives this errorfile:

nk = 8: Process affinity not being set. Machine is already loaded.
Note: Rank = 6: Process affinity not being set. Machine is already loaded.
Note: Rank = 0: Process affinity not being set. Machine is already loaded.
Note: Rank = 5: Process affinity not being set. Machine is already loaded.

Error: eval: unbound variable
Error Object: 1500

Error: eval: unbound variable
Error Object: /file/write-case-data

Error: eval: unbound variable
Error Object: k120mixdda_sg0lambda21.cas

Error: eval: unbound variable
Error Object: *eof*
danobis is offline   Reply With Quote

Old   April 16, 2012, 09:58
Default
  #5
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
so at that point, you could run fluent right ? usually when i run fluent in parallel i get the error "machine is already loaded" when i try to run fluent in a pc where fluent is already loaded . also for the process affinity problem that comes from your nodes. check the setting in your cluster, make sure the file is not too big too handle, add more nodes if you can. this is what i use to launch fluent :

./fluent 3ddp -gu -i -t42 -ssh < /home/maghazlani/Analysis/test.jou > /home/maghazlani/Analysis/outputfile-test
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 10, 2012, 12:39
Default
  #6
New Member
 
Join Date: Apr 2012
Posts: 7
Rep Power: 5
j01234 is on a distinguished road
Quote:
Originally Posted by diamondx View Post
danobis, here is a working example of a journal files (.jou), when you see a ";", it means i'm asking fluent to skip that command:

/file/read-case-data /home/maghazlani/Analysis/intake_test_3-1-23000.cas
;/define/operating-conditions/operating-pressure 0
;/define/models/solver/density-based yes
;/define/models/energy yes
;/define/models/viscous/kw yes
;/define/boundary-conditions/modify-zones/zone-type 11 pressure-inlet
;/define/materials/change-create air air yes ideal-gas no no no no no no
;/define/boundary-conditions/pressure-inlet inlet yes no 101325 no 27357 no 300 no yes no no no yes 01 0.05268
;/define/boundary-conditions/modify-zones/zone-type 10 pressure-outlet
;/define/operating-conditions/operating-pressure 0
;/adapt/adapt-to-gradients pressure curvature 0 0.7 0.3 yes 100
;/adapt/set/max-number-cells 2000
;/solve/initialize/compute-defaults/pressure-inlet 11
;/solve/initialize/repair-wall-distance yes
;/solve/initialize/initialize-flow
;/adapt/mark-inout-hex yes no 0.000515079 0.205496 0.0156082 0.0451296 -0.000208354 -0.0265887
;/file/auto-save/data-frequency 20000
;/mesh/polyhedra/convert-domain yes yes
;/solve/set/under-relaxation/k 0.5
;/solve/set/under-relaxation/epsilon 0.5
;/solve/set/under-relaxation/turb-viscosity 0.7
;/solve/set/under-relaxation/solid 0.7
;/solve/set/limits 1 5e10 1 5000 1e-14 1e-20 100000 0.05
/solve/iterate 24000
;/display/set/contours/surfaces 0 ()
;/display/set/picture/color-mode color
;/display/set/picture/driver jpeg
;/display/set/contours/n-contour 99
;/display/set/contours/filled-contours yes
;/display/contour mach-number
;/solve/monitors/surface/set-monitor mass-flow "Mass Flow Rate" 0 () no no yes massf 1000
;/display/views/restore-view left
;/display/views/auto-scale
;/display/views/camera/zoom-camera 2
;/display/save-picture /home/maghazlani/Analysis/screenshot-mach-extended_5-4000.jpeg
/file/write-case-data /home/maghazlani/Analysis/intake_test_3-1-47000.cas
Hi diamondx,
I also have some problems with my journal file.
I want to save hardcopys of the contour plot of the phases, (water and air), with 10 levels.
The following is what I have so far. Can you tell me whats wrong?

/display/set/contours/water 0 1
/display/set/picture/color-mode color
/display/set/picture/driver jpeg
/display/set/contours/n-contour 10
/display/set/contours/filled-contours yes
/display/save-picture /xxx/xxx/xxx/xxx/case10_2.jpeg

Thanks!
/Jen
j01234 is offline   Reply With Quote

Old   June 11, 2012, 05:55
Default
  #7
New Member
 
Krzysztof
Join Date: May 2012
Posts: 7
Rep Power: 5
thess is on a distinguished road
Hello,

About journal file I think the extension doesn't really matter. But I'm not sure about end of your script.
I for example used fluent_journal.jou like that:
/file/read-case-data/
name_of_case.cas
/solve/iterate
1000
/file/write-case-data
name_of_case_end.cas
exit
yes
exit
I used it yesterday ant it worked perfectly fine. However I put submission and journal scripts in the root folder so had no issue with filepath.
thess is offline   Reply With Quote

Old   June 11, 2012, 15:36
Default
  #8
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
Quote:
Originally Posted by j01234 View Post
Hi diamondx,
I also have some problems with my journal file.
I want to save hardcopys of the contour plot of the phases, (water and air), with 10 levels.
The following is what I have so far. Can you tell me whats wrong?

/display/set/contours/water 0 1
/display/set/picture/color-mode color
/display/set/picture/driver jpeg
/display/set/contours/n-contour 10
/display/set/contours/filled-contours yes
/display/save-picture /xxx/xxx/xxx/xxx/case10_2.jpeg

Thanks!
/Jen
If you made a copy paste of commands. they have to work without any problem. if not, make sure you are using the right surface number, it's where the issue can lie. when you set up your case on the your pc, check the commands before sending it to the cluster.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 11, 2012, 17:50
Default
  #9
New Member
 
Join Date: Apr 2012
Posts: 7
Rep Power: 5
j01234 is on a distinguished road
Quote:
Originally Posted by diamondx View Post
If you made a copy paste of commands. they have to work without any problem. if not, make sure you are using the right surface number, it's where the issue can lie. when you set up your case on the your pc, check the commands before sending it to the cluster.
Thank you for the tip. I will try. But how can I check the commands in advance?

/Jen
j01234 is offline   Reply With Quote

Old   June 11, 2012, 18:36
Default
  #10
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
you just press enter and start typing in the console command in the bottom right
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx 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
mesh airfoil NACA0012 anand_30 OpenFOAM Meshing & Mesh Conversion 12 December 12, 2011 05:16
Changing the Max level of Refine in a journal file in batch mode (without GUI)? tohid FLUENT 0 April 18, 2011 20:24
BlockMesh FOAM warning gaottino OpenFOAM Native Meshers: blockMesh 7 July 19, 2010 14:11
Problem installing on Ubuntu 9.10 -> 'Cannot open : No such file or directory' mfiandor OpenFOAM Installation 2 January 25, 2010 10:50
OpenFOAM on MinGW crosscompiler hosted on Linux allenzhao OpenFOAM Installation 127 January 30, 2009 20:08


All times are GMT -4. The time now is 05:32.