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

Exporting cdat files using journal file

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

Like Tree1Likes
  • 1 Post By fanch33

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 8, 2018, 10:48
Default Exporting cdat files using journal file
  #1
rku
New Member
 
Join Date: Feb 2018
Posts: 8
Rep Power: 6
rku is on a distinguished road
Hello,

I want to write output of fluent transient simulation in 2 output files:
1. Normal .dat file every 600 seconds.
2. cdat file with selected variables every 2 seconds.

I want to use the journal file as i will be submitting the simulations on a cluster. Could you please tell me what the text inputs for that are? The information that I collected online and found from the journal is as follows:

For file type 1:
/file/auto-save/data-frequency 600
/file/write-data Test.dat.gz

Is that sufficient?


For file type 2 I tried to get the possible commands from the GUI, but I don't know how to translate that to TUI. Example from the text editor of GUI shown below:

/file/transient-export> cfd
CFD-Post Compatible file name [] 'Test.dat.gz'
()
Surfaces(1) [()] (foundation)
(*)
cell zone id/name(1)[*] 1
Invalid cell zone.
cell zone id/name(1)[*] domain-solid
cell zone id/name(2) [()]

CFD-Post Compatible scalar(1)> 1
invalid command [1]
Binary format?, if Binary not chosen, Ascii format is written [no] y
Write Case File Every Time? [yes] n
Export Name ["export-2"] "Test.dat.gz"
Specify Export Frequency [1] 2

Specify the filename append type> timestep
"CFD-Post Compatible"

---------
I'm pretty sure those may be wrong..
Can someone please let me know what the possible text commands would be for saving file type 2?

Cheers.
rku is offline   Reply With Quote

Old   February 8, 2018, 12:08
Default
  #2
Member
 
Join Date: Feb 2015
Posts: 32
Rep Power: 9
fanch33 is on a distinguished road
Hi,

here are my commands if it can help you.

1) automatic save
/file/auto-save/data-frequency 10000
/file/auto-save/case-frequency if-case-is-modified
/file/auto-save/root-name "export.gz"
/file/auto-save/append-file-name-with flow-time 3 ;; don't really remember what this command is for ...
/file/auto-save/retain-most-recent-files y
/file/auto-save/max-files 1 ;; you can save more than one file if you want

2) exporting data for Ensigth

/file/export/ensight-gold export_name
x-velocity
pressure-coefficient
()
yes
* ()
()
no

Hope it helps.
Fanch
rku likes this.
fanch33 is offline   Reply With Quote

Old   February 8, 2018, 14:56
Default
  #3
rku
New Member
 
Join Date: Feb 2018
Posts: 8
Rep Power: 6
rku is on a distinguished road
Thank you so much!
rku is offline   Reply With Quote

Old   February 14, 2020, 09:26
Default
  #4
New Member
 
Amaury jamin
Join Date: Feb 2020
Posts: 2
Rep Power: 0
AGATEN is on a distinguished road
Hello,

I need to run a simulation with the following parameters for transient simulation
time step 0.05s
Max 50 iter/time step
save at every 0.1s
But the problem is witth the autosave data

With this journal file and the two add lines, it's only to save dat file. how to change to save case file also
/file/auto-save/data-frequency 0.1
/file/write-data Test.dat.gz

Would this journal file run, would it work properly

Thank you in advance for your help

EXAMPLE FLUENT JOURNAL FILE FOR TRANSIENT SIMULATION
================================================== ==
; lines beginning with a semicolon are comments

; Read only the input case file:
/file/read-case "FFF-transient-inp.cas.gz"
; In case of a continuation, you need to read both ".cas" and "*.dat":
; /file/read-case-data "FFF-transient-inp.cas.gz"
; ##### settings for Transient simulation : ######
; # Set the magnitude of the (physical) time step (delta-t)
/solve/set/time-step 0.05
; # Set the number of time steps for a transient simulation:
/solve/set/max-iterations-per-time-step 50
; # Set the number of iterations for which convergence monitors are reported:
/solve/set/reporting-interval 1
; ##### End of settings for Transient simulation. ######
; Initialize using the hybrid initialization method:
/solve/initialize/hyb-initialization
; Perform unsteady iterations for a specified number of time steps:
/solve/dual-time-iterate 1000
; write the output (both "FFF-transient-out.cas.gz" and "FFF-transient-out.dat.gz"):
/file/write-case-data "FFF-transient-out.cas.gz"
; write the auto-save backups every 0.1s
/file/auto-save/data-frequency 0.1
/file/write-data "FFF-transient-out.dat.gz"

; Write simulation report to file (optional):
/report/summary y "Report_Transient_Simulation.txt"
; Exit fluent:
exit
AGATEN is offline   Reply With Quote

Old   February 14, 2020, 13:36
Default Command
  #5
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
If you want to save case and data both, modify the command write-data to write-case-data and give the name of only case file. You can also use %i or %t in the name of the file. %i is replaced by iteration number and %t is replaced by time-step
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 19, 2020, 04:45
Default
  #6
New Member
 
Amaury jamin
Join Date: Feb 2020
Posts: 2
Rep Power: 0
AGATEN is on a distinguished road
Hello, thank you for your response.
But can you check my code because I also have to compile and load a UDF.

Best Regards.

EXAMPLE FLUENT JOURNAL FILE FOR TRANSIENT SIMULATION
================================================== ==
; lines beginning with a semicolon are comments
 
; Read only the input case file:
;/file/read-case "FFF-transient-out.cas.gz"
 
 
; In case of a continuation, you need to read both ".cas" and "*.dat":
/file/read-case-data "FFF-transient-out.cas.gz"

UDF :compile and load
===
/define/user-defined/compiled-functions compile libudf yes sourcename.c ""
/define/user-defined/compiled-funcitons load libudf

 
; ##### settings for Transient simulation : ######
; # Set the magnitude of the (physical) time step (delta-t)
/solve/set/time-step 0.05
 
; # Set the number of time steps for a transient simulation:
/solve/set/max-iterations-per-time-step 50
 
; # Set the number of iterations for which convergence monitors are reported:
;/solve/set/reporting-interval 1
; ##### End of settings for Transient simulation. ######
 
; Initialize using the hybrid initialization method:
/solve/initialize/hyb-initialization
; Perform unsteady iterations for a specified number of time steps:
/solve/dual-time-iterate 1000
; write the output (both "FFF-transient-out.cas.gz" and "FFF-transient-out.dat.gz"):
;/file/write-case-data "FFF-transient-out.cas.gz"
; write the auto-save backups every 0.1s
/file/auto-save/data-frequency 0.1
/file/write-case-data "validco2-kepsr-005s-mole-coupled-%t.case.gz"
 
; Write simulation report to file (optional):
:/report/summary y "Report_Transient_Simulation.txt"
; Exit fluent:
exit
AGATEN is offline   Reply With Quote

Old   February 19, 2020, 05:07
Default Two points
  #7
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 34
vinerm will become famous soon enough
I suppose it should run alright. You need to make two changes

1. No need to define solve set max-iterations-per... Rather use full command at solve level like following

solve dti 1000 50

Last number is max-iterations-per-time-step

2. Change .case. to .cas. in the write command
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Reply

Tags
cdat, fluent 18.2, tui

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[swak4Foam] funkyDoCalc with OF2.3 massflow NiFl OpenFOAM Community Contributions 14 November 25, 2020 03:30
[OpenFOAM.org] Error creating ParaView-4.1.0 OpenFOAM 2.3.0 tlcoons OpenFOAM Installation 13 April 20, 2016 17:34
[swak4Foam] build problem swak4Foam OF 2.2.0 mcathela OpenFOAM Community Contributions 14 April 23, 2013 13:59
"parabolicVelocity" in OpenFoam 2.1.0 ? sawyer86 OpenFOAM Running, Solving & CFD 21 February 7, 2012 11:44
Problems in compiling paraview in Suse 10.3 platform chiven OpenFOAM Installation 3 December 1, 2009 07:21


All times are GMT -4. The time now is 14:14.