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

can not continue running simulation with trn file

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

Like Tree2Likes
  • 1 Post By Lance
  • 1 Post By Opaque

Reply
 
LinkBack Thread Tools Display Modes
Old   September 14, 2016, 12:14
Post can not continue running simulation with trn file
  #1
mao
New Member
 
mao
Join Date: Mar 2016
Posts: 17
Rep Power: 3
mao is on a distinguished road
hello,i am now running one simulation in cluster, i stooped in the middle and have a file.trn(finished 2000steps), i wanna start with this file to finish another 1500steps, however, the new simulation starts from beggining(0step) instead of the file.trn(2000steps), hope someone can give some suggestions, thank you very much.
mao is offline   Reply With Quote

Old   September 14, 2016, 16:26
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 717
Rep Power: 15
Opaque is on a distinguished road
Can you describe how you are restarting the simulation ? Either from the command line (cfx5solve), or the steps you are following in the ANSYS CFX Solver Manager
Opaque is offline   Reply With Quote

Old   September 15, 2016, 04:32
Default
  #3
mao
New Member
 
mao
Join Date: Mar 2016
Posts: 17
Rep Power: 3
mao is on a distinguished road
hi,opaque, thanks for your kind reply.following are some details about my simulation.
1,i have an unsteady simulation,totaltime=8s,
2.first stage. i have to stop at t=2s due to some reasons, then we have some trn files(let us call the last trn file as 2.trn).
3.second stage, i should regard 2.trn as initial file in the second simulation, and then keep going the next 6 seconds.
4.in the first simulation,totaltime=2s, whereas it equals 8s in the second simulation,
5,in normal computer or severs, i can choose "continue history from" in solver define run. but now i have to use cluster where i give a command file whiched showed in 6, either i start from bak file or trn file, the second simulation starts from 0 second rather than 2 second.
6.
#!/bin/bash -l
#PBS -N XiuliSimulation
#PBS -l nodes=2pn=16:NRM
#PBS -l walltime=999:00:00

SIMNAME=casoCFX
export SIMNAME
ANSYSLMD_LICENSE_FILE=1055@147.162.153.181
export ANSYSLMD_LICENSE_FILE
ANSYSLI_SERVERS=2325@147.162.153.181
export ANSYSLI_SERVERS

cd $PBS_O_WORKDIR
#mkdir /usr/data/$SIMNAME/
#cp -R * /usr/data/$SIMNAME/
#cd /usr/data/$SIMNAME/

nodes=`cat $PBS_NODEFILE`
nodes=`echo $nodes | sed -e 's/ /,/g'`

# con initial file
/opt/ansys/v161/CFX/bin/cfx5solve -double -initial-file /home/wissam/xiuli/foldername/filename.trn -def /home/wissam/xiuli/foldername/filename.def -par-dist $nodes -sizepar 1.1 -size 1.1

# senza initial file
# /opt/ansys/v161/CFX/bin/cfx5solve -def /home/wissam/christian/td600_unsteady/td600_unsteady.def -par-dist $nodes -sizepar 1.1 -size 1.1


#mv /usr/data/$SIMNAME/* $PBS_O_WORKDIR
#rm /usr/data/$SIMNAME/* -r
mao is offline   Reply With Quote

Old   September 15, 2016, 04:48
Default
  #4
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 620
Rep Power: 15
Lance is on a distinguished road
your batch script was not very clear, but make sure you understand the difference between -initial-file and -continue-from-file
the first will make the simulation start from zero with initial values from the specified file, the second will continue the simulation using the initial values file.
mao likes this.
Lance is offline   Reply With Quote

Old   September 15, 2016, 10:50
Default
  #5
Senior Member
 
Join Date: Jun 2009
Posts: 717
Rep Power: 15
Opaque is on a distinguished road
To complement Lance's response, you must also understand the differences between n.trn and n_full.trn files.

n_full.trn files are effectively final results file for a given timestep (n), and you can safely restart from them.

n.trn files are considered minimal transient files, and only contain data to be visualized by a successfully finished run. That is, on their own they do not have enough information to be used.

Hope the above helps,
mao likes this.
Opaque is offline   Reply With Quote

Old   September 23, 2016, 10:31
Default
  #6
mao
New Member
 
mao
Join Date: Mar 2016
Posts: 17
Rep Power: 3
mao is on a distinguished road
thank you,guys, your information are very useful to me, thanks again sincerely.
mao 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
Swak4Foam funkyDoCalc with OF2.3 massflow NiFl OpenFOAM 11 November 1, 2016 07:43
How to use finite area method in official OpenFOAM 2.2.0? Detian Liu OpenFOAM Meshing & Mesh Conversion 4 November 3, 2015 04:04
centOS 5.6 : paraFoam not working yossi OpenFOAM Installation 2 October 9, 2013 01:41
Version 15 on Mac OS X gschaider OpenFOAM Installation 113 December 2, 2009 11:23
ParaView Compilation jakaranda OpenFOAM Installation 3 October 27, 2008 12:46


All times are GMT -4. The time now is 14:34.