CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Message truncated, error stack: MPIDI_CH3U_Receive_data_found

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

Like Tree1Likes
  • 1 Post By mmmn036

Reply
 
LinkBack Thread Tools Display Modes
Old   October 27, 2013, 17:05
Default Message truncated, error stack: MPIDI_CH3U_Receive_data_found
  #1
Senior Member
 
Vishal Nandigana
Join Date: Mar 2009
Location: Champaign, Illinois, U.S.A
Posts: 208
Rep Power: 9
nandiganavishal is on a distinguished road
Hi Brunos,

I was trying to install OF 2.0.0 in CentOS version 4.x. It did not work. Anyway, I think I would update the OS and install it in the future.

However, I have another question regarding running codes in parallel in OF. It appears that my solver runs fine in serial mode, however, when I run it in solver, I received the following error message.

Fatal error in MPI_Recv:
Message truncated, error stack:
MPIDI_CH3U_Receive_data_found(257): Message from rank 2 and tag 1 truncated; 8 bytes received but buffer size is 4


I tried to search for any similar errors encountered by the OF users before, but could not find any good suggestion. Please let me know what is the source for this error and how to fix this issue.

Thanks

Regards,
Vishal
nandiganavishal is offline   Reply With Quote

Old   October 28, 2013, 03:47
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Vishal,

I suspect that you need to find the correct environment variable for setting the buffer size for the MPI toolbox to use. For example, OpenFOAM sets for Open-MPI the variable "MPI_BUFFER_SIZE": https://github.com/OpenFOAM/OpenFOAM...ttings.sh#L580

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   October 28, 2013, 11:28
Default
  #3
Senior Member
 
Vishal Nandigana
Join Date: Mar 2009
Location: Champaign, Illinois, U.S.A
Posts: 208
Rep Power: 9
nandiganavishal is on a distinguished road
Hi Brunos,

Could you provide more details on this one. I am not that familiar on how to identify the environment variables to set the buffer size. I did look at the settings.sh file and the MPI_BUFFER_SIZE is set similar to the link you had mentioned. It would be great if you could help me out in this one.

Thanks

Regards,
Vishal
nandiganavishal is offline   Reply With Quote

Old   October 28, 2013, 17:12
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Vishal,

I've moved this line of conversation from OpenFOAM-1.7.0 for CentOS/RHEL/SL 5.x 64bit released to this new thread, because the other one refers to installing OpenFOAM, not regarding running it in parallel

As for your problem, I need to know a few things:
  1. On which Linux Distribution are you trying to run OpenFOAM in parallel?
  2. Which OpenFOAM version are you using for this?
  3. Which MPI toolbox is being used with OpenFOAM? To ascertain this:
    1. Check which MPI is chosen on OpenFOAM's environment:
      Code:
      echo $FOAM_MPI
    2. Check which mpirun is being found:
      Code:
      which mpirun
      ls -l $(which mpirun)
    3. Check which version of MPI it's being used:
      Code:
      mpirun --version
  4. What exact command are you using for launching the application in parallel?
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   October 29, 2013, 12:38
Default
  #5
Senior Member
 
Vishal Nandigana
Join Date: Mar 2009
Location: Champaign, Illinois, U.S.A
Posts: 208
Rep Power: 9
nandiganavishal is on a distinguished road
Hi Brunos,

Below is the reply for all your questions.

1. Linux distribution:

Linux taubh1 2.6.32-358.23.2.el6.x86_64 #1 SMP Wed Oct 16 11:13:47 CDT 2013 x86_64 x86_64 x86_64 GNU/Linux
Scientific Linux release 6.1 (Carbon)

2. OpenFoam version: OpenFoam-1.7.1

3. Which MPI toolbox is being used with OpenFOAM?

Command: echo $FOAM_MPI (did not work)

Command used: echo $FOAM_MPI_LIBBIN
message: /home/nandiga1/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/mvapich2-1.6-gcc+ifort

3.2. Check which mpirun is being found:

which mpirun
/usr/local/mvapich2-1.6-gcc+ifort/bin/mpirun

ls -l $(which mpirun)
lrwxrwxrwx 1 394298 394298 13 2011-11-18 16:53 /usr/local/mvapich2-1.6-gcc+ifort/bin/mpirun -> mpiexec.hydra

3.3. Check which version of MPI it's being used:

mpirun --version

HYDRA build details:
Version: 1.6rc3
Release Date: unreleased development copy
CC: gcc -fpic
CXX: g++ -fpic
F77: ifort -fpic
F90: ifort -fpic
Configure options: '--prefix=/usr/local/mvapich2-1.6-gcc+ifort' 'CC=gcc -fpic' 'CXX=g++ -fpic' 'F77=ifort -fpic' 'F90=ifort -fpic' 'FC=ifort -fpic' '--with-mpe' '--enable-sharedlibs=gcc' '--disable-checkerrors' '--with-atomic-primitives=auto_allow_emulation' 'CFLAGS= -DNDEBUG -O2' 'LDFLAGS= ' 'LIBS= -lpthread -libverbs -libumad -ldl -lrt ' 'CPPFLAGS= -I/usr/local/src/mvapich/mvapich2-1.6/src/openpa/src -I/usr/local/src/mvapich/mvapich2-1.6/src/openpa/src'
Process Manager: pmi
Launchers available: ssh rsh fork slurm ll lsf sge none persist
Binding libraries available: hwloc plpa
Resource management kernels available: none slurm ll lsf sge pbs
Checkpointing libraries available:
Demux engines available: poll select

3.4 What exact command are you using for launching the application in parallel?

#PBS -q cse
#PBS -l nodes=1pn=12
#PBS -l walltime=60:30:00
#PBS -j oe
#PBS -o simout
#PBS -N 2D_circular
cd ${PBS_O_WORKDIR}
module load mvapich2/1.6-gcc+ifort
mpiexec -np 12 circularFoam_full -parallel

Hope this would provide you some idea regarding the problem.

Thanks

Regards,
Vishal
nandiganavishal is offline   Reply With Quote

Old   November 2, 2013, 17:24
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Vishal,

OK, I got a better idea of the system you've got, but no clear notion as to why this error occurs.

Some searching online gave me the indication that it could be a memory limitation problem on the machines themselves. In other words, perhaps the mesh is too big for the machines you want to use.

Another indication was that there is no way to control the buffer size on mvapich2.

I suggest that you do a basic communication test on the cluster, following the instructions given here on how to test if MPI is working: post #4 of "openfoam 1.6 on debian etch", and/or post #19 of "OpenFOAM updates"

Then try to run one of OpenFOAM's tutorials in parallel, such as the tutorial "multiphase/interFoam/laminar/damBreak".

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   August 19, 2015, 01:21
Default
  #7
Member
 
Manjura Maula Md. Nayamatullah
Join Date: May 2013
Location: San Antonio, Texas, USA
Posts: 36
Rep Power: 4
mmmn036 is on a distinguished road
Hello,

I am also getting the same error for my parallel simulations:

Fatal error in MPI_Recv:
Message truncated, error stack:
MPI_Recv(184).......................: MPI_Recv(buf=0x12e3180, count=21, MPI_PACKED, src=1, tag=1, MPI_COMM_WORLD, status=0x7fff4975d160) failed
MPIDI_CH3U_Request_unpack_uebuf(691): Message truncated; 7776 bytes received but buffer size is 21

I am also using mvapich2 on my machine in cluster.

But I was running the tutorial on "multiphase/interFoam/laminar/damBreak" and that case is running good in parallel without any error.

My domain is 2D and very small (1.5m x 0.4m) and mesh (500x150).

I am not sure why I am getting that error for some specific cases.

Anyone have the solution?

Thanks
mmmn036 is offline   Reply With Quote

Old   August 19, 2015, 07:58
Default
  #8
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings mmmn036,

After some more researching online, that seems to be a problem with mvapich2 1.9. Which version are you using?
Beyond that, my guess is that the problem is related to a wrongly configured shell environment for using mvapich2? Check its manual for more details.

There is a way to test running in parallel in OpenFOAM, namely by compiling and using the Test-parallel application. More details available here:
Quote:
On how to test if MPI is working: post #4 of "openfoam 1.6 on debian etch", and/or post #19 of "OpenFOAM updates" - Note: As of OpenFOAM 2.0.0, the application "parallelTest" is now called "Test-parallel".
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   August 19, 2015, 11:44
Default
  #9
Member
 
Manjura Maula Md. Nayamatullah
Join Date: May 2013
Location: San Antonio, Texas, USA
Posts: 36
Rep Power: 4
mmmn036 is on a distinguished road
I run the following command:

which mpirun
/opt/apps/intel14/mvapich2/2.0b/bin/mpirun
mmmn036 is offline   Reply With Quote

Old   August 19, 2015, 16:07
Default
  #10
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Then please the Test-parallel application
wyldckat is offline   Reply With Quote

Old   August 19, 2015, 18:11
Default
  #11
Member
 
Manjura Maula Md. Nayamatullah
Join Date: May 2013
Location: San Antonio, Texas, USA
Posts: 36
Rep Power: 4
mmmn036 is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Then please the Test-parallel application
I have installed foam-extend-3.1, where I could not find the "test/parallel" file.

Is there any other way to test parallel in that version of OpenFoam?
mmmn036 is offline   Reply With Quote

Old   August 20, 2015, 13:16
Default
  #12
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi mmmn036,

Sigh... you could have stated that sooner And I had forgotten that foam-extend didn't have the test folder for some reason...

OK, run the following commands, for getting and building the application:
Code:
mkdir -p $FOAM_RUN
cd $FOAM_RUN
mkdir parallelTest
wget https://raw.githubusercontent.com/OpenCFD/OpenFOAM-1.7.x/master/applications/test/parallel/parallelTest.C
mkdir Make
cd Make/
wget https://raw.githubusercontent.com/OpenCFD/OpenFOAM-1.7.x/master/applications/test/parallel/Make/options
wget https://raw.githubusercontent.com/OpenCFD/OpenFOAM-1.7.x/master/applications/test/parallel/Make/files
Then run the parallelTest application the same way you ran the solver and in the same case folder.
If it works, it should output something like this:
Code:
Create  time

[1]
Starting transfers
[1]
[1] slave sending to master 0
[1] slave receiving from master 0
[0]
Starting transfers
[0]
[0] master receiving from slave 1
[0] (0 1 2)
[0] master sending to slave 1
End

[1] (0 1 2)
Finalising parallel run
Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   August 20, 2015, 19:34
Default
  #13
Member
 
Manjura Maula Md. Nayamatullah
Join Date: May 2013
Location: San Antonio, Texas, USA
Posts: 36
Rep Power: 4
mmmn036 is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Hi mmmn036,

Sigh... you could have stated that sooner And I had forgotten that foam-extend didn't have the test folder for some reason...

OK, run the following commands, for getting and building the application:
Code:
mkdir -p $FOAM_RUN
cd $FOAM_RUN
mkdir parallelTest
wget https://raw.githubusercontent.com/OpenCFD/OpenFOAM-1.7.x/master/applications/test/parallel/parallelTest.C
mkdir Make
cd Make/
wget https://raw.githubusercontent.com/OpenCFD/OpenFOAM-1.7.x/master/applications/test/parallel/Make/options
wget https://raw.githubusercontent.com/OpenCFD/OpenFOAM-1.7.x/master/applications/test/parallel/Make/files
Then run the parallelTest application the same way you ran the solver and in the same case folder.
If it works, it should output something like this:
Code:
Create  time

[1]
Starting transfers
[1]
[1] slave sending to master 0
[1] slave receiving from master 0
[0]
Starting transfers
[0]
[0] master receiving from slave 1
[0] (0 1 2)
[0] master sending to slave 1
End

[1] (0 1 2)
Finalising parallel run
Best regards,
Bruno
I followed the instructions and complied the parallelTest.
I ran the following command :
Code:
foamJob -p -s parallelTest
and gor the following results:
Code:
Parallel processing using MV2MPI with 16 processors
Executing: mpirun -np 16 /work/02813/jzb292/foam/foam-extend-3.1/bin/foamExec parallelTest -parallel | tee log
Nothing is written in the "log" file.

It is still showing the same error while I run in parallel.
mmmn036 is offline   Reply With Quote

Old   August 20, 2015, 20:53
Default
  #14
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
It's strange that nothing got written into the log file...

What happens if you run it like this:
Code:
mpirun -np 16 parallelTest -parallel
wyldckat is offline   Reply With Quote

Old   August 20, 2015, 22:25
Default
  #15
Member
 
Manjura Maula Md. Nayamatullah
Join Date: May 2013
Location: San Antonio, Texas, USA
Posts: 36
Rep Power: 4
mmmn036 is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
It's strange that nothing got written into the log file...

What happens if you run it like this:
Code:
mpirun -np 16 parallelTest -parallel
In my system I had to run "ibrun" instead of "mpirun" for parallel:

Now i got something in my log file which looks similar to the thread you mentioned. Please see the attached log file.

But I am still seeing the same error in parallel simulation.
Attached Files
File Type: txt log.txt (2.7 KB, 2 views)
mmmn036 is offline   Reply With Quote

Old   August 21, 2015, 11:28
Default
  #16
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Quote:
Originally Posted by mmmn036 View Post
Now i got something in my log file which looks similar to the thread you mentioned. Please see the attached log file.

But I am still seeing the same error in parallel simulation.
OK, this was to try and figure out the origin of the problem. It seems that the problem has to do with the specific cases that you are having problems with, because the error is not triggered with the test applications, nor with other cases you tested.
And since you're using mvapich2 2.0b, then it's not a problem related to the version itself.

You wrote on your first post on this topic:
Quote:
Originally Posted by mmmn036 View Post
I am also using mvapich2 on my machine in cluster.

But I was running the tutorial on "multiphase/interFoam/laminar/damBreak" and that case is running good in parallel without any error.

My domain is 2D and very small (1.5m x 0.4m) and mesh (500x150).
Then the mesh has 75000 cells. A few questions:
  1. In how many sub-domains are you dividing the mesh and what decomposition settings are you using?
    • In other words: please provide the "system/decomposeParDict" file you're using, so that we can see what settings you're using.
    • If you're using 16 sub-domains, as reported by the test, then each sub-domain as around 4687 cells each. Can you please also provide the text output that decomposePar gave you? Because that tells us how many cells and faces were assigned to each sub-domain; there might be one or two sub-domains that have very few cells being shared.
  2. How is the case distributed among the various machines on the cluster? In other words, is the case running in a single machine or 2, 3 or 4 machines?
  3. Does your mesh have any special boundary conditions? Such as baffles or cyclic patches?
  4. Which solver/application are you using? I ask this because there are some settings in "system/fvSchemes" that might help with the problem and usually that depends on the simulation being done.
I ask all of these questions because the error message you're getting is related to an improperly defined memory size on the receiving side on one of the processes. Some MPI toolboxes don't have this issue, because they use some explicit or implicit size reset/definition, but some other MPI toolboxes don't take into account some corner case uses. Therefore, this is usually related to a situation which is not contemplated in the standard operation of OpenFOAM or foam-extend.

By the way, has you tried using one of the latest versions of OpenFOAM, such as 2.4.0 or 2.4.x, to see if it works with mvapich2? I ask this for the same reason as the above, as this could be a corner case that is not be contemplated in foam-extend 3.1, but might be already contemplated in OpenFOAM.
wyldckat is offline   Reply With Quote

Old   August 22, 2015, 03:03
Default
  #17
Member
 
Manjura Maula Md. Nayamatullah
Join Date: May 2013
Location: San Antonio, Texas, USA
Posts: 36
Rep Power: 4
mmmn036 is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
OK, this was to try and figure out the origin of the problem. It seems that the problem has to do with the specific cases that you are having problems with, because the error is not triggered with the test applications, nor with other cases you tested.
And since you're using mvapich2 2.0b, then it's not a problem related to the version itself.

You wrote on your first post on this topic:

Then the mesh has 75000 cells. A few questions:
  1. In how many sub-domains are you dividing the mesh and what decomposition settings are you using?
    • In other words: please provide the "system/decomposeParDict" file you're using, so that we can see what settings you're using.
    • If you're using 16 sub-domains, as reported by the test, then each sub-domain as around 4687 cells each. Can you please also provide the text output that decomposePar gave you? Because that tells us how many cells and faces were assigned to each sub-domain; there might be one or two sub-domains that have very few cells being shared.
  2. How is the case distributed among the various machines on the cluster? In other words, is the case running in a single machine or 2, 3 or 4 machines?
  3. Does your mesh have any special boundary conditions? Such as baffles or cyclic patches?
  4. Which solver/application are you using? I ask this because there are some settings in "system/fvSchemes" that might help with the problem and usually that depends on the simulation being done.
I ask all of these questions because the error message you're getting is related to an improperly defined memory size on the receiving side on one of the processes. Some MPI toolboxes don't have this issue, because they use some explicit or implicit size reset/definition, but some other MPI toolboxes don't take into account some corner case uses. Therefore, this is usually related to a situation which is not contemplated in the standard operation of OpenFOAM or foam-extend.

By the way, has you tried using one of the latest versions of OpenFOAM, such as 2.4.0 or 2.4.x, to see if it works with mvapich2? I ask this for the same reason as the above, as this could be a corner case that is not be contemplated in foam-extend 3.1, but might be already contemplated in OpenFOAM.
First of All, I appreciate your support on this issue.
Here is the information you asked:

Which solver/application are you using? I ask this because there are some settings in "system/fvSchemes" that might help with the problem and usually that depends on the simulation being done.
Quote:
I am using a modified buoyanBoussiesqPimpleFoam solver with Immersed Boundary treatment that has been implemented by Hrjasak. The solver is working good in my local work station with 16 processor. But it is giving me error for parallel run in cluster. I have also included the error message file below
In how many sub-domains are you dividing the mesh and what decomposition settings are you using?
Quote:
the mesh size in my domain is now 600X80X1. I am testing for 16 subdomains, but I also tried with 128 or 256 subdomains which gives me the same error. I attached the decomposeparDic below
If you're using 16 sub-domains, as reported by the test, then each sub-domain as around 4687 cells each. Can you please also provide the text output that decomposePar gave you?
Quote:
I have attached the log file for decomposePar run results
How is the case distributed among the various machines on the cluster? In other words, is the case running in a single machine or 2, 3 or 4 machines?
Quote:
In the cluster, each node has 16 processor
[*]Does your mesh have any special boundary conditions? Such as baffles or cyclic patches?
Quote:
I have immersed boundary for all the fields. No cyclic boundary condition, but I will use cyclic boundary for 3D simulation later on.
By the way, has you tried using one of the latest versions of OpenFOAM, such as 2.4.0 or 2.4.x, to see if it works with mvapich2?
Quote:
Since Immersed boundary method platform only implemented on foam-extend, I couldn't used that solver in OpenFoam 2.4 or 2.4.x. But all other cases is running ok in parallel in OpnFoam-2.3 on the same cluster.
Thanks
Attached Files
File Type: txt decomposeParDict.txt (3.3 KB, 2 views)
File Type: txt log.decomposePar.txt (6.8 KB, 2 views)
File Type: txt ERROR.txt (3.0 KB, 1 views)
mmmn036 is offline   Reply With Quote

Old   August 22, 2015, 08:25
Default
  #18
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
OK, with any luck I found the answer that might help your problem, as reported in these two locations:
As reported in both posts, try running this command before running in parallel with 16 cores in the cluster:
Code:
export MV2_ON_DEMAND_THRESHOLD=16
When you need to run with more cores, change the 16 to the number you need.


I had seen this solution before, but the answer in the second location referred to another error message, which was why I hadn't suggested this before.
wyldckat is offline   Reply With Quote

Old   August 22, 2015, 12:50
Default
  #19
Member
 
Manjura Maula Md. Nayamatullah
Join Date: May 2013
Location: San Antonio, Texas, USA
Posts: 36
Rep Power: 4
mmmn036 is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
OK, with any luck I found the answer that might help your problem, as reported in these two locations:
As reported in both posts, try running this command before running in parallel with 16 cores in the cluster:
Code:
export MV2_ON_DEMAND_THRESHOLD=16
When you need to run with more cores, change the 16 to the number you need.


I had seen this solution before, but the answer in the second location referred to another error message, which was why I hadn't suggested this before.
This doesn't fix my error. I appreciate your support a lot though.
I got a answer in other thread Immersed Boundary Method in OpenFOAM-3.1-ext

Following the change in below fix my issue. I can run my cases parallel now.
Quote:
Edit $WM_PROJECT_DIR/etc/controlDict and change commsType to nonBlocking .
Thanks
wyldckat likes this.
mmmn036 is offline   Reply With Quote

Old   August 22, 2015, 13:24
Default
  #20
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,511
Blog Entries: 34
Rep Power: 86
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
I'm glad you've found the solution!

Changing the blocking/non-blocking option had already crossed my mind, but it always felt that the issue was on the side of MVAPICH2.

The other reason is that I thought that foam-extend was set to non-blocking by default, was because OpenFOAM is like that since at least 1.5.x!? But apparently it was changed in foam-extend without an explicit explanation in the respective commit, on the 2010-09-21 15:32:04...
wyldckat 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
Guide: Getting Started with the CFD Online Discussion Forums pete Site Help, Feedback & Discussions 6 July 20, 2015 07:20
single directional message transmit in parallel model su_junwei OpenFOAM Programming & Development 1 December 17, 2009 08:00
Error message in CFX-10 CFDworker CFX 2 October 12, 2007 07:23
error message susan CD-adapco 0 August 17, 2007 00:27
MPI Message truncated josef OpenFOAM Running, Solving & CFD 1 January 9, 2006 07:29


All times are GMT -4. The time now is 17:43.