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

No reconstruction for times!

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 20, 2017, 07:58
Default No reconstruction for times!
  #1
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 11
alinuman15 is on a distinguished road
Dear All:-
I made different runs for my OpenFoam transient two phase flow case on Stampede on 252 processors. However, I could not create the time files from those runs.
To give you an idea about the error I got, I have inserted the obtained results in the attached files.
To summerize, I got:-
--> FOAM FATAL ERROR:
No times selected

From function reconstructPar
in file reconstructPar.C at line 210.

FOAM exiting

Any clue ?
I appreciate any suggestions.
Attached Files
File Type: gz reportTo_CFD_Online.tar.gz (41.9 KB, 2 views)
alinuman15 is offline   Reply With Quote

Old   August 21, 2017, 00:39
Default
  #2
Senior Member
 
Join Date: Aug 2013
Posts: 407
Rep Power: 16
Antimony is on a distinguished road
Hi,

I would guess that your simulation terminated before any time output was written. Check your controlDict for the write frequency and also check in one of your processor directory to see if there are any time folders there.

If there aren't any there or if your write interval is greater than the time for the simulation, it explains the issue with reconstructPar - it can't find anything to reconstruct!

On the other hand, if in the processor directory, there is a time folder present then try running reconstructPar with the -times flag and specify that particular time.

Cheers,
Antimony
Antimony is offline   Reply With Quote

Old   August 21, 2017, 01:06
Default
  #3
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 11
alinuman15 is on a distinguished road
Dear Antimony:-
Thank you so much for your suggestions!
Regarding the write frequency it had been set as:-
writeInterval 0.0004;
( Have a look at the inserted controlDictfile). As addition, there wasnot any time folder available except the folder "0".
on the other hand, I tried reconstructPar -time 0:0.4 and on another trial : reconstructPar -time latestTime
but I got the same result.
My best
Attached Files
File Type: gz controlDict.tar.gz (562 Bytes, 1 views)
alinuman15 is offline   Reply With Quote

Old   August 21, 2017, 03:20
Default
  #4
Senior Member
 
Join Date: Aug 2013
Posts: 407
Rep Power: 16
Antimony is on a distinguished road
Hi,

From your log file, the last time step is
Quote:
Time = 3.96401663435e-05
While your write interval is:
Quote:
writeInterval 0.0004;
So it is straightforward to see why there is no output and why you won't have a folder with the most recent time.

Couple of things:
1. If you are reconstructing only the most recent time then:
Code:
reconstructPar -latestTime
is what you should type instead of
Code:
reconstructPar -time latestTime
2. Did you simulation terminate normally? From the log file, I would guess that the solver blew up and thus exited with an error.
I am not an expert in interFoam, but it appears to me that the values reported in the log file are not physical. k and epsilon seem to reach large negative values and very high positive values, which to me, aren't right. Also your phase fractions seem to take on negative values. Check your BCs and setup.

My guess is that if it runs smoothly, then you will be able to see outputs at the writeInterval frequency. If you are trying to debug, then I suggest you change your writeInterval to 1e-7 or so. Will be slower, but you will know what is happening and maybe that will help you to debug your case.

Cheers,
Antimony
Antimony is offline   Reply With Quote

Old   August 21, 2017, 07:04
Default
  #5
Member
 
Ali Noaman Ibrahim
Join Date: Sep 2015
Location: US_Chicago
Posts: 97
Rep Power: 11
alinuman15 is on a distinguished road
Thanks again for reply.
1. It was a typo when I mistakenly put -time latestTime. I did it as you described but unfortunately it gives the same error.
2. The solved case is a laminar case so there is no consideration for k and epsilon values. However, it is important to me to investigate having negative values for the phase fraction.
My guess is:-
Beside what you have mentioned about decreasing the time step ( I assume you meant by writeInterval, the deltaT), I would change the fvschemes and make tight convergence criterion with more precise solver instead of linear one.
Thanks again



Sent from my iPhone using CFD Online Forum mobile app
alinuman15 is offline   Reply With Quote

Reply

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
Reconstruction of the parallel case with dynamic mesh makaveli_lcf OpenFOAM Post-Processing 8 December 3, 2024 12:16
Handling higher order reconstruction shainath SU2 1 December 14, 2014 17:24
Finite volume methods, reconstruction, etc. Nereus Main CFD Forum 9 January 31, 2012 17:12
[Commercial meshers] ST_Malloc: out of memory.malloc_storage: unable to malloc Velocity SA, cfdproject OpenFOAM Meshing & Mesh Conversion 0 April 14, 2009 16:45
Smooth reconstruction of flowsolution Carlos Main CFD Forum 2 February 14, 2008 13:25


All times are GMT -4. The time now is 12:08.