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

OpenFOAM-2.1.0 Writes Data in Old Format and Reads in New Format

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

Like Tree2Likes
  • 2 Post By JLight

Reply
 
LinkBack Thread Tools Display Modes
Old   October 4, 2012, 01:38
Default OpenFOAM-2.1.0 Writes Data in Old Format and Reads in New Format
  #1
New Member
 
Nishit Joseph
Join Date: Nov 2010
Posts: 29
Rep Power: 6
JLight is on a distinguished road
Hi OF Users!
I am having a seprate difficulity regarding OF-2.1 with the 'parallel' patches influencing the the solution here. In trying to diagnose that issue I have hit a seprate one.

Here is what I am trying to do. Run the solver as a single process for a few time steps. Use the intermediat solution to deocmpose the case. Then run the case from the last computed time step.

I can
  • View the solution in ParaView without any issues.
  • Decompose the case without any issues.

I cannot
  • Contine the solution in parallel
  • Continue the solution as a single processor

Here is my output when I try to run the solver again as a single processor
Code:
$ rhoCentralFoam 
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.0-bd7367f93311
Exec   : rhoCentralFoam
Date   : Oct 04 2012
Time   : 14:26:10
Host   : "jlightDell"
PID    : 10761
Case   : /home/jlight/CFD/DSTO/MainWork/Wire_OF_New
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 1.000000e-08

Reading thermophysical properties

Selecting thermodynamics package ePsiThermo<pureMixture<sutherlandTransport<specieThermo<hConstThermo<perfectGas>>>>>
Reading field U

--> FOAM Warning : 
    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
    in file /home/jlight/OpenFOAM/OpenFOAM-2.1.0/src/OpenFOAM/lnInclude/Field.C at line 262
    Reading "/home/jlight/CFD/DSTO/MainWork/Wire_OF_New/1.000000e-08/U::boundaryField::wire" from line 166680 to line 167095
    expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.


--> FOAM FATAL IO ERROR: 
Expected a '(' while reading VectorSpace<Form, Cmpt, nCmpt>, found on line 166686 the label 200

file: /home/jlight/CFD/DSTO/MainWork/Wire_OF_New/1.000000e-08/U::boundaryField::wire::refValue at line 166686.

    From function Istream::readBegin(const char*)
    in file db/IOstreams/IOstreams/Istream.C at line 94.

FOAM exiting
Any suggestion on how I am solve this?

JLight

Last edited by JLight; October 4, 2012 at 09:18.
JLight is offline   Reply With Quote

Old   October 4, 2012, 08:12
Default Missing Keyword
  #2
New Member
 
Nishit Joseph
Join Date: Nov 2010
Posts: 29
Rep Power: 6
JLight is on a distinguished road
Just an update on this.

I was looking at the U files and found that the keyword 'nonuniform' was missing for the refValues and valueFraction.

However I am not sure which file controls the output for boundary fields like this one (being the maxwellSlipU from rhoCentralFoam's BC). I will like to edit the source and fix this issue.

JLight
JLight is offline   Reply With Quote

Old   October 4, 2012, 09:59
Default The Fix
  #3
New Member
 
Nishit Joseph
Join Date: Nov 2010
Posts: 29
Rep Power: 6
JLight is on a distinguished road
The fix is simple and I have reported a bug to OpenFOAM.

Just edit the file $FOAM_APP/solvers/compressible/rhoCentralFoam/BCs/U/maxwellSlipUFvPatchVectorField.C.

Code:
--- ../../../rhoCentralFoam/BCs/U/maxwellSlipUFvPatchVectorField.C	2011-11-25 03:59:50.000000000 +1100
+++ maxwellSlipUFvPatchVectorField.C	2012-10-04 22:30:46.318141418 +1000
@@ -194,11 +194,9 @@
     os.writeKeyword("thermalCreep")
         << thermalCreep_ << token::END_STATEMENT << nl;
     os.writeKeyword("curvature") << curvature_ << token::END_STATEMENT << nl;
-
-    os.writeKeyword("refValue")
-        << refValue() << token::END_STATEMENT << nl;
-    os.writeKeyword("valueFraction")
-        << valueFraction() << token::END_STATEMENT << nl;
+   
+    refValue().writeEntry("refValue", os);
+    valueFraction().writeEntry("valueFraction", os);
 
     writeEntry("value", os);
 }
Hope this helps.

JLight
wyldckat and caduqued like this.
JLight 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
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 17 August 22, 2009 04:59


All times are GMT -4. The time now is 16:58.