[JLight]

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

$ 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

[JLight]

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]

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.

--- ../../../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