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

A problem of groovyWaveTank

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 1, 2011, 04:34
Default A problem of groovyWaveTank
  #1
Member
 
bojiezhang
Join Date: Jan 2010
Posts: 64
Rep Power: 7
bojiezhang is on a distinguished road
hello everyone:
when I run the case groovyWaveTank (http://idisk.mac.com/egpaterson-Publ...ovyWaveTank.gz), it says error
" --> FOAM FATAL IO ERROR:
keyword PIMPLE is undefined in dictionary "/home/host/OpenFOAM/OpenFOAM-2.0.0/swak4Foam/Examples/groovyBC/groovyWaveTank/system/fvSolution".
I have downloaded swak4Foam and compiled it well and I do not know how to solve it, please help me, thank you in advance!
bojiezhang
bojiezhang is offline   Reply With Quote

Old   August 1, 2011, 04:57
Default
  #2
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Location: London, UK
Posts: 242
Rep Power: 7
Phicau is on a distinguished road
Hi

just change word "SIMPLE" to "PIMPLE" in your fvSolution dictionary.
Phicau is offline   Reply With Quote

Old   August 1, 2011, 05:09
Default
  #3
Member
 
bojiezhang
Join Date: Jan 2010
Posts: 64
Rep Power: 7
bojiezhang is on a distinguished road
Dear Phicau,
Thank you for your reply! There is no SIMPLE in the fvSolution dictionary.The whole content is:
PISO
{
momentumPredictor no;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
nGammaCorr 1;
nGammaSubCycles 3;
cGamma 1;
pdRefCell 0;
pdRefValue 0;
pRefProbe
{
fields (pd);
probeLocations ((0.51 0.51 0.51));
};
}

// ************************************************** *********************** //

But when I change PISO to PIMPLE , the error like this:

PIMPLE: Operating solver in PISO mode

Reading field p_rgh



--> FOAM FATAL IO ERROR:
cannot find file

file: /home/host/OpenFOAM/OpenFOAM-2.0.0/swak4Foam/Examples/groovyBC/groovyWaveTank/0/p_rgh at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

can you help me?
bojiezhang

Last edited by bojiezhang; August 1, 2011 at 06:06.
bojiezhang is offline   Reply With Quote

Old   August 1, 2011, 05:59
Default
  #4
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Location: London, UK
Posts: 242
Rep Power: 7
Phicau is on a distinguished road
Sorry, I meant PIMPLE instead of PISO...
Phicau is offline   Reply With Quote

Old   August 1, 2011, 06:07
Default
  #5
Member
 
bojiezhang
Join Date: Jan 2010
Posts: 64
Rep Power: 7
bojiezhang is on a distinguished road
Quote:
Originally Posted by Phicau View Post
Sorry, I meant PIMPLE instead of PISO...
But when I change PISO to PIMPLE , the error like this:

PIMPLE: Operating solver in PISO mode

Reading field p_rgh



--> FOAM FATAL IO ERROR:
cannot find file

file: /home/host/OpenFOAM/OpenFOAM-2.0.0/swak4Foam/Examples/groovyBC/groovyWaveTank/0/p_rgh at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting
bojiezhang is offline   Reply With Quote

Old   August 1, 2011, 06:14
Default
  #6
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Location: London, UK
Posts: 242
Rep Power: 7
Phicau is on a distinguished road
Do you have p_rgh file (which provides the BCs for pressure) in the 0 directory?
Phicau is offline   Reply With Quote

Old   August 1, 2011, 06:28
Default
  #7
Member
 
bojiezhang
Join Date: Jan 2010
Posts: 64
Rep Power: 7
bojiezhang is on a distinguished road
Quote:
Originally Posted by Phicau View Post
Do you have p_rgh file (which provides the BCs for pressure) in the 0 directory?
no, just have the file "pd", and the fvsolution also use the name pd as below:
pd GAMG
{
tolerance 1e-8;
relTol 0.05;

smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;

cacheAgglomeration false;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
};

pdFinal PCG
{
preconditioner
{
type GAMG;
tolerance 1e-8;
relTol 0;

nVcycles 2;

smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;

cacheAgglomeration false;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
};

tolerance 1e-8;
relTol 0;
maxIter 20;
};
bojiezhang is offline   Reply With Quote

Old   August 1, 2011, 06:35
Default
  #8
Senior Member
 
Pablo Higuera
Join Date: Jan 2011
Location: London, UK
Posts: 242
Rep Power: 7
Phicau is on a distinguished road
Then I guess you will have to rewrite certain things of your case in order for it to work, since it seems it is from a very old OF version.

Take a look at damBreak tutorial case and modify consistently the files.
Phicau is offline   Reply With Quote

Old   August 1, 2011, 06:36
Default
  #9
Member
 
bojiezhang
Join Date: Jan 2010
Posts: 64
Rep Power: 7
bojiezhang is on a distinguished road
Quote:
Originally Posted by Phicau View Post
Do you have p_rgh file (which provides the BCs for pressure) in the 0 directory?
I use the swak4Foam in the openfoam 2.0.0, not in the openfoam-extended, does it matter?
bojiezhang is offline   Reply With Quote

Old   August 1, 2011, 06:40
Default
  #10
Member
 
bojiezhang
Join Date: Jan 2010
Posts: 64
Rep Power: 7
bojiezhang is on a distinguished road
But the file version which written is 2.0
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object pd;
}
bojiezhang is offline   Reply With Quote

Old   August 1, 2011, 09:25
Default
  #11
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by bojiezhang View Post
I use the swak4Foam in the openfoam 2.0.0, not in the openfoam-extended, does it matter?
The problem you're experiencing have got to do with the face that the waveTank-case was set up for OF and 1.5 and interFoam went through some changes since then. The best thing would be to compare the dambreak-case for 1.5 and 2.0 and apply the same changes you see there to the waveTank
gschaider is offline   Reply With Quote

Old   August 1, 2011, 10:01
Default
  #12
Member
 
bojiezhang
Join Date: Jan 2010
Posts: 64
Rep Power: 7
bojiezhang is on a distinguished road
Thank you very much, I know it now! But I have another question, I defined the alpha1 inlet like:
inlet
{
type groovyBC;
valueExpression "(pos().y<=A*cos(-w*time())) ? 1 : 0";
variables "l=1.56;A=0.01;g=vector(0,-9.81,0);k=2*pi/l;w=sqrt(k*mag(g));";
timelines ();
}

but it does not work, and says that
"--> FOAM Warning :
From function groovyBCFvPatchField<Type>::groovyBCFvPatchField(c onst fvPatch& p,const DimensionedField<Type, volMesh>& iF,const dictionary& dict)
in file groovyBCFvPatchField.C at line 119
No value defined for alpha1 on inlet therefore using 40{0}
"


No value is defined in the inlet boundary and the value is set to be zero at last, I do not know how to modify it, can you help me? Thank you in advance!
bojiezhang is offline   Reply With Quote

Old   August 1, 2011, 10:16
Default
  #13
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by bojiezhang View Post
Thank you very much, I know it now! But I have another question, I defined the alpha1 inlet like:
inlet
{
type groovyBC;
valueExpression "(pos().y<=A*cos(-w*time())) ? 1 : 0";
variables "l=1.56;A=0.01;g=vector(0,-9.81,0);k=2*pi/l;w=sqrt(k*mag(g));";
timelines ();
}

but it does not work, and says that
"--> FOAM Warning :
From function groovyBCFvPatchField<Type>::groovyBCFvPatchField(c onst fvPatch& p,const DimensionedField<Type, volMesh>& iF,const dictionary& dict)
in file groovyBCFvPatchField.C at line 119
No value defined for alpha1 on inlet therefore using 40{0}
"


No value is defined in the inlet boundary and the value is set to be zero at last, I do not know how to modify it, can you help me? Thank you in advance!
Just add a

value uniform 0;

line or so to the BC. This warning is only of consequence if another groovyBC uses alpha1 before that BC is evaluated for the first time. Very unlikely that this will happens, that's why it is only a warning

Bernhard
gschaider is offline   Reply With Quote

Old   August 1, 2011, 10:58
Default
  #14
Member
 
bojiezhang
Join Date: Jan 2010
Posts: 64
Rep Power: 7
bojiezhang is on a distinguished road
Quote:
Originally Posted by gschaider View Post
Just add a

value uniform 0;

line or so to the BC. This warning is only of consequence if another groovyBC uses alpha1 before that BC is evaluated for the first time. Very unlikely that this will happens, that's why it is only a warning

Bernhard
Yeah, it does work, thank you very much! But if I add "value uniform 0" to the inlet boundary, when the wave begins to transmit, it is not like wave and the phenomenon is strange. If I add "value uniform 1" to it, the phenomenon in the boundary is not true! Do you have any advice? Thank you!
bojiezhang is offline   Reply With Quote

Old   August 1, 2011, 12:11
Default
  #15
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by bojiezhang View Post
Yeah, it does work, thank you very much! But if I add "value uniform 0" to the inlet boundary, when the wave begins to transmit, it is not like wave and the phenomenon is strange. If I add "value uniform 1" to it, the phenomenon in the boundary is not true! Do you have any advice? Thank you!
Not familiar enough with interFoam to say when which BC is evaluated. Maybe setting the value with funkySetBoundaryCondition to be consistent with the evaluated value at t=0 may help
gschaider is offline   Reply With Quote

Old   August 1, 2011, 23:51
Default
  #16
Member
 
bojiezhang
Join Date: Jan 2010
Posts: 64
Rep Power: 7
bojiezhang is on a distinguished road
Quote:
Originally Posted by gschaider View Post
Not familiar enough with interFoam to say when which BC is evaluated. Maybe setting the value with funkySetBoundaryCondition to be consistent with the evaluated value at t=0 may help
OK! Thank you very much! I will try it later!
bojiezhang is offline   Reply With Quote

Old   August 9, 2011, 05:12
Default
  #17
Member
 
Join Date: Aug 2011
Posts: 81
Rep Power: 6
idefix is on a distinguished road
I have the same problem now. How did you solve yours?

Last edited by idefix; August 9, 2011 at 06:19.
idefix is offline   Reply With Quote

Old   August 9, 2011, 05:14
Default
  #18
Member
 
Join Date: Aug 2011
Posts: 81
Rep Power: 6
idefix is on a distinguished road
Here´s the error massage:

--> FOAM FATAL IO ERROR:
cannot find file

file: /OpenFOAM/test/0.001/p_rgh at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

Last edited by idefix; August 9, 2011 at 06:19.
idefix 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
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Gambit - meshing over airfoil wrapping (?) problem JFDC FLUENT 1 July 11, 2011 05:59
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13
Is this problem well posed? Thomas P. Abraham Main CFD Forum 5 September 8, 1999 14:52


All times are GMT -4. The time now is 15:02.