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

Adding Temperature field to IcoFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 3, 2009, 20:39
Default Adding Temperature field to IcoFoam
  #1
Member
 
Ramesh Yapalparvi
Join Date: Jun 2009
Posts: 53
Rep Power: 8
yapalparvi is on a distinguished road
Hi,

I followed this tutorial on the wiki page
http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam

I ran my_icoFoam

and it gave me this message

FOAM Warning :
From function Field<Type>::Field(const word& keyword, const dictionary& dict, const label s)
in file /home/ramesh/OpenFOAM/OpenFOAM-1.5/src/OpenFOAM/lnInclude/Field.C at line 252
Reading "/home/ramesh/OpenFOAM/ramesh-1.5/run/my_icoFoam_cavity/0/T::movingWall" from line 25 to line 26
expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
--> FOAM Warning :
From function Field<Type>::Field(const word& keyword, const dictionary& dict, const label s)
in file /home/ramesh/OpenFOAM/OpenFOAM-1.5/src/OpenFOAM/lnInclude/Field.C at line 252
Reading "/home/ramesh/OpenFOAM/ramesh-1.5/run/my_icoFoam_cavity/0/T::fixedWalls" from line 31 to line 32
expected keyword 'uniform' or 'nonuniform', assuming deprecated Field format from Foam version 2.0.
Reading/calculating face flux field phi


Starting time loop

Time = 0.005

Courant Number mean: 0 max: 0
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 2.96338e-06, No Iterations 8
DILUPBiCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
DICPCG: Solving for p, Initial residual = 1, Final residual = 7.55402e-07, No Iterations 35
time step continuity errors : sum local = 5.03809e-09, global = 1.94884e-19, cumulative = 1.94884e-19
DICPCG: Solving for p, Initial residual = 0.523591, Final residual = 9.72352e-07, No Iterations 34
time step continuity errors : sum local = 1.07766e-08, global = 4.49324e-19, cumulative = 6.44208e-19



gradientInternalCoeffs cannot be called for a genericFvPatchField (actual type fixedvalue)
on patch movingWall of field T in file "/home/ramesh/OpenFOAM/ramesh-1.5/run/my_icoFoam_cavity/0/T"
You are probably trying to solve for a field with a generic boundary condition.

From function genericFvPatchField<Type>::gradientInternalCoeffs( ) const
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 692.

FOAM exiting


any help would be appreciated. Thanks

Ramesh
yapalparvi is offline   Reply With Quote

Old   August 3, 2009, 21:01
Default
  #2
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9
sandy is on a distinguished road
Yes, I guess my supervisor will also push me to do similar works in the next step ...
sandy is offline   Reply With Quote

Old   August 3, 2009, 22:02
Default
  #3
Member
 
Ramesh Yapalparvi
Join Date: Jun 2009
Posts: 53
Rep Power: 8
yapalparvi is on a distinguished road
Hi,

Thanks!. I have fixed the bug......


Ramesh
yapalparvi is offline   Reply With Quote

Old   February 16, 2010, 16:15
Default
  #4
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 8
nishant_hull is on a distinguished road
how did you fix the bug mate? I am also having similar bug when i tried a different boundary condition say parabolicVelocityInlet.
nishant_hull is offline   Reply With Quote

Old   February 25, 2010, 12:06
Default
  #5
Member
 
Ramesh Yapalparvi
Join Date: Jun 2009
Posts: 53
Rep Power: 8
yapalparvi is on a distinguished road
Can you please be more specific?. Share your code so that I can have a look
yapalparvi is offline   Reply With Quote

Old   March 1, 2010, 22:06
Default
  #6
Senior Member
 
Michael Jaworski
Join Date: Mar 2009
Location: Champaign, IL, USA
Posts: 126
Rep Power: 8
mike_jaworski is on a distinguished road
The tutorial listings lacked the keyword "uniform" from the definition of the value in the boundary conditions.

The wiki's been edited to fix this - but the information is contained in the "warning" messages that were posted.

-Mike
mike_jaworski is offline   Reply With Quote

Old   April 7, 2010, 07:37
Default
  #7
Member
 
Javed
Join Date: Mar 2010
Location: Mumbai,India
Posts: 32
Rep Power: 7
Javed is on a distinguished road
Hi friends,

I am facing sm pbm while compiling my own icoFOAM solver using wmake command..I m getting following pbm

javed@javed:~/OpenFOAM-RUN/OpenFOAM-1.6/applications/solvers/incompressible/icoFoam_temp$ wmake
make: *** No rule to make target `icoFoam.dep', needed by `Make/linuxGccDPOpt/dependencies'. Stop.


Please help me out.
Javed is offline   Reply With Quote

Old   April 7, 2010, 09:09
Default
  #8
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 8
nishant_hull is on a distinguished road
Always use wclean before wmake. Or make sure there is no .dep file while doing wmake.

Nishant
nishant_hull is offline   Reply With Quote

Old   April 7, 2010, 13:46
Default
  #9
Member
 
Javed
Join Date: Mar 2010
Location: Mumbai,India
Posts: 32
Rep Power: 7
Javed is on a distinguished road
Thanks Nishant for the quick reply..

Now after doing all the changes as per given in http://openfoamwiki.net/index.php/How_to_add_temperature_to_icoFoam, I am not able to run it as follow...plz help friends...As i m running

javed@javed:~/OpenFOAM-RUN/OpenFOAM-1.6/tutorials/incompressible/icoFoam/mycavity$ myicoFoam

Case : /home/javed/OpenFOAM-RUN/OpenFOAM-1.6/tutorials/incompressible/icoFoam/mycavity
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0

// using new solver syntax:
p
{
solver PCG;
preconditioner
{
type DIC;
}
minIter 0;
maxIter 2000;
tolerance 1e-06;
relTol 0;
}

// using new solver syntax:
T
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-07;
relTol 0;
}

// using new solver syntax:
U
{
solver PBiCG;
preconditioner
{
type DILU;
}
minIter 0;
maxIter 500;
tolerance 1e-05;
relTol 0;
}

Reading transportProperties

Reading field p

Reading field U

Reading field T

Reading/calculating face flux field phi


Starting time loop

Time = 0.005

Courant Number mean: 0 max: 0


keyword preconditioner is undefined in dictionary ":reconditioner"

file: :reconditioner from line 47 to line 47.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 388.

FOAM exiting

Plz help...

Thanks
Javed is offline   Reply With Quote

Old   April 7, 2010, 16:37
Default
  #10
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 8
nishant_hull is on a distinguished road
As far as I can see, there is some mismatch in the format of the other fields and Temperature field. Change that and see if it works.
But If you dont get it right after that, then post the line 47 (lets make it line: 40-50) of the asked file here.
regards,
Nishant
nishant_hull is offline   Reply With Quote

Old   April 8, 2010, 02:47
Default
  #11
Senior Member
 
Gijsbert Wierink
Join Date: Mar 2009
Posts: 382
Rep Power: 9
gwierink is on a distinguished road
Hi Javed,

Hmm, I think system/fvSolution should look something like this:


Code:
    
solvers
{
    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-06;
        relTol          0;
    }

    // GW Add a solver for T
    T
    {
        solver          BICCG;
        preconditioner  DILU; //GW or: none, GAMG, diagonal
        tolerance       1e-7;
        relTol          0;
    }

    U
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0;
    }
}

PISO
{
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
}
__________________
Regards, Gijs
gwierink is offline   Reply With Quote

Old   March 1, 2013, 10:27
Default
  #12
New Member
 
Mussie
Join Date: Feb 2011
Posts: 7
Rep Power: 6
afeworkimussie is on a distinguished road
Quote:
Originally Posted by Javed View Post
Thanks Nishant for the quick reply..

Now after doing all the changes as per given in http://openfoamwiki.net/index.php/How_to_add_temperature_to_icoFoam, I am not able to run it as follow...plz help friends...As i m running

javed@javed:~/OpenFOAM-RUN/OpenFOAM-1.6/tutorials/incompressible/icoFoam/mycavity$ myicoFoam

Case : /home/javed/OpenFOAM-RUN/OpenFOAM-1.6/tutorials/incompressible/icoFoam/mycavity
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0

// using new solver syntax:
p
{
solver PCG;
preconditioner
{
type DIC;
}
minIter 0;
maxIter 2000;
tolerance 1e-06;
relTol 0;
}

// using new solver syntax:
T
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-07;
relTol 0;
}

// using new solver syntax:
U
{
solver PBiCG;
preconditioner
{
type DILU;
}
minIter 0;
maxIter 500;
tolerance 1e-05;
relTol 0;
}

Reading transportProperties

Reading field p

Reading field U

Reading field T

Reading/calculating face flux field phi


Starting time loop

Time = 0.005

Courant Number mean: 0 max: 0


keyword preconditioner is undefined in dictionary ":reconditioner"

file: :reconditioner from line 47 to line 47.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 388.

FOAM exiting

Plz help...

Thanks
Hi

p
{
solver PCG;
preconditioner DIC;
minIter 0;
maxIter 2000;
tolerance 1e-06;
relTol 0;
}

This sort of presenting the fvSolution will solve the problem
afeworkimussie is offline   Reply With Quote

Old   January 18, 2014, 07:59
Default
  #13
New Member
 
Umut
Join Date: May 2011
Posts: 3
Rep Power: 6
Umut is on a distinguished road
Hello,

I need to add energy equation to simpleFoam. There are some threads about it but they all used laminar model. Is there any model for turbulent, steady, incompressible (official or non) flow solver? Can you give me some hints?

Kind regards

Umut
Umut is offline   Reply With Quote

Old   January 18, 2014, 09:25
Default
  #14
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
buoyantBoussinesqSimpleFoam
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess 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
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Problem with rhoSimpleFoam matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51
transient temperature field with constant velocity Törnquist CFX 0 September 16, 2003 04:22
Question concering about validating Temperature field ghlee Main CFD Forum 1 December 1, 1998 13:36


All times are GMT -4. The time now is 23:03.