How to output other properties?

wagnergaluppo · April 23, 2012, 18:13

Hi,
I am using the OpenFOAM-210 and I Know that with foamCalc utility I can get the components of velocity and I also know how to get mach number and vorticity, but does anybody know how to output other variables such as viscosity, Reynolds number and etc?
thanks,
Wagner

akidess · April 24, 2012, 02:42

Viscosity will be written to the time directories if it's not constant, and you can plot it with paraview. You can also use paraview to calculate the Reynolds number. If you want a command line utility, you'll have to get your hands dirty.

wagnergaluppo · April 26, 2012, 23:51

Thank you for your reply. I'm ready to get my hands dirty. Even though my viscosity is constant, I would still like to know how to output it at each time-step. I would like to verify that I am getting the correct value for my viscosity. I'm using the rhoCentralFoam solver. This is the output of the "createFields.H" file:

13--> const volScalarField& mu = thermo.mu();

So what I did was change this file to something like this:

13--> volScalarField mu
14--> (
15--> IOobject
16--> (
17--> "mu",
18--> runTime.timeName(),
19--> mesh,
20--> IOobject::MUST_READ,
21--> IOobject::AUTO_WRITE
22--> ),
23--> mesh
24--> );

Then I recompiled and created a "mu" file at my "/0/" directory. But after I running, the other time directories do not have the mu property. It's not autowriting as ordered. For the Reynolds number I'm still having problems. Do you know of any documentation about the command line utility for this?
thanks,
Wagner

wagnergaluppo · May 1, 2012, 14:42

Hi Akidess,

I followed your suggestion and set the viscosity to sutherland. Now that the viscosity is not constant, I would have expected it to write to the time directories like you suggested. Unfortunately, viscosity does not appear in any of the time directories.

Have I missed something?

Here is the output of my thermophysical properties

Code:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType      ePsiThermo<pureMixture<sutherlandTransport<specieThermo<eConstThermo<perfectGas>>>>>;

mixture
{
    // normalised gas
    specie
    {
        nMoles          1;
        molWeight       50;
    }
    thermodynamics
    {
        Cv              1007.8039105;
        Hf              2.544e+06;
    }
    transport
    {
        As              1.67212e-06;
        Ts              170.672;
    }
}

wagnergaluppo · May 1, 2012, 14:48

This is what I've specified in the createfields.H file

Code:

const volScalarField& psi = thermo.psi();
volScalarField mu
(
IOobject
(
"mu",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

akidess · May 2, 2012, 03:39

Which solver are you using? I'll try it out and see if I can get it to work.

wagnergaluppo · May 2, 2012, 12:36

I'm using the rhoCentralFoam.
Thanks,
Wagner

wagnergaluppo · May 16, 2012, 15:28

I figure it out.
Thank you,
Wagner Galuppo

akidess · May 19, 2012, 05:09

Sorry I couldn't help much, I got busy with other things. Can you add a post on how you solved the problem? It might help others in the future.

wagnergaluppo · May 24, 2012, 12:29

Actually I partly figured it out. I found the file "basicThermo.C" in (/opt/openfoam210/src/thermophysicalModels/basic/basicThermo/)
If you have look from the 201st until 213th line you will find this:

Code:

mu_
    (
        IOobject
        (
            "mu",
            mesh.time().timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::NO_WRITE
        ),
        mesh,
        dimensionSet(1, -1, -1, 0, 0)
    ),

I copied the directory (/opt/openfoam210/src/thermophysicalModels/basic/) to my workplace and I changed the name from /basic/ to /myBasic/.
in terminal:

Code:

$ cd /opt/openfoam210
$ cp -r --parents src/thermophysicalModels/basic/ /home/cfd02/OpenFOAM/USER-2.1.0/
$ cd ~/OpenFOAM/USER-2.1.0/src/thermophysicalModels/
$ mv basic myBasic

Next I edited line 209 in the file myBasic/basicThermo/basicThermo.C from:

Code:

IOobject::NO_WRITE

to

Code:

IOobject::AUTO_WRITE

and saved and closed it.

Then I changed the 27th line in the file myBasic/Make/files from:

Code:

LIB = $(FOAM_LIBBIN)/libbasicThermophysicalModels

to

Code:

LIB = $(FOAM_USER_LIBBIN)/libbasicThermophysicalModels

and saved and closed it.

Next I compiled the code:

Code:

$ cd ~/OpenFOAM/USER-2.1.0/src/thermophysicalModels/myBasic/
$ wmake libso

It works, if you run rhoCentralFoam will output mu and doesn't matter if it is constant.
The Problem is that I'm overwriting the main library basicThermophysicalModels instead of creating a new one.

wagnergaluppo · May 24, 2012, 19:20

I changed the last modifications for mu on line 209 (in myBasic/basicThermo/basicThermo.C) back to

Code:

IOobject::NO_WRITE

and doing so reverted to the original configuration of OpenFoam for basic thermophysical property. I recompiled it overwriting my last changes.

Now OpenFoam is using the original configuration, and so I try to make a new basic thermoPhysical model.

First, I reset mu to AUTO_WRITE (since I want to output mu).

Next, I changed line 27 in the file myBasic/Make/files from

Code:

LIB = $(FOAM_USER_LIBBIN)/libbasicThermophysicalModels

to:

Code:

LIB = $(FOAM_USER_LIBBIN)/libmubasicThermophysicalModels

and compiled it with the wmake libso command.

Then I copied rhoCentralFoam solver to my workplace and renamed the directory from /rhoCentralFoam/ to /muRhoCentralFoam/, and after that in the new /muRhoCentralFoam/ directory I changed the file from rhoCentralFoam.C to muRhoCentralFoam.C.

Code:

$ cd /opt/opefoam210/
$ cp -r --parents applications/solvers/compressible/rhoCentralFoam/ $WM_PROJECT_USER_DIR
$ cd $WM_PROJECT_USER_DIR/applications/solvers/compressible/
$ mv rhoCentralFoam muRhoCentralFoam
$ cd muRhoCentralFoam
$ mv rhoCentralFoam.C muRhoCentralFoam.C

Next, in the /muRhoCentralFoam/Make/ directory I changed the file files from

Code:

rhoCentralFoam.C

EXE = $(FOAM_APPBIN)/rhoCentralFoam

to

Code:

muRhoCentralFoam.C

EXE = $(FOAM_USER_APPBIN)/muRhoCentralFoam

And the file options from

Code:

EXE_INC = \
    -IBCs/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/turbulenceModels/compressible/turbulenceModel \
    -I$(LIB_SRC)/dynamicMesh/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lbasicThermophysicalModels \
    -lspecie \
    -lrhoCentralFoam \
    -lcompressibleTurbulenceModel \
    -lcompressibleRASModels \
    -lcompressibleLESModels \
    -lmeshTools

to

Code:

EXE_INC = \
    -IBCs/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(WM_PROJECT_USER_DIR)/src/thermophysicalModels/myBasic/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/turbulenceModels/compressible/turbulenceModel \
    -I$(LIB_SRC)/dynamicMesh/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lmubasicThermophysicalModels \
    -lspecie \
    -lrhoCentralFoam \
    -lcompressibleTurbulenceModel \
    -lcompressibleRASModels \
    -lcompressibleLESModels \
    -lmeshTools

Then I tried to compile it, but it cannot find -lmubasicThermophysicalModels, the solver compilation is not reading my new basic thermophysicalModel.

Copilation error message:

Code:

Making dependency list for source file muRhoCentralFoam.C
SOURCE=muRhoCentralFoam.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -IBCs/lnInclude -I/opt/openfoam210/src/finiteVolume/lnInclude -I/home/USER/OpenFOAM/USER-2.1.0/src/thermophysicalModels/myBasic/lnInclude -I/opt/openfoam210/src/thermophysicalModels/specie/lnInclude -I/opt/openfoam210/src/turbulenceModels/compressible/turbulenceModel -I/opt/openfoam210/src/dynamicMesh/lnInclude -I/opt/openfoam210/src/meshTools/lnInclude -IlnInclude -I. -I/opt/openfoam210/src/OpenFOAM/lnInclude -I/opt/openfoam210/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/muRhoCentralFoam.o
/opt/openfoam210/src/finiteVolume/lnInclude/readTimeControls.H: In function ‘int main(int, char**)’:
/opt/openfoam210/src/finiteVolume/lnInclude/readTimeControls.H:32: warning: unused variable ‘adjustTimeStep’
/opt/openfoam210/src/finiteVolume/lnInclude/readTimeControls.H:35: warning: unused variable ‘maxCo’
/opt/openfoam210/src/finiteVolume/lnInclude/readTimeControls.H:38: warning: unused variable ‘maxDeltaT’
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -IBCs/lnInclude -I/opt/openfoam210/src/finiteVolume/lnInclude -I/home/USER/OpenFOAM/USER-2.1.0/src/thermophysicalModels/myBasic/lnInclude -I/opt/openfoam210/src/thermophysicalModels/specie/lnInclude -I/opt/openfoam210/src/turbulenceModels/compressible/turbulenceModel -I/opt/openfoam210/src/dynamicMesh/lnInclude -I/opt/openfoam210/src/meshTools/lnInclude -IlnInclude -I. -I/opt/openfoam210/src/OpenFOAM/lnInclude -I/opt/openfoam210/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/muRhoCentralFoam.o -L/opt/openfoam210/platforms/linux64GccDPOpt/lib \
	     -lfiniteVolume -lmubasicThermophysicalModels -lspecie -lrhoCentralFoam -lcompressibleTurbulenceModel -lcompressibleRASModels -lcompressibleLESModels -lmeshTools -lOpenFOAM -ldl   -lm -o /home/USER/OpenFOAM/USER-2.1.0/platforms/linux64GccDPOpt/bin/muRhoCentralFoam
/usr/bin/ld: cannot find -lmubasicThermophysicalModels
collect2: ld returned 1 exit status
make: *** [/home/USER/OpenFOAM/USER-2.1.0/platforms/linux64GccDPOpt/bin/muRhoCentralFoam] Error 1

I also tried replacing in the file /Make/options

Code:

-lmubasicThermophysicalModels \

for the original one

Code:

-lbasicThermophysicalModels \

but it loads the main basic thermophysicalModel from OpenFoam.
Do you have any suggestions or ideas about how can I create this new basic thermophysicalModel and load it in my new solver, or what I am doing wrong?

Thanks,
Wagner Galuppo

Lisandro Maders · September 1, 2015, 08:49

Quote:

Originally Posted by wagnergaluppo

I changed the last modifications for mu on line 209 (in myBasic/basicThermo/basicThermo.C) back to

Code:

IOobject::NO_WRITE

and doing so reverted to the original configuration of OpenFoam for basic thermophysical property. I recompiled it overwriting my last changes.

Now OpenFoam is using the original configuration, and so I try to make a new basic thermoPhysical model.

First, I reset mu to AUTO_WRITE (since I want to output mu).

Next, I changed line 27 in the file myBasic/Make/files from

Code:

LIB = $(FOAM_USER_LIBBIN)/libbasicThermophysicalModels

to:

Code:

LIB = $(FOAM_USER_LIBBIN)/libmubasicThermophysicalModels

and compiled it with the wmake libso command.

Then I copied rhoCentralFoam solver to my workplace and renamed the directory from /rhoCentralFoam/ to /muRhoCentralFoam/, and after that in the new /muRhoCentralFoam/ directory I changed the file from rhoCentralFoam.C to muRhoCentralFoam.C.

Code:

$ cd /opt/opefoam210/
$ cp -r --parents applications/solvers/compressible/rhoCentralFoam/ $WM_PROJECT_USER_DIR
$ cd $WM_PROJECT_USER_DIR/applications/solvers/compressible/
$ mv rhoCentralFoam muRhoCentralFoam
$ cd muRhoCentralFoam
$ mv rhoCentralFoam.C muRhoCentralFoam.C

Next, in the /muRhoCentralFoam/Make/ directory I changed the file files from

Code:

rhoCentralFoam.C

EXE = $(FOAM_APPBIN)/rhoCentralFoam

to

Code:

muRhoCentralFoam.C

EXE = $(FOAM_USER_APPBIN)/muRhoCentralFoam

And the file options from

Code:

EXE_INC = \
    -IBCs/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/turbulenceModels/compressible/turbulenceModel \
    -I$(LIB_SRC)/dynamicMesh/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lbasicThermophysicalModels \
    -lspecie \
    -lrhoCentralFoam \
    -lcompressibleTurbulenceModel \
    -lcompressibleRASModels \
    -lcompressibleLESModels \
    -lmeshTools

to

Code:

EXE_INC = \
    -IBCs/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(WM_PROJECT_USER_DIR)/src/thermophysicalModels/myBasic/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/turbulenceModels/compressible/turbulenceModel \
    -I$(LIB_SRC)/dynamicMesh/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude

EXE_LIBS = \
    -lfiniteVolume \
    -lmubasicThermophysicalModels \
    -lspecie \
    -lrhoCentralFoam \
    -lcompressibleTurbulenceModel \
    -lcompressibleRASModels \
    -lcompressibleLESModels \
    -lmeshTools

Then I tried to compile it, but it cannot find -lmubasicThermophysicalModels, the solver compilation is not reading my new basic thermophysicalModel.

Copilation error message:

Code:

Making dependency list for source file muRhoCentralFoam.C
SOURCE=muRhoCentralFoam.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -IBCs/lnInclude -I/opt/openfoam210/src/finiteVolume/lnInclude -I/home/USER/OpenFOAM/USER-2.1.0/src/thermophysicalModels/myBasic/lnInclude -I/opt/openfoam210/src/thermophysicalModels/specie/lnInclude -I/opt/openfoam210/src/turbulenceModels/compressible/turbulenceModel -I/opt/openfoam210/src/dynamicMesh/lnInclude -I/opt/openfoam210/src/meshTools/lnInclude -IlnInclude -I. -I/opt/openfoam210/src/OpenFOAM/lnInclude -I/opt/openfoam210/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/muRhoCentralFoam.o
/opt/openfoam210/src/finiteVolume/lnInclude/readTimeControls.H: In function ‘int main(int, char**)’:
/opt/openfoam210/src/finiteVolume/lnInclude/readTimeControls.H:32: warning: unused variable ‘adjustTimeStep’
/opt/openfoam210/src/finiteVolume/lnInclude/readTimeControls.H:35: warning: unused variable ‘maxCo’
/opt/openfoam210/src/finiteVolume/lnInclude/readTimeControls.H:38: warning: unused variable ‘maxDeltaT’
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -IBCs/lnInclude -I/opt/openfoam210/src/finiteVolume/lnInclude -I/home/USER/OpenFOAM/USER-2.1.0/src/thermophysicalModels/myBasic/lnInclude -I/opt/openfoam210/src/thermophysicalModels/specie/lnInclude -I/opt/openfoam210/src/turbulenceModels/compressible/turbulenceModel -I/opt/openfoam210/src/dynamicMesh/lnInclude -I/opt/openfoam210/src/meshTools/lnInclude -IlnInclude -I. -I/opt/openfoam210/src/OpenFOAM/lnInclude -I/opt/openfoam210/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/muRhoCentralFoam.o -L/opt/openfoam210/platforms/linux64GccDPOpt/lib \
         -lfiniteVolume -lmubasicThermophysicalModels -lspecie -lrhoCentralFoam -lcompressibleTurbulenceModel -lcompressibleRASModels -lcompressibleLESModels -lmeshTools -lOpenFOAM -ldl   -lm -o /home/USER/OpenFOAM/USER-2.1.0/platforms/linux64GccDPOpt/bin/muRhoCentralFoam
/usr/bin/ld: cannot find -lmubasicThermophysicalModels
collect2: ld returned 1 exit status
make: *** [/home/USER/OpenFOAM/USER-2.1.0/platforms/linux64GccDPOpt/bin/muRhoCentralFoam] Error 1

I also tried replacing in the file /Make/options

Code:

-lmubasicThermophysicalModels \

for the original one

Code:

-lbasicThermophysicalModels \

but it loads the main basic thermophysicalModel from OpenFoam.
Do you have any suggestions or ideas about how can I create this new basic thermophysicalModel and load it in my new solver, or what I am doing wrong?

Thanks,
Wagner Galuppo

Hello Wagner,

did you figure out your issue? It would be good if you write what you have done then other people could make use of this knowledge as well. I am trying to make a very similar implementation and I am getting similar errors..

Regards,

Lisandro

olivierG · September 1, 2015, 10:04

Hello,

You don't need to do this to output viscosity, just use the functions objects "writeRegisteredObject".
ex:

Code:

{
type writeRegisteredObject;
functionObjectLibs ("libIOFunctionObjects.so");
objectNames ("bananas");
outputControl outputTime;
outputInterval 1;
}

Here, "bananas" will give you the list of all registered object, replace by the one you want.

regards,
olivier

Lisandro Maders · September 1, 2015, 10:42

Thanks for your tip Olivier, it seems much more straightforward and ease to get this value.

However, I am not able to find it working.

I put transportProperties instead of bananas but it does not write the nu field in any step.. (by the way,I think I am doing the basic things right. I put the "functions" subdict in the controlDict file, etc..)

Lisandro

olivierG · September 1, 2015, 10:49

hello,

Yes, function object should be in controlDict.
First, run your solver with bananas => you will get an error message with the full list of possible object, and there is no bananas.
Then, pick up the good one (name here can be something::nu instead of nu)

regards,
olivier

Lisandro Maders · September 3, 2015, 09:10

Hi Olivier,

Does it work even if my viscosity has a constant value in all points? Because it seems not to be working.. The maximum I got was having a nu file in the time directories when I created it as a volScalarField in the createFields.H file in the solver directory..

Regards,
Lisandro

Lisandro Maders · September 11, 2015, 09:24

I solved it a couple of days ago, here is what I have done in order to make it:

I wanted to write the viscosity and Cp values any written time in the case folder.

1. In the createFields.H file:

Code:

 
volScalarField mu_output
(
    IOobject
    (
        "mu_output",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    turbulence->mu()
);

and

Code:

volScalarField cp_output
(
    IOobject
    (
        "cp_output",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    thermo.Cp()
);

2. In the solver.C file:

Code:

    while (runTime.run())
    {
        ....
        ....

        runTime.write();

        mu_output = turbulence->mu();
        cp_output = thermo.Cp();
    
    }

That worked for me! Later when I finish my project I will try to use the functionObject tool as recommended by Olivier. It seems much easier but I was not able to make it work! Thanks anyway!

Regards,

Lisandro

thunde47 · December 14, 2015, 17:24

I want to plot Reynold's number. Not, Reynold's number is dependent on velocity. So, all I should do is provide a formula to calculate Re in the code. Also, I am going to calculate Re with mag(U). Please suggest how to incorporate these features in the code. I will appreciate if replies are relevant to icoFoam solver.

hcl734 · January 5, 2016, 03:12

Hi olivier,

your approach using function objects seems quite comfortable and I can reproduce some results for the thermo:... properties.
But when I put thermophysicalProperties for function object names, there is no result at all.
It says writing thermophysicalProperties object in the log-file but there is no output.
Ok there seems to be a bug in this function since it manipulates the header of the thermophysicalProperties-Dict adding the thermoType{...} entries into the FoamFile-header.
Could you help me to figure this one out?

olivierG · January 5, 2016, 03:40

hello,

function object work only with registered object. So there is 2 solution:
1) the properties you want is an object => just use the fuctionObject
2) you need some coding, and create a custom solver

the part 2) is easy, so don"t be scare.

regards,
olivier

April 23, 2012, 18:13	How to output other properties?	#1
wagnergaluppo New Member Wagner C. Galuppo Join Date: Feb 2012 Location: Portugal Posts: 12 Rep Power: 14	Hi, I am using the OpenFOAM-210 and I Know that with foamCalc utility I can get the components of velocity and I also know how to get mach number and vorticity, but does anybody know how to output other variables such as viscosity, Reynolds number and etc? thanks, Wagner

April 24, 2012, 02:42		#2
akidess Senior Member Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,377 Rep Power: 29	Viscosity will be written to the time directories if it's not constant, and you can plot it with paraview. You can also use paraview to calculate the Reynolds number. If you want a command line utility, you'll have to get your hands dirty. __________________ On twitter @akidTwit Spend as much time formulating your questions as you expect people to spend on their answer.

May 1, 2012, 14:42	sutherland viscosity	#4
wagnergaluppo New Member Wagner C. Galuppo Join Date: Feb 2012 Location: Portugal Posts: 12 Rep Power: 14	Hi Akidess, I followed your suggestion and set the viscosity to sutherland. Now that the viscosity is not constant, I would have expected it to write to the time directories like you suggested. Unfortunately, viscosity does not appear in any of the time directories. Have I missed something? Here is the output of my thermophysical properties Code: FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object thermophysicalProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // thermoType ePsiThermo<pureMixture<sutherlandTransport<specieThermo<eConstThermo<perfectGas>>>>>; mixture { // normalised gas specie { nMoles 1; molWeight 50; } thermodynamics { Cv 1007.8039105; Hf 2.544e+06; } transport { As 1.67212e-06; Ts 170.672; } }

May 1, 2012, 14:48	createfields.H	#5
wagnergaluppo New Member Wagner C. Galuppo Join Date: Feb 2012 Location: Portugal Posts: 12 Rep Power: 14	This is what I've specified in the createfields.H file Code: const volScalarField& psi = thermo.psi(); volScalarField mu ( IOobject ( "mu", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh );

May 2, 2012, 03:39		#6
akidess Senior Member Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,377 Rep Power: 29	Which solver are you using? I'll try it out and see if I can get it to work. __________________ On twitter @akidTwit Spend as much time formulating your questions as you expect people to spend on their answer.

April 26, 2012, 23:51		#3
wagnergaluppo New Member Wagner C. Galuppo Join Date: Feb 2012 Location: Portugal Posts: 12 Rep Power: 14	Thank you for your reply. I'm ready to get my hands dirty. Even though my viscosity is constant, I would still like to know how to output it at each time-step. I would like to verify that I am getting the correct value for my viscosity. I'm using the rhoCentralFoam solver. This is the output of the "createFields.H" file: 13--> const volScalarField& mu = thermo.mu(); So what I did was change this file to something like this: 13--> volScalarField mu 14--> ( 15--> IOobject 16--> ( 17--> "mu", 18--> runTime.timeName(), 19--> mesh, 20--> IOobject::MUST_READ, 21--> IOobject::AUTO_WRITE 22--> ), 23--> mesh 24--> ); Then I recompiled and created a "mu" file at my "/0/" directory. But after I running, the other time directories do not have the mu property. It's not autowriting as ordered. For the Reynolds number I'm still having problems. Do you know of any documentation about the command line utility for this? thanks, Wagner

May 2, 2012, 12:36		#7
wagnergaluppo New Member Wagner C. Galuppo Join Date: Feb 2012 Location: Portugal Posts: 12 Rep Power: 14	I'm using the rhoCentralFoam. Thanks, Wagner

May 16, 2012, 15:28		#8
wagnergaluppo New Member Wagner C. Galuppo Join Date: Feb 2012 Location: Portugal Posts: 12 Rep Power: 14	I figure it out. Thank you, Wagner Galuppo

May 19, 2012, 05:09		#9
akidess Senior Member Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,377 Rep Power: 29	Sorry I couldn't help much, I got busy with other things. Can you add a post on how you solved the problem? It might help others in the future. __________________ On twitter @akidTwit Spend as much time formulating your questions as you expect people to spend on their answer.

May 24, 2012, 12:29		#10
wagnergaluppo New Member Wagner C. Galuppo Join Date: Feb 2012 Location: Portugal Posts: 12 Rep Power: 14	Actually I partly figured it out. I found the file "basicThermo.C" in (/opt/openfoam210/src/thermophysicalModels/basic/basicThermo/) If you have look from the 201st until 213th line you will find this: Code: mu_ ( IOobject ( "mu", mesh.time().timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), mesh, dimensionSet(1, -1, -1, 0, 0) ), I copied the directory (/opt/openfoam210/src/thermophysicalModels/basic/) to my workplace and I changed the name from /basic/ to /myBasic/. in terminal: Code: $ cd /opt/openfoam210 $ cp -r --parents src/thermophysicalModels/basic/ /home/cfd02/OpenFOAM/USER-2.1.0/ $ cd ~/OpenFOAM/USER-2.1.0/src/thermophysicalModels/ $ mv basic myBasic Next I edited line 209 in the file myBasic/basicThermo/basicThermo.C from: Code: IOobject::NO_WRITE to Code: IOobject::AUTO_WRITE and saved and closed it. Then I changed the 27th line in the file myBasic/Make/files from: Code: LIB = $(FOAM_LIBBIN)/libbasicThermophysicalModels to Code: LIB = $(FOAM_USER_LIBBIN)/libbasicThermophysicalModels and saved and closed it. Next I compiled the code: Code: $ cd ~/OpenFOAM/USER-2.1.0/src/thermophysicalModels/myBasic/ $ wmake libso It works, if you run rhoCentralFoam will output mu and doesn't matter if it is constant. The Problem is that I'm overwriting the main library basicThermophysicalModels instead of creating a new one.

September 1, 2015, 10:04		#13
olivierG Senior Member Olivier Join Date: Jun 2009 Location: France, grenoble Posts: 272 Rep Power: 17	Hello, You don't need to do this to output viscosity, just use the functions objects "writeRegisteredObject". ex: Code: { type writeRegisteredObject; functionObjectLibs ("libIOFunctionObjects.so"); objectNames ("bananas"); outputControl outputTime; outputInterval 1; } Here, "bananas" will give you the list of all registered object, replace by the one you want. regards, olivier LuckyTran, hcl734 and anfaenger like this.

September 1, 2015, 10:42		#14
Lisandro Maders Member Lisandro Maders Join Date: Feb 2013 Posts: 98 Rep Power: 13	Thanks for your tip Olivier, it seems much more straightforward and ease to get this value. However, I am not able to find it working. I put transportProperties instead of bananas but it does not write the nu field in any step.. (by the way,I think I am doing the basic things right. I put the "functions" subdict in the controlDict file, etc..) Lisandro

September 1, 2015, 10:49		#15
olivierG Senior Member Olivier Join Date: Jun 2009 Location: France, grenoble Posts: 272 Rep Power: 17	hello, Yes, function object should be in controlDict. First, run your solver with bananas => you will get an error message with the full list of possible object, and there is no bananas. Then, pick up the good one (name here can be something::nu instead of nu) regards, olivier

September 3, 2015, 09:10		#16
Lisandro Maders Member Lisandro Maders Join Date: Feb 2013 Posts: 98 Rep Power: 13	Hi Olivier, Does it work even if my viscosity has a constant value in all points? Because it seems not to be working.. The maximum I got was having a nu file in the time directories when I created it as a volScalarField in the createFields.H file in the solver directory.. Regards, Lisandro

September 11, 2015, 09:24		#17
Lisandro Maders Member Lisandro Maders Join Date: Feb 2013 Posts: 98 Rep Power: 13	I solved it a couple of days ago, here is what I have done in order to make it: I wanted to write the viscosity and Cp values any written time in the case folder. 1. In the createFields.H file: Code: volScalarField mu_output ( IOobject ( "mu_output", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), turbulence->mu() ); and Code: volScalarField cp_output ( IOobject ( "cp_output", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), thermo.Cp() ); 2. In the solver.C file: Code: while (runTime.run()) { .... .... runTime.write(); mu_output = turbulence->mu(); cp_output = thermo.Cp(); } That worked for me! Later when I finish my project I will try to use the functionObject tool as recommended by Olivier. It seems much easier but I was not able to make it work! Thanks anyway! Regards, Lisandro Kummi, shock77 and S1mple like this.

December 14, 2015, 17:24	and Reynold's number	#18
thunde47 Senior Member thunde47 Join Date: Dec 2015 Location: India, USA Posts: 129 Blog Entries: 1 Rep Power: 10	I want to plot Reynold's number. Not, Reynold's number is dependent on velocity. So, all I should do is provide a formula to calculate Re in the code. Also, I am going to calculate Re with mag(U). Please suggest how to incorporate these features in the code. I will appreciate if replies are relevant to icoFoam solver.

January 5, 2016, 03:12		#19
hcl734 Member Join Date: May 2015 Posts: 68 Rep Power: 10	Hi olivier, your approach using function objects seems quite comfortable and I can reproduce some results for the thermo:... properties. But when I put thermophysicalProperties for function object names, there is no result at all. It says writing thermophysicalProperties object in the log-file but there is no output. Ok there seems to be a bug in this function since it manipulates the header of the thermophysicalProperties-Dict adding the thermoType{...} entries into the FoamFile-header. Could you help me to figure this one out?

January 5, 2016, 03:40		#20
olivierG Senior Member Olivier Join Date: Jun 2009 Location: France, grenoble Posts: 272 Rep Power: 17	hello, function object work only with registered object. So there is 2 solution: 1) the properties you want is an object => just use the fuctionObject 2) you need some coding, and create a custom solver the part 2) is easy, so don"t be scare. regards, olivier S1mple likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
mass flow in is not equal to mass flow out	saii	CFX	12	March 19, 2018 05:21
error message	cuteapathy	CFX	14	March 20, 2012 06:45
Constant velocity of the material	Sas	CFX	15	July 13, 2010 08:56
lift and drag on ship superstructures	vaina74	OpenFOAM Running, Solving & CFD	3	June 8, 2010 12:30
Two-Phase Buoyant Flow Issue	Miguel Baritto	CFX	4	August 31, 2006 12:02