Explanation of thermophysical variables (e.g. kappa) + tutorial example

MBttR · August 4, 2016, 10:09

Hi,

I was wondering if someone has an overview of the thermophysical variables used in OpenFOAM and their explanation and units? For example I have most difficulty with kappa, I can't seem to figure out what it stands for, nor can Google. I looked in src/transportModels but I'm not sure..

Also, I thought Hf was Heat of Fusion expressed in kJ/kg. For steel this is roughly 260. In the chtMultiRegionFoam/heater tutorial however, this is 0 (see below). Am I wrong? I assume the heater in this tutorial is approximated by steel, judging from the density and Cp.

Thanks!

Code:

mixture
{
    specie
    {
        nMoles      1;
        molWeight   50;
    }

    transport
    {
        kappa   80;
    }

    thermodynamics
    {
        Hf      0;
        Cp      450;
    }

    equationOfState
    {
        rho     8000;
    }
}

MBttR · August 4, 2016, 10:47

Hi!

It seems that Hf = 0 for simulations with just one fluid type, as there is no fusion happening. Still looking for kappa though.

Cheers!

http://www.cfd-online.com/Forums/ope...roperties.html
http://www.cfd-online.com/Forums/ope...n-hf-role.html

Coris · August 4, 2016, 10:58

kappa is the thermal conductivity

Bloerb · August 4, 2016, 11:41

http://cfd.direct/openfoam/user-guide/thermophysical/ gives a decent description. As mentioned kappa is the thermal conductivity. (not the thermal diffusivity)

MBttR · August 4, 2016, 19:21

Thanks Bloerb and Coris! That's in W/(m*K) I assume? I looked over it in the manual, I was scanning for the word kappa and looked over the Greek letter.

Is natural convection automatically active in simpleFoam? I have a heat source using fvOptions, and am afraid the temperature will just keep increasing into infinity. I am solving a single heater in a body of air. I think I am confusing convection and conduction. Is this kappa (thermal conductivity) defininig natural convection and is forced convection following from my boundary conditions on e.g. U?

Cheers!

Coris · August 5, 2016, 04:35

You have to use chtMuliRegion(Simple)Foam or one of the Boussinesq solver for that. Here is a good overview: https://github.com/OpenFOAM/OpenFOAM...s/heatTransfer

What is your exact geometry and BC? I am also studying a case with NC (natural convection).

Thermal conductivity is in W/(mK) yes. I think you have to check some theory or at least look at some heat transfer correlations. They will make clear which quantities are important. Generally, this are the Reynolds and Prandtl numbers for forced and Grashof and Prandtl for natural convection.

MBttR · August 5, 2016, 05:37

Ah yes Coris, my bad, I meant chtMultiRegionSimpleFoam, not simpleFoam

I asked about the units mainly because OpenFOAM sometimes does some division that you need to be aware of (which I guess is mainly in the case of things related to dynamic pressure), or works in different units as expected.

Anyway! I was just about to post before you posted, I think I get it.

Natural convection is governed by the Rayleigh number. This requires kinematic viscosity, which can be calculated from dynamic viscosity and rho. It requires thermal diffusivity, which can be calculated from kappa, rho and cp. It require the thermal expansion coefficient which can be approximated by 1/T. Forced convection is just governed by the same coefficients, with the addition of velocity.

Conduction seems to be pretty much just governed by kappa and is the exact same thing as diffusion.

Please let me know if I am right at all. I was confused and posted this thread because indeed I was not seeing all the relations behind it and wanted to know if all methods of heat transfer were governed by just these few thermphysical properties. I also think it's not a matter of "activating" forced or free convection, as they are always present in these heat transfer solvers?

Also my solution did indeed stabilize, just at a way too high temperature than expected from testing. Now that I know the variables better, I can try again.

And concerning my geometry: I am researching the heating of an electric motor with a rotor. The rotor is not present in the model, the motor is just modelled as a ring, representing the motor coils. This is of course an approximation, since I now still model the coils as one material block while in reality there are slots and it is made of copper and iron. I do think however I should be able to get close enough by using average values. I'll update this post in a few minutes from my linux machine with BCs.

Cheers, thanks!

*edit*
Boundary Conditions. So remember I have an air volume shaped as a block with air flowing in on one side and flowing out the other. These are not exact copies, I edited them to shorten the post For the air volume:

T

Code:

internalField   uniform 294;

boundaryField
{
    minX, maxX, minY, maxY, minZ and maxZ
    {
        type            zeroGradient;
        value           uniform 294;
    }
    air_to_motorcoil
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 294;
        Tnbr            T;
        kappaMethod     fluidThermo;
    }
}

U (very low velocity) I should probably make minY, maxY, minX and maxX zeroGradient in stead of fixedValue to better approach my test values, which were on a bench in open space.

Code:

internalField   uniform ( 0 0 0.1 );

boundaryField
{
    minZ
    {
        type            fixedValue;
        value           uniform ( 0 0 0.1 );
    }
    maxZ
    {
        type            inletOutlet;
        value           uniform ( 0 0 0.1 );
        inletValue      uniform ( 0 0 0 );
    }
    minY, maxY, minX and maxX
    {
        type            fixedValue;
        value           uniform ( 0 0 0 );
    }
    air_to_motorcoil
    {
        type            fixedValue;
        value           uniform ( 0 0 0 );
    }
}

k

Code:

internalField   uniform 0.1;

boundaryField
{
    minZ
    {
        type            fixedValue;
        value           uniform 0.1;
    }
    maxZ
    {
        type            inletOutlet;
        value           uniform 0.1;
        inletValue      uniform 0.1;
    }
    minY, maxY, minX and maxX
    {
        type            kqRWallFunction;
        value           uniform 0.1;
    }
    air_to_motorcoil
    {
        type            kqRWallFunction;
        value           uniform 0.1;
    }
}

For the coils:
T:

Code:

internalField   uniform 300;

boundaryField
{
    motorcoil_to_air
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value           uniform 294;
        Tnbr            T;
        kappaMethod     solidThermo;
    }
}

U:

Code:

internalField   uniform (0 0 0);

boundaryField
{
    motorcoil_to_air
    {
        type            calculated;
        value           uniform (0 0 0);
    }
}

k:

Code:

internalField   uniform 0;

boundaryField
{
    motorcoil_to_air
    {
        type            calculated;
        value           uniform 0;
    }
}

Also have this fvOptions in motorcoil/system:

Code:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvOptions;
}

volumetricHeatSource
{
    type            scalarSemiImplicitSource;
    active          true;

    
    scalarSemiImplicitSourceCoeffs
    {
        volumeMode      absolute;
        selectionMode   all;  //cellSet // points //all  (other options)
        injectionRateSuSp
        {
            h (40 0);   // S(T)=S_u+S_p*T  ===>  S_u=g    S_p=0   
        }              // g= specific volumetric generation (W/m3)
    }                  // g= absolute volumetric generation (W) ===> in the example 3W are considered
}

Coris · August 5, 2016, 05:50

Quote:

Originally Posted by MBttR

Ah yes Coris, my bad, I meant
Please let me know if I am right at all. I was confused and posted this thread because indeed I was not seeing all the relations behind it and wanted to know if all methods of heat transfer were governed by just these few thermphysical properties. I also think it's not a matter of "activating" forced or free convection, as they are always present in these heat transfer solvers?

Cheers, thanks!

You can deactivate NC by making the density independent of temperature. That works for eg water, but I don't know by heart how it works for gases (can you set beta to zero explicitly?).

MBttR · August 5, 2016, 06:03

Quote:

Originally Posted by Coris

You can deactivate NC by making the density independent of temperature. That works for eg water, but I don't know by heart how it works for gases (can you set beta to zero explicitly?).

I'm not familiar enough with heat transfer problems to judge whether NC is negligible. Surely, even with a fan this must still play some effect?

And I don't think you can specify beta specifically.

Updated my post with BCs, if you can take a look at that?

Cheers!

MBttR · August 5, 2016, 06:53

If I switch my boundaries on U from fixedValue (0 0 0) to zeroGradient my air temperature decreases (already under 0°C and descending), which clearly doesn't make sense. Any clue what's wrong?

Coris · August 8, 2016, 03:34

Seeing your heat source, my first guess is that it's role will be negligible in NC. But you can check it by setting g to 0.

There is something odd with your BC's. You should set the inlet velocity at and zeroGradient pressure at the inlet side and zeroGradient velocity and zero pressure at the outlet.

The problem you experience is related to the BC for temperature. I advise to set it to inletOutlet.

August 4, 2016, 10:09	Explanation of thermophysical variables (e.g. kappa) + tutorial example	#1
MBttR Member Bruno Join Date: Jun 2016 Location: Siegen, Germany Posts: 59 Rep Power: 10	Hi, I was wondering if someone has an overview of the thermophysical variables used in OpenFOAM and their explanation and units? For example I have most difficulty with kappa, I can't seem to figure out what it stands for, nor can Google. I looked in src/transportModels but I'm not sure.. Also, I thought Hf was Heat of Fusion expressed in kJ/kg. For steel this is roughly 260. In the chtMultiRegionFoam/heater tutorial however, this is 0 (see below). Am I wrong? I assume the heater in this tutorial is approximated by steel, judging from the density and Cp. Thanks! Code: mixture { specie { nMoles 1; molWeight 50; } transport { kappa 80; } thermodynamics { Hf 0; Cp 450; } equationOfState { rho 8000; } }

August 4, 2016, 10:58		#3
Coris New Member Joris C. Join Date: Jan 2013 Posts: 29 Rep Power: 13	kappa is the thermal conductivity saidc. and madmemed like this.

August 5, 2016, 05:37		#7
MBttR Member Bruno Join Date: Jun 2016 Location: Siegen, Germany Posts: 59 Rep Power: 10	Ah yes Coris, my bad, I meant chtMultiRegionSimpleFoam, not simpleFoam I asked about the units mainly because OpenFOAM sometimes does some division that you need to be aware of (which I guess is mainly in the case of things related to dynamic pressure), or works in different units as expected. Anyway! I was just about to post before you posted, I think I get it. Natural convection is governed by the Rayleigh number. This requires kinematic viscosity, which can be calculated from dynamic viscosity and rho. It requires thermal diffusivity, which can be calculated from kappa, rho and cp. It require the thermal expansion coefficient which can be approximated by 1/T. Forced convection is just governed by the same coefficients, with the addition of velocity. Conduction seems to be pretty much just governed by kappa and is the exact same thing as diffusion. Please let me know if I am right at all. I was confused and posted this thread because indeed I was not seeing all the relations behind it and wanted to know if all methods of heat transfer were governed by just these few thermphysical properties. I also think it's not a matter of "activating" forced or free convection, as they are always present in these heat transfer solvers? Also my solution did indeed stabilize, just at a way too high temperature than expected from testing. Now that I know the variables better, I can try again. And concerning my geometry: I am researching the heating of an electric motor with a rotor. The rotor is not present in the model, the motor is just modelled as a ring, representing the motor coils. This is of course an approximation, since I now still model the coils as one material block while in reality there are slots and it is made of copper and iron. I do think however I should be able to get close enough by using average values. I'll update this post in a few minutes from my linux machine with BCs. Cheers, thanks! edit Boundary Conditions. So remember I have an air volume shaped as a block with air flowing in on one side and flowing out the other. These are not exact copies, I edited them to shorten the post For the air volume: T Code: internalField uniform 294; boundaryField { minX, maxX, minY, maxY, minZ and maxZ { type zeroGradient; value uniform 294; } air_to_motorcoil { type compressible::turbulentTemperatureCoupledBaffleMixed; value uniform 294; Tnbr T; kappaMethod fluidThermo; } } U (very low velocity) I should probably make minY, maxY, minX and maxX zeroGradient in stead of fixedValue to better approach my test values, which were on a bench in open space. Code: internalField uniform ( 0 0 0.1 ); boundaryField { minZ { type fixedValue; value uniform ( 0 0 0.1 ); } maxZ { type inletOutlet; value uniform ( 0 0 0.1 ); inletValue uniform ( 0 0 0 ); } minY, maxY, minX and maxX { type fixedValue; value uniform ( 0 0 0 ); } air_to_motorcoil { type fixedValue; value uniform ( 0 0 0 ); } } k Code: internalField uniform 0.1; boundaryField { minZ { type fixedValue; value uniform 0.1; } maxZ { type inletOutlet; value uniform 0.1; inletValue uniform 0.1; } minY, maxY, minX and maxX { type kqRWallFunction; value uniform 0.1; } air_to_motorcoil { type kqRWallFunction; value uniform 0.1; } } For the coils: T: Code: internalField uniform 300; boundaryField { motorcoil_to_air { type compressible::turbulentTemperatureCoupledBaffleMixed; value uniform 294; Tnbr T; kappaMethod solidThermo; } } U: Code: internalField uniform (0 0 0); boundaryField { motorcoil_to_air { type calculated; value uniform (0 0 0); } } k: Code: internalField uniform 0; boundaryField { motorcoil_to_air { type calculated; value uniform 0; } } Also have this fvOptions in motorcoil/system: Code: FoamFile { version 2.0; format ascii; class dictionary; object fvOptions; } volumetricHeatSource { type scalarSemiImplicitSource; active true; scalarSemiImplicitSourceCoeffs { volumeMode absolute; selectionMode all; //cellSet // points //all (other options) injectionRateSuSp { h (40 0); // S(T)=S_u+S_p*T ===> S_u=g S_p=0 } // g= specific volumetric generation (W/m3) } // g= absolute volumetric generation (W) ===> in the example 3W are considered }

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Accessing thermoPhysical Property Functions - e.g. mixture_.rho(scalar p, scalar T)	will.logie	OpenFOAM Programming & Development	2	June 24, 2015 00:38
Explanation of airFoil2D tutorial in OpenFOAM	akku	OpenFOAM Running, Solving & CFD	0	February 28, 2013 01:21

August 4, 2016, 10:47		#2
MBttR Member Bruno Join Date: Jun 2016 Location: Siegen, Germany Posts: 59 Rep Power: 10	Hi! It seems that Hf = 0 for simulations with just one fluid type, as there is no fusion happening. Still looking for kappa though. Cheers! http://www.cfd-online.com/Forums/ope...roperties.html http://www.cfd-online.com/Forums/ope...n-hf-role.html

August 4, 2016, 11:41		#4
Bloerb Senior Member Join Date: Sep 2013 Posts: 353 Rep Power: 21	http://cfd.direct/openfoam/user-guide/thermophysical/ gives a decent description. As mentioned kappa is the thermal conductivity. (not the thermal diffusivity)

August 4, 2016, 19:21		#5
MBttR Member Bruno Join Date: Jun 2016 Location: Siegen, Germany Posts: 59 Rep Power: 10	Thanks Bloerb and Coris! That's in W/(m*K) I assume? I looked over it in the manual, I was scanning for the word kappa and looked over the Greek letter. Is natural convection automatically active in simpleFoam? I have a heat source using fvOptions, and am afraid the temperature will just keep increasing into infinity. I am solving a single heater in a body of air. I think I am confusing convection and conduction. Is this kappa (thermal conductivity) defininig natural convection and is forced convection following from my boundary conditions on e.g. U? Cheers!

August 5, 2016, 04:35		#6
Coris New Member Joris C. Join Date: Jan 2013 Posts: 29 Rep Power: 13	You have to use chtMuliRegion(Simple)Foam or one of the Boussinesq solver for that. Here is a good overview: https://github.com/OpenFOAM/OpenFOAM...s/heatTransfer What is your exact geometry and BC? I am also studying a case with NC (natural convection). Thermal conductivity is in W/(mK) yes. I think you have to check some theory or at least look at some heat transfer correlations. They will make clear which quantities are important. Generally, this are the Reynolds and Prandtl numbers for forced and Grashof and Prandtl for natural convection.

August 5, 2016, 06:53		#10
MBttR Member Bruno Join Date: Jun 2016 Location: Siegen, Germany Posts: 59 Rep Power: 10	If I switch my boundaries on U from fixedValue (0 0 0) to zeroGradient my air temperature decreases (already under 0°C and descending), which clearly doesn't make sense. Any clue what's wrong?

August 8, 2016, 03:34		#11
Coris New Member Joris C. Join Date: Jan 2013 Posts: 29 Rep Power: 13	Seeing your heat source, my first guess is that it's role will be negligible in NC. But you can check it by setting g to 0. There is something odd with your BC's. You should set the inlet velocity at and zeroGradient pressure at the inlet side and zeroGradient velocity and zero pressure at the outlet. The problem you experience is related to the BC for temperature. I advise to set it to inletOutlet.