CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Programming & Development

Adding different properties to Thermophysical Model

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

Like Tree2Likes
  • 1 Post By DanAndrea87
  • 1 Post By tomislav_maric

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 27, 2014, 15:16
Default Adding different properties to Thermophysical Model
  #1
New Member
 
DanAndrea87's Avatar
 
Andrea Prestigiacomo
Join Date: Jun 2013
Location: Milan
Posts: 10
Rep Power: 13
DanAndrea87 is on a distinguished road
Hi,

I'm trying to change the thermal conductivity and heat capacity in a solid region, depending on position. I've already create the file Kappa and Cp in the 0/solid directory with the command:

Code:
setFields -region solid
Now I'm changing the solver.
The first idea was to simply import these quantities, with this code, in the createSolidFields.H file

Code:
KappaSolid.set
(
    i,
    new volScalarField
    (
        IOobject
        (
            "Kappa",
            runTime.timeName(),
            solidRegions[i],
            IOobject::READ_IF_PRESENT,
            IOobject::AUTO_WRITE
        ),
        solidRegions[i]
    )
);
And it works for the solid, but there is a problem in coupling with fluid region.
The problem is that the coupling fvPatch read the solid thermal conductivity from thermo.kappa().
So now my goal is to replace the thermo.kappa() with the readed values, directly in the file createSolidFields.H.
I've tried booth these codes, without results:

Code:
KappaSolid.set
(
    i,
    new volScalarField
    (
        IOobject
        (
            "Kappa",
            runTime.timeName(),
            solidRegions[i],
            IOobject::READ_IF_PRESENT,
            IOobject::AUTO_WRITE
        ),
        solidRegions[i]
    )
);
thermos[i].kappa() = KappaSolid[i];
Code:
thermos[i].kappa() = IOdictionary
(
    IOobject
    (
        "Kappa",
        runTime.timeName(),
        solidRegions[i],
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    )
);
Any ideas?
Thanks for the help
DanAndrea87 is offline   Reply With Quote

Old   April 28, 2014, 04:40
Default
  #2
Senior Member
 
Tomislav Maric
Join Date: Mar 2009
Location: Darmstadt, Germany
Posts: 284
Blog Entries: 5
Rep Power: 21
tomislav_maric is on a distinguished road
Which solver and which OF version are you using?
__________________
When asking a question, prepare a SSCCE.
tomislav_maric is offline   Reply With Quote

Old   April 28, 2014, 05:08
Default
  #3
New Member
 
DanAndrea87's Avatar
 
Andrea Prestigiacomo
Join Date: Jun 2013
Location: Milan
Posts: 10
Rep Power: 13
DanAndrea87 is on a distinguished road
Thanks for reply!
I'm using OF-2.2.1 and the solver is a modified version of chtMultiregionFoam (see attachment).
Attached Files
File Type: gz trigaFoam.tar.gz (26.2 KB, 44 views)
Zhiheng Wang likes this.
DanAndrea87 is offline   Reply With Quote

Old   April 28, 2014, 05:42
Default
  #4
Senior Member
 
Tomislav Maric
Join Date: Mar 2009
Location: Darmstadt, Germany
Posts: 284
Blog Entries: 5
Rep Power: 21
tomislav_maric is on a distinguished road
I have zero experience with multiregion coupling, but I'll give you a few hints code-wise.

For a start, this line:

Code:
 PtrList<solidThermo> thermos(solidRegions.size());
States that 'thermos' is a list of pointers to 'solidThermo' objects. When you try to do this:

Code:
//    thermos[i].kappa() = KappaSolid[i];
you are assigning a volumeScalarField to a temporary object. The 'kappa' member function comes inherited from the 'basicThermo' class:

Code:
                        virtual tmp<volScalarField> kappa() const = 0;
And you can see here that the implementation of this pure virtual member function will return a temporary volScalarField. As a result, your expression has no effect.

What is it you are trying to do actually? Providing more background on the actual idea would make it easier for someone to help you...
__________________
When asking a question, prepare a SSCCE.
tomislav_maric is offline   Reply With Quote

Old   April 28, 2014, 06:13
Default
  #5
New Member
 
DanAndrea87's Avatar
 
Andrea Prestigiacomo
Join Date: Jun 2013
Location: Milan
Posts: 10
Rep Power: 13
DanAndrea87 is on a distinguished road
Well, the idea was to replace the volScalarField in kappa with the volScalarField readed from the IOobject.
But, if I've well understood, kappa is not a volScalarField. The volScalarField is generated every time the member function kappa() is called.
Is it right?
Thanks for the help.
DanAndrea87 is offline   Reply With Quote

Old   April 28, 2014, 06:25
Default
  #6
Senior Member
 
Tomislav Maric
Join Date: Mar 2009
Location: Darmstadt, Germany
Posts: 284
Blog Entries: 5
Rep Power: 21
tomislav_maric is on a distinguished road
The 'kappa()' member function generates a temporary volume scalar field.

If you are searching for a way to set such a field for an object of the 'solidThermo' class, you can easily find out if the class stores such a field:

Code:
class solidThermo
:
    public basicThermo
{

protected:

    // Protected data

        //- Density field [kg/m^3]
        //  Named 'rhoThermo' to avoid (potential) conflict with solver density
        volScalarField rho_;
or if it's parent class 'basicThermo' stores it:

Code:
class basicThermo
:
    public IOdictionary
{

protected:

    // Protected data

        //- Phase-name
        const word& phaseName_;


        // Fields

            //- Pressure [Pa]
            volScalarField& p_;

            //- Temperature [K]
            volScalarField T_;

            //- Laminar thermal diffusuvity [kg/m/s]
            volScalarField alpha_; // This might be your candidate right here.
And then you can extend the solidThermo by deriving from it and provide a public member function that modifies such a field - if it exists. If not and you need that - derive from solidThermo, add the field you want to modify and the member function that does the modification.

One thing though - looking at 'createSolidFields.H', I have noticed that the solidThermo objects are set by constructing new objects using run-time selection:

Code:
        Info<< "    Adding to thermos\n" << endl;
        thermos.set(i, solidThermo::New(solidRegions[i]));
The 'New' selector is defined in 'basicThermoTemplates.C':

Code:
template<class Thermo>
Foam::autoPtr<Thermo> Foam::basicThermo::New
(
    const fvMesh& mesh,
    const word& phaseName
)
{
    IOdictionary thermoDict
    (
        IOobject
        (
            phasePropertyName(dictName, phaseName),
            mesh.time().constant(),
            mesh,
            IOobject::MUST_READ_IF_MODIFIED,
            IOobject::NO_WRITE,
            false
        )
    );

    typename Thermo::fvMeshConstructorTable::iterator cstrIter =
        lookupThermo<Thermo, typename Thermo::fvMeshConstructorTable>
        (
            thermoDict,
            Thermo::fvMeshConstructorTablePtr_
        );

    return autoPtr<Thermo>(cstrIter()(mesh, phaseName));
}
And it seems to read a dictionary (as usual) and select the object.

So the next question is: why are you trying to do the object modification afterwards, using the volume fields, when this is not done in the original solver?

Your answer:

Quote:
Well, the idea was to replace the volScalarField in kappa with the volScalarField readed from the IOobject.
does not help me understand what you are trying to do - it doesn't explain what you are trying to do conceptually. Your explanation already describes the way you have decided to implement your idea. What is the actual idea, what are you trying to achieve? Explain it without using class names.
__________________
When asking a question, prepare a SSCCE.
tomislav_maric is offline   Reply With Quote

Old   April 28, 2014, 07:10
Default
  #7
New Member
 
DanAndrea87's Avatar
 
Andrea Prestigiacomo
Join Date: Jun 2013
Location: Milan
Posts: 10
Rep Power: 13
DanAndrea87 is on a distinguished road
Ok, i will try to explain better: the problem is in the coupling between solid and fluids regions. In particular the coupling boundary condition (compressible::turbulentTemperatureCoupledBaffleMix ed) takes into account the conservation of heat flux between patches as follow:

kappa_fluid*d(T_fluid)/dn = kappa_solid*d(T_solid)/dn

where n is the vector normal to the contact surface.
The problem is that kappa_solid is taken form the thermophysicalProperties file in constant/solid (in which the thermal conductivity is a constant for the whole solid), while I need to use the value taken from the IOobject (because my solid has different thermal conductivity, depending on position).
At this point, probably, it's more convenient to modify the fvPatchScalarField library...
DanAndrea87 is offline   Reply With Quote

Old   April 29, 2014, 07:02
Default
  #8
Senior Member
 
Tomislav Maric
Join Date: Mar 2009
Location: Darmstadt, Germany
Posts: 284
Blog Entries: 5
Rep Power: 21
tomislav_maric is on a distinguished road
Quote:
Originally Posted by DanAndrea87 View Post
In particular the coupling boundary condition (compressible::turbulentTemperatureCoupledBaffleMix ed) takes into account the conservation of heat flux between patches as follow:

kappa_fluid*d(T_fluid)/dn = kappa_solid*d(T_solid)/dn

where n is the vector normal to the contact surface.

The problem is that kappa_solid is taken form the thermophysicalProperties file in constant/solid (in which the thermal conductivity is a constant for the whole solid)...

(because my solid has different thermal conductivity, depending on position).

...
Thank you for describing the problem on the conceptual level.

I'll describe how I would approach this problem. Beware, I'm using pseudocode to describe the idea, the code below is not something you should copy and paste + compile.

I would suggest you to think about first implementing a heat conduction model that computes thermal conducitivity depending on position.

When you do that properly, the model will be run-time selectable.

Make sure that the selection of the conductivity model is dictionary based.

Extend the turbulentTemperatureCoupledBaffleMixed boundary condition into a BC that makes use of a modeled thermal conductivity and not a constant. Make the BC contain the model and select it during run-time. Make the 'updateCoeffs' delegate the conductivity calculation to the model : constant or variable, depending on the sub-dict entry.

The dictionary entry of your new ('turbulentTemperatureCoupledeBaffleMixedModel') boundary condition should contain a sub-dictionary

Code:
turbulentTemperatureHowEverYouNameYourBc
{
    conductivityModels {
        solid  spatiallyVariable someFunctionName; 
        fluid  constant 0.007;
     } 
    // Whatever other parameters go with the original BC.
}
This way, you don't have to touch the original solver at all.

Your new model will be contained within your new BC class (depending on the OF smart pointer you decide on for the run-time selection):

Code:
class turbulentTemperatureBlah
{
    private:
        autoPtr<spatiallyVariableThermalConductivityModel> modelPtr_;

    public: 
        turbulentTemperatureBlah(IOobject const & io)
        :
            modelPtr_ = transportModel::New(io.subdict(" .... 
};
So, in the end, you have a new BC that replaced the line:
Code:
    kappa_fluid*d(T_fluid)/dn = kappa_solid*d(T_solid)/dn
with something like:

Code:
     modelPtr->kappa_fluid()*d(T_fluid)/dn = modelPtr->kappa_solid()*d(T_solid)/dn
And the 'kappa_fluid' and 'kappa_solid' can be either constants (if you select a 'constant' model) or variable values - in whatever way you want to vary them - you just write a new variable model.

Note: No solver application is touched, and you have a small library that you can share with anyone that is using OF.

You'll have to understand RTS in OF to do this, there is a great page about that in the OF Wiki.
Zhiheng Wang likes this.
__________________
When asking a question, prepare a SSCCE.
tomislav_maric is offline   Reply With Quote

Old   May 1, 2014, 11:33
Default
  #9
New Member
 
DanAndrea87's Avatar
 
Andrea Prestigiacomo
Join Date: Jun 2013
Location: Milan
Posts: 10
Rep Power: 13
DanAndrea87 is on a distinguished road
Thanks for the help and sorry for the late I answer you.
This way seems to be easier than modifying the thermophysical model, and your explanation was very clear.
I will try to make it on next week. I will write again in case of problems
Thanks again
DanAndrea87 is offline   Reply With Quote

Old   May 1, 2014, 11:37
Default
  #10
Senior Member
 
Tomislav Maric
Join Date: Mar 2009
Location: Darmstadt, Germany
Posts: 284
Blog Entries: 5
Rep Power: 21
tomislav_maric is on a distinguished road
Np, glad to be of help! Good luck with the work!
__________________
When asking a question, prepare a SSCCE.
tomislav_maric is offline   Reply With Quote

Reply

Tags
coupled patches, heat conduction, space dependent terms, thermal conductivity, thermophysical model

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Adding a new viscosity model ICL OpenFOAM Running, Solving & CFD 20 April 10, 2017 23:44
chtMultiRegionSimpleFoam: strange error samiam1000 OpenFOAM Running, Solving & CFD 26 December 29, 2015 23:14
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
error message cuteapathy CFX 14 March 20, 2012 07:45
Eulerian Model - properties ssamton FLUENT 1 March 16, 2012 02:34


All times are GMT -4. The time now is 20:51.