[zyy]

In openFOAM 10, sigle phase turbulence is constructed using following codes:

autoPtr<incompressible::turbulenceModel> turbulence
(
    incompressible::turbulenceModel::New(U, phi, laminarTransport)
);

However, I can't find similar codes in multiphaseEulerFoam. I guess it might be hidden in the class "phaseSystem". But I have no idea where the turbulenceModels are constructed.

[dlahaye]

Euler is non-viscous and has there zero-viscosity?

[zyy]

Thank you for your reply. The tutorial of multiphaseEulerFoam can set simulationType to RAS and applys mixtureKEpsilon model instead of single phase kEpsilon. The model code can be found in src/MomentumTransportModels/PhaseCompressible. So the solver should have access to viscosity models.

The UEqns.H file constructed a momentumTransferPtr using the member function momentumTransfer() of class PhaseSystem. But the function momentumTransfer() is virtual, and I don't know if there are any subclass that rewrite that function.

[Severus]

Hello,
What you are looking for is in the phaseCompressibleMomentumTransportModel.H file
https://cpp.openfoam.org/v10/phaseCo...8H_source.html

You first have to take a look at multiphaseCompressibleMomentumTransportModels.C which is present under the multiphaseEulerFoam application folder
https://cpp.openfoam.org/v10/multiph...8C_source.html
If you carefully follow the dependencies and header files from this class you will finally get to phaseCompressibleMomentumTransportModel.H file

Thanks

[zyy]

Thank you so much for your response. That's a great point. However, I'm still a bit unsure about how the solver uses those models. I'm hoping to find something like "phase1.turbulence().nut()" as a way to express it. I actually tried removing #include "phaseCompressibleMomentumTransportModel.H" in multiphaseEulerFoam.C, but the solver still compiles and runs as usual, which is a bit confusing. How does the solver manage to construct fields like nut.air and nut.water?

[Severus]

Hello,
If you want to use nut fields for a specific phase (like nut.air or nut.water), the best way will be to take a look at the phaseScalarTransport functionObject, where it is easy to follow and adapt.
https://cpp.openfoam.org/v10/phaseSc...8C_source.html
Here, see lines 272-275. When adapting it for your case, check this class carefully so that you don't forget to add the right header files.

Within multiphaseEulerFoam it is not that easy to find out as the code is quite generalized and complicated. However, in the older versions, for instance in twoPhaseEulerFoam is easier to find how they use the turbulent viscosity.
https://cpp.openfoam.org/v7/twoPhase...8H_source.html
See line 27 and 60

Thanks

[zyy]

Thanks a lot for your advice. I have inplemented my code on twoPhaseEulerFoam in OF 7. I did some comparasion with multiphaseEulerFoam in OF 10 and find out that multiphaseEulerFoam is more stable when dealing with advetion term. I will update this post if I find a entry to the nut fields in multiphaseEulerFoam.

[Severus]

Hello,
Alright. In the past I have used the nut fields in multiphaseEulerFoam in OpenFOAM v9. I followed a similar procedure to that implemented in the phaseScalarTransport.C file. So, I think it should also work in your case.

Since you mentioned that you have issues with stability with the twoPhaseEulerFoam solver, I would recommend you to check out the faceMomentum formulation.
https://github.com/OpenFOAM/OpenFOAM...777bb10a3e1dda
What is "faceMomentum" in twoPhaseEulerFoam in OF 3.0.0

I have used it and it has proven to ensure stability for some cases.

Thanks

[zyy]

Thanks! That’s really helpful.