Compressible module and internal coupling

[bstorti]

Hello,

I'm working on a gas turbine blade simulation. Air velocities are rounding Mach 1, therefore I'm using the compressible module of code saturne.
The idea is to solve the hot gases around the airfoil using the compressible module, and do an internal coupling over the surface vane (Fluid-Solid interface), in order to solve only heat diffusion on the profile.

The thing is, when I choose the Compressible model in the GUI, I can not set a heat flux condition over the profile (which has a smooth wall condition). Is this a bug in the GUI? Or is not possible to solve this internal coupling for compressible flows?.

Regards,

Bruno.

[Yvan Fournier]

Hello,

I am not sure about this, but I suspect this is just missing from the GUI. I'll ask Erwan, who knows the compressible model better than I do, but I recommend checking if this is possible with user subroutines.

As the compressible module uses a specific thermal model (total energy), some things like prescibed temperatures may not be handled (though there is probably no fundamental reason preventing this; rather missing energy/temperature conversions).

Since you try to prescribe a simple heat flux, this should probably be possible with cs_user_boundary_conditions.f90. I'll ask, but I would recommend trying.

Best regards,

Yvan

[Erwan Le Coupanec]

Hi,

Yvan is right.

For the thermal flux at a wall with the compressible module, go by the user source, it is just not implemented through the GUI but we could do it.

Just check out example 6 at the below Doxygen link to see how to do it in cs_user_boundary_conditions
https://www.code-saturne.org/cms/sites/ ... mples.html

For the internal coupling, I actually haven't had the occasion to try it out with the compressible module.
But thinking about it, you should try and it should probably work as it is.
Have in mind that when the compressible module is enabled, the energy equation is solved in total energy, as Yvan was saying, hence CS needs the volume-specific heat capacity Cv (diffusion coefficient is lambda/Cv). You were giving it for the fluid, for a coupled computation, you need to set it right for the solid as well.

Regards,
Erwan.

[bstorti]

Yvan and Erwan,

I've tried imposing the heat flux on the vane surface using user subroutines and worked like a charm!. It was just missing from the GUI.
Now I'll try to do the internal coupling, I'll let you know how the coupling turns out with the compressible module. I'll have in mind your recommendations about the thermal model.
Thanks a lot for your help!.

Regards,
Bruno.

[bstorti]

Hello Yvan and Erwan,

I've done the internal coupling between the vane and air, coupling the field "total_energy" because of the compressible module. Code saturne seems to run without any problems(see figure "temp_vel.png"), but I think I'm doing something wrong with the coupling. Although the thermal diffusion is solved correctly inside the airfoil as well as velocity/pressure for the fluid, the heat flux over the vane surface is very close to zero(see figure "thermal_flux.png"). Therefore the thermal boundary layer of the fluid over the vane surface is not generated. The coolant holes inside the airfoil have defined a Robin condition (just to clarify the case I'm solving).

Also I've tried a simpler case posted in the forum of a square cavity which contains fluid in the middle of the domain and solid walls on both sides. The left wall has a Dirichlet boundary condition in x=0(see figure "square_coupling.png"). In this case it can be seen that there is a heat flux over the solid-fluid interface, but is very low. I've tried changing the thermal diffusion coefficient for the fluid
(lambda/Cv) rising the value of lambda, but without success (the thermal diffusion coefficient rises but the heat flux remains very low).

My questions are: 1) Am I setting something wrong for the coupling?
2) How are the exchange coefficients computed by CS in order to do the coupling?

Thank you in advance!

Regards.

Bruno

[Erwan Le Coupanec]

Hello,

The exchange coefficient is computed using a harmonic mean of a left and right diffusion coefficient.
On fluid side, the coefficient is seeing the turbulent wall model.

Is the second test case (square) laminar ?
Could you send me this test case as you set it ? It's hard to answer your second question without seeing the settings. From your description it seems fine (lambda, cv on fluid and solid sides + coupling on total energy).

Thanks,
Erwan.

[Erwan Le Coupanec]

Nice geometry by the way !

[bstorti]

Thanks for your help Erwan.

Here I send you the square case that i've runned in Code Saturne version 5.0. I've tried both, laminar and turbulent regimes without success.
From the user subroutines you will see that I'm rising up the thermal conductivity of the fluid domain to 720, this is in order to obatin a higher thermal diffusivity (near 1). It was just a try value. The specific heat capacity is set to 1017 J/kgK for the entire domain (solid and fluid). I didn't change this values because in the real case of the vane, the Cp of the vane is approximately just a half of the air. I'm only setting the Cp values because as i can see from the routine "cs_user_physical_properties-compressible_flow", the Cv is computed calling "cs_cf_thermo_cv" as Cv = Cp - (R/M). I'm setting it right?.

Regards,

Bruno.