[reza_k]

Dear Experts
Recently, I'm Trying to define a new turbulence model in ANSYS CFX. I know how to define a new variable and solve transport equation for that, but defining a new turbulence model is a different case; the result of the new equation, "vt" or turbulent viscosity should be inserted in momentum equation directly.
Anyway, the qustion is:

- Is it possible to define a new variable which has direct influence on flow solution?

If yes, please give me some general information about that.

I would really appreciate your help.

[ghorrocks]

Yes, you can define viscosity to be a CEL expression and a function of many things. So set the material viscosity to be equal to your vt (+ the laminar viscosity as well I guess).

[reza_k]

Thank you sir,

Whether the mentioned method is applicable to Turbulence prandtl number "Prt".
I tried to modify Turbulence Prandtl as a function of (Density, Dynamic viscosity and Turbulence Kinetic Energy), and this error is observed :

"Error in subroutine GETCORE. There is circularity in recursive calls to GETVAR. A variable depends on itself ..."

Do you have any Idea?

Thanks a lot sir.

[ghorrocks]

The error message is quite clear: You have made Turbulence Prandtl number a function of a variable which depends on it, so it has become recursive. You are going to have to remove at least one of your input variables (density, viscosity, TKE) from your function.

[Opaque]

Implementing a turbulence model is not only about solving a transport equation (or more) and evaluating the turbulent viscosity, but also about how the boundary conditions for other equations are implemented.

What is your goal ? Are you trying to replace the formula used for the turbulent viscosity (mu_t), based on a formula using the transport equations you solved , but still keeping ANSYS CFX boundary treatment as well as turbulent flux treatment for every other equations (say momentum, energy and other scalars).

If you do not activate any of the default turbulence models, you will not get any of the boundary treatments nor access to the turbulent flux evaluation. However, you can use the algebraic Zero Equation model (cost you nothing), and override the "Eddy Viscosity" (same as mu_t) with your own formula. The turbulent fluxes will be mu_t/Pr_t for the other equations, and the boundary conditions will use the default wall function treatment.

If you need special wall function treatment, you must code the Wall Function Transfer Coefficient yourself for every equation that requires one.

hope the above helps,

[Turbo_hrf]

hello, do you solve this problem? recently, I want to define a new turbulence model,too. and I need to modify the Sigma_k, Sigma_eplison in k, elipson turbulence model, which seems to be defined in tuburlent schmidt number, how define the turbulent schmidt number as a function of density?

If you find out the method, please help me

[reza_k]

[QUOTE=Turbo_hrf;575306]hello, do you solve this problem? recently, I want to define a new turbulence model,too. and I need to modify the Sigma_k, Sigma_eplison in k, elipson turbulence model, which seems to be defined in tuburlent schmidt number, how define the turbulent schmidt number as a function of density?



Dear angela,
when I was working on this issue ( define nu_t as function of density) someone told me it is not possible because it is a
recursive problem ...
although I could not accept this argument (because it is an iterative solution and I did it many times in Openfoam and Fluent), I think
that Ansys CFX doesn't allow you to define a new variable as function of density ( may be u, v,... and other flow variables). Anyway, I
recommend you to

1) read the CFX manual one more time, may be you could find a way...
2) Think about doing your job in ANSYS Fluent,... it has a well written user manual and you can use the User Defined Functin (UDF) to define a new turbulence model
3) If you have enough time try to learn Openfoam and rid yourself of the limitation of these softwares.

[Turbo_hrf]

kiarash, thank you for message. I now learn to use the UDF in fluent, it is more useful. one 2D aifoil case confuses me, which come to a convergence at 200 steps in CFX, but 15000 steps in FLUENT. I found the fluent is hard to get a good convergence, instead always shows errors, shows errors. did you have this problem?

[reza_k]

Originally Posted by Turbo_hrf

kiarash, thank you for message. I now learn to use the UDF in fluent, it is more useful. one 2D aifoil case confuses me, which come to a convergence at 200 steps in CFX, but 15000 steps in FLUENT. I found the fluent is hard to get a good convergence, instead always shows errors, shows errors. did you have this problem?

Dear angela,
both of the ANSYS Fluent and ANSYS CFX are robust cfd solvers. Rate of convergence
depends on many things such as: solver, time step, CFL, grid, initialization, turbulence model and ...
but these solvers have some basic differences. I think that the primary reason for the fast convergence
you see in CFX is related to it's fully coupled solver and fully implicit multigrid, (note CFX has just
a coupled pressure based solver). ANSYS Fluent is different, it has both of the coupled and segregated
solvers and an advanced multigrid option for advanced users. Anyway, it is hard to answer your question
about the rate convergence of solving flow over 2D airfoil, because I need more information about that,

for example:

1) type of the airfoil
2) Mach number and Reynolds number
3) Turbulent intensity ( if the flow is turbulent)
4) angle of attack
5) type of the solver you have selected
6) discritization accuracy
...

if you provide me the above information, I could better help you. You can contact me via first_kv@yahoo.com

[vcvedant]

Dear Reza,

Can you tell me how to modify turbulent viscosity in FLUENT? When I use the macro it I get the same results for CMU = 0.09 but the results for CMU = 0.05 in UDF does not match when the change is made from GUI panel.

Thanks

[QUOTE=reza_k;575308]

Originally Posted by Turbo_hrf

hello, do you solve this problem? recently, I want to define a new turbulence model,too. and I need to modify the Sigma_k, Sigma_eplison in k, elipson turbulence model, which seems to be defined in tuburlent schmidt number, how define the turbulent schmidt number as a function of density?



Dear angela,
when I was working on this issue ( define nu_t as function of density) someone told me it is not possible because it is a
recursive problem ...
although I could not accept this argument (because it is an iterative solution and I did it many times in Openfoam and Fluent), I think
that Ansys CFX doesn't allow you to define a new variable as function of density ( may be u, v,... and other flow variables). Anyway, I
recommend you to

1) read the CFX manual one more time, may be you could find a way...
2) Think about doing your job in ANSYS Fluent,... it has a well written user manual and you can use the User Defined Functin (UDF) to define a new turbulence model
3) If you have enough time try to learn Openfoam and rid yourself of the limitation of these softwares.

[ghorrocks]

Try the fluent forum.