Turbulent flow around fuselage at low mach number
I'm trying to solve for the flow around a three-dimensional helicopter fuselage represented by an unstructured grid. Could you advice on typical settings for that type of problems? The flow conditions are Mach = 0.2, Alpha = -2.0 and Beta = 0.0. Accuracy is not of first importance here, but convergence is. I could accept a margin of error of 10% on lift and drag.
More specifically, I would like to know:
1) Which type of turbulence model to use. SA?
2) Which type of numerical method to use. JST or Roe-2ND_ORDER?
Any help would be appreciated.
You can try either JST or Roe with the SA turbulence model. I would also recommend you try the incompressible solver. You also might want to play with the choice of linear solvers. GMRES or BCGSTAB could be good choices.
% Linear solver for the implicit (or discrete adjoint) formulation (LU_SGS,
% SYM_GAUSS_SEIDEL, BCGSTAB, GMRES)
% Min error of the linear solver for the implicit formulation
% Max number of iterations of the linear solver for the implicit formulation
For an incompressible formulation, the configuration file should include
% Value of the Bulk Modulus (1.01E5 N/m^2 (air), 2.2E9 N/m^2 (water),
% only for incompressible flows)
% Artifical compressibility factor (1.0 by default,
% only for incompressible flows)
If there are problems with convergence, try to turn off multigrid. If none of these work, send us the grid and we will try to develop a good configuration file for you.
Thank you for the proposed solutions.
It turned out that I've managed to converge a solution last night using JST scheme and SA turbulence model. However, the convergence rate was poor and highly non monotonic. I'll try to incorporate the settings you suggested to see if it improves things. I might also need to improve the quality of the grid.
What exactly is the purpose of activating the linear_solver? How can it improve the convergence?
I assume the INCOMPRESSIBLE_FORMULATION may be used since the Mach Number is very low and compressibility effects may be neglected? Using this setting only simplify the governing equations or is introducing new algorithms?
Choosing a different linear solver like GMRES or BCGSTAB helps with convergence of those problems which are hard to convergence because of inherent stiffness in the equations.
Incompressible solver solves a simplified set of equations in primitive variables as opposed to the conservative variables, and assumes that the density is constant everywhere (assumption of incompressibility). I think you can try the incompressible solver since the Mach number is so low.
To improve the rate of convergence, you can try ramping the CFL up a bit, you can also try a numerical solver like GMRES, which allows higher CFL values, but a downside could be that it takes slightly more time per iteration.
If you are not using multigrid, I suggest turning it on, it helps accelerate convergence, but for stiff problems, it can run into problems with stability. Trying it won't hurt.
After refining my grid and boosting the CFL number, I get reasonable convergence results, as shown in attached pictures.
Choosing a different linear solver didn't help to improve residual vs computational time (although it did for residual vs iteration).
Multigrid proven to be unstable and I could not use it.
If you believe that I could achieve faster convergence for the type of problem I'm solving, could you please take a look at the configuration file I've attached to this post and let me know how it can be improved. My computational grid contains 1.5 million interior elements, which have been reduced to 0.6 million elements by combining anisotropic tetrahedra.
Could you please post some pictures of the geometry? and details of the grid to have an idea of the problem complexity.
|All times are GMT -4. The time now is 03:51.|