CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > SU2

Turbulent flow around fuselage at low mach number

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 17, 2013, 15:36
Default Turbulent flow around fuselage at low mach number
  #1
New Member
 
Olivier Soucy
Join Date: Oct 2012
Location: Montreal, Canada
Posts: 6
Rep Power: 4
osoucy is on a distinguished road
Hi,

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.

Regards,
osoucy is offline   Reply With Quote

Old   January 18, 2013, 14:47
Default
  #2
New Member
 
Amrita Lonkar
Join Date: Nov 2012
Posts: 14
Rep Power: 4
Amrita Lonkar is on a distinguished road
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.

For example:
% Linear solver for the implicit (or discrete adjoint) formulation (LU_SGS,
% SYM_GAUSS_SEIDEL, BCGSTAB, GMRES)
LINEAR_SOLVER= GMRES
%
% Min error of the linear solver for the implicit formulation
LINEAR_SOLVER_ERROR= 1E-6
%
% Max number of iterations of the linear solver for the implicit formulation
LINEAR_SOLVER_ITER= 20

For an incompressible formulation, the configuration file should include

INCOMPRESSIBLE_FORMULATION= YES
%
% Value of the Bulk Modulus (1.01E5 N/m^2 (air), 2.2E9 N/m^2 (water),
% only for incompressible flows)
BULK_MODULUS= 1.01E5
%
% Artifical compressibility factor (1.0 by default,
% only for incompressible flows)
ARTCOMP_FACTOR= 1.0


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.

Last edited by Amrita Lonkar; January 18, 2013 at 15:14.
Amrita Lonkar is offline   Reply With Quote

Old   January 18, 2013, 16:51
Default
  #3
New Member
 
Olivier Soucy
Join Date: Oct 2012
Location: Montreal, Canada
Posts: 6
Rep Power: 4
osoucy is on a distinguished road
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?

Thanks again,
osoucy is offline   Reply With Quote

Old   January 18, 2013, 17:04
Default
  #4
New Member
 
Amrita Lonkar
Join Date: Nov 2012
Posts: 14
Rep Power: 4
Amrita Lonkar is on a distinguished road
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.

Last edited by Amrita Lonkar; January 18, 2013 at 17:34.
Amrita Lonkar is offline   Reply With Quote

Old   January 23, 2013, 21:13
Default
  #5
New Member
 
Olivier Soucy
Join Date: Oct 2012
Location: Montreal, Canada
Posts: 6
Rep Power: 4
osoucy is on a distinguished road
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.
Attached Images
File Type: jpg Res0Conv.jpg (24.9 KB, 25 views)
File Type: jpg ClConv.jpg (19.9 KB, 25 views)
File Type: jpg CdConv.jpg (17.3 KB, 20 views)
Attached Files
File Type: txt turb_fuselage.txt (9.3 KB, 16 views)
osoucy is offline   Reply With Quote

Old   February 5, 2013, 01:06
Default
  #6
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
Could you please post some pictures of the geometry? and details of the grid to have an idea of the problem complexity.

Thanks,
Francisco
fpalacios is offline   Reply With Quote

Reply

Tags
fuselage, three-dimensional, turbulent

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
pre-conditioning for low mach number compressible flow solver Shenren_CN Main CFD Forum 0 April 29, 2011 21:07
Unaligned accesses on IA64 andre OpenFOAM 5 June 23, 2008 10:37
acoustics and low mach number George Main CFD Forum 42 November 3, 2005 07:05
compressible at low Mach number with uniteration ricklee Main CFD Forum 2 October 20, 2005 23:15
About low Re number turbulent flows gorka Main CFD Forum 13 April 2, 2003 05:19


All times are GMT -4. The time now is 05:55.