CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   SU2 (http://www.cfd-online.com/Forums/su2/)
-   -   transient laminar flow simulation setup (http://www.cfd-online.com/Forums/su2/122395-transient-laminar-flow-simulation-setup.html)

zhengjg August 19, 2013 05:02

transient laminar flow simulation setup
 
Dear SU2 developer and user,
I wish to resolve an unsteady, time-accurate laminar flow using SU2 CFD module. I want to set up simulation with following options:
1. to use explicit multi-stage time stepping scheme to perform temporal integration.
2. to print results every time interval of Tint.
I have generated mesh and initialized the flow flied. But I do not know how to specify the above options in configuration file.
Is there any existing unsteady calculation case with SU2 that I can follow?

Thanks

fpalacios August 19, 2013 12:06

Using the latest version of SU2 that you can folk from https://github.com/su2code/SU2 . At least, you will need the following parameters in the config file.

% ------------------------- UNSTEADY SIMULATION -------------------------------%
%
% Unsteady simulation (NO, TIME_STEPPING, DUAL_TIME_STEPPING-1ST_ORDER, DUAL_TIME_STEPPING-2ND_ORDER, TIME_SPECTRAL)
UNSTEADY_SIMULATION= DUAL_TIME_STEPPING-2ND_ORDER
%
% Time Step for dual time stepping simulations (s)
UNST_TIMESTEP= 0.001
%
% Total Physical Time for dual time stepping simulations (s)
UNST_TIME= 1.0
%
% Unsteady Courant-Friedrichs-Lewy number of the finest grid
UNST_CFL_NUMBER= 0.0
%
% Number of internal iterations (dual time method)
UNST_INT_ITER= 200

% ------------------------- INPUT/OUTPUT INFORMATION --------------------------%
%
% Writing solution file frequency
WRT_SOL_FREQ= 1000
%
% Writing solution file frequency for physical time steps (dual time)
WRT_SOL_FREQ_DUALTIME= 10
%
% Writing convergence history frequency
WRT_CON_FREQ= 1
%
% Writing convergence history frequency (dual time, only written to screen)
WRT_CON_FREQ_DUALTIME= 10

Best,
Francisco

Quote:

Originally Posted by zhengjg (Post 446576)
Dear SU2 developer and user,
I wish to resolve an unsteady, time-accurate laminar flow using SU2 CFD module. I want to set up simulation with following options:
1. to use explicit multi-stage time stepping scheme to perform temporal integration.
2. to print results every time interval of Tint.
I have generated mesh and initialized the flow flied. But I do not know how to specify the above options in configuration file.
Is there any existing unsteady calculation case with SU2 that I can follow?

Thanks


nilesh March 10, 2014 07:23

Variable Inlet Velocity
 
Hi,
I am trying to simulate an airfoil starting from t=0 seconds with zero velocity and then increase velocity as a tan hyperbolic function of time. Please help me with specifying such variable velocity boundary condition.
Thank You.

fpalacios March 10, 2014 17:24

Quote:

Originally Posted by nilesh (Post 479112)
Hi,
I am trying to simulate an airfoil starting from t=0 seconds with zero velocity and then increase velocity as a tan hyperbolic function of time. Please help me with specifying such variable velocity boundary condition.
Thank You.

If you are using far-field boundary condition, my recommendation is modify the subroutine
void CEulerSolver::BC_Far_Field(CGeometry *geometry, CSolver **solver_container, CNumerics *conv_numerics, CNumerics *visc_numerics, CConfig *config, unsigned short val_marker)
that you can find in solver_direct_mean.cpp.

In short, the idea is to specify the value for V_infty at each time step. Using config->GetExtIter() you will know what is the current iteration.

Cheers,
Francisco

nilesh March 31, 2014 07:14

Quote:

Originally Posted by fpalacios (Post 479218)
If you are using far-field boundary condition, my recommendation is modify the subroutine
void CEulerSolver::BC_Far_Field(CGeometry *geometry, CSolver **solver_container, CNumerics *conv_numerics, CNumerics *visc_numerics, CConfig *config, unsigned short val_marker)
that you can find in solver_direct_mean.cpp.

In short, the idea is to specify the value for V_infty at each time step. Using config->GetExtIter() you will know what is the current iteration.

Cheers,
Francisco


Thanks. Which is the line this this subroutine that is to be modified. Is it
'V_infty = GetCharacPrimVar(val_marker, iVertex)' ?
For example, if my function is U=0.8*tanh(t/100) where t is the flow time,what is the exact modification that is to be done? Do I have to write the function or generate velocity at different steps in a file and feed it to the program? Sorry, I do not have any experience in working with C. I will be thankful if you could give me the command/statement.


All times are GMT -4. The time now is 04:34.