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

transient laminar flow simulation setup

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 19, 2013, 05:02
Default transient laminar flow simulation setup
  #1
New Member
 
Jianguo
Join Date: May 2011
Posts: 9
Rep Power: 6
zhengjg is on a distinguished road
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
zhengjg is offline   Reply With Quote

Old   August 19, 2013, 12:06
Default
  #2
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
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 View Post
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 is offline   Reply With Quote

Old   March 10, 2014, 07:23
Default Variable Inlet Velocity
  #3
New Member
 
nilesh
Join Date: Mar 2014
Location: Kanpur / Mumbai, India
Posts: 27
Rep Power: 3
nilesh is on a distinguished road
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.
nilesh is offline   Reply With Quote

Old   March 10, 2014, 17:24
Default
  #4
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
Quote:
Originally Posted by nilesh View Post
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
fpalacios is offline   Reply With Quote

Old   March 31, 2014, 07:14
Default
  #5
New Member
 
nilesh
Join Date: Mar 2014
Location: Kanpur / Mumbai, India
Posts: 27
Rep Power: 3
nilesh is on a distinguished road
Quote:
Originally Posted by fpalacios View Post
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.
nilesh is offline   Reply With Quote

Reply

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
Boundary Layer of Laminar Flow over a Flat Plate Blasius_Pohlhausen_Crocco Main CFD Forum 12 September 30, 2013 17:35
CFX Treatment of Laminar and Turbulent Flows Jade M CFX 6 January 26, 2013 11:11
kutta condition and separated flow in transient simulation Nick R CFX 5 April 19, 2011 23:37
Laminar flow or Turbulent flow mech FLUENT 0 January 27, 2007 19:51
laminar and turbulent flow in one simulation msna FLUENT 0 January 27, 2007 18:35


All times are GMT -4. The time now is 06:03.