CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   SU2 (http://www.cfd-online.com/Forums/su2/)
-   -   Problem with Isothermal wall boundary condition (http://www.cfd-online.com/Forums/su2/123570-problem-isothermal-wall-boundary-condition.html)

Harold Tian September 16, 2013 10:48

Problem with Isothermal wall boundary condition
 
Hello,
I’m running SU2 in hypersonic case. I need use isothermal wall boundary condition. But the option values of ISOTHERMAL_WALL not involve temperature of the wall(just YES or NO). How can I define the temperature of the isothermal wall and export the surface heat flux data?

Thanks

Harold

economon October 3, 2013 01:03

Hi Harold,

Glad to hear that you're trying out SU2, and thanks for posting your question on the forum.

Starting with version 2.0.4 of SU2, we adjusted the way that one specifies the no-slip wall boundary conditions. As an example, an isothermal wall could now be specified as

%
% Navier-Stokes (no-slip), isothermal wall marker(s) (NONE = no marker)
% Format: ( marker name, constant wall temperature (K), ... )
MARKER_ISOTHERMAL= ( wall, 300.0 )

where 'wall' is the name of the boundary marker and we are setting the wall temperature to 300 K. By continuing the list with more marker names and temperatures, you can specify different values for any number of markers. Lastly, note that the ISOTHERMAL_WALL option has been deprecated.

Hope this helps,
Tom

Harold Tian October 11, 2013 05:10

Hi Tom,
Thanks alot for the reply!
I have tried version 2.06 of SU2 to solve my problem. The flow flied looks good, but the heat transfer data is strange, it is a small negative value anywhere of the flow flied. The range of heat transfer is about 0 to 1E-5. I need the surface heat flux data to compare with experiment result. How can I deal with the strange heat transfer data and get right surface heat flux?
Thanks

Harold

economon October 11, 2013 15:57

Dear Harold,

While the volume solution file, 'flow.dat' for instance will have mostly zero values for the heat transfer (it is only defined on the surface in the code), the surface solution file, 'surface_flow.dat', file will contain the values directly on the surface. This will be more suitable for post-processing and comparing with experiment.

If you still see weird behavior with the heat transfer, please don't hesitate to let us know.

Hope this helps,
Tom

Harold Tian October 12, 2013 02:14

3 Attachment(s)
Dear Tom,

I find the differences of heat transfer between volume solution file and surface solution file. As you mentioned, heat transfer values is in the volume solution file except on the solid surface. Though the value of heat transfer on the surface is not zero, but it is very small negative value(about -1E-5 to -1E-8). what's the unit of heat transfer in SU2? Is it w/m^2? Is this problem caused by the unit?

I attach my surface solution file and configure file, maybe these is helpful to solve the problem.

Thanks a lot.
Harold

Attachment 26017

Attachment 26018

Attachment 26019

jentink October 15, 2013 08:08

I needed dimensional heat transfer to compare with data, so I made the changes shown below. I don't know if I broke anything else with these changes, but it has been working fine for me. Changes are to solver_direct_mean.cpp

-------------------------------------------------------------------------------------
/* tj CHeatTransfer[iMarker][iVertex] = (Cp * Viscosity/PRANDTL)*GradTemperature/(0.5*RefDensity*RefVel2); */
CHeatTransfer[iMarker][iVertex] = (Cp * Viscosity/PRANDTL)*GradTemperature/Area;
Q_Visc[iMarker] += CHeatTransfer[iMarker][iVertex];

/* tj if ((CHeatTransfer[iMarker][iVertex]/Area) > Maxq_Visc[iMarker]) */
if ((CHeatTransfer[iMarker][iVertex]) > Maxq_Visc[iMarker])
/* tj Maxq_Visc[iMarker] = (CHeatTransfer[iMarker][iVertex]/Area); */
Maxq_Visc[iMarker] = (CHeatTransfer[iMarker][iVertex]);

Harold Tian October 19, 2013 08:03

Dear Jentink,

You are right! Your reply is very helpful. Under your advice, I have got the right heat transfer solution and match well with experiment.
Thanks a lot.

Harold


All times are GMT -4. The time now is 23:01.