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

Problem with Isothermal wall boundary condition

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

Like Tree2Likes
  • 1 Post By economon
  • 1 Post By jentink

Reply
 
LinkBack Thread Tools Display Modes
Old   September 16, 2013, 10:48
Question Problem with Isothermal wall boundary condition
  #1
New Member
 
Harold
Join Date: Sep 2013
Posts: 4
Rep Power: 3
Harold Tian is on a distinguished road
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

Last edited by Harold Tian; September 17, 2013 at 09:50.
Harold Tian is offline   Reply With Quote

Old   October 3, 2013, 01:03
Default
  #2
Super Moderator
 
Thomas D. Economon
Join Date: Jan 2013
Location: Stanford, CA
Posts: 260
Rep Power: 5
economon is on a distinguished road
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 likes this.
economon is offline   Reply With Quote

Old   October 11, 2013, 05:10
Default
  #3
New Member
 
Harold
Join Date: Sep 2013
Posts: 4
Rep Power: 3
Harold Tian is on a distinguished road
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
Harold Tian is offline   Reply With Quote

Old   October 11, 2013, 15:57
Default
  #4
Super Moderator
 
Thomas D. Economon
Join Date: Jan 2013
Location: Stanford, CA
Posts: 260
Rep Power: 5
economon is on a distinguished road
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
economon is offline   Reply With Quote

Old   October 12, 2013, 02:14
Default
  #5
New Member
 
Harold
Join Date: Sep 2013
Posts: 4
Rep Power: 3
Harold Tian is on a distinguished road
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

surface.part01.zip

surface.part02.zip

biconic-vis.cfg.txt
Harold Tian is offline   Reply With Quote

Old   October 15, 2013, 08:08
Default
  #6
Member
 
Tom Jentink
Join Date: Jan 2013
Posts: 48
Rep Power: 4
jentink is on a distinguished road
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 likes this.
jentink is offline   Reply With Quote

Old   October 19, 2013, 08:03
Default
  #7
New Member
 
Harold
Join Date: Sep 2013
Posts: 4
Rep Power: 3
Harold Tian is on a distinguished road
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
Harold Tian is offline   Reply With Quote

Reply

Tags
isothermal wall

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
Pressure Boundary Condition Problem rbjet CFX 3 July 15, 2013 21:45
Low Mixing time Problem Mavier CFX 5 April 29, 2013 00:00
Import problem ARC Open Source Meshers: Gmsh, Netgen, CGNS, ... 0 February 27, 2010 11:56
isothermal wall boundary condition Neil Main CFD Forum 2 December 18, 2004 13:15
Periodic flow boundary condition problem sudha FLUENT 3 April 28, 2004 08:40


All times are GMT -4. The time now is 13:24.