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

Simulating a G├Âttingen type wind tunnel in FLUENT

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 27, 2006, 13:21
Default Simulating a G├Âttingen type wind tunnel in FLUENT
  #1
Chris
Guest
 
Posts: n/a
Hello FLUENT experts! I try to simulate a G÷ttingen type wind tunnel in FLUENT. You can find the technical details about the wind tunnel when you follow this link: http://www.tu-harburg.de/fds/testfacilities/index.html . As you can see the test section of the tunnel is not closed and forms a brick type volume of the following dimensions: length= 5m, width= 3m and height= 2m. The model for the wind tunnel test I try to simulate in FLUENT, is a wing (NACA 23012 airfoil) with a slotted flap attached to the trailing edge. The wing measures a total height of 0.8 m and is vertically mounted on the underfloor weighing platform. I use GAMBIT as preprocessor and formed my controll volume by substracting the volume of the wing from the volume of the test section. I meshed the remaining volume with a Tet/Hyb-Mesh consisting of 1300000 cells. I used size functions to get a finer mesh in the near wing area and the near floor area, because I want to resolve the boundary layer. Before meshing I estimated the boundary layer thickness by using the flat plate theory. After this quite long description, here comes my question. What type of boundary conditions would you choose, to simulate the test section of the wind tunnel? In my first approach I used velocity inlet (v=20 m/s) at the entrance of the test section. For the exit of the test section I used the pressure outlet boundary condition (standard pressure). The ground of the test section and the wingmodel were defined as walls. The left, right and upper surfaces of the test section I defined as symmetry boundary conditions. I did some calculations with inviscid, viscous and the two turbulence models S-A and k-e. None of them reached my limit of 1e-6 for the residuals. I am not very sure about my defined boundary conditions. Maybe you can help me with some suggestions to simulate this kind of air tunnel with an open test section. Many thanks for your efforts!! Bye. Chris.
  Reply With Quote

Old   November 28, 2006, 05:28
Default Re: Simulating a G├Âttingen type wind tunnel in FL
  #2
Thomas
Guest
 
Posts: n/a
Your BC are OK in my opinion (when simulating wind tunnels I usually prefer to use pressure inlet cause I usually have datas regarding the total pressure at inlet). The residuals are high-dependent on the quality of the mesh, expecially when utilizing tet grids: so if u want to have lower residuals concentrate your work on the mesh: I usually employ the 80% of time of a complete CFD analysis working on the mesh. If you want more physical values use the RSM model and a 2nd order spatial interpolation scheme after the k-e and first order.

Thomas
  Reply With Quote

Old   November 29, 2006, 09:57
Default Re: Simulating a G├Âttingen type wind tunnel in FL
  #3
Ed Reed
Guest
 
Posts: n/a
You mentioned resolving the boundary layer on the bottom of the tunnel. I don't think it is reasonable to resolve the turbulent boundary layer using a purely tet mesh with size functions. You may want to look into using the boundary layer meshing scheme in gambit or using a y+ of 30-100 and S-A with wall functions.

Residuals aren't really the end-all of convergence. If you have some test data, see if your lift/drag converge to near that. If not, you'll have to do a method verification on an airfoil for which you do have test data and then move to the one you actually want to test.
  Reply With Quote

Old   December 4, 2006, 18:33
Default Re: Simulating a G├Âttingen type wind tunnel in FL
  #4
Chris
Guest
 
Posts: n/a
Thank you Thomas and Ed for your answers! I tried it a few times to use the boundary layer functions in GAMBIT to cover the wing and the ground of the test section with a boundary layer mesh. I used the internal continuity option to connect the boundary layers of the wing and the ground. Before I attached the boundary layers to the surfaces I used the viscous grid spacing calculator from this site http://geolab.larc.nasa.gov/APPS/YPlus/ to estimate the spacing between the wall and the first line of my boundary layers to get good values for y+. I calculated the spacings for my wing, the flap and the ground of the test section. But I wasn't very successful with this strategy because meshing of the volume aborted for different types of volume meshing schemes. Inspired by the Cornell airfoil tutorial http://instruct1.cit.cornell.edu/cou...foil/index.htm I tried to build the grid by myself. The tutorial is fine for a simple airfoil without a flap and freestream conditions. Unfortunately the profile of my wing got an slotted flap at its trailing edge and the profile is embedded in a rectangular plane (the ground of the test section). I found some very interesting pictures of meshes build with Gridgen, showing airfoils with slotted flaps http://www.pointwise.com/apps/mfoil.shtml. Is there a possibility to build such grids in GAMBIT? Thanks for your answers!
  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 conditions for simpleFoam calculation foam_noob OpenFOAM Running, Solving & CFD 8 July 1, 2015 08:07
GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM 300 October 29, 2014 19:00
cgnsToFoam problems with "QUAD_4" cells lentschi OpenFOAM Meshing & Mesh Conversion 1 March 9, 2011 05:49
flow in cyclic wind tunnel yogesh@cfd Main CFD Forum 0 November 8, 2010 05:28
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 20:50


All times are GMT -4. The time now is 05:07.