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

Unsteady simulation for NACA0012 airfoil

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 1, 2014, 01:03
Default Unsteady simulation for NACA0012 airfoil
  #1
Member
 
Anant Diwakar
Join Date: Jan 2013
Posts: 68
Rep Power: 4
diwakaranant is on a distinguished road
Hi

I am trying to run unsteady flow simulation for NACA0012 airfoil
for Mach = 0.5, Re = 10000 and AoA = 0 degree
The flow is unsteady for this case due to vortex shedding.

But I am not able to get this result in SU2. I am not getting
any periodic oscillations in lift/drag coefficients with time.

I am attaching the .cfg used.

Can anyone tell why is this happening ?

Thanks
Anant
Attached Files
File Type: txt naca0012_unsteady.cfg.txt (8.2 KB, 43 views)
diwakaranant is offline   Reply With Quote

Old   February 1, 2014, 08:19
Default
  #2
New Member
 
Eduardo Molina
Join Date: Sep 2010
Location: Brazil
Posts: 27
Rep Power: 6
EMolina is on a distinguished road
Hi Anant.

Your configuration file is correct. I think your teste case is incorrect! How can you expect periodic vortex shedding on a symmetric airfoil with AoA=0???? Where did you see this? Can you show to us?

Regards

Eduardo
EMolina is offline   Reply With Quote

Old   February 1, 2014, 13:52
Default
  #3
Member
 
Anant Diwakar
Join Date: Jan 2013
Posts: 68
Rep Power: 4
diwakaranant is on a distinguished road
Hi

Please refer to this paper by M. Braza
http://www.sciencedirect.com/science...45793002001007

Thanks
Anant
diwakaranant is offline   Reply With Quote

Old   February 1, 2014, 22:00
Default Unsteady simulation for NACA0012 airfoil
  #4
New Member
 
David Manosalvas
Join Date: Feb 2014
Posts: 19
Rep Power: 3
demanosalvas is on a distinguished road
Anant,

Your config file looks fine for what you are trying to model. A few suggestions that work very good when trying to model vortex shedding on bluff bodies are:
  • Reduce the time steps to make sure that you have around 25 steps per period.
  • Sometimes it takes a very long time for the vortex shedding to develop, so its good to insert a disturbance in the flow (run the simulation for a few iterations with a slight angle of attack)
  • The size of the elements on the wake could be introducing numerical dissipation (if they are too big) make sure to refine the mesh in the regions where you expect vortex shedding to take place
Hope this helps,


David
demanosalvas is offline   Reply With Quote

Old   February 18, 2014, 07:10
Default
  #5
Member
 
Anant Diwakar
Join Date: Jan 2013
Posts: 68
Rep Power: 4
diwakaranant is on a distinguished road
Hi

I tried using restart file to induce some disturbance, but still I am not
getting the flow as mentioned in the paper attached in the Post 2 of
this thread.

The config file is attached (without restart option).
I am using the hybrid mesh for NACA0012 given in the testcases
folder ( mesh_NACA0012_lam_hybrid_v3.su2).

Can anyone help ?

Thanks
Anant
Attached Files
File Type: txt lam_NACA0012.cfg.txt (15.5 KB, 19 views)
diwakaranant is offline   Reply With Quote

Old   February 20, 2014, 00:10
Default
  #6
New Member
 
David Manosalvas
Join Date: Feb 2014
Posts: 19
Rep Power: 3
demanosalvas is on a distinguished road
Anant,

I noticed that you are using JST, and this scheme can be a bit dissipative. Try lowering the coefficient of the 4th order artificial dissipation term, about one order of magnitude, and if this doesn't work give Roe 2nd order a try.

Have you tried refining your mesh and inserting a disturbance in the flow yet?

Hope this helps,

David
demanosalvas is offline   Reply With Quote

Old   February 20, 2014, 03:47
Default
  #7
Super Moderator
 
Thomas D. Economon
Join Date: Jan 2013
Location: Stanford, CA
Posts: 251
Rep Power: 5
economon is on a distinguished road
Hi guys,

You can achieve the type of results you see in the paper above if you make a few adjustments:

1. I think a c-mesh is better suited for this case, which gives extra refinement in the wake region.

2. Check that you have ~30 mesh points in the boundary layer for this Reynolds number (laminar flow).

3. I would second that the 2nd-order Roe method should be a good choice for this problem.

Please see the attached figure of SU2 results for a shedding NACA 0012 @ M = 0.8 and Re = 10,000. I have posted the files for this case here temporarily if you want to give it a try: http://www.stanford.edu/~economon/dr...m_naca0012.tgz. There are several other small changes that I've made to the config file you'll find in that directory.

All the best,
Tom
Attached Images
File Type: jpg naca0012_shedding.jpg (26.6 KB, 56 views)
economon is offline   Reply With Quote

Old   February 24, 2014, 00:47
Default
  #8
Member
 
Anant Diwakar
Join Date: Jan 2013
Posts: 68
Rep Power: 4
diwakaranant is on a distinguished road
Hi Thomas

I tried running the simulation for Mach = 0.8, using the config file and the
mesh file given by you.

The results are not matching to that given in the paper.

In the paper, the time period of the primary oscillation of cl coefficient is around 0.55 seconds, where in SU2 it is much less.

Moreover the secondary oscillation is not observed in SU2.

I am using time step for dual time stepping as 0.0001. So while plotting
cl vs t, I am multiplying no. of external iterations with this time step.

Please look into it. Cl vs time plot is attached.
Attached Files
File Type: pdf cl.pdf (42.3 KB, 34 views)
diwakaranant is offline   Reply With Quote

Old   February 24, 2014, 23:16
Default
  #9
Super Moderator
 
Thomas D. Economon
Join Date: Jan 2013
Location: Stanford, CA
Posts: 251
Rep Power: 5
economon is on a distinguished road
Hi Anant,

I should mention that I did not optimize/investigate any of the parameters in the config file and mesh that I provided above, but rather just wanted to give an example where shedding is observed.

You may want to perform a grid refinement study to make sure that the mesh is suitable for the conditions that you are simulating (again, I would recommend a c-mesh with decent resolution in the wake). You can also check that you are using exactly the same parameters as in the paper above. In particular, you may need to investigate the effect of the limiter coefficient for the 2nd-order Roe method or that the physical time step chosen is adequate to capture the effects that you are expecting.

Cheers,
Tom
economon 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
Comparison the airfoil 0012 experimental result and simulation result harrislcy FLUENT 30 August 29, 2013 10:27
Problem with airfoil shape optimization robyTKD SU2 Shape Design 6 June 13, 2013 19:13
Problem with restart solution in shape_optimization.py robyTKD SU2 Shape Design 21 May 29, 2013 09:26
result on airfoil wortmann fx63-137 simulation jdfortune FLUENT 5 January 31, 2011 20:26
Simulation of a moving airfoil in Fluent M.Sc_Student FLUENT 2 October 25, 2010 03:03


All times are GMT -4. The time now is 23:31.