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

NACA0012 Validation Case Questions

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 3, 2010, 11:07
Default NACA0012 Validation Case Questions
  #1
Senior Member
 
jeff osborne
Join Date: Mar 2010
Posts: 108
Rep Power: 7
ozzythewise is on a distinguished road
Hello all,

I am brand spanking new to CFD and am trying my hand at multiple validation cases to gain some experience. I am about to try flow over an NACA0012 airfoil but I have a few questions that I was hoping anybody could help me resolve. Details about my simulation: I will be performing the simulation on OpenFOAM. I want the Reynolds numbers to be 3e6, 6e6 and 1e7. I'm going to do at 0, 10 and 15 degrees angle of attack. I think I'll use the Spallart-Allmaras turbulent model. My inlet will be ~10 chord lengths from the body and outlet maybe ~20. My questions were:

1) At these Reynolds numbers will I not be able to use a central differencing interpolation scheme? And if not, what could I use (because I will have flow non-parallel to the grid, I'm worried about false diffusion with an upwind scheme).

2) I've read that drag coefficients can be off for this simulation because of using a turbulent model when much of the flow is laminar. Is there any way of accurately simulating this without having to compare the results to trip-wire results?

I'm sure I'll have more questions as I start and I'll post them if I do, but if anyone has an answer to these or any other suggestions, that would be very much appreciated.

Thanks in advance
-Jeff
ozzythewise is offline   Reply With Quote

Old   August 3, 2010, 12:13
Default
  #2
agd
Senior Member
 
Join Date: Jul 2009
Posts: 191
Rep Power: 7
agd is on a distinguished road
You can use central differencing at any Re, but you will need to add artificial viscosity to stabilize the scheme. A good high-resolution upwind scheme can work well also. As far as drag numbers are concerned, the SA model should "trip" naturally very close to the flow attachment point at those Re numbers. Provided you have gridded the airfoil to obtain sufficient accuracy, I would expect your drag numbers to come out in reasonable agreement with experiment. This means a y+ ~ 1 for the standard SA model, or y+~30-50 if you are using wall function boundary conditions.
agd is offline   Reply With Quote

Old   August 3, 2010, 12:23
Default
  #3
Senior Member
 
jeff osborne
Join Date: Mar 2010
Posts: 108
Rep Power: 7
ozzythewise is on a distinguished road
Thanks for this, I have some follow-up questions though

- What is artificial viscosity and how do I add it?
- Does the SA model account properly for the large amount of laminar flow over an airfoil? Like, will the results I get match up to an experiment on an airfoil with a trip wire or without?

Thanks for the help
Jeff
ozzythewise is offline   Reply With Quote

Old   August 3, 2010, 14:39
Default
  #4
agd
Senior Member
 
Join Date: Jul 2009
Posts: 191
Rep Power: 7
agd is on a distinguished road
What flow solver are you using? A commercial code should have documentation on the artificial viscosity scheme it uses if it allows central differencing. If you are writing your own code, then you need to do some research on artificial viscosity (possibly start in the CFD wiki), as there are several different approaches to its inclusion. In short, though, artificial viscosity serves to give a central difference scheme a slight upwind flavor.

Assuming that the SA model is properly formulated, it should not affect a uniform flow until the model encounters something that triggers the source terms. That's what the trip terms essentially do - they allow the user to specify a point where the source terms drive the model to produce eddy viscosity. With the SA model you can also leave the trip terms out and specify a reasonable initial value of nu_tilda and let the vorticity-driven production do the rest. Spalart and Allmaras discuss this in their paper. However, for the Re numbers you are using, how much of the airfoil is going to remain laminar? If you have information on trip locations in experimental data, then you can use that in your simulations. But even at the lowest Re you are using, it's a fair guess that only about 10% (at most) of the airfoil surface would be laminar - I would be willing to try running turbulent with no explicit trips to see how the results compare.

A bigger question is the validity of the turbulence model when the flow separates at high angle of attack - but again, at this point I would say give it a shot and see what you can learn.
agd 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
Changing the grid on the same set-up Katya FLUENT 12 October 8, 2009 16:31
icoFsiFoam case needed vivekcfd OpenFOAM 1 May 6, 2009 13:41
Different Flow in One Case Dong Fu FLUENT 0 February 1, 2008 10:28
Body force - Does it work? Jan Rusås CFX 5 August 27, 2002 09:50
Heat Transfer Validation test case Chris Whitney Main CFD Forum 1 July 21, 1999 14:36


All times are GMT -4. The time now is 00:38.