CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM

OpenFOAM AirFoil2D example

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 22, 2011, 23:52
Default OpenFOAM AirFoil2D example
  #1
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 381
Rep Power: 7
Martin Hegedus is on a distinguished road
Continuation of OpenFOAM Convergence

I tried to converge the simpleFoam airfoild2D example to machine zero, or at least the tolerance (which I set to 1.0e-8 for all variables). I was successful until I got to zero degrees angle of attack. It failed for zero. Then I backed off a bit in regards to alpha (2.2036e-6 degrees) and was successful!!

Results Are:

Case 1, After 1000 iterations
U -> internalField uniform (26.000000 0.000001 0); = approx zero degrees,
smoothSolver: Solving for Ux, Initial residual = 1.00795e-08, Final residual = 5.50998e-11, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 8.04807e-09, Final residual = 8.04807e-09, No Iterations 0
GAMG: Solving for p, Initial residual = 1.03209e-07, Final residual = 1.00942e-08, No Iterations 1
time step continuity errors : sum local = 1.54372e-11, global = 7.48481e-19, cumulative = -1.77796e-14
smoothSolver: Solving for nuTilda, Initial residual = 9.11008e-09, Final residual = 9.11008e-09, No Iterations 0
ExecutionTime = 79.64 s ClockTime = 82 s

Case 2, After 1000 iterations
U -> internalField uniform (26.000000 0.000000 0); = 0 degrees, outlet = free stream
1000 iterations
smoothSolver: Solving for Ux, Initial residual = 5.60021e-05, Final residual = 3.20606e-06, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 3.15896e-05, Final residual = 1.81395e-06, No Iterations 4
GAMG: Solving for p, Initial residual = 0.000320099, Final residual = 3.03047e-05, No Iterations 7
time step continuity errors : sum local = 4.62797e-08, global = 1.18427e-17, cumulative = -3.77372e-15
smoothSolver: Solving for nuTilda, Initial residual = 2.10995e-06, Final residual = 4.48997e-08, No Iterations 2
ExecutionTime = 94.83 s ClockTime = 97 s

Anyone know what the story is? I gather there is a good chance it is some sort of a switch or bug. I can't believe I'm the first to experience this, so I guess it is a switch.

I'm using version 1.6 of OpenFOAM.
Martin Hegedus is offline   Reply With Quote

Old   June 23, 2011, 01:49
Default
  #2
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 381
Rep Power: 7
Martin Hegedus is on a distinguished road
checked the negative values,

v=-0.001 converges, v=-0.0001 does not.

Unfortunately the airfoil is not symmetric, therefore I can't check symmetry for this case.

I also searched inside the code but couldn't figure out how things work.

The fact that the input deck seems to say that the inlet and outlet is set to the freestream seems to indicate that the boundary condition would be rather simple to implement.
Martin Hegedus is offline   Reply With Quote

Old   June 23, 2011, 10:40
Default
  #3
Super Moderator
 
praveen's Avatar
 
Praveen. C
Join Date: Mar 2009
Location: Bangalore
Posts: 239
Blog Entries: 6
Rep Power: 8
praveen is on a distinguished road
Upwind scheme or non-smooth limiters could cause such behaviour.
praveen is offline   Reply With Quote

Old   June 23, 2011, 12:00
Default
  #4
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 381
Rep Power: 7
Martin Hegedus is on a distinguished road
Since the non convergence happens over such a narrow band, is non symmetric in regards to alpha, and occurs at a point where the freestream vector is parallel to the outer boundary, means that proper verification of OpenFOAM requires that the issue is investigated as is. Unfortunately, after looking at the insides of the code, I'm not the person to do it. For me personally, my understanding of C/C++ and the general workings of a CFD code are not enough to make my way around OpenFOAM.

In the near future I'll update to version 2.0 of OpenFOAM and if the problem still exists, and no one else addresses it or points out an input error on my part, I'll submit it to the bugs area.
Martin Hegedus is offline   Reply With Quote

Old   June 24, 2011, 16:21
Default
  #5
Senior Member
 
Martin Hegedus
Join Date: Feb 2011
Posts: 381
Rep Power: 7
Martin Hegedus is on a distinguished road
Apparently it is the use of the freestream boundary condition (it acts like an inletOutlet condition) on the inlet face (the front, top, and bottom of the box which surrounds airfoil) which prevents the case from converging to machine zero when the angle of attack is 0.

I was able to converge the problem by setting the inlet face to a wall boundary and then setting the values (fixedValues) to the freestream values. I kept the outlet as the original freestream boundary condition.

I was also able to converge the problem to machine zero by setting the velocity for the inlet face to freestream fixed values and the pressure to zero gradient.
Martin Hegedus 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
Cross-compiling OpenFOAM 1.7.0 on Linux for Windows 32 and 64bits with Mingw-w64 wyldckat OpenFOAM Announcements from Other Sources 3 September 8, 2010 07:25
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 17 August 22, 2009 04:59
Modified OpenFOAM Forum Structure and New Mailing-List pete Site News & Announcements 0 June 29, 2009 06:56
64bitrhel5 OF installation instructions mirko OpenFOAM Installation 2 August 12, 2008 19:07
Adventure of fisrst openfoam installation on Ubuntu 710 jussi OpenFOAM Installation 0 April 24, 2008 15:25


All times are GMT -4. The time now is 09:38.