# OpenFOAM AirFoil2D example

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

 June 22, 2011, 22:52 OpenFOAM AirFoil2D example #1 Senior Member   Martin Hegedus Join Date: Feb 2011 Posts: 480 Rep Power: 12 Continuation of http://www.cfd-online.com/Forums/ope...nvergence.html 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.

 June 23, 2011, 00:49 #2 Senior Member   Martin Hegedus Join Date: Feb 2011 Posts: 480 Rep Power: 12 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.

 June 23, 2011, 09:40 #3 Super Moderator     Praveen. C Join Date: Mar 2009 Location: Bangalore Posts: 263 Blog Entries: 6 Rep Power: 11 Upwind scheme or non-smooth limiters could cause such behaviour.

 June 23, 2011, 11:00 #4 Senior Member   Martin Hegedus Join Date: Feb 2011 Posts: 480 Rep Power: 12 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.

 June 24, 2011, 15:21 #5 Senior Member   Martin Hegedus Join Date: Feb 2011 Posts: 480 Rep Power: 12 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36 wyldckat OpenFOAM Announcements from Other Sources 3 September 8, 2010 06:25 pete Site News & Announcements 0 June 29, 2009 05:56 mirko OpenFOAM Installation 2 August 12, 2008 18:07 jussi OpenFOAM Installation 0 April 24, 2008 14:25

All times are GMT -4. The time now is 21:00.