# Running an airfoil case

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 2, 2012, 09:01 Running an airfoil case #1 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 4 Hi to everyone, I want to run a simulation over a 2D airfoil with the following hypothesis: It's a 2D, steady-state, laminar, incompressible simulation so I've modified the simpleFoam solver, switching the turbulence to "off". I've also build a "C mesh" over the airfoil. What I'm now troubling with are the boundary conditions: I thought that the most appropriate BCs would be: - freestream BC for velocity (everywhere except on the foil, where I've put the no slip condition); -freestreamPressure for the pressure; openFoam doesn't like these condition, I think because there isn't a "reference value" for the pressure, but also USING a reference value for the pressure, the simulation "explode" and doesn't converge to any reasonable result. This is my problem. Has anyone any suggestion? Thanks in advance Simone

 October 2, 2012, 09:43 #2 Senior Member   Join Date: Aug 2010 Location: Groningen, The Netherlands Posts: 216 Rep Power: 9 Why don't you use fixed value and zero Gradient? With these two you should be able to define your system sufficiently for both velocity and pressure. freestream doesn't make any sense since you know your velocity in most parts of your domain regards

 October 2, 2012, 10:52 #3 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 4 So you're suggesting: -U fixedValue (equal to zero) over the airfoil for the no-slip condition; -U fixedValue (different from zero and equal to my desired velocity) over the other patches; -p zeroGradient on every patch except inside the domain where i can fix an arbitrary value? Thanks again Colin

 October 3, 2012, 09:41 #4 Senior Member   Join Date: Aug 2010 Location: Groningen, The Netherlands Posts: 216 Rep Power: 9 not exactly: all values you know you should specify with fixed value. That includes the velocity at the inlet and in the internal field all values you don't know you assign with zero Gradient that includes all pressure values (outlet foil inlet) and velocity at the outlet. The velocity on the foil depends on whether you want to take into account friction or not If so set it to zero if not use slip

 October 3, 2012, 10:23 #5 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 4 This is the error I get if I use zeroGradient for every pressure patch: FOAM FATAL IO ERROR: Unable to set reference cell for field p Please supply either pRefCell or pRefPoint Because of that I had thought to set a reference value in one patch. Is there another solution to fix this problem?

 October 5, 2012, 03:24 #6 Senior Member   Join Date: Aug 2010 Location: Groningen, The Netherlands Posts: 216 Rep Power: 9 maybe this helps: what is the internal field of your p file? I set it to uniform 0

 October 5, 2012, 06:12 #7 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 4 Me too! Here's the full list of my patches and relative BC for P: internalField uniform 0; boundaryField { inlet { type fixedValue; value uniform 0; } outlet { type zeroGradient; } top { type zeroGradient; } bottom { type zeroGradient; } foil { type zeroGradient; } front { type empty; } back { type empty; } } if instead of inlet BC set as fixedValue I would set it as zeroGradient I'll obtain that error.

 October 5, 2012, 07:04 #8 Senior Member   Join Date: Aug 2010 Location: Groningen, The Netherlands Posts: 216 Rep Power: 9 I found an old p file from my graduation thesis: (at that time I used OF 1.7.1): Code: ```dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { wInlet { type zeroGradient; } outlet { type zeroGradient; } foil { type zeroGradient; } frontAndBack { type empty; }``` and this is how my fvSolution file looked like: Code: ```solvers { p { solver GAMG; tolerance 1e-07; relTol 0.1; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } U { solver smoothSolver; smoother GaussSeidel; nSweeps 2; tolerance 1e-08; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 4; pRefCell 0; pRefValue 0; } relaxationFactors { default 0; p 0.3; U 0.7; nuTilda 0.7; }``` note that there is a reference cell defined, of which I wasn't aware anymore. This would make your fixedValue definition at the inlet for the pressure obsolete, which I think is better, for you don't know, what pressure values there actually are Further I have to mention, that I didn't use a top and bottom patch for my flow was inclined! Finally I would suggest you to collect all patches with the same properties in one patch (e.g. frontAndBack instead of separate patches front, back -> simply collect the node numbers in the blockMeshDict in one patch definition), this improves readability.

 October 7, 2012, 11:27 #9 New Member   saeid oqaz Join Date: Feb 2012 Posts: 19 Rep Power: 5 hi Simone & colin i working on same project but in 3D. i have 2 question. what is the internal field of your U file? is the freestream velocity? and colin you what solver use for this case? and in fvsolution dic GAMG relevant for P. i use CG. can u attach fvSchemes file & B.C file for U? Last edited by saeid.oqaz; October 7, 2012 at 11:57.

 October 8, 2012, 02:38 #10 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 4 @Colin: I try to run your mesh with "zeroGradient" everywhere on "my" solver with this parameters for p: solvers { p { solver PCG; preconditioner DIC; tolerance 1e-06; relTol 0.01; } It runs and doesn't create problems! So I can't still understand where the problem is. @Saeid: For U i used fixedValue everywhere except on the outlet patch where i put zero gradient. For the solver I can tell you that, since my simulation is steady, I used simpleFoam solver.

October 16, 2012, 03:37
#11
Senior Member

Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 9
Hi there,

Quote:
 (...) what is the internal field of your U file? is the freestream velocity? (...)
usually the internal field is a vector specified with the key word internal field
see therefore the user manual as reference.

Quote:
 (...) and colin you what solver use for this case? and in fvsolution dic GAMG relevant for P. i use CG. (...)
as Simone I used the simpleFoam solver, but my knowledge concerning the
solvers is limited and I used the GAMG according to a recommendation.

My settings for U you can read from my previous posts

and the fvSchemes looks as follows:

Code:
```ddtSchemes
{
}

{
default         Gauss linear;
}

divSchemes
{
default         none;
div(phi,U)      Gauss linearUpwind Gauss linear;
div(phi,nuTilda) Gauss linearUpwind Gauss linear;
}

laplacianSchemes
{
default         none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
laplacian(1,p)  Gauss linear corrected;
}

interpolationSchemes
{
default         linear;
interpolate(U)  linear;
}

{
default         corrected;
}

fluxRequired
{
default         no;
p               ;
}```
NOTE: this is what I used for OF 1.7.1 eventually notation and settings
have changed

 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 ysh1227 OpenFOAM Running, Solving & CFD 2 May 7, 2015 10:13 ysh1227 OpenFOAM Running, Solving & CFD 0 May 23, 2012 05:26 doug OpenFOAM Running, Solving & CFD 8 October 13, 2010 07:06 Frank Main CFD Forum 1 April 21, 2008 18:36 Akbar Main CFD Forum 1 July 22, 2005 11:49

All times are GMT -4. The time now is 21:11.

 Contact Us - CFD Online - Top