|
[Sponsors] |
Boundary conditions for 2D Navie-Stockes simulation |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
March 7, 2011, 09:46 |
Boundary conditions for 2D Navie-Stockes simulation
|
#1 |
New Member
Join Date: Feb 2011
Posts: 20
Rep Power: 15 |
Hi Foamers!
In the past days I tried to set the case of a simple 2D-incompressible simulation of an airfoil using a O-mesh with the influence of both viscosity and turbulence (SST model) using pisoFoam. As shown on the figure below, the topology of my case is made of:
Based on searches in the forum I have 3 questions for you: A) In the 0/ folder, why do we need to set boundary conditions for all the working variables on all the boundaries? (For example, at wall, couldn't we just set the velocity to 0 instead of adding also a BC for the pressure ?) B) How can I set non-reflecting boundary conditions for the farfield? C) Based on my experience, I tried the boundary conditions mentioned hereafter. The computation ran properly but I do not get the right cp distribution nor aerodynamic coefficient values. Did I make a major mistake? Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.4.1 | | \\ / A nd | Web: http://www.openfoam.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ // Field Dictionary FoamFile { version 2.0; format ascii; root ""; case ""; instance ""; local ""; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (25 0 0); boundaryField { inlet-outlet { type fixedValue; value uniform (25 0 0); } body { type fixedValue; value uniform (0 0 0) } defaultFaces { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.4.1 | | \\ / A nd | Web: http://www.openfoam.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ // Field Dictionary FoamFile { version 2.0; format ascii; root ""; case ""; instance ""; local ""; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 82714; boundaryField { inlet-outlet { type zeroGradient; } body { type zeroGradient; } defaultFaces { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object k; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 0.001; boundaryField { inlet-outlet { type fixedValue; value uniform 0.001; } body { type zeroGradient; } defaultFaces { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.x | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object mut; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -1 0 0 0 0]; internalField uniform 0; boundaryField { inlet-outlet { type calculated; value uniform 0; } body { type mutLowReWallFunction; Cmu 0.09; kappa 0.41; E 9.8; value uniform 0; } defaultFaces { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volSymmTensorField; object R; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform (0 0 0 0 0 0); boundaryField { inlet-outlet { type kqRWallFunction; value uniform ( 0 0 0 0 0 0 ); } body { type kqRWallFunction; value uniform ( 0 0 0 0 0 0 ); } defaultFaces { type empty; } } // ************************************************************************* // L1011 |
|
March 9, 2011, 05:33 |
|
#2 |
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 18 |
Hello,
A) There is not "default condition" in OF, so you must set boundary condition for all variables. B) 1) For airfoil simulation, first rule is to set your far field domain to 30 - 50 chord lenght. From your picture, you are at 2 only, and you will have big reflexion and distorsion in the u and p field. 2) Your boundary conditions are not optimal. Try: For U, at inlet-outlet, try the inletOutlet condition For p, at inlet-outlet, try outletInlet For k, at inlet-outlet: inletOutlet, and for your wall: fixedValue if y+<1 or kqRWallFunction if y+>30 For omega (if kw SST), the same, i.e inletOutlet and omegaWallFunction at wall. For mut, seem ok if you use a low Re turbulence model (kw SST is not a low Re model), or mutWallFunction For R, at inlet-outlet you should try inletOutlet too. FvScheme: don't forget to use Gauss upwind for div scheme with k/epsilon/omega at first. FvSolution: set tolerance for omega/k/epsion to a low value , i.e 1e-15, and play with relTol (start at 0.1 to ...1e-6) Hope this help olivier |
|
March 9, 2011, 22:32 |
|
#3 |
New Member
Join Date: Feb 2011
Posts: 20
Rep Power: 15 |
Hi Olivier,
Thank you for your hints, I'll try to make a comparative study with the results already get. L1011 |
|
December 11, 2012, 10:26 |
|
#4 |
Member
VS
Join Date: Nov 2012
Posts: 86
Rep Power: 13 |
OivierG,
your post was very helpful to me also,but i want to ask if there is any specific reason or criteria for using outletInlet for p and not inletOutlet? The same question occurs for velocity.How do we choose one or the other? |
|
December 11, 2012, 12:08 |
|
#5 |
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 18 |
hello,
outletInlet use zeroGradient in case of inflow, and fixedValue for outflow, inletOutlet use fixedValue for inflow, and zeroGradient for outflow, so you see that you will use inletOutlet for U at both inlet & outlet, and outletInlet for p (inlet & outlet). You may try the opposite (i.e use a fixed outflow velocity), but this is realy not a good idea. regards, olivier |
|
December 13, 2012, 08:17 |
rhosimplecfoam
|
#6 |
Member
Join Date: Oct 2012
Posts: 47
Rep Power: 14 |
Hi
I want simulate a supercritical airfoil by using rhosimplecfoam.mach number is 0.5.but, I do not know what boundary conditions should I use? pleas help me? |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Impinging Jet Boundary Conditions | Anindya | Main CFD Forum | 25 | February 27, 2016 12:58 |
CFX does not continue | Shafiul | CFX | 10 | February 17, 2011 07:57 |
Boundary conditions for pipework simulation | metro | OpenFOAM Running, Solving & CFD | 0 | August 12, 2010 03:13 |
transient simulation of a rotating rectangle | icesniffer | CFX | 1 | August 8, 2009 07:25 |
Need help about boundary conditions for a francis runner flow simulation | Rodrigo Escobar Moragas | Main CFD Forum | 1 | October 26, 1998 08:20 |