|
[Sponsors] |
January 14, 2015, 05:18 |
Boundary Layer strange result
|
#1 |
Member
daniel fernex
Join Date: Oct 2014
Location: Braunschweig, Germany
Posts: 36
Rep Power: 12 |
Dear all,
I'm coming to you because I'm facing a boundary layer problem on a simulation... I'm simulating a body in a flow with an inlet velocity Ux=5m/s. But right from the first iterations, the results close to the body gets strange... This can be seen on the attached pictures. One can see that the velocity is 0 on the wall, but gets much bigger around the first cell, and then decreases again. And because of this my simulation blows up after a few iterations. What I've done :
I'm running out of ideas, so if anyone has any hint it would be very appreciated ! Regards, Daniel |
|
January 14, 2015, 08:07 |
|
#2 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
Daniel, what do you need, steady-state or unsteady solutions?
__________________
The skeleton ran out of shampoo in the shower. |
|
January 14, 2015, 08:46 |
|
#3 |
Member
daniel fernex
Join Date: Oct 2014
Location: Braunschweig, Germany
Posts: 36
Rep Power: 12 |
Hi, thanks for the quick reply.
In the end I need an unsteady simulation with moving mesh (with pimpleDyMFoam), but the error occurs for all cases. I am currently trying with a steady-state simulation to check the mesh convergence (minimum mesh size to have a mesh-independent solution). |
|
January 14, 2015, 08:47 |
|
#4 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
That means simpleFoam? Then post the log output of that until it becomes ugly...
__________________
The skeleton ran out of shampoo in the shower. |
|
January 14, 2015, 09:53 |
|
#5 |
Member
daniel fernex
Join Date: Oct 2014
Location: Braunschweig, Germany
Posts: 36
Rep Power: 12 |
Yes I'm using simpleFoam.
Here a sample of the log : Code:
Time = 319 smoothSolver: Solving for Ux, Initial residual = 0.057221157, Final residual = 3.568287e-06, No Iterations 16 smoothSolver: Solving for Uy, Initial residual = 0.063087545, Final residual = 4.5084555e-06, No Iterations 18 GAMG: Solving for p, Initial residual = 0.0037987384, Final residual = 2.7417897e-07, No Iterations 23 GAMG: Solving for p, Initial residual = 0.00020201867, Final residual = 9.5084443e-08, No Iterations 12 time step continuity errors : sum local = 1.6112304, global = -0.03484718, cumulative = -0.77715832 smoothSolver: Solving for nuTilda, Initial residual = 0.046411558, Final residual = 4.2056708e-06, No Iterations 3 ExecutionTime = 870.68 s ClockTime = 886 s forces forcesPaddle0 output: sum of forces: pressure : (0 0 0) viscous : (2.6813238e+13 5.6435289e+11 -1.4963997) porous : (0 0 0) sum of moments: pressure : (0 0 0) viscous : (-2.8217644e+11 1.3406619e+13 -2.6081707e+13) porous : (0 0 0) forceCoeffs forceCoeffsPaddle0 output: Cm = -5.2163414e+11 Cd = 5.3626477e+11 Cl = 1.1287058e+10 Cl(f) = -5.1599061e+11 Cl(r) = 5.2727767e+11 forceCoeffs forceCoeffsPaddle1 output: Cm = -96904.785 Cd = -66422.036 Cl = 297601.6 Cl(f) = 51896.014 Cl(r) = 245705.58 Time = 320 smoothSolver: Solving for Ux, Initial residual = 0.052995367, Final residual = 4.8433206e-06, No Iterations 15 smoothSolver: Solving for Uy, Initial residual = 0.062183782, Final residual = 5.6252108e-06, No Iterations 17 GAMG: Solving for p, Initial residual = 0.0037642096, Final residual = 3.4332139e-07, No Iterations 21 GAMG: Solving for p, Initial residual = 0.00017745207, Final residual = 5.9287776e-08, No Iterations 12 time step continuity errors : sum local = 1.085192, global = -0.02221701, cumulative = -0.79937533 smoothSolver: Solving for nuTilda, Initial residual = 0.061514173, Final residual = 3.6499883e-06, No Iterations 3 ExecutionTime = 874.44 s ClockTime = 890 s forces forcesPaddle0 output: sum of forces: pressure : (0 0 0) viscous : (3.1377491e+13 6.8424339e+11 -1.8496672) porous : (0 0 0) sum of moments: pressure : (0 0 0) viscous : (-3.421217e+11 1.5688745e+13 -3.0631529e+13) porous : (0 0 0) forceCoeffs forceCoeffsPaddle0 output: Cm = -6.1263058e+11 Cd = 6.2754982e+11 Cl = 1.3684868e+10 Cl(f) = -6.0578814e+11 Cl(r) = 6.1947301e+11 forceCoeffs forceCoeffsPaddle1 output: Cm = -114884.08 Cd = -78823.833 Cl = 351014.44 Cl(f) = 60623.139 Cl(r) = 290391.3 Time = 321 And as I said, this simulation works just fine when the mesh on the BL is finer. |
|
January 14, 2015, 09:58 |
|
#6 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
1) In my experience your linear solvers take too many iterations in each outer (SIMPLE) iteration. Did you set relTol to 1e-4? This is normally not needed in SIMPLE. But fixing this will make your solver only faster... not better You can post the fvSolution to get some help.
2) Can you post checkMesh output and fvSchemes? What about your boundary conditions? Are you sure, they are correct? If not, you can post them, too.
__________________
The skeleton ran out of shampoo in the shower. |
|
January 14, 2015, 10:18 |
|
#7 |
Member
daniel fernex
Join Date: Oct 2014
Location: Braunschweig, Germany
Posts: 36
Rep Power: 12 |
I'm rather confident about the boundary conditions. After trying many of them, the only one working are those from the motorBike example (with Spalart-Allmaras model).
The problem occurs with different schemes (accurate as well as diffusive schemes). Same with the tolerances. I've tried with maxIter=1000 (tolerance and relTol = 0) just for fun, and it still doesn't work. To sum up, the problem appears as soon as I increase the cells size around the body. I understand this could cause troubles with a turbulent case without using a wall function, but it also causes troubles in laminar... Concerning the wall function, as far as I know I just have to specify the wall function in 0/nut, right ? Are the initial conditions as posted here ok considering I'm using a wall function ? nut Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.3.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object nut; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [ 0 2 -1 0 0 0 0 ]; internalField uniform 0; boundaryField { Inlet { type calculated; value uniform 0; } Outlet { type calculated; value uniform 0; } upperSym { type symmetryPlane; value uniform 0; } lowerSym { type symmetryPlane; value uniform 0; } paddle0 { type nutUSpaldingWallFunction; value uniform 0; } paddle1 { type nutUSpaldingWallFunction; value uniform 0; } AMI_P0S { type cyclicAMI; value $internalField; } AMI_P1S { type cyclicAMI; value $internalField; } AMI_SP0 { type cyclicAMI; value $internalField; } AMI_SP1 { type cyclicAMI; value $internalField; } AMI_SF { type cyclicAMI; value $internalField; } AMI_FS { type cyclicAMI; value $internalField; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.3.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object nuTilda; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [ 0 2 -1 0 0 0 0 ]; internalField uniform 0.05; //internalField uniform 0.05; boundaryField { Inlet { type fixedValue; value uniform 0.05; } Outlet { type inletOutlet; inletValue uniform 0.05; value uniform 0.05; } upperSym { type symmetryPlane; } lowerSym { type symmetryPlane; } paddle0 { type fixedValue; value uniform 0; } paddle1 { type fixedValue; value uniform 0; } AMI_P0S { type cyclicAMI; value $internalField; } AMI_P1S { type cyclicAMI; value $internalField; } AMI_SP0 { type cyclicAMI; value $internalField; } AMI_SP1 { type cyclicAMI; value $internalField; } AMI_SF { type cyclicAMI; value $internalField; } AMI_FS { type cyclicAMI; value $internalField; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.3.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; location "0"; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (5 0 0); boundaryField { Inlet { type fixedValue; value uniform (5 0 0); } Outlet { type inletOutlet; inletValue uniform (0 0 0); value uniform (5 0 0); } upperSym { type symmetryPlane; } lowerSym { type symmetryPlane; } paddle0 { type fixedValue; value uniform (0 0 0); } paddle1 { type fixedValue; value uniform (0 0 0); } AMI_P0S { type cyclicAMI; value $internalField; } AMI_P1S { type cyclicAMI; value $internalField; } AMI_SP0 { type cyclicAMI; value $internalField; } AMI_SP1 { type cyclicAMI; value $internalField; } AMI_SF { type cyclicAMI; value $internalField; } AMI_FS { type cyclicAMI; value $internalField; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.3.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; location "0"; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [ 0 2 -2 0 0 0 0 ]; internalField uniform 0; boundaryField { Inlet { type zeroGradient; } Outlet { type fixedValue; value uniform 0; } upperSym { type symmetryPlane; } lowerSym { type symmetryPlane; } paddle0 { type fixedValue; value uniform 0; } paddle1 { type fixedValue; value uniform 0; } AMI_P0S { type cyclicAMI; value $internalField; } AMI_P1S { type cyclicAMI; value $internalField; } AMI_SP0 { type cyclicAMI; value $internalField; } AMI_SP1 { type cyclicAMI; value $internalField; } AMI_SF { type cyclicAMI; value $internalField; } AMI_FS { type cyclicAMI; value $internalField; } } // ************************************************************************* // |
|
January 14, 2015, 10:20 |
|
#8 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
paddle0 and paddle1 are walls? If so, why did you set pressure to zero and not zerogradient?
__________________
The skeleton ran out of shampoo in the shower. |
|
January 14, 2015, 10:25 |
|
#9 |
Member
daniel fernex
Join Date: Oct 2014
Location: Braunschweig, Germany
Posts: 36
Rep Power: 12 |
Oh my god............
I hadn't noticed, it the same for all simulations I've run......... I guess I'm sometimes being confused with all the files... This could definitely create problems... I change this and I keep you posted. Thank you for seeing this ! |
|
January 14, 2015, 10:28 |
|
#10 |
Member
daniel fernex
Join Date: Oct 2014
Location: Braunschweig, Germany
Posts: 36
Rep Power: 12 |
And concerning the wall function definition, do you agree on what I've put ?
|
|
January 14, 2015, 10:29 |
|
#11 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
I don't use SA-model but the airfoil2d tutorial uses it the same way.
__________________
The skeleton ran out of shampoo in the shower. |
|
January 15, 2015, 08:14 |
|
#12 |
Member
daniel fernex
Join Date: Oct 2014
Location: Braunschweig, Germany
Posts: 36
Rep Power: 12 |
Ok, that was the problem... Everything works just fine now !
I would never have thought the error could come from initial conditions... Thanks a lot for this, you saved me many hours of work ! Regards, Daniel |
|
January 15, 2015, 08:16 |
|
#13 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
Maybe just a typo, but it should be "boundary" not "initial" conditions in your last post.
__________________
The skeleton ran out of shampoo in the shower. |
|
January 15, 2015, 08:18 |
|
#14 |
Member
daniel fernex
Join Date: Oct 2014
Location: Braunschweig, Germany
Posts: 36
Rep Power: 12 |
You don't miss anything
It's boundary condition indeed. |
|
January 15, 2015, 08:21 |
|
#15 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 27 |
Now you can tune your solver settings to get rid of these horrible iterations. If you need any consecutive help or are not sure just post again.
__________________
The skeleton ran out of shampoo in the shower. |
|
Tags |
boundary layer, diverging, openfoam |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
sliding mesh problem in CFX | Saima | CFX | 46 | September 11, 2021 08:38 |
[snappyHexMesh] Snappy creates strange cells far away from boundary | vainilreb | OpenFOAM Meshing & Mesh Conversion | 3 | December 16, 2020 06:11 |
[snappyHexMesh] snappyHexMesh Boundary Layer at Corner | panpanzhong | OpenFOAM Meshing & Mesh Conversion | 5 | July 3, 2018 06:53 |
Divide Prismatic Boundary Layer Mesh causes overlapping faces | SilentRunner42 | enGrid | 4 | May 4, 2015 04:37 |
[GAMBIT] 3D boundary layer and meshing problem in GAMBIT 2.4.6 | prashanthreddyh | ANSYS Meshing & Geometry | 1 | December 20, 2011 01:35 |