Propeller tutorial with air instead of water

JShnyder · June 25, 2016, 09:31

Hi everyone,

I want to run the propeller tutorial with air. I've read somewhere that with the pimpleDym-solver the only thing to do were to change

Code:

nu[0 2 -1 0 0 0 0] 1e-5; //the kinematic viscosity of water(1e-6) or air(1e-5)

in the transportProperties-file. I can't imagine that's all - wouldn't the simulation lead to different results at different altitudes/air pressures or be influenced by other factors?

SirIsaac90 · June 27, 2016, 03:58

Hi JShnyder,

That is almost all for incompressible flows. I would also adapt the turbulent dissipation by a factor of 10^(-1), because it depends on viscosity.

Gravitation is not considered at all in this case example.

Regards
JW

crusen mind · June 28, 2016, 08:10

Quote:

Originally Posted by JShnyder

Hi everyone,

I want to run the propeller tutorial with air. I've read somewhere that with the pimpleDym-solver the only thing to do were to change

Code:

nu[0 2 -1 0 0 0 0] 1e-5; //the kinematic viscosity of water(1e-6) or air(1e-5)

in the transportProperties-file. I can't imagine that's all - wouldn't the simulation lead to different results at different altitudes/air pressures or be influenced by other factors?

hello shnyder
do you know how to set up a propeller case

SirIsaac90 · June 29, 2016, 03:04

Quote:

Originally Posted by crusen mind

hello shnyder
do you know how to set up a propeller case

Hi,

Maybe you can have a look here.

I managed my simulations with this description. Of course, there is a difference between transient and stationary simulations. In the stationary case you need for example the MRF function. In the transient case you can use a dynamic mesh (just look into the tutorial cases of pimpleDyMFoam).

If you have any further questions to the procedure, don't hesitate to ask.

Regards
JW

crusen mind · June 30, 2016, 02:19

hi SirIssac
I am using ANSA for meshing. The link you posted show how to do rotor and stator mesh in snappy hex mesh.
basically I am not able to run my ALL RUN script in simpleFOAM rotor disk tutorial
i Will post my log files for rotor disk case

log create patch
./Allrun: 81: ./Allrun: createPatch: not found

log.simpleFoam

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v3.0+ |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : v3.0+-e941ee6c15e9
Exec : simpleFoam
Date : Jun 27 2016
Time : 15:30:33
Host : "velan-OptiPlex-9020"
PID : 3025
Case : /home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

SIMPLE: convergence criteria
field U tolerance 0.0001
field p tolerance 0.001
field "(k|epsilon|omega)" tolerance 0.001

Reading field p

Reading field U

Reading/calculating face flux field phi

--> FOAM FATAL IO ERROR:
Unable to set reference cell for field p
Please supply either pRefCell or pRefPoint

file: /home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk/system/fvSolution.SIMPLE from line 42 to line 49.

From function void Foam::setRefCell(const volScalarField&, const volScalarField&, const Foam::dictionary&, Foam::label&, Foam::scalar&, bool)
in file cfdTools/general/findRefCell/findRefCell.C at line 105.

FOAM exiting

log.snappyHEXMESH

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v3.0+ |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : v3.0+-e941ee6c15e9
Exec : snappyHexMesh -overwrite
Date : Jun 27 2016
Time : 15:30:32
Host : "velan-OptiPlex-9020"
PID : 3022
Case : /home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Read mesh in = 0.01 s

Overall mesh bounding box : (-1.26 -2.01 -1.26) (1.26 2.01 1.26)
Relative tolerance : 1e-06
Absolute matching distance : 5.3722621e-06

Reading refinement surfaces.
Read refinement surfaces in = 0.03 s

Reading refinement shells.
Refinement level 1 for all cells inside fixed.obj
Refinement level 4 for all cells inside rotatingZone.obj
shellSurfaces : Flipped orientation of surface rotatingZone.obj so point (3.75 6 3.75) is outside.
Read refinement shells in = 0.02 s

Setting refinement level of surface to be consistent with shells.
For geometry fixed.obj detected 0 uncached triangles out of 5012
For geometry rotatingZone.obj detected 0 uncached triangles out of 3964
Checked shell refinement in = 0.05 s

Reading features.

--> FOAM FATAL IO ERROR:
Could not open "/home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk/constant/triSurface/fixed.eMesh"

file: /home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk/system/snappyHexMeshDict.castellatedMeshControls.features from line 47 to line 47.

From function void Foam::refinementFeatures::read(const Foam:

bjectRegistry&, const Foam::PtrList<Foam::dictionary>&)
in file autoHexMesh/refinementFeatures/refinementFeatures.C at line 97.

FOAM exiting

log.surfaceFeature EXtract

./Allrun: 81: ./Allrun: surfaceFeatureExtract: not found

SirIsaac90 · July 6, 2016, 04:05

Hi!

I always do it in the following manner:

1) Meshing of propeller region and then rest of the model without propeller region
--> Does not depend on the meshing tool

2) Merge both meshes with mergeMeshes

3) Define the region, where the propeller is inside with topoSet

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.4.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

actions
(

    // Get all faces in cellSet

    {
        name    Rotator;
        type    cellSet;
        action  new;
        source  regionToCell;
        sourceInfo
        {
            nErode 0;
            insidePoints ((0 -0.1 0));
        }
    }

    {
        name    Rotator;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set     Rotator;
        }
    }
);

4) Depending on your OpenFOAM version use fvOptions or MRFProperties for defining the rotation (stationary). Otherwise use dynamicMeshDict.

fvOptions:

Code:

    cellZone_3_mrf
    {
        type MRFSource;
        active true;
        selectionMode cellZone;
        cellZone Rotator;
        MRFSourceCoeffs
        {
            origin (2.43 1.74 -0.52);
            axis (0 0 1);
            omega constant 18.95; //18.95
        }

    }

In your tutorial case, it seems that there are missing some files. Sorry, I can't see other problems from your logs. Maybe you should download the tutorial case again or look whether your OpenFOAM version is alright. All other tutorials run fine?

Regards,
JW

JShnyder · July 6, 2016, 04:19

Hi guys,
thanks for your help, it has gotten me a lot further down the road =) It helps to know that I don't have to re-do all my simulations.
I haven't tried the rotor-stator experiment yet, but I'll let you know if I make any progress with its setup.

crusen mind · July 27, 2016, 05:18

I am getting a error in my simulation. I am getting following warning message if use Decompose par dict

Quote:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 4.0-665f1db4c1f1
Exec : decomposePar
Date : Jul 27 2016
Time : 11:14:23
Host : "velan-OptiPlex-9020"
PID : 3882
Case : /home/velan/prop
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Decomposing mesh region0

Create mesh

Calculating distribution of cells
Selecting decompositionMethod hierarchical

Finished decomposition in 0.1 s

Calculating original mesh data

Distributing cells to processors

Distributing faces to processors

Distributing points to processors

Constructing processor meshes

Processor 0
Number of cells = 56362
Number of faces shared with processor 1 = 1823
Number of processor patches = 1
Number of processor faces = 1823
Number of boundary faces = 6561

Processor 1
Number of cells = 56362
Number of faces shared with processor 0 = 1823
Number of faces shared with processor 2 = 6545
Number of processor patches = 2
Number of processor faces = 8368
Number of boundary faces = 6410

Processor 2
Number of cells = 56362
Number of faces shared with processor 1 = 6545
Number of faces shared with processor 3 = 1306
Number of processor patches = 2
Number of processor faces = 7851
Number of boundary faces = 6429

Processor 3
Number of cells = 56363
Number of faces shared with processor 2 = 1306
Number of processor patches = 1
Number of processor faces = 1306
Number of boundary faces = 6664

Number of processor faces = 9674
Max number of cells = 56363 (0.00133068% above average 56362.2)
Max number of processor patches = 2 (33.3333% above average 1.5)
Max number of faces between processors = 8368 (72.9998% above average 4837)

Time = 0
--> FOAM Warning :
From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam:

olyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 448
Patch default_exterior specifies a group wall which is also a patch name. This might give problems later on.
--> FOAM Warning :
From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam:

olyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 448
Patch propeller specifies a group wall which is also a patch name. This might give problems later on.
--> FOAM Warning :
From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam:

olyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 448
Patch wall specifies a group wall which is also a patch name. This might give problems later on.
--> FOAM Warning :
From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam:

olyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 448
Patch inlet specifies a group wall which is also a patch name. This might give problems later on.

Processor 0: field transfer
Processor 1: field transfer
Processor 2: field transfer
Processor 3: field transfer

End

crusen mind · July 27, 2016, 05:20

When I run my pimpleDYMFoam

Quote:

QUOTE]/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 4.0-665f1db4c1f1
Exec : pimpleDyMFoam
Date : Jul 27 2016
Time : 11:15:09
Host : "velan-OptiPlex-9020"
PID : 3899
Case : /home/velan/prop
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Selecting dynamicFvMesh solidBodyMotionFvMesh
Selecting solid-body motion function rotatingMotion
Applying solid body motion to cellZone innersmallcyclinder

PIMPLE: no residual control data found. Calculations will employ 2 corrector loops

Reading field p

--> FOAM Warning :
From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam:

olyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 448
Patch default_exterior specifies a group wall which is also a patch name. This might give problems later on.
--> FOAM Warning :
From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam:

olyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 448
Patch propeller specifies a group wall which is also a patch name. This might give problems later on.
--> FOAM Warning :
From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam:

olyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 448
Patch wall specifies a group wall which is also a patch name. This might give problems later on.
--> FOAM Warning :
From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam:

olyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 448
Patch inlet specifies a group wall which is also a patch name. This might give problems later on.
Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
C3 -0.33;
sigmak 1;
sigmaEps 1.3;
}

No MRF models present

Reading/calculating face velocity Uf

No finite volume options present

Courant Number mean: 0.00238054 max: 0.721818
Reading surface description:
zNormal
isoQ
propeller

forces forces:
Not including porosity effects

Starting time loop

Courant Number mean: 0.00238054 max: 0.721818
deltaT = 0.001
Time = 0.001

PIMPLE: iteration 1
smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.0988632, No Iterations 91
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.0852269, No Iterations 6
smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.0991305, No Iterations 82
GAMG: Solving for p, Initial residual = 1, Final residual = 0.00407502, No Iterations 7
time step continuity errors : sum local = 1.99384e-05, global = -4.21686e-06, cumulative = -4.21686e-06
PIMPLE: iteration 2
smoothSolver: Solving for Ux, Initial residual = 0.294163, Final residual = 9.97563e-07, No Iterations 665
smoothSolver: Solving for Uy, Initial residual = 0.684399, Final residual = 9.99339e-07, No Iterations 617
smoothSolver: Solving for Uz, Initial residual = 0.288704, Final residual = 9.99241e-07, No Iterations 448
GAMG: Solving for p, Initial residual = 0.31277, Final residual = 5.27961e-07, No Iterations 13
time step continuity errors : sum local = 4.32085e-07, global = 8.9708e-08, cumulative = -4.12715e-06
smoothSolver: Solving for epsilon, Initial residual = 1, Final residual = 9.91358e-07, No Iterations 995
smoothSolver: Solving for k, Initial residual = 1, Final residual = 9.72718e-07, No Iterations 104
ExecutionTime = 26.46 s ClockTime = 26 s

functionObjects::Q Q writing field: Q
forces forces write:
sum of forces:
pressure : (-17.27 -3469.95 4.0674)
viscous : (0.00436087 -1.70123 0.0141931)
porous : (0 0 0)
sum of moments:
pressure : (8.68466 67.6964 1.10294)
viscous : (0.00172311 0.0453866 0.000329318)
porous : (0 0 0)

Courant Number mean: 1.47354 max: 2286.41
deltaT = 8.74126e-07
Time = 0.00100087

PIMPLE: iteration 1
smoothSolver: Solving for Ux, Initial residual = 0.250646, Final residual = 0.0156788, No Iterations 1
smoothSolver: Solving for Uy, Initial residual = 0.110441, Final residual = 0.00607957, No Iterations 1
smoothSolver: Solving for Uz, Initial residual = 0.233234, Final residual = 0.010357, No Iterations 1
GAMG: Solving for p, Initial residual = 0.970302, Final residual = 0.00542451, No Iterations 2
time step continuity errors : sum local = 2.75984e-06, global = -6.24351e-07, cumulative = -4.7515e-06
PIMPLE: iteration 2
smoothSolver: Solving for Ux, Initial residual = 0.103294, Final residual = 2.44492e-06, No Iterations 1000
smoothSolver: Solving for Uy, Initial residual = 0.0536587, Final residual = 2.27732e-06, No Iterations 1000
smoothSolver: Solving for Uz, Initial residual = 0.0845601, Final residual = 9.93136e-07, No Iterations 876
GAMG: Solving for p, Initial residual = 0.20666, Final residual = 8.5285e-07, No Iterations 13
time step continuity errors : sum local = 1.06544e-09, global = 2.3016e-10, cumulative = -4.75127e-06
smoothSolver: Solving for epsilon, Initial residual = 0.912522, Final residual = 9.46356e-06, No Iterations 1000
smoothSolver: Solving for k, Initial residual = 0.969117, Final residual = 9.93881e-07, No Iterations 760
ExecutionTime = 68.53 s ClockTime = 68 s

forces forces write:
sum of forces:
pressure : (-119217 7.43074e+06 -92324.3)
viscous : (-179.611 2492.3 -44.8134)
porous : (0 0 0)
sum of moments:
pressure : (-32375 -177431 -11144.1)
viscous : (-32.7615 -64.753 -6.1826)
porous : (0 0 0)

Courant Number mean: 0.0019634 max: 99.2883
deltaT = 1.76076e-08
Time = 0.00100089

PIMPLE: iteration 1
smoothSolver: Solving for Ux, Initial residual = 0.869036, Final residual = 0.0685572, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 0.776813, Final residual = 0.0615109, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 0.864936, Final residual = 0.036364, No Iterations 2
GAMG: Solving for p, Initial residual = 0.705699, Final residual = 0.00609574, No Iterations 3
time step continuity errors : sum local = 6.39503e-08, global = 4.16889e-09, cumulative = -4.74711e-06
PIMPLE: iteration 2
smoothSolver: Solving for Ux, Initial residual = 0.504846, Final residual = 0.181382, No Iterations 1000
smoothSolver: Solving for Uy, Initial residual = 0.552374, Final residual = 0.392143, No Iterations 1000
smoothSolver: Solving for Uz, Initial residual = 0.393844, Final residual = 0.0352148, No Iterations 1000
GAMG: Solving for p, Initial residual = 0.0950948, Final residual = 5.47965e-07, No Iterations 14
time step continuity errors : sum local = 8.72584e-09, global = 7.07557e-10, cumulative = -4.7464e-06
smoothSolver: Solving for epsilon, Initial residual = 0.999949, Final residual = 0.705503, No Iterations 1000
smoothSolver: Solving for k, Initial residual = 0.900049, Final residual = 0.207524, No Iterations 1000
ExecutionTime = 109.51 s ClockTime = 109 s

forces forces write:
sum of forces:
pressure : (2.58549e+12 -2.55467e+13 5.07164e+11)
viscous : (1.07972e+08 -5.94208e+08 6.42849e+06)
porous : (0 0 0)
sum of moments:
pressure : (4.72569e+11 6.13075e+11 9.49853e+10)
viscous : (1.60875e+07 1.81943e+07 2.15182e+06)
porous : (0 0 0)

Courant Number mean: 0.0195984 max: 453.402
deltaT = 7.76688e-11
Time = 0.00100089

PIMPLE: iteration 1
smoothSolver: Solving for Ux, Initial residual = 0.873339, Final residual = 0.063251, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 0.863947, Final residual = 0.050543, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 0.8848, Final residual = 0.0354364, No Iterations 2
GAMG: Solving for p, Initial residual = 0.0721614, Final residual = 0.000457538, No Iterations 3
time step continuity errors : sum local = 1.08142e-07, global = 5.28154e-12, cumulative = -4.74639e-06
PIMPLE: iteration 2
smoothSolver: Solving for Ux, Initial residual = 0.509627, Final residual = 0.24077, No Iterations 1000
smoothSolver: Solving for Uy, Initial residual = 0.628854, Final residual = 0.545989, No Iterations 1000
smoothSolver: Solving for Uz, Initial residual = 0.404636, Final residual = 0.0438719, No Iterations 1000
GAMG: Solving for p, Initial residual = 0.000318388, Final residual = 8.43188e-07, No Iterations 10
time step continuity errors : sum local = 6.05119e-06, global = 3.83784e-12, cumulative = -4.74639e-06
smoothSolver: Solving for epsilon, Initial residual = 0.970056, Final residual = 0.0265452, No Iterations 1000
smoothSolver: Solving for k, Initial residual = 0.986158, Final residual = 0.98383, No Iterations 1000
ExecutionTime = 150.09 s ClockTime = 150 s

forces forces write:
sum of forces:
pressure : (-2.58759e+20 1.33492e+21 -3.47276e+19)
viscous : (-1.95552e+13 7.81419e+13 -4.08411e+12)
porous : (0 0 0)
sum of moments:
pressure : (-4.73542e+19 -3.13867e+19 -7.88186e+18)
viscous : (-2.81138e+12 -1.83021e+12 -1.40974e+11)
porous : (0 0 0)

Courant Number mean: 0.0302344 max: 415.474
deltaT = 3.73881e-13
Time = 0.00100089

PIMPLE: iteration 1
smoothSolver: Solving for Ux, Initial residual = 0.876678, Final residual = 0.0509362, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 0.868974, Final residual = 0.0449426, No Iterations 2
smoothSolver: Solving for Uz, Initial residual = 0.885472, Final residual = 0.034666, No Iterations 2
GAMG: Solving for p, Initial residual = 0.000142708, Final residual = 9.27656e-06, No Iterations 1
time step continuity errors : sum local = 2.02959e-06, global = 2.41601e-14, cumulative = -4.74639e-06
PIMPLE: iteration 2
smoothSolver: Solving for Ux, Initial residual = 0.537781, Final residual = 0.191154, No Iterations 1000
smoothSolver: Solving for Uy, Initial residual = 0.636365, Final residual = 0.483579, No Iterations 1000
smoothSolver: Solving for Uz, Initial residual = 0.488395, Final residual = 0.02293, No Iterations 1000
GAMG: Solving for p, Initial residual = 1.5044e-06, Final residual = 6.3472e-07, No Iterations 1
time step continuity errors : sum local = 0.000927275, global = 2.95669e-14, cumulative = -4.74639e-06
smoothSolver: Solving for epsilon, Initial residual = 0.138125, Final residual = 0.000355419, No Iterations 1000
smoothSolver: Solving for k, Initial residual = 0.000102969, Final residual = 0.000102375, No Iterations 1000
bounding k, min: 3.23491e-22 max: 5.08122e+23 average: 3.73543e+22
ExecutionTime = 190.44 s ClockTime = 190 s

forces forces write:
sum of forces:
pressure : (3.45618e+27 -1.54611e+28 2.804e+26)
viscous : (3.01901e+17 -1.40668e+18 4.17949e+15)
porous : (0 0 0)
sum of moments:
pressure : (6.72639e+26 2.86854e+26 5.97548e+25)
viscous : (4.93112e+16 2.9574e+16 1.23978e+15)
porous : (0 0 0)

Courant Number mean: 0.022645 max: 659.73
deltaT = 1.13344e-15
Time = 0.00100089

PIMPLE: iteration 1
smoothSolver: Solving for Ux, Initial residual = 0.809177, Final residual = 0.0241364, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 0.833929, Final residual = 0.0569514, No Iterations 1
smoothSolver: Solving for Uz, Initial residual = 0.875089, Final residual = 0.0404306, No Iterations 1
GAMG: Solving for p, Initial residual = 8.14349e-07, Final residual = 8.14349e-07, No Iterations 0
time step continuity errors : sum local = 1.30146e-05, global = 2.81731e-16, cumulative = -4.74639e-06
PIMPLE: iteration 2
smoothSolver: Solving for Ux, Initial residual = 0.920569, Final residual = 5.698e-05, No Iterations 1000
smoothSolver: Solving for Uy, Initial residual = 0.862661, Final residual = 6.39026e-05, No Iterations 1000
smoothSolver: Solving for Uz, Initial residual = 0.859611, Final residual = 9.22457e-05, No Iterations 1000
GAMG: Solving for p, Initial residual = 7.72332e-07, Final residual = 7.72332e-07, No Iterations 0
time step continuity errors : sum local = 1.23431e-05, global = 2.81742e-16, cumulative = -4.74639e-06
smoothSolver: Solving for epsilon, Initial residual = 0.996379, Final residual = 7.80371e-20, No Iterations 1
bounding epsilon, min: -5.30644e+28 max: 7.19695e+32 average: 1.44367e+28

[/QUOTE]

teuk · July 27, 2016, 05:49

Hi crusen mind,

what you get there is just a WARNING not an ERROR statement. It tells you to change your group name in your boundary definition from "wall" to something else because "wall" is allready used by wall-patches. Maybe change it da "WALL" to be sure. But if you're not using the "wall"-group in your field definitions it should not influence your calculations.

BTW: Check your CFL-number...

regards,
teuk

crusen mind · July 27, 2016, 05:55

Quote:

Originally Posted by teuk

Hi crusen mind,

what you get there is just a WARNING not an ERROR statement. It tells you to change your group name in your boundary definition from "wall" to something else because "wall" is allready used by wall-patches. Maybe change it da "WALL" to be sure. But if you're not using the "wall"-group in your field definitions it should not influence your calculations.

BTW: Check your CFL-number...

regards,
teuk

thanks for the reply
After sew iterations my simulation stops displaying this
#0 Foam::error:: printStack(Foam::Ostream&) at ??:?
#1 Foam:: sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam:

ICPreconditioner::calcReciprocalD(Foam::Fie ld<double>&, Foam::lduMatrix const&) at ??:?
#4 Foam:

ICSmoother:

ICSmoother(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) at ??:?
#5 Foam:

ICGaussSeidelSmoother:

ICGaussSeidelSmooth er(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) at ??:?
#6 Foam::lduMatrix::smoother::addsymMatrixConstructor ToTable<Foam:

ICGaussSeidelSmoother>::New(Foam::w ord const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&) at ??:?
#7 Foam::lduMatrix::smoother::New(Foam::word const&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::dictionary const&) at ??:?
#8 Foam::GAMGSolver::initVcycle(Foam::PtrList<Foam::F ield<double> >&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::lduMatrix::smoother>&, Foam::Field<double>&, Foam::Field<double>&) const at ??:?
#9 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#10 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) at ??:?
#11 Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
#12 ? at ??:?
#13 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#14 ? at ??:?
Floating point exception (core dumped)

teuk · July 27, 2016, 06:38

Hi crusen mind,

did you check your CFL- or Courant-number?

regards,
teuk

crusen mind · July 29, 2016, 00:19

hi teuk
I have reduced my time step. But I am not getting any solution I will post my check mesh, controldict, Fv solutions
checkMesh File

PHP Code:


			
Build  : 4.0-665f1db4c1f1

Exec   : checkMesh

Date   : Jul 28 2016

Time   : 11:36:29

Host   : "velan-OptiPlex-9020"

PID    : 3301

Case   : /home/velan/prop

nProcs : 1

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster

allowSystemOperations : Allowing user-supplied system call operations



// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time



Create polyMesh for time = 0



Time = 0



Mesh stats

    points:           43715

    faces:            463930

    internal faces:   437866

    cells:            225449

    faces per cell:   4

    boundary patches: 5

    point zones:      0

    face zones:       0

    cell zones:       2



Overall number of cells of each type:

    hexahedra:     0

    prisms:        0

    wedges:        0

    pyramids:      0

    tet wedges:    0

    tetrahedra:    225449

    polyhedra:     0



Checking topology...

    Boundary definition OK.

    Cell to face addressing OK.

    Point usage OK.

    Upper triangular ordering OK.

    Face vertices OK.

   *Number of regions: 2

    The mesh has multiple regions which are not connected by any face.

  <<Writing region information to "0/cellToRegion"

  <<Writing region 0 with 94543 cells to cellSet region0

  <<Writing region 1 with 130906 cells to cellSet region1



Checking patch topology for multiply connected surfaces...

    Patch               Faces    Points   Surface topology                  

    default_exterior    4376     2192     ok (closed singly connected)      

    propeller           6596     3298     ok (closed singly connected)      

    wall                11740    5964     ok (non-closed singly connected)  

    outlet              1672     884      ok (non-closed singly connected)  

    inlet               1680     888      ok (non-closed singly connected)  



Checking geometry...

    Overall domain bounding box (-0.3 -0.5 -0.3) (0.3 0.55 0.299999)

    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)

    Mesh has 3 solution (non-empty) directions (1 1 1)

    Boundary openness (1.79007e-16 1.7051e-16 1.35631e-15) OK.

    Max cell openness = 3.87662e-16 OK.

    Max aspect ratio = 10.1853 OK.

    Minimum face area = 6.27344e-08. Maximum face area = 0.000731502.  Face area magnitudes OK.

    Min volume = 1.54049e-11. Max volume = 6.02718e-06.  Total volume = 0.296711.  Cell volumes OK.

    Mesh non-orthogonality Max: 60.8432 average: 18.7601

    Non-orthogonality check OK.

    Face pyramids OK.

    Max skewness = 1.11566 OK.

    Coupled point location match (average 0) OK.



Mesh OK.



End





control dict file

PHP Code:


			
/application     pimpleDyMFoam;



startFrom       startTime;



startTime       0;



stopAt          endTime;



endTime         0.1;



deltaT          0.000001;

writeControl    adjustableRunTime;

writeInterval   0.001;



////- For testing with moveDynamicMesh

//deltaT          0.01;

//writeControl    timeStep;

//writeInterval   1;



purgeWrite      0;



writeFormat     binary;



writePrecision  6;



writeCompression off;



timeFormat      general;



timePrecision   6;



runTimeModifiable true;



adjustTimeStep  yes;



maxCo           2;



functions

{

    #includeFunc Q

    #include "surfaces"

    #include "forces"

}

my Fv solution file

PHP Code:


			
solvers

{

    pcorr

    {

        solver          GAMG;

        tolerance       1e-2;

        relTol          0;

        smoother        DICGaussSeidel;

        cacheAgglomeration no;

        maxIter         50;

    }



    p

    {

        $pcorr;

        tolerance       1e-5;

        relTol          0.01;

    }



    pFinal

    {

        $p;

        tolerance       1e-6;

        relTol          0;

    }



    "(U|k|epsilon)"

    {

        solver          smoothSolver;

        smoother        symGaussSeidel;

        tolerance       1e-6;

        relTol          0.1;

    }



    "(U|k|epsilon)Final"

    {

        solver          smoothSolver;

        smoother        symGaussSeidel;

        tolerance       1e-6;

        relTol          0;

    }

}



PIMPLE

{

    correctPhi          no;

    nOuterCorrectors    2;

    nCorrectors         1;

    nNonOrthogonalCorrectors 1;

}



relaxationFactors

{

    "(U|k|epsilon).*"   1;

}



cache

{

    grad(U);

}

teuk · July 29, 2016, 10:50

Hi crusen mind,

if interpret your checkMesh correct you are using a terahedral mesh? I'm only familiar with hexahedral meshes...

But I have some suggestions anyways. Your max nonorthogonality and skewness are pretty high. But maybe that's because of the tetrahedral mesh.

Quote:

runTimeModifiable true;

adjustTimeStep yes;

maxCo 2;

So your max Co number is still 2?

I'm not sure about GAMG for p-fields. The mesh is not "that" big.

Quote:

relaxationFactors
{
"(U|k|epsilon).*" 1;
}

Since your calculations crashes at k calculation you could try lower k and epsilon relaxation.

regards,
teuk

teuk · July 29, 2016, 11:08

Hi crusen mind,

if interpret your checkMesh correct you are using a terahedral mesh? I'm only familiar with hexahedral meshes...

But I have some suggestions anyways. Your max nonorthogonality and skewness are pretty high. But maybe that's because of the tetrahedral mesh.

Quote:

runTimeModifiable true;

adjustTimeStep yes;

maxCo 2;

So your max Co number is still 2?

I'm not sure about GAMG for p-fields. The mesh is not "that" big.

Quote:

relaxationFactors
{
"(U|k|epsilon).*" 1;
}

Since your calculations crashes at k calculation you could try lower k and epsilon relaxation.

regards,
teuk

crusen mind · July 30, 2016, 02:51

Quote:

Originally Posted by teuk

Hi crusen mind,

if interpret your checkMesh correct you are using a terahedral mesh? I'm only familiar with hexahedral meshes...

But I have some suggestions anyways. Your max nonorthogonality and skewness are pretty high. But maybe that's because of the tetrahedral mesh.

So your max Co number is still 2?

I'm not sure about GAMG for p-fields. The mesh is not "that" big.

Since your calculations crashes at k calculation you could try lower k and epsilon relaxation.

regards,
teuk

hi teuk thanks for the reply
so courant number ensures stability of the simulation, so would setting higher max co affect simulation?

I selected fv solution from propeller case pimpleDYM. Is there any thumb rule to select Fv solution based on meshing.

Or simply improving mesh quality with fine meshing, reducing skewness will work?

teuk · July 31, 2016, 20:05

Hi crusen mind,

Quote:

hi teuk thanks for the reply
so courant number ensures stability of the simulation, so would setting higher max co affect simulation?

http://www.cfd-online.com/Wiki/Coura...Lewy_condition

By setting higher CFL-number you will run into different uncoupled solutions on your mesh ...in worst case.

Quote:

I selected fv solution from propeller case pimpleDYM. Is there any thumb rule to select Fv solution based on meshing.

Not really besides nonorthogonal correctors...
And special decomposition in specific cases...

Quote:

Or simply improving mesh quality with fine meshing, reducing skewness will work?

Maybe ...Maybe not...

But improved mesh quality is always favourable

regards,
teuk

June 25, 2016, 09:31	Propeller tutorial with air instead of water	#1
JShnyder New Member Jonathan Join Date: Apr 2016 Posts: 3 Rep Power: 9	Hi everyone, I want to run the propeller tutorial with air. I've read somewhere that with the pimpleDym-solver the only thing to do were to change Code: nu[0 2 -1 0 0 0 0] 1e-5; //the kinematic viscosity of water(1e-6) or air(1e-5) in the transportProperties-file. I can't imagine that's all - wouldn't the simulation lead to different results at different altitudes/air pressures or be influenced by other factors?

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Water diffusion into air	MGabr	CFX	19	September 3, 2023 19:06
compressibleInterFoam case – a flat wall air cavity filling up with water	Zeppo	OpenFOAM Running, Solving & CFD	0	October 3, 2015 10:01
3D multiphase micro model: mixing effect of air and water at the T junction	ehsanfareed	FLUENT	2	March 22, 2015 22:29
Evaporatin water in the air	Morteza	FLUENT	1	August 20, 2008 05:04
VOF-compression of air with rising water	yavuz	FLUENT	0	November 26, 2005 09:00

June 27, 2016, 03:58		#2
SirIsaac90 New Member Justin Wiegmann Join Date: Aug 2015 Posts: 20 Rep Power: 10	Hi JShnyder, That is almost all for incompressible flows. I would also adapt the turbulent dissipation by a factor of 10^(-1), because it depends on viscosity. Gravitation is not considered at all in this case example. Regards JW

June 30, 2016, 02:19		#5
crusen mind Member alex Join Date: Feb 2016 Location: chennai Posts: 48 Rep Power: 10	hi SirIssac I am using ANSA for meshing. The link you posted show how to do rotor and stator mesh in snappy hex mesh. basically I am not able to run my ALL RUN script in simpleFOAM rotor disk tutorial i Will post my log files for rotor disk case log create patch ./Allrun: 81: ./Allrun: createPatch: not found log.simpleFoam /---------------------------------------------------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: v3.0+ \| \| \\ / A nd \| Web: www.OpenFOAM.com \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ Build : v3.0+-e941ee6c15e9 Exec : simpleFoam Date : Jun 27 2016 Time : 15:30:33 Host : "velan-OptiPlex-9020" PID : 3025 Case : /home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 SIMPLE: convergence criteria field U tolerance 0.0001 field p tolerance 0.001 field "(k\|epsilon\|omega)" tolerance 0.001 Reading field p Reading field U Reading/calculating face flux field phi --> FOAM FATAL IO ERROR: Unable to set reference cell for field p Please supply either pRefCell or pRefPoint file: /home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk/system/fvSolution.SIMPLE from line 42 to line 49. From function void Foam::setRefCell(const volScalarField&, const volScalarField&, const Foam::dictionary&, Foam::label&, Foam::scalar&, bool) in file cfdTools/general/findRefCell/findRefCell.C at line 105. FOAM exiting log.snappyHEXMESH /---------------------------------------------------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: v3.0+ \| \| \\ / A nd \| Web: www.OpenFOAM.com \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ Build : v3.0+-e941ee6c15e9 Exec : snappyHexMesh -overwrite Date : Jun 27 2016 Time : 15:30:32 Host : "velan-OptiPlex-9020" PID : 3022 Case : /home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Read mesh in = 0.01 s Overall mesh bounding box : (-1.26 -2.01 -1.26) (1.26 2.01 1.26) Relative tolerance : 1e-06 Absolute matching distance : 5.3722621e-06 Reading refinement surfaces. Read refinement surfaces in = 0.03 s Reading refinement shells. Refinement level 1 for all cells inside fixed.obj Refinement level 4 for all cells inside rotatingZone.obj shellSurfaces : Flipped orientation of surface rotatingZone.obj so point (3.75 6 3.75) is outside. Read refinement shells in = 0.02 s Setting refinement level of surface to be consistent with shells. For geometry fixed.obj detected 0 uncached triangles out of 5012 For geometry rotatingZone.obj detected 0 uncached triangles out of 3964 Checked shell refinement in = 0.05 s Reading features. --> FOAM FATAL IO ERROR: Could not open "/home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk/constant/triSurface/fixed.eMesh" file: /home/velan/OpenFOAM/velan-v3.0+/run/tutorials/incompressible/simpleFoam/rotorDisk/system/snappyHexMeshDict.castellatedMeshControls.features from line 47 to line 47. From function void Foam::refinementFeatures::read(const Foam:bjectRegistry&, const Foam::PtrList<Foam::dictionary>&) in file autoHexMesh/refinementFeatures/refinementFeatures.C at line 97. FOAM exiting log.surfaceFeature EXtract ./Allrun: 81: ./Allrun: surfaceFeatureExtract: not found

July 6, 2016, 04:19		#7
JShnyder New Member Jonathan Join Date: Apr 2016 Posts: 3 Rep Power: 9	Hi guys, thanks for your help, it has gotten me a lot further down the road =) It helps to know that I don't have to re-do all my simulations. I haven't tried the rotor-stator experiment yet, but I'll let you know if I make any progress with its setup.

July 27, 2016, 05:49		#10
teuk New Member Join Date: Oct 2014 Posts: 26 Rep Power: 11	Hi crusen mind, what you get there is just a WARNING not an ERROR statement. It tells you to change your group name in your boundary definition from "wall" to something else because "wall" is allready used by wall-patches. Maybe change it da "WALL" to be sure. But if you're not using the "wall"-group in your field definitions it should not influence your calculations. BTW: Check your CFL-number... regards, teuk

July 27, 2016, 06:38		#12
teuk New Member Join Date: Oct 2014 Posts: 26 Rep Power: 11	Hi crusen mind, did you check your CFL- or Courant-number? regards, teuk

July 29, 2016, 00:19		#13
crusen mind Member alex Join Date: Feb 2016 Location: chennai Posts: 48 Rep Power: 10	hi teuk I have reduced my time step. But I am not getting any solution I will post my check mesh, controldict, Fv solutions checkMesh File PHP Code: Build : 4.0-665f1db4c1f1 Exec : checkMesh Date : Jul 28 2016 Time : 11:36:29 Host : "velan-OptiPlex-9020" PID : 3301 Case : /home/velan/prop nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Allowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 43715 faces: 463930 internal faces: 437866 cells: 225449 faces per cell: 4 boundary patches: 5 point zones: 0 face zones: 0 cell zones: 2 Overall number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 225449 polyhedra: 0 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 2 The mesh has multiple regions which are not connected by any face. <<Writing region information to "0/cellToRegion" <<Writing region 0 with 94543 cells to cellSet region0 <<Writing region 1 with 130906 cells to cellSet region1 Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology default_exterior 4376 2192 ok (closed singly connected) propeller 6596 3298 ok (closed singly connected) wall 11740 5964 ok (non-closed singly connected) outlet 1672 884 ok (non-closed singly connected) inlet 1680 888 ok (non-closed singly connected) Checking geometry... Overall domain bounding box (-0.3 -0.5 -0.3) (0.3 0.55 0.299999) Mesh has 3 geometric (non-empty/wedge) directions (1 1 1) Mesh has 3 solution (non-empty) directions (1 1 1) Boundary openness (1.79007e-16 1.7051e-16 1.35631e-15) OK. Max cell openness = 3.87662e-16 OK. Max aspect ratio = 10.1853 OK. Minimum face area = 6.27344e-08. Maximum face area = 0.000731502. Face area magnitudes OK. Min volume = 1.54049e-11. Max volume = 6.02718e-06. Total volume = 0.296711. Cell volumes OK. Mesh non-orthogonality Max: 60.8432 average: 18.7601 Non-orthogonality check OK. Face pyramids OK. Max skewness = 1.11566 OK. Coupled point location match (average 0) OK. Mesh OK. End control dict file PHP Code: /application pimpleDyMFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 0.1; deltaT 0.000001; writeControl adjustableRunTime; writeInterval 0.001; ////- For testing with moveDynamicMesh //deltaT 0.01; //writeControl timeStep; //writeInterval 1; purgeWrite 0; writeFormat binary; writePrecision 6; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; adjustTimeStep yes; maxCo 2; functions { #includeFunc Q #include "surfaces" #include "forces" } my Fv solution file PHP Code: solvers { pcorr { solver GAMG; tolerance 1e-2; relTol 0; smoother DICGaussSeidel; cacheAgglomeration no; maxIter 50; } p { $pcorr; tolerance 1e-5; relTol 0.01; } pFinal { $p; tolerance 1e-6; relTol 0; } "(U\|k\|epsilon)" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e-6; relTol 0.1; } "(U\|k\|epsilon)Final" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e-6; relTol 0; } } PIMPLE { correctPhi no; nOuterCorrectors 2; nCorrectors 1; nNonOrthogonalCorrectors 1; } relaxationFactors { "(U\|k\|epsilon)." 1; } cache { grad(U); }