CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Propeller tutorial with air instead of water

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 25, 2016, 10:31
Default Propeller tutorial with air instead of water
  #1
New Member
 
Jonathan
Join Date: Apr 2016
Posts: 3
Rep Power: 8
JShnyder is on a distinguished road
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?
JShnyder is offline   Reply With Quote

Old   June 27, 2016, 04:58
Post
  #2
New Member
 
Justin Wiegmann
Join Date: Aug 2015
Posts: 20
Rep Power: 9
SirIsaac90 is on a distinguished road
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
SirIsaac90 is offline   Reply With Quote

Old   June 28, 2016, 09:10
Default
  #3
Member
 
alex
Join Date: Feb 2016
Location: chennai
Posts: 48
Rep Power: 8
crusen mind is on a distinguished road
Quote:
Originally Posted by JShnyder View Post
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
crusen mind is offline   Reply With Quote

Old   June 29, 2016, 04:04
Default
  #4
New Member
 
Justin Wiegmann
Join Date: Aug 2015
Posts: 20
Rep Power: 9
SirIsaac90 is on a distinguished road
Quote:
Originally Posted by crusen mind View Post
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
SirIsaac90 is offline   Reply With Quote

Old   June 30, 2016, 03:19
Default
  #5
Member
 
alex
Join Date: Feb 2016
Location: chennai
Posts: 48
Rep Power: 8
crusen mind is on a distinguished road
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
crusen mind is offline   Reply With Quote

Old   July 6, 2016, 05:05
Default
  #6
New Member
 
Justin Wiegmann
Join Date: Aug 2015
Posts: 20
Rep Power: 9
SirIsaac90 is on a distinguished road
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
SirIsaac90 is offline   Reply With Quote

Old   July 6, 2016, 05:19
Default
  #7
New Member
 
Jonathan
Join Date: Apr 2016
Posts: 3
Rep Power: 8
JShnyder is on a distinguished road
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.
JShnyder is offline   Reply With Quote

Old   July 27, 2016, 06:18
Default
  #8
Member
 
alex
Join Date: Feb 2016
Location: chennai
Posts: 48
Rep Power: 8
crusen mind is on a distinguished road
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 is offline   Reply With Quote

Old   July 27, 2016, 06:20
Default
  #9
Member
 
alex
Join Date: Feb 2016
Location: chennai
Posts: 48
Rep Power: 8
crusen mind is on a distinguished road
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]
crusen mind is offline   Reply With Quote

Old   July 27, 2016, 06:49
Default
  #10
New Member
 
Join Date: Oct 2014
Posts: 26
Rep Power: 10
teuk is on a distinguished road
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
teuk is offline   Reply With Quote

Old   July 27, 2016, 06:55
Default
  #11
Member
 
alex
Join Date: Feb 2016
Location: chennai
Posts: 48
Rep Power: 8
crusen mind is on a distinguished road
Quote:
Originally Posted by teuk View Post
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)
crusen mind is offline   Reply With Quote

Old   July 27, 2016, 07:38
Default
  #12
New Member
 
Join Date: Oct 2014
Posts: 26
Rep Power: 10
teuk is on a distinguished road
Hi crusen mind,

did you check your CFL- or Courant-number?


regards,
teuk
teuk is offline   Reply With Quote

Old   July 29, 2016, 01:19
Default
  #13
Member
 
alex
Join Date: Feb 2016
Location: chennai
Posts: 48
Rep Power: 8
crusen mind is on a distinguished road
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 regions2
    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/wedgedirections (1 1 1)
    
Mesh has 3 solution (non-empty) directions (1 1 1)
    
Boundary openness (1.79007e-16 1.7051e-16 1.35631e-15OK.
    
Max cell openness 3.87662e-16 OK.
    
Max aspect ratio 10.1853 OK.
    
Minimum face area 6.27344e-08Maximum face area 0.000731502.  Face area magnitudes OK.
    
Min volume 1.54049e-11Max volume 6.02718e-06.  Total volume 0.296711.  Cell volumes OK.
    
Mesh non-orthogonality Max60.8432 average18.7601
    Non
-orthogonality check OK.
    
Face pyramids OK.
    
Max skewness 1.11566 OK.
    
Coupled point location match (average 0OK.

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);

crusen mind is offline   Reply With Quote

Old   July 29, 2016, 11:50
Default
  #14
New Member
 
Join Date: Oct 2014
Posts: 26
Rep Power: 10
teuk is on a distinguished road
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 is offline   Reply With Quote

Old   July 29, 2016, 12:08
Default
  #15
New Member
 
Join Date: Oct 2014
Posts: 26
Rep Power: 10
teuk is on a distinguished road
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 is offline   Reply With Quote

Old   July 30, 2016, 03:51
Default
  #16
Member
 
alex
Join Date: Feb 2016
Location: chennai
Posts: 48
Rep Power: 8
crusen mind is on a distinguished road
Quote:
Originally Posted by teuk View Post
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?
crusen mind is offline   Reply With Quote

Old   July 31, 2016, 21:05
Default
  #17
New Member
 
Join Date: Oct 2014
Posts: 26
Rep Power: 10
teuk is on a distinguished road
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
teuk is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Water diffusion into air MGabr CFX 16 November 20, 2020 02:35
compressibleInterFoam case a flat wall air cavity filling up with water Zeppo OpenFOAM Running, Solving & CFD 0 October 3, 2015 11:01
3D multiphase micro model: mixing effect of air and water at the T junction ehsanfareed FLUENT 2 March 22, 2015 23:29
Evaporatin water in the air Morteza FLUENT 1 August 20, 2008 06:04
VOF-compression of air with rising water yavuz FLUENT 0 November 26, 2005 10:00


All times are GMT -4. The time now is 10:27.