[rvilum]

Hi,

Iam trying to run a simulation using PimpleDyMFoam. It is a porppeller with AMI method. I run the calculation, but when it achieve 0.0125s, it automatically stops, showing the next message:

Courant Number mean: 0.00302633 max: 9.72945
deltaT = 3.57143e-05
Time = 0.00125

AMI: Creating addressing and weights between 8127 source faces and 7269 target faces
AMI: Patch source sum(weights) min/max/average = 0.51174, 1.52396, 0.999245
AMI: Patch target sum(weights) min/max/average = 0, 1.6436, 0.99057
PIMPLE: iteration 1
smoothSolver: Solving for Ux, Initial residual = 0.000391146, Final residual = 1.12138e-07, No Iterations 1
smoothSolver: Solving for Uy, Initial residual = 0.000303682, Final residual = 1.33307e-08, No Iterations 1
smoothSolver: Solving for Uz, Initial residual = 0.00382204, Final residual = 6.69954e-07, No Iterations 1
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) at ??:?
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:?
#5 ? at ??:?
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7 ? at ??:?
Excepción de coma flotante (`core' generado)

Somebody knows what is the problem?

Thanks a lot.

[piu58]

>

Courant Number mean: 0.00302633 max: 9.72945

It may be that the Co number ist too large, even for pimple. My first try were to reduce it by controlDict.maxCo.

[JeanDidier]

AMI: Creating addressing and weights between 8127 source faces and 7269 target faces
AMI: Patch source sum(weights) min/max/average = 0.51174, 1.52396, 0.999245
AMI: Patch target sum(weights) min/max/average = 0, 1.6436, 0.99057

The problem comes from your mesh. The checkMesh might be OK but that's not OK to use it with pimpleDyMFoam.
Check the shape of your AMI cylinder, you should have a perfect round cylinder to use pimpleDyMFoam else it will crash because of some discontinuity between the moving mesh and the non-moving mesh. In a normal case, you should at least have 0.99 or 0.98 for minimum weight when running a pimpleDyMFoam simulation.
Here is a link of a ppt about AMI : https://fr.slideshare.net/fumiyanoza...using-openfoam
Go directly at slide 84, it will teach you what those numbers mean.

[rvilum]

Originally Posted by JeanDidier

The problem comes from your mesh. The checkMesh might be OK but that's not OK to use it with pimpleDyMFoam.
Check the shape of your AMI cylinder, you should have a perfect round cylinder to use pimpleDyMFoam else it will crash because of some discontinuity between the moving mesh and the non-moving mesh. In a normal case, you should at least have 0.99 or 0.98 for minimum weight when running a pimpleDyMFoam simulation.
Here is a link of a ppt about AMI : https://fr.slideshare.net/fumiyanoza...using-openfoam
Go directly at slide 84, it will teach you what those numbers mean.

Hi!

Thanks a lot for your help. Definitely. it is the problem. BUt, do you know how can I solve it?

[JeanDidier]

I can guide you to get something better but first :

1) What does your checkMesh indicate ? (send a copy/paste)

2) Did you use the propeller tutorial for your case ? (located in the openfoam files tutorials/incompressible/pimpleDyMFoam/propeller) It gives you a lot of information on how to set AMI.

3) If yes, you might have use something like InnerCylinder and InnerCylinderSmall like in the tutorial. Are you sure about the definition of your InnerCylinderSmall (AMI) ? It might be the problem for this message :

AMI: Creating addressing and weights between 8127 source faces and 7269 target faces

An example from my case :

name InnerCylinderSmall;
type cellSet;
action new;
source cylinderToCell;
sourceInfo
{
p1 (0 0 22.5);
p2 (0 0 -2.5);
radius 3.5;
}

4) What does your AMI patch look like ? It should be a perfectly round cylinder like AMI_1 and AMI_2 attached, and i guess that yours look like AMI_3.

[rvilum]

Originally Posted by JeanDidier

I can guide you to get something better but first :

1) What does your checkMesh indicate ? (send a copy/paste)

2) Did you use the propeller tutorial for your case ? (located in the openfoam files tutorials/incompressible/pimpleDyMFoam/propeller) It gives you a lot of information on how to set AMI.

3) If yes, you might have use something like InnerCylinder and InnerCylinderSmall like in the tutorial. Are you sure about the definition of your InnerCylinderSmall (AMI) ? It might be the problem for this message :

An example from my case :

name InnerCylinderSmall;
type cellSet;
action new;
source cylinderToCell;
sourceInfo
{
p1 (0 0 22.5);
p2 (0 0 -2.5);
radius 3.5;
}

4) What does your AMI patch look like ? It should be a perfectly round cylinder like AMI_1 and AMI_2 attached, and i guess that yours look like AMI_3.

Thanks a lot again. I am going to do it exactly as in propeller tutorial. I will explain you my results later

[rvilum]

[rvilum]

Originally Posted by JeanDidier

I can guide you to get something better but first :

1) What does your checkMesh indicate ? (send a copy/paste)

2) Did you use the propeller tutorial for your case ? (located in the openfoam files tutorials/incompressible/pimpleDyMFoam/propeller) It gives you a lot of information on how to set AMI.

3) If yes, you might have use something like InnerCylinder and InnerCylinderSmall like in the tutorial. Are you sure about the definition of your InnerCylinderSmall (AMI) ? It might be the problem for this message :

An example from my case :

name InnerCylinderSmall;
type cellSet;
action new;
source cylinderToCell;
sourceInfo
{
p1 (0 0 22.5);
p2 (0 0 -2.5);
radius 3.5;
}

4) What does your AMI patch look like ? It should be a perfectly round cylinder like AMI_1 and AMI_2 attached, and i guess that yours look like AMI_3.

My checkMesh



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

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 3371504
faces: 9639571
internal faces: 9441899
cells: 3136719
faces per cell: 6.08326
boundary patches: 6
point zones: 0
face zones: 1
cell zones: 1

Overall number of cells of each type:
hexahedra: 3018901
prisms: 12794
wedges: 0
pyramids: 0
tet wedges: 286
tetrahedra: 0
polyhedra: 104738
Breakdown of polyhedra by number of faces:
faces number of cells
4 1696
5 3125
6 22125
7 414
8 243
9 63244
10 81
11 95
12 11469
13 7
14 18
15 2015
16 1
17 4
18 201

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 2639593 cells to cellSet region0
<<Writing region 1 with 497126 cells to cellSet region1

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
helice 44564 48802 ok (closed singly connected)
fuera 9682 9902 ok (non-closed singly connected)
AMI1 68725 69107 ok (closed singly connected)
AMI2 69326 69574 ok (closed singly connected)
inlet 2700 2772 ok (non-closed singly connected)
outlet 2675 2753 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-0.699718 -1.50005 -0.700285) (0.700285 0.700045 0.700282)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
Boundary openness (-1.15377e-18 6.741e-16 8.13694e-17) OK.
Max cell openness = 3.95941e-16 OK.
Max aspect ratio = 27.5449 OK.
Minimum face area = 1.97898e-09. Maximum face area = 0.00133388. Face area magnitudes OK.
Min volume = 9.17722e-13. Max volume = 2.89277e-05. Total volume = 3.38425. Cell volumes OK.
Mesh non-orthogonality Max: 64.9964 average: 5.52116
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 3.99985 OK.
Coupled point location match (average 0) OK.

Mesh OK.

End

IN the previous message you can see some pictures of the mesh. I still have the same problem:

Create time

Create mesh for time = 0

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

PIMPLE: Operating solver in PISO mode

Reading field p

AMI: Creating addressing and weights between 68725 source faces and 69326 target faces
AMI: Patch source sum(weights) min/max/average = 0.734303, 1.83632, 1.0016
AMI: Patch target sum(weights) min/max/average = 0.0681461, 1.17642, 0.999495
Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
alphaK1 0.85;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.856;
gamma1 0.555556;
gamma2 0.44;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
b1 1;
c1 10;
F3 false;
}

No MRF models present

Reading/calculating face velocity Uf

No finite volume options present

Courant Number mean: 0.0113655 max: 0.922332
forces forces:
Not including porosity effects

Starting time loop

Courant Number mean: 0.0113655 max: 0.922332
deltaT = 0.012
Time = 0.012

AMI: Creating addressing and weights between 68725 source faces and 69326 target faces
AMI: Patch source sum(weights) min/max/average = 4.32027e-05, 2.08694, 0.995326
AMI: Patch target sum(weights) min/max/average = 0, 3.0766, 0.989366
PIMPLE: iteration 1
smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.399665, No Iterations 6
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.38192, No Iterations 15
smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.399895, No Iterations 112
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) at ??:?
#4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:?
#5 ? at ??:?
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7 ? at ??:?

[piu58]

checkMesh says:

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

This is: You made several regions and forgot to couple them. This leads to a geometry where the flow cannot move between the blocks. Usual that is be handled by

mergePatchPairs();

as last line in the blockMeshDict.

[JeanDidier]

Well, you still have some AMI weights trouble, so my advices are :

1) You should check your "createAMIFaces.topoSetDict" file, you might have not correctly define your AMI. You should have the same number of faces at the end.

AMI: Creating addressing and weights between 68725 source faces and 69326 target faces

2) If it's still not working, you should try with a coarser mesh. Maybe with 1.5 or 2 millions cells instead of 3 millions.

[rvilum]

Originally Posted by JeanDidier

Well, you still have some AMI weights trouble, so my advices are :

1) You should check your "createAMIFaces.topoSetDict" file, you might have not correctly define your AMI. You should have the same number of faces at the end.


2) If it's still not working, you should try with a coarser mesh. Maybe with 1.5 or 2 millions cells instead of 3 millions.

I finally found the problem. My propeller was going trought the rotor. Very stupid mistake. But thank you all for your help. I am here if you have any doubt or need any help.

[rvilum]

The problem in the attachment

[hoemmaria]

Hi Rvilum!

I am quite new to OpenFOAM and I aim to simulate a specific wind turbine in a specific wind tunnel for my master thesis.

First, I was wondering how you changed the design of the blades in the tutorials/Incompressible/pimpleDyMFoam/propeller case. Did you create a CAD model using another program? What commands do you use to include it?

Secondly, do you think it will be hard to make the stator a rectangle instead of a cylinder to simulate the wind tunnel? I am thinking maybe the meshing will be hard?

Kind regards,
Maria Hoem

[rvilum]

First, I was wondering how you changed the design of the blades in the tutorials/Incompressible/pimpleDyMFoam/propeller case. Did you create a CAD model using another program? What commands do you use to include it?

You just have to create another geometry (I used catia), after that, save it as a .stl, and the save it in /constant/trisurface, overwriting the other geometry.

Secondly, do you think it will be hard to make the stator a rectangle instead of a cylinder to simulate the wind tunnel? I am thinking maybe the meshing will be hard?


No, not at all. Actually, I think it would be easier. It really does not matter (at least not too much), the mesh of the quality in the borders of the volume. But it is better if you mesh it with good quality, of course.

[hoemmaria]

Thank you for your answer, Juan.

I have not yet started to implement the blade desing, because I need to understand how the dynamic mesh works. So I am looking into the mixerVesselAMI2D tutorial. I want to do some of the same changes here - add a channel outside the mixer vessel. But I am having some troubles.

If you would be so kind, would you look into my thread and see if you understand what I am doing wrong?

Change the mesh in mixerVesselAMI2D tutorial

Kind regards,
Maria

[hoemmaria]

Hey!

I was wondering if anyone knew how to make the propeller tutorial work as a turbine? I want to extract kinetic energy from the flow instead of adding kinetic energy.

Kind regards,
Maria