[arvindpj]

I am trying to simulate a blower fan assly. I am trying to solve for the mass flow driven by the blower, by imposing the rpm.

The mesh for the stator and rotor were separately created using cfMesh. The individual cellSets for rotor and stator regions were identified.

Then the two regions were merged. MRF conditions were applied on the rotor region.

Attached are the qualitative comparisons between contours of velocities from OF (right) and Fluent (left).

Quantitatively too, I see discrepancy between the fluxes between AMI_stator and AMI_rotor cyclicAMIs. AMI_stator flux is a small negative value and AMI_rotor flux is close to zero.

But the total flux entering - total flux exiting the domain = the AMI_stator - AMI_rotor flux difference.

I tried playing with the matchTolerence and that did not help either. Anyways my AMI weights are very close to 1.0, indicating almost conformal interface.

Any help is appreciated.

Cheers,
-Jay

EDIT: ISSUE RESOLVED!! See solution in post#4

[piu58]

From what I recognise form the images:
In the Fluent simulation the fresh air comes from the inner of the fan, you have a medium velocity here. The cross section for the air reduces at the outlet of the fan and the velocity gets higher. This is like a fan in 2D should be modeled. In reality, the air comes from above.

In the OF simulation the velocity in the inner of the fan is very low. It seems that the fresh air comes form the main volume (where you want to blow in).
Or the total flow in OF is much lower. I cannot decide which happened form this graphs. Glyphs would be help to understand more.

[arvindpj]

Dear Uwe,

Thanks much for your questions. The geometries are 3D and I use the same mesh in OF and Fluent.

To retrace this issue with a simple geometry, I picked the propeller tutorial from the $FOAM_TUTORIALS and tried comparing the MRFSimple foam solutions with/without cyclicAMIs.

All the initial and boundary conditions are same as in the tutorial.

To split the mesh regions, I used:

 

>> createBaffles -overwrite
>> mergeOrSplitBaffles -split -overwrite

Clearly, there is something wrong at the region interface.

surfaceRegion flowRatePatch(name=inlet):
    total faces  = 4824
    total area   = 0.28064177

surfaceRegion flowRatePatch(name=inlet) write:
    sum(inlet) of phi = -1.4032089


surfaceRegion flowRatePatch(name=outlet):
    total faces  = 4836
    total area   = 0.28272456

surfaceRegion flowRatePatch(name=outlet) write:
    sum(outlet) of phi = 1.3241247


surfaceRegion flowRatePatch(name=AMI1):
    total faces  = 32148
    total area   = 0.19384123

surfaceRegion flowRatePatch(name=AMI1) write:
    sum(AMI1) of phi = 8.4450081e-06


surfaceRegion flowRatePatch(name=AMI2):
    total faces  = 32148
    total area   = 0.19384123

surfaceRegion flowRatePatch(name=AMI2) write:
    sum(AMI2) of phi = 0.079005531

L1.jpg

L2.jpg

L3.jpg

As expected, the MRF solution with conformal interface converged faster.

L4.jpg

L5.jpg

Thanks!
Jay

[arvindpj]

Mass is now conserved!

When using non-conformal mesh and MRF with simpleFoam, in the rotatingZoneProperties include the non-rotating AMI patches.

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

origin    (0 0 0);
axis      (0 1 0);
omega     constant  157.1; //<rad/s>;
nonRotatingPatches (AMI1 AMI2); 

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

[Aurelius]

Dear Jay,

if you are using simpleFoam with MRF in MRFproperties file (at constant directory) it is possible to specify the nonRotating patches:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version               2.0;
    format              ascii;
    class          dictionary;
    location       "constant";
    object      MRFProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

MRF
{
    cellZone           fluid_rotor;
    active                     yes;

    // Fixed patches (by default they 'move' with the MRF zone)
    nonRotatingPatches (AMI1 AMI2);
    origin                 (0 0 0);
    axis                   (0 1 0);
    omega                    157.1; //rad/s

}

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

I am using OF5.x and I have not seen anywhere "rotatingZoneProperties" file, which are the benefits of it?
Pherphaps you know, can be used in combination with dynamicMeshDict in order to specify precisely the non-rotating patches?

Thanks in advance!

[arvindpj]

In OF v5.0 and newer, "rotatingZoneProperties" file is replaced by "MRFProperties" file.
You specify the "nonRotatingPatches" in that file.

Cheers,
Jay