[DiegoNaval]

Hi All
Some one have some reference about the theory of the MRF? In particularly I'm interesting about how write the N-S equation for a non-inertial reference frame starting from the classical N-S equation for the inertial reference frame. And how convert the equation for the non-inertial reference frame from the relative velocity terms to the absolute velocity terms.

Thank a lot.

Diego

[sleepdeprivation]

Talk to Maki. He seems to understand it really well.

[DiegoNaval]

Thank you very much, Alton.
But now I'm working with him. And I hope that there is a book where I can find the theory and the hypothesis of the conversion of the non-inertial equation from the relative velocity to the absolute one.
I'm already ask him, but we can't find anything, till now!

Thank you in any case for the quick answer!

Diego.

[david]

http://openfoamwiki.net/index.php/Si.../_Developments

Regards
David

[DiegoNaval]

Thank you a lot David,
Now all is more clear for me!
There are already some terms that are equal to zero that i should demostrate...
But in generaly all it's ok.

Diego

[viraj20feb]

I have a 3D geometry consisting of a vessel which has a rotating shaft and blades assembly inside it. I am trying to set a MRF zone for this case when the shaft and blades rotate and the vessel is stationary. In all the cases which I have scene, the MRF zone is defined only in the region surrounding these impeller blades.

My question is, since the rotating patches will have an effect over the entire volume, why don't we define the MRF zone for the entire volume(instead of the volume surrounding the blades) and define the vessel in the nonRotatingPatches condition?

Also, what happens at the interface of MRF zone and non-MRF zone? Which equations are solved?

Thank you!

[DiegoNaval]

Dear Viray,
If you derive the MRF equations from the flow equations, you find that the two systems are formally very similar. Consequently, you could set the MRF zone in all the flow domain. Your main issue concerns the boundary conditions for the wall or for the interface surface. In fact, the flux through the interface is equal inside the MRF zone and outside it only if the boundary surface normal is perpendicular the rotational axes. This means that the hull boundaries or the external surfaces can generate spurious fluxes.

Regarding the equations on the interface surface, the classical N-S equations are solved under the constraint that the velocity flux in the two side of the interface needs to be equal in terms of absolute and relative velocities.

Diego

[viraj20feb]

Dear Diego,

Thank you for your quick reply! I now understand what happens at the interface. But I am still not clear about the selection of the size of the MRF zone. Why do they generally select only the volume which has the rotating blades rather than the whole volume since the rotation of the blades will cause motion in the entire volume?

Thank you again!

Regards
Viraj

Originally Posted by DiegoNaval

Dear Viray,
If you derive the MRF equations from the flow equations, you find that the two systems are formally very similar. Consequently, you could set the MRF zone in all the flow domain. Your main issue concerns the boundary conditions for the wall or for the interface surface. In fact, the flux through the interface is equal inside the MRF zone and outside it only if the boundary surface normal is perpendicular the rotational axes. This means that the hull boundaries or the external surfaces can generate spurious fluxes.

Regarding the equations on the interface surface, the classical N-S equations are solved under the constraint that the velocity flux in the two side of the interface needs to be equal in terms of absolute and relative velocities.

Diego

[DiegoNaval]

Dear Viraj,
The problem is almost the same as in correspondence of the interface. The problem that you solve is in a non-Inertial reference frame, therefore if you have a non-cylindrical surface the computed flux equal to zero (impermeable condition) is valid in the same reference frame. This means that your body rotates with the prescribed rotational velocity.
For the ship, this is not feasible.

Regards
Diego

[viraj20feb]

Hello Diego,

Thanks again!

So let's say if I select the whole domain as a cylindrical MRF zone and define the outer vessel in non-rotating patches. Then, my whole domain will be rotating at the same velocity which is not feasible, right?

Now, if I select a cylindrical MRF zone which consists of only the rotating blades of my impeller geometry. The volume inside this smaller MRF zone will only be rotating at the given angular velocity and the fluid flow outside this cylindrical geometry will be computed in a non rotating frame. So the second one is the correct approach right?

Regards
Viraj

Originally Posted by DiegoNaval

Dear Viraj,
The problem is almost the same as in correspondence of the interface. The problem that you solve is in a non-Inertial reference frame, therefore if you have a non-cylindrical surface the computed flux equal to zero (impermeable condition) is valid in the same reference frame. This means that your body rotates with the prescribed rotational velocity.
For the ship, this is not feasible.

Regards
Diego

[DiegoNaval]

Yes, the second way is the correct one. You should only remember that your interface (mesh faces between the two zones) need to have a normal vector lying in the plane given by the axes of rotation and the center of the face.

Best regards
Diego

[viraj20feb]

Hi Diego,

In the MRF equations development, do you know why
1) del dot (omega cross r) = 0?
2) gradient of (omega cross r) = 0?
3) u_R dot gradient of (omega cross r) = omega cross u_R?

I tried all the vector-tensor identities and relations but I am unable to get the answer.

Thanks a lot!

Viraj

Originally Posted by DiegoNaval

Yes, the second way is the correct one. You should only remember that your interface (mesh faces between the two zones) need to have a normal vector lying in the plane given by the axes of rotation and the center of the face.

Best regards
Diego

[Raphael_Santos]

Originally Posted by DiegoNaval

Yes, the second way is the correct one. You should only remember that your interface (mesh faces between the two zones) need to have a normal vector lying in the plane given by the axes of rotation and the center of the face.

Best regards
Diego

Hi all,

can anyone help me with introductory documents related with MRF and MRF in OpenFOAM.

I have doubt concerning:

(i) Does the MRF zone need to be a cylinder? I tried to run a simulation using it just as a cube, in OpenFOAM with simpleFoam, and it worked fine.

(ii) Does the MRF zone and stationary domain need a boundary interface? OpenFOAM tutorial (mixerVessel2D, incompressible using simpleFoam) does not use any boundary between the domains.

[DiegoNaval]

Originally Posted by Raphael_Santos

Hi all,

can anyone help me with introductory documents related with MRF and MRF in OpenFOAM.

I have doubt concerning:

(i) Does the MRF zone need to be a cylinder? I tried to run a simulation using it just as a cube, in OpenFOAM with simpleFoam, and it worked fine.

(ii) Does the MRF zone and stationary domain need a boundary interface? OpenFOAM tutorial (mixerVessel2D, incompressible using simpleFoam) does not use any boundary between the domains.

Hi Santos,
This was my very old post. I'm happy to hear that someone is still interested in this topic.
To answer your questions:
(i) Yes, it needs to be a cylinder if it communicates with a fixed region. If you set the motions for all the domain, the shape should not be a problem. (This was valid for old OF implementations, I never recheck it in the newer versions)
(ii) No, you didn't need a real interface. The problem was that the faces between the two selected zones (fixed and rotated) should have only radial normal, respect to the MRF reference frames.
This was connected to how the code computes/corrects the fluxes between the two regions.

Best,
Diego

[unilord]

Originally Posted by DiegoNaval

Hi Santos,
This was my very old post. I'm happy to hear that someone is still interested in this topic.
To answer your questions:
(i) Yes, it needs to be a cylinder if it communicates with a fixed region. If you set the motions for all the domain, the shape should not be a problem. (This was valid for old OF implementations, I never recheck it in the newer versions)
(ii) No, you didn't need a real interface. The problem was that the faces between the two selected zones (fixed and rotated) should have only radial normal, respect to the MRF reference frames.
This was connected to how the code computes/corrects the fluxes between the two regions.

Best,
Diego

Hi everyone,

I am currently trying to simulate a centrifugal pump with the MRF approach. However, I am not sure how I can define the MRF region. I am using SALOME to do the CAD geometry, as you can see in the attached file. The region I want to define as the MRF is an annulus, with outer radius corresponding to the circular edge on the trailing edge of the blades, and inner radius is the circular edge close to the leading edge of the blades.

How should I proceed, to let OpenFOAM know that that is the region I want to be corresponding to the MRF zone?

Thank you in advance,
Pedro Gouveia

[DiegoNaval]

Dear Pedro,
To set the MRF in a simulation, firstly, you have to create a new set using the topoSet function, then, you have to convert it into a zone using setsToZones. Finally, in the fvOption you can link the MRF dictionary with your zone.
Consider that actually I use the V8 version, so if something is different in the newer one it is out of my knowledge.

Best,

Diego

[unilord]

Originally Posted by DiegoNaval

Dear Pedro,
To set the MRF in a simulation, firstly, you have to create a new set using the topoSet function, then, you have to convert it into a zone using setsToZones. Finally, in the fvOption you can link the MRF dictionary with your zone.
Consider that actually I use the V8 version, so if something is different in the newer one it is out of my knowledge.

Best,

Diego

Diego, I actually managed to do it with the topoSet dictionary, not using the setsToZones. I think that option is implemented, in v11, already in the topoSetDict. The code is the following:

actions
(

{
name MRFSet;
type cellSet;
action new;
source cylinderAnnulusToCell;
p1 (0 0 0);
p2 (0 0.005 0);
outerRadius 0.142;
innerRadius 0.058;
}
{
name MRFZone;
type cellZoneSet;
action new;
source setToCellZone;
sourceInfo
{
set MRFSet;
}
}
);

However, the zone is not being shown in paraview, in the mesh regions. It is being detected by the paraview software, since when I turn off all the mesh regions selections, I am left with the zone, just like in the pictures. I can't tell if this is supposed to happen or not, since the simulation I ran gave me strange results. I will keep the forum updated though.

[Raphael_Santos]

Originally Posted by unilord

However, the zone is not being shown in paraview, in the mesh regions. It is being detected by the paraview software, since when I turn off all the mesh regions selections, I am left with the zone, just like in the pictures. I can't tell if this is supposed to happen or not, since the simulation I ran gave me strange results. I will keep the forum updated though.

You can check if the cellZones was created in: constant/polyMesh/cellZones, and check if you find the name of your cellZone there (you named it MRFZone).

To check it in paraview, maybe you can use foamToVTK

foamToVTK -cellSet "zone_name"

Have a look here: How to visualize cellset region in OF?

[DiegoNaval]

Dear Pedro,
I worked on this topic several years ago (it was OF v.3). But at that time, you could not adopt an interface between the MRF zone and the rest of the domain with a step shape (like yours). The interface surface (the faces in between the two zones) has to be tangential to the relative velocities (in your case, they have to be cylindrical). This arose from the fact that the flux between the two zones is equal only if, on these faces, the imposed motion does not generate any additional flux.
I do not know if newer versions are able to overcome the problem.

I hope to be useful,

Diego

[unilord]

Originally Posted by DiegoNaval

Dear Pedro,
I worked on this topic several years ago (it was OF v.3). But at that time, you could not adopt an interface between the MRF zone and the rest of the domain with a step shape (like yours). The interface surface (the faces in between the two zones) has to be tangential to the relative velocities (in your case, they have to be cylindrical). This arose from the fact that the flux between the two zones is equal only if, on these faces, the imposed motion does not generate any additional flux.
I do not know if newer versions are able to overcome the problem.

I hope to be useful,

Diego

Hey,

I have surpassed the difficulties of the pre-processing. However, I am running the analysis with the MRF approach, and it seems to be an "aureola" where the MRF cell zone is, as you can see in the picture below. Does anyone have any idea why this could be happening?