[hiuluom]

I would like to simulation conjugate heat transfer fluid and solid with a zone MRF in fluid. The mesh was built from STL SHM with 4 zones. This is the of my solve.

1. The problem:
   When using chtMultiRegionSimpleFoam solver, I must to split mesh into region including MRF zone and other zone. So I need to merge fluid contain MRF zone.
   
2. Solution
   My method is to get cell zone using mergeMeshs because splitMeshRegions will divide all zone from cell zone.
   Here is example description:
   Model:
   
   Front view:
   
   
   
   Side view:
   
   
   
   Iso view:
   
   
   
   The model includes solid1, solid2, fluid and MRF zone
   
3. Command:
   Split mesh into regions with the name v1(solid1), v2(solid1), v3(fluid), v4(MRFzone):
   
   

   splitMeshRegions -cellZonesOnly -overwrite -useFaceZones

   I will combine v4 to v3. In v3 and v4 folder in constant directory, I make sub-directory 0, constant, system inside v3, v4 and then merge mesh. Remember that in system folder must have controlDict, fvSolution and fvScheme file.
   
   

   mergeMeshes v3 v4 -overwrite

   The last step of the mesh genesis is renaming of the boundary, changing patch type. Because boundary of v3 will have mappWall between v3 and v4. Changing this wall to cyclicAMI type. This managed by the utility createPatch.
   
   

   patches
   (
       {
           name            v4_ami1;
           patchInfo       
           { 
               type cyclicAMI; 
               neighbourPatch v4_ami2;
           }
           constructFrom   patches;
           patches         ( default-interior_v3_to_v4 );
       }
       {
           name            v4_ami2;
           patchInfo       
           { 
               type cyclicAMI; 
               neighbourPatch v4_ami1; 
           }
           constructFrom   patches;
           patches         ( default-interior_v4_to_v3 );
       }
   )

The result seemly good, but I am not sure the cyclicAMI from face mappWall type is the same which make from MRF zone.

I will show result of my test model later

[hiuluom]

Hi everybody,

I show my test case with fluid, solid, fan and propeller. The velocity of propeller in my guess.

This is domain:


Inside solid zone has water volume and fan.



Rotating velocity of propeller



water velocity inside solid make by fan



Finally, the path line and temperature of simulation



My question: Do the method to solve MRF with chtMultiregionSimpleFoam and the result test model as I mention above correct or incorrect for this model?
If anybody suggest run MRF with multi region better, you can suggest me other ways.

Best,
Thanh

[Tobi]

Dear Thanh, where do you have your MRF ? First I have to mention that I am not familiar with SRF/MRF but in your case you have a propellor that is rotating by a special speed or is there your MRF ? In any case, the streamlines you get are stationary but should be instationary due to the fact that the fan is rotating and "cutting" through the fluid.

I tried to understand the geometry but I am sorry, do not get the point. Can you explain it again?

[hiuluom]

Dear Tobi,

Thanks your reply.

Sorry my description did not detail. I update my explanation:

This is MRF zone as well as cyclicAMI



After running splitMeshRegions, I have 4 zones: Air, MRF_zone (including propeller), water and solid.
I merge the MRF_zone into Air. So in the Air and MRF_zone sub-directory in constant directory, I make folder 0, constant and system, respectively.
In the Air sub-directory I copy polyMesh into constant and rename polyMesh outside to polyMesh.old. Similarly for the MRF_zone.
And then I start merge 2 meshes by command mergeMeshe. When finish, I copy polyMesh directory in constant/Air/constant/polyMesh to constant/Air/.

Finally, I set createPatchDict file for Air in system/Air to change the boundary mapedwall between Air and MRF_zone to cyclicAMI and run topoSet for MRF_zone also.

I upload my case on Microsoft onedrive, you can download it at:https://1drv.ms/u/s!AkLk2AeMilR1gtZ73idBPAHaSBbRXg

I think the operation is complicated. Hope you understand it.

Best regards,
Thanh

[Tobi]

Just a question - do you use AMI or MRF now ?

[hiuluom]

Dear Tobi,

What does it mean your question?

In my experience if I want to run a propeller simulation, I make MRF zone as well as cyclicAMI from face MRF. Do my understand miss?

[Tobi]

Yes normally you are wrong.

AMI (arbitrary mesh interface) are the patches that connects a rotating cell zone with a stationary cellZone and hence you are able to rotate the rotating cell zone (where your propeller is in). The AMI just interpolates and maps values from one side of the baffle to the other one.

MRF is a model to avoid moving meshes and make life easier. See here: tutorials/compressible/rhoPimpleFoam/ras/mixerVessel2D

That was the reason why I was confused about your MRF and AMI. So finally you just added the motion libraries to the cht solver (actually you changed the derivative of the fvMesh to become a non-const object).

If you did this, I hope you also have all flux corrections in your equations because due to the rotation, you get mesh-fluxes that have to be corrected.

[hiuluom]

Hi Tobi,

I always run propeller with MRFzone. In addtions I also get cyclicAMI and the result has been good. I based on a tutorials/incompressible/pimpleDymFoam/propeller to set up case.

As you told me, if I simulate with one fluid no other zones, do I only need to add MRFzone name in fvOptions file?

Otherwise I make cyclicAMI and do not need use fvOptions file, but how to give the rotate velocity?

Best regards,
Thanh

[hiuluom]

I saw difference cyclicAMI and MRF zone in fvOptions file that is zone active or inactive. "cyclicAMI and do not need use fvOptions file" that is my stupid questions
Thanks Tobi.

[Tobi]

Hi,

• if you are using a rotating mesh (mesh is moving in OpenFOAM), you have to define a cellzone that is rotating. To couple the rotating and stationary mesh, you have to need AMI boundary conditions.
• If you have rotation somewhere and don't want to move the mesh or lets say, you can use the SRF or MRF approach, use it because here you do not need any mesh motion. Therefore you do not have to take care about additional mesh fluxes, interpolations between rotating and stationary mesh and so forth ... it is a model (but I never used it, hence I am not so familiar with that).

If you build a cellZone around your rotor and you really move this cellZone with dynamic mesh, you need AMI and hence there is no MRF approach.

If you somehow model the rotation with the MRF/SRF approach, there is no physical mesh motion in your case (you model the motion but the mesh stays the same during the calculation).

[hiuluom]

I tested with simpleFoam OF2.2.x. Both of models take from tutorial.
MRF and AMI 2D model ran with simpleFoam. The result pressure, velocity are not difference.
So I think that if I make AMI ratotating for solver not support dynamic mesh, the value do not effect when compares with MRF. In chtMultiRegionSimple does not support dynamic mesh, I can make AMI face as mention above but it doesn't have a mesh flux, interpolation between station and rotation mesh.


Here is my setup case fvOptions file:

MRF:

MRF1
{
    type            MRFSource;
    active          true;
    selectionMode   cellZone;
    cellZone        rotor;

    MRFSourceCoeffs
    {
        origin      (0 0 0);
        axis        (0 0 1);
        omega       104.72;
    }
}

AMI:

MRF1
{
    type            MRFSource;
    active          true;
    selectionMode   cellZone;
    cellZone        rotor;
    
    MRFSourceCoeffs
    {
    	nonRotatingPatches (AMI1 AMI2);
        origin      (0 0 0);
        axis        (0 0 1);
        omega       104.72;
    }
}

You can review in the following figures.

[hiuluom]

I tested between AMI and MRF 3D model, got moment coefficient with simpleFoam.
The result also is no difference.
Finally, I think if simpleFoam or chtMultiRegionSimpleFoam solver, which do not support dynamic mesh, can run with AMI or not.

[atlan]

Hi all,
I am trying to use MRF in chtMultiRegionSimpleFoam just to ad centrifugal force to fluid. This should represent a heated rotating disk with a cooling fluid inside. So I added the MRF to the fluid region only (solid region does not works for me with MRF), but the results are strange. Do you thing is my approach suitable?

[hiuluom]

Hi atlan,

As I discussed with Tobi above, what is the way adding MRF to fluid region?

[atlan]

Hi hiuluom,
Thank you for the reply I would like to simulate cooling of rotating disk (attached picture) and MRF I supposed to by the way, how to implement the centrifugal forces to the model.
Atlan

[hiuluom]

Hi altan,

You can see the tutorial chtMultiRegionSimpleFoam heatExchanger.
The rotating volume is setup in fvOption file.

[atlan]

Hi hiuluom,

thank you for the answer.
I added the rotation with fvOption for the fluid and it works. However adding this option to the solid section does not work. I would like to rotate with the complete assembly (fluid and solid) or at least to rotate with the fluid solid interface. May be I can use the rotating wall velocity for the interface in U boundary condition?
I have now other problem using turbulent model in chtMultiRegionSimpleFoam, which crash after 3 iterations. The temperature increases uncontrolled over 10000K, even when the temperature on boundary and initial conditions is homogenous 300K. Laminar model works without any problem.
Best regards
Atlan

[hiuluom]

Hi Altan,

Sorry too late answer.

1. I know MRF which does not integrate in solid region up to now. It only is solution for temperature.

2.

I would like to rotate with the complete assembly (fluid and solid) or at least to rotate with the fluid solid interface

I think you want to rotate with dynamic mesh. You should modify solver and reference other dynamic solvers how to work.

Best,
Thanh

[sitajeje]

Hallo Thanh,

It is exciting to see your simulation with cht solvers and MRF. Thank you very much for sharing your experience!

I couldn't download your file but I have only one thing to clear: do you have mesh grids in the solid part in the MRF? I have a similar problem as yours, but the fan has its base connected to the heat source. I didn't figure out how to simulate the heat conduction inside the fan as well. I would appreciate if you could give me some hints.

Thank you very much in advance!

sitajeje

[hiuluom]

Hi sitajeje,

The model did not have solid part inside MRF zone. I only applied heat flux on the wall of solid part. If you use OF 4.x (I use 2.1), it will easy to set MRF for a zone with fvOption file.