foam-extend lacking rhoCentralDyMFoam - what to do? I need ggi BC
 

I want to use density-based solver to solve rotating case (turbomachinery) so I chose solver rhoCentralDyMFoam. I successfully ran the simulation and it took 25 hours on 1 core. Geometry is periodic so now I want to simulate only one period of it. I tried with cyclicAMI boundary condition on periodic patches, but it didn't work.
Looks like I need to use ggi, I mean cyclicGgi BC. The problem is that original Openfoam doesn't have ggi BCs so I installed foam-extend - but this one lacks rhoCentralDyMFoam, it only has rhoCentralFoam.
I tried to use rhoCentralFoam with dynamicMeshDict but it didn't work. Is there any possibility to use rhoCentralDyMFoam with ggi BCs?
What else can I do?

Let's jump back to your original case with rhoCentralDyMFoam on "original openfoam".
I think we can fix the cyclicAMI. Can you share more information? If the case is not secret and isn't too big, can you archive the whole thing and share it. Otherwise can you share the 0 and system folders and the boundary file from constant.
A diagram or dimensioned drawing of the geometry/mesh would also be super useful.
Also please let us know exactly which version you are running

-Peter

I am using OpenFoam 6 (openfoam.org). Here is the whole thing: https://drive.google.com/drive/folde...3D?usp=sharing
So there are 3 cellZones, the main one is called rotor, it is rotating in the middle of other two zones which are stationary.
I did "createPatch" successfully so I have some cyclic patches which are correctly linked (I need cyclic because mesh is just one period (1/7) of impeller). I also have 2 pairs of cyclicAMI patches - one pair is located where "inlet zone" is connected to rotor and another pair where rotor is connected to "outlet zone".
If you look at the file "boundary", cyclicAMI patches are at the bottom and there is this setting:
This way the case starts running but crashes after 3.2e-06 seconds because the patch target weight drops to zero (see log01). If you look at the results at time 3e-06 with paraview, you can see that cellZone rotor rotated for approximately one cell face so some cell faces lose contact with their neighbour cell faces. I think this is the problem. But AMI should connect them even after the mesh is moved, right?

The original setting I had was
but in this case, the case doesn't even start running (see log02)

If you want to see the mesh in Paraview, you need to rename folder 0 to 0_, otherwise Paraview crashes. Attaching picture of mesh and picture of second cyclicAMI pair. As you can see, faces are not exactly the same, number of faces is slightly different as well, but patches are similar enough for AMI to work, in my opinion.

cyclicRepeatAMI !!
 

Apparently cyclicAMI boundary condition does not support transient simulation of cyclic (periodic) geometries. It lacks ability to connect faces from one side of geometry to faces on other side. This was implemented only recently in Openfoam 6 with new type of BC - cyclicRepeatAMI. More info about it: https://github.com/OpenFOAM/OpenFOAM...29439fac374a60


Now my case finally runs past that time 3.2e-6
Edit: If you want to run my case, change U/massFlowRate to 0.005 (0.035 is appropriate for whole 360° geometry, so 0.005 for 1/7 period) and dynamicMeshDict/omega to 4294 (41000 RPM)