[Lookid]

EDIT : I failed to do what I wanted finally, but I summarized the fails below, if someone in interested.
And so this post would suit better in Running/Solving rather than Community Contribution, sorry for that but when I first posted I thought I did it right
Feel free to correct the mistakes I am saying.
Foam-extend 4.0 is used to run.


The goal is to simulate a Radial Pump with a 3 parts : The inlet tube, the impeller (periodic was the first goal) and the volute.

• The mesh is created with cfMesh, but the overall mesh is coarse since I couldn't have a nice quality mesh for the impeller.
• cyclicGgi is applied to the inlet tube and the impeller when the impeller is periodic.
• The connection between the inlet/impeller and the impeller/volute is the main topic here that made me fail over and over.
• The solver used are MRFSimpleFoam for steady-state simulation and pimpleDyMFoam for unsteady
• To compare the results, I have CFX Data, but no experimental ones.


> Periodic impeller - Steady - ggi connection (inlet/impeller and the impeller/volute) (Frozen Rotor and periodic impeller is not good I know, but it was to try it)

The flow in the impeller is nice, torque and inlet pressure are similar to CFX, the thing is the outlet is equal to my inlet flow instead of being multiplied by the number of passages. The periodicity is not taken in account. If in understood well, all the volute inlet part not in contact with the impeller outlet is treated as a slip wall in this kind of situation, anyway, this is not the goal.

> Periodic impeller - Steady - MixingPlane (inlet/impeller and the impeller/volute)

The result are pretty similar to the ones before. The only difference is that the outlet of the impeller is averaged over the 360 degrees of the volute inlet and not multipled once again.

> Periodic impeller - Steady - overlapGgi (inlet/impeller and the impeller/volute)

This one should work, since the overlapGgi BC has a parameter to specific what you want, it is called 'nCopies' and I fixed it to 6 for the impeller outlet and 1 for the volute inlet. I ended up with very unphysical results and an outflow of some m3/s instead of 30l/s.

> Full impeller - Steady - MixingPlane (inlet/impeller and the impeller/volute)

The periodicity problem is now not a problem anymore, since the full impeller is modeled.
The simulation runs properly, the torque converges to a similar value than CFX, but the head is highly underestimated (around 15m instead of 32m)
See the first image

Side note: to run in parallel, the cyclic or any connected patches have to be on the same processor. Using the scotch decomposition with periodic impeller, it managed to do this while keeping the same number of cells in each processors. In the case of the full impeller, it could not find a way to do this, but the priority is given to the good repartition of the number of cells instead of keeping the specified patches in the same processor.

> Periodic impeller - UnSteady - overlapggi (inlet/impeller and the impeller/volute)

This is the last try I did, and once again, the outflow is nonsense and 10x higher than my inflow. For detail of the flow rate over the patches:
- Inflow = 5l/s (periodic, the real one is 30l/s)
- Inlet ggi = 5.33 l/s
- impeller_inlet ggi = 5.33 l/s
- impeller_outlet ggi = 6.62 l/s
- volute inlet = 57 l/s
- Outflow = 317 l/s

See the second image


Here is the case of the periodic impeller, steady state with overlapGgi, you won't have good results with this, but if you want to try, go for it. Moreover it treats other stuff that may interest some like:

- cfMesh
- topoSet
- mergeMeshes
- tranformPoints
- createPatch
- decomposePar (with ggi connected patches in the same processors)
- setSet / setsToZones

https://drive.google.com/file/d/1Kw4...ew?usp=sharing



Be sure to join the OpenFOAM Discord !
https://discord.gg/P9p9eHn

If you don't know what Discord is, see this thread
The OpenFOAM Discord !

Lilian.

[Lookid]

First post edited, I finally did not succeed, so it is not a tutorial ^^'
Maybe some moderator can move the thread to OpenFOAM Running, Solving & CFD ?
Sorry about that

[Lookid]

Sorry for uping a >1 year old subject, but in case it interests someone, it is done finally ^^.

MRF approach, comparison of OpenFOAM with a commercial software.

case : https://github.com/jnmlujnmlu/OpenFO...abannes.tar.gz

pdf : https://github.com/jnmlujnmlu/OpenFO...mp_oimuo_2.pdf

presentation : https://www.youtube.com/watch?v=hBQUcaPHbk4