[Destouches]

Hi everybody, I'm Adrien, a new and (still) enthousiast Foamer !


I would like to send a stream of water in a 3D turbine (still and helicoidal, 10cm long) at about 100m/s (3D mesh OK from Salome).


I'm using interFoam (damBreak) with laminar turbulent properties, but whatever I do, I keep getting the usual endless deltaT decreasing (with adjustTimeStep).


Do I have to pick other solver/properties to solve this case ?


Cheers

[eric]

A few questions for you:

• What does the geometry and mesh look like?
• Are you sure you need a multiphase flow solver? Normally, a turbine operates in single-phase flow, i.e. you would typically only simulate the water.
• 100 m/s is extremely fast and demanding for a numerical solver. Have you tried using a (much) lower velocity to see if it works then? With 100 m/s you would also need to account for turbulent effects, turbulence could help stabilize the simulation but also introduce additional difficulties in choice of model etc.

[Destouches]

Thank you very much for your concern.

• What does the geometry and mesh look like?

https://imgur.com/a/JZX4V

A 5 to 1 mm mesh size, inside a 40*40*140mm box (12Mo).

• Are you sure you need a multiphase flow solver? Normally, a turbine operates in single-phase flow, i.e. you would typically only simulate the water.

Multiphase indeed, it must be installed on a plane (100m/s, our ATR42 is fairly slow) and is aimed to separate air from water droplets, which are expelled on the outside of the tube thanks to the helicoidal wings.

• 100 m/s is extremely fast and demanding for a numerical solver. Have you tried using a (much) lower velocity to see if it works then? With 100 m/s you would also need to account for turbulent effects, turbulence could help stabilize the simulation but also introduce additional difficulties in choice of model etc.

Enlighting, thanks. So, turbulences may help stabilize stuff...it is...interesting . I will try harder on the RAS/k-epsilon. Before working on this geometry, I tried different BC on a 3D interfoam "shower" simulation, linked below, it worked great. The only issue is that the buddy may drown at the end of the calculation, please be careful if you run it.


Time step and turbulences seem to be the key...

[BlnPhoenix]

Hi,

you mentioned that you want to use interFoam for dispersed water droplets. I'm not so sure about this approach since droplet size needs to be fairly large or element size fairly low to resolve each droplet. From your mesh pic, i'm sceptical.. BTW What does "(12Mo)" mean? Do you mean 12 Mio elements?

Also regarding the low time step, have you checked by hand if the Co is in the same ball park as the simulation calculates it? If not you may have mesh issues. Also, i would start with 1 m/s just to make sure it's running stable and slowly increase velocity. InterFoam should run also w/o turbulence modelling imo.

[kera]

Hallo,

if you are working with interFoam, I would start with "hex" mesh instead of "tetra" mesh.

regards,
Ricky

Originally Posted by Destouches

Thank you very much for your concern.

• What does the geometry and mesh look like?

https://imgur.com/a/JZX4V

[Destouches]

Hi Foamers, thanks for your replies.


My simulation is working, so I make a quick debrief for whoever would someday be interested (I don't bet on it though).


Abstract:
Behaviour of a mixed water/air high speed input in a turbine shaped static collector designed for phase separation


Issue:
Very small mesh (<1E-3m) and very high speed (1E2m/s) makes adjustableTimeStep a dull boy (1E-20 s)


Solutions to improve stability:
- local imrovement of mesh size: I localized 'divergence points' after several simulation (wing's extremities) and increased mesh there until I obtain a 100Mo UNV file, not more.

- static solution: Instead of calculating 2ms of stream with Euler, I aimed for stationnary solution with localEuler (LTS simulation, a godsent), then play with nAlphaSubCycles and relaxation factors until the the calculation doesn't diverge anymore

- a truck load of patience: for 10 alpha cycles and a relaxation of 0.01 (don't laugh), I ran a 60 hours simulation (13 000 steps), which was already converged around 30 hours.

- The rest is comparable to the shower case I already linked in my OP.


Theeeere you go:
https://imgur.com/a/tcTam



Morale of the story:
OpenFoam can accomplish anything, as long as you ask nicely




Cheers Foamers