Multiphase
 

Hi

I'm trying to simulate a multiphase system using Euler method, the problem is when I go into boundary conditions;Velocity inlet, there is no option to specify the inlet velocity, only K and E. Also how can I define the volume fraction of the second phase?

Re: Multiphase
 

Look at the left hand bottom section of the Boundary Conditions panel, you'll find a drop down list that specifies 3 phases (for a 2 phase system) - Mixture, phase-1 and phase-2. Choose your phase and click on set. You'll find all your input boxes for velocity/volume fraction etc there.

Re: Multiphase
 

Where you are describing is exactly where I looked but it doesn't appear to be there. I also notice that when I change the multiphase model to VOF or Mixture, the input boxes reappear???

Is there a seperate procedure for running Euler model? I am thinking that I have to have a fully solved single phase solution before I attempt Euler, and only then will it recognise the inlet velocities, or am I way off?

Re: Multiphase
 

"... I am thinking that I have to have a fully solved single phase solution before I attempt Euler, and only then will it recognise the inlet velocities...."

No, that is not true.

Re: Multiphase
 

Hi

Like u said u need to have single phase solution means that u defined an inlet velocity of the first phase already .... after running u put the multiphase model/Euler ON. Next go to the material and define the second phase (like air) and than go to operating condtions and boundary conditions. When u open the boundary condition box, u will see the all the zones defined in your mesh to be present in the left side box, while the right box shows the boundary conditions. Below to the zones box u will see the drop down box (Phase) indicating the material... SEE first phase (i.e. one u run your simulation with), second phase (defined in after you put multiphase model ON) and the mixture model. Specify the boundary conditions for each of the phase after selecting here. Example select the zone (let say inlet for second phase – left hand box, fluent will automatically select the boundary condition in the right box) now select the second phase in the Phase drop down box. Click the set button and u can specify the velocity for the second phase as well as the volume fraction.

In VOF model u cant specify the velocity for the second pahse as single moemtum equation is solved everywhere in domain and other parameters are calculated based on the voulme fraction of the seocnd phase.

I hope this will solve your problem.

Re: Multiphase
 

Many Thanks

Re: Multiphase
 

Hi again,

I have now a fully converged solution of a single phase axisymmetric jet using standard KE model. I know set the Euler model to turn on model phase and enter inlet velocities of 30m/s and 23 m/s for continious and dispersed phases respectively.

The solution proceeds and after a few iterations gives an error message: Error: divergence detected in AMG solver: pressure correction Error Object: ()

What am I doing wrong?

Thanks in advance

Re: Multiphase
 

Check your Grid, URFs (try bringing them down and see if that helps). If not, turn off calculation of volume fraction for some time after initialization, then turn it on once the solution is stable.

Re: Multiphase
 

The approach to solve a complex multiphase flow is not what you're following.

The FLUENT manual explicitly says that, in order to get a better convergence behaviour, you should:

1. Solve the single phase flow by solving the *Eulerian model* equations and deactivating the volume fraction equation in the Solve -> Controls -> Solution panel. This is different from solving a single phase flow with a single phase model.

2. Activate the solution of the volume fraction equation and start to iterate.

This approach is useful in some critical situation, but it's just a trick, which. in many cases is not necessary.

What does it happen if you just start the simulation with the full Eulerian model and, maybe, with low under-relaxation factors?

Considering the velocity magnitude you have, try reducing momentum URF to 0.4 and turbulent kinetic energy and dissipation rate URFs to 0.4 too.

Let me know.

Regards,

ap :)

Re: Multiphase
 

I have followed your suggestions and first developed a flow field using Euler, with the second phase switched off. This worked fine although it took a long time to converge (approx 6000 iterations). Now when I try to turn on the second phase the same problem persists and reports the exact same message.

I also tried lowering the URFs as suggested with no luck. The mesh I am using is a simple rectangle with a velocity inlet, pressure oulet, axis, and pressure inlet on remaing edges. Grid size is 250*250 with tetrahedral mesh.

I would really appreciate your advice guys.

Re: Multiphase
 

I do not think you have to wait till the solution converges. You can activate the volume fraction solution as soon as you think the solution would have stabilized (For example, the velocity field might have stabilized).

Re: Multiphase
 

I would need some more information on the case you're considering to be of more help.

However, you tell you did 6000 iteration to get the single phase solution. Are you using the steady solver? Remember that a multiphase flow is rarely steady. Also, in most cases they are not symmetric.

Then, if your domain is rectangular, there's no reason to use a tet grid. If possible, always use an hexahedral grid.

The coupling of pressure inlet and pressure outlet in the Eulerian model is not a good idea. The Eulerian model assumes all phases are not compressible, so it's better to use velocity inlets and pressure outlets only.

P.S. Feel free to use my e-mail if needed.

Best regards,

ap

Re: Multiphase porous
 

Can any body tell me E-E multiphase flow is use with porous zone with counter current configuration??.I have divergence problem despite my porous zone is isotropic and it also show -ve presure. regards