[MengyingShu]

Hi friends,

I'm using CFX to simulate an air-droplet flow in a radial turbine. The droplet is produced by hydrogen fuel cell stack. Phase change is not considered here. The diameter of water droplets is 0.3mm. The mass ratio of air to water is about 10 to 1. Since the volume fraction of droplet is very low, I am not sure to use dispersed fluid or particle transport fluid. Then I gave the continuous-dispersed model a go.

The simulation ran well, but in the result I found the mass flow of water is evidently imbalanced. About 15g/s water flows into the turbine, but almost none flows out. When I monitor the mass flow of water at exit, it is always zero.

Then I used a bend pipe to test the model, to exclude the influence of turbine geometry and rotating etc.

Some of my setting are as follows:
Air is continuous, and water is dispersed fluid. Free surface model is none. Particle model is used as interphase transfer model. Drag force is set as Schiller Naumann model. Boundary condition at wall is default (Volume Fraction). Total pressure and temperature is given at inlet, and static pressure at outlet. A CCL file of a bend pipe is attached.

Followings are what I've tried:
1. set Free Surface Model to standard:
The outlet mass flow slightly increased. It is about 0.5g/s when converged, but still imbalanced.
2. based on 1, change wall boundary condition to area fraction, and set the value of water as 1.
Nothing changed.
3. change the bend pipe to a straight one:
Mass is balanced.
4. using particle transport fluid, and set wall absorption as 0, both perpendicular and parallel coef. are 1.
Mass is balanced in bend pipe, but only 1g/s flows out when I change the model back to a turbine volute. The droplets just go round and round in the volute, can’t escape.
5. still particle transport fluid, and use a wall film boundary.
Transient simulation can’t converge after about 100 steps. The droplets hit the wall then like “disappear”.

Is the main problem here the wall boundary condition, or some other settings in the continuous-disperse flow? And, if I use LPT, is there any setting that can simulate the movement of droplets along the wall?

Could someone give me some advice? Thanks a lot.

[Gert-Jan]

When running Euler-Euler, then you could read this post:
H-energy imbalance and P-mass imbalance does not converge.
However, where I write energy, you should read massfraction.

[ghorrocks]

I have done quite a lot of work recently on aerosol deposition on walls. My experience is:

When using the Eularian model when particles hit to walls you get several effects occurring:
1) The volume fraction of the aerosol builds up in the element adjacent to the wall. Once it builds up a bit (or maybe even gets to 1.0) then it overflows into adjacent cells and can start spurious flows along the wall and release particles back into the flow.
2) You want aerosol which hit the walls to be eliminated, rather than just building up in the wall adjacent cell. I tried using a source term to destroy any aerosol in the wall adjacent cell, but it lead to non-physical jumps in the volume fraction field.

In short, I have not found a way yet of modelling aerosol deposition on surfaces yet with a Eularian approach.

When you use a Lagrangian approach you have much better control over the wall behaviour, but you will require a very fine wall mesh to accurately predict which droplets hit the wall and which ones miss. Note you need to set the wall restitution coefficients to 0 or the particle will bounce off the wall, and you need a super-fine wall mesh to capture this accurately. Often the mesh required for this is far finer than the mesh required for a turbulent boundary layer.

Looking at your output file, I see two weird things:
1) You are injecting water at 85K. Do you really intend to inject water at almost -200C? Isn't it ice at those conditions?
2) You have left the restitution coefficients for the wall at 1.0. You will need this to be 0.0 if you want particles to hit the wall and stop.

And finally, You will probably need a super fine wall mesh to get mesh independence on the particles depositing on the wall.

[MengyingShu]

Thank you so much. I’ll try it in Euler-Euler simulation.

[MengyingShu]

Originally Posted by ghorrocks

Looking at your output file, I see two weird things:
1) You are injecting water at 85K. Do you really intend to inject water at almost -200C? Isn't it ice at those conditions?
2) You have left the restitution coefficients for the wall at 1.0. You will need this to be 0.0 if you want particles to hit the wall and stop.

Thank you for the reply.

Sorry. It's a mistake. The temperature should be 85C, not Kelvin.
I've tried to set restitution coefficients as 0. Then particles stop at the inlet part of the volute, where they hit the wall. No droplets at all in the downstream domains, but we want to see how the particles 'flow' in the whole turbine.
As for the mesh, I'll improve the near wall grid and simulate the volute only to see if it changes anything.

Thanks again.

[ghorrocks]

If you read my previous post you will see I recommend you do not use the Eularian approach, at least not until you fix the problem I discussed.

The Lagrangian approach models droplet in the air. Are you trying to model flow of the accumulated liquid on the surface as well? This is an entirely different model with different physics. CFX has a wall film model which is meant to do this but I have never used it - but note it was designed to model wall accumulation of fuel in the walls of IC engines, so use of this model in different applications is at the user's risk.

[MengyingShu]

Originally Posted by ghorrocks

Are you trying to model flow of the accumulated liquid on the surface as well?

No, the accumulated fluid can be neglected.

In our experiment in a pipe, we see small droplets (diameter less than 0.3mm) hit the wall and don't stick on. We also see the water droplets flow out of the turbine with the air, instead of along the wall. I think it is reasonable to ignore the accumulation on the surface.

I want to model the movement of droplets in the turbine rotor that located downstream the volute. How they approach the blades: like velocity, direction, where they hit the blades, and so on. The problem is in the simulation all droplets hit the wall which they first encountered in the volute and stop (restitution coefficient as 0.0).

This result is much far away from what we see in the experiment. That's why I'm confused. I'm hoping to see at least some droplets leave the turbine with air.

In addition, is there any principle to set the 'number of positions'? I'm having 15g/s water flow with diameter 0.3mm. Are 100 particles too less? Would that be the problem?

[ghorrocks]

You need to do a sensitivity study on the key simulation settings. I can tell you that 100 droplets is going to be nowhere near enough. But I cannot tell you how many you need, you need to establish that with a sensitivity analysis.

A sensitivity analysis is:
1) Do a baseline simulation (like the 100 particle simulation you have just done)
2) Double or halve the important parameter (so do a 200 particle simulation)
3a) If the results of the two simulations for an output of importance are the same within a tolerance you are happy with then the baseline simulation settings is OK
3b) If the results of the two simulations are different by an unacceptable amount then return to point 1 with the 200 particle simulation as the baseline, and repeat with a 400 particle simulation.
4) Keep doubling the number of particles until you obtain convergence

I would recommend a sensitivity analysis on number of particles and mesh resolution near the wall. So that is two sensitivity studies you will need to run. I am sure you will find you need thousands to millions of particles, and a VERY fine wall mesh.

You will also find that the simulations required to obtain sensitivity convergence are large and take a long time to run. That is why CFD is run on supercomputers.

[MengyingShu]

Thank you Glenn.

Glad to have some idea on this problem. I’ll sun some cases and update my results.