[srinidhi4u]

Hi all,

I am working on a problem with annular cylinder with cone shaped structure at the bottom. I inject 3 different diameter solid particles from the bottom of the annular space which hits the cones and leads to erosion of it.

This is a steady state compressible air flow problem. I inject the particles from bottom and there is a fluid jet around the cone which hits this bottom annular space, carry the particles and bombard it against the cones and erode it before exiting on the top of annular surface. I am using Tabakoff and Grant erosion model which should help me to find the erosion rate on the cones.

I am facing problem of non-uniform erosion results after each particle iteration. I am using 20 as particle iteration frequency. When I try to check for erosion rate density at one time step and the next one there is a change(even though it is not very major). It is kind of fluctuating and coming back to almost same values if I check values of say 10 particle iterations like a cycle. Is this common to happen in Lagrangian particle tracking? Does turbulent particle dispersion has any role to play here?

I am monitoring air pressure and mass flow and it has normalised. I am using 2 way particle and air coupling to address the issues of particles affecting the air flow. My particle loading is less than 12% which tells me that I should be using Lagrangian approach for modelling particles. Can someone guide me why there should be non-uniform values between particle to particle iterations even though it has converged? Or should I take average of say 10 time steps approximately to say that this is my erosion density rate?

Thanks in advance

Best regards,

Shri

[ghorrocks]

Have you read the documentation? A quick search found:

Note: If you encounter convergence difficulties when using a turbulence dispersion model in conjunction with Segregated volume fraction coupling, then you should consider reducing the physical time scale, or switching to Coupled volume fraction coupling.

There is plenty of other information on this in the documentation as well.

[srinidhi4u]

Thanks Glenn. I have not seen this. I will check for that.

What are your thoughts? is it because of the convergence problem from turbulent dispersion we see the difference between the particle iterations?

Is my approach to the problem appropriate?

[ghorrocks]

I would try what the documentation suggests first (reduce time scale, coupled VF solver). If that does not work I recall that convergence can be difficult in turbulent dispersion force simulations as the turbulent dispersion force is recalculated periodically and is applied as a random force on the particles. That means whenever it recalculates the residuals will go up, then it converges on that for a while then recalculates again and the residuals go up again. This means it is difficult to get convergence in the normal sense. So best to use a parameter of importance to you (such as flow rate, pressure drop or whatever) and monitor that parameter for convergence.

[srinidhi4u]

Thanks a lot Glenn. I will try with the suggested approach.

[srinidhi4u]

Glenn, I am confused how important is it to consider Turbulent dispersion in my problem. If I skip dispersion will I be missing to capture the actual physics?

[ghorrocks]

That is up to you to decide. Turbulence dispersion force is a difficult and expensive model to include so only include it if you have to. So you have to work out if it is significant in your case or not.

The easiest way is to do a benchmark run with it on and off and see if it makes any difference. A better approach is to estimate dispersion due to the various forces and see if turbulence is significant or not.

[srinidhi4u]

That makes perfect sense to me. I have started the simulation without dispersion and I am already seeing all the particle integration error disappear, which I had seen earlier. I will compare the two cases and see if I see a big difference.

Thanks a ton again.