[amin.z]

Hi everybody,

I'm trying to simulate a 2-phase flow passing some bends using Discrete Phase Method. air is the career phase and the discrete phase is coal powder.
I have convergence problem and tried several trick to control the solution, but I'm afraid I wasn't able to make it converge adequately.
I will appreciate if everybody share with me his suggestion for my trouble.

Here there are some specification:
Grid: Hexa, 3D
iso-thermal condition, incompressible gas
sst k-omega turbulent model,
injection from surface,
steady state solver
two-way turbulent coupling: active

Thanks in advance

[CeesH]

Hi Amin!

In what respect is it not converging? Is it the Eulerian or Lagrangian phase you are having trouble with?

In general, the SST model needs quite dense meshes to give a proper solution; does your simulation run properly for k-e or regular k-w?

[amin.z]

Dear Cees,

Distribution of the discrete phase in not logical, and also the residual of the equations especially continuity are around 5e-03, and it should plunge further,
I think turbulence behavior and the residuals are more stable and converge further using K-omega

[CeesH]

does the SST simulation converge in single phase?

[amin.z]

Yes, it does,

The problem is about DPM iterations, after each DPM Iteration, the residuals jump and they didn't decrease enough till next one, is it logical?

And there is vague point for me about there dpm iteration per continuous iterations,
If we incresed it from default value (I think it's 20 by default) to, for example, 200 the residuals adequately plunge, but I have red somewhere it's not a good choice to increase it a lot, what do you think of that?

[CeesH]

Of course, the addition of transient motion by the parcel displacement due to 2-way coupling will make the simulation more intensive, and an adequate number of iterations will be required - which may be more due to the inclusion of that additional effect than it is in single phase.

First off, is the use of 2-way coupling over 1 way important? (what is the stokes number in your simulations)

If it is, then indeed the higher burden may mean more iterations, or perhaps a shorter timestep size such that the differences between subsequent timesteps are smaller. What is the courant number you are running at?

[amin.z]

So do you mean that's fine if I increase the iterations to around 200?

At the inlet the average volume fraction of discrete phase is 3.5e-04 but in some positions it goes to near 0.1, so I think it should be solved using two way coupling, isn't it?
And about St nu. It's around 3.5e-3, I think.

About courant number, I have ben using coupled solver only for steady, and set it as 50

[CeesH]

At such low Stokes numbers, the particles will more or less instantaneously adapt to the velocity of the fluid, it sound to me like you can treat the particles as essentially massless in that respect (saves a lot of time, too). The higher volume fractions may indeed lead to some issues strictly; but you can try a 1-way coupled massless simulation and compare it with the results of a 2-way coupled lateron, to see if they differ significantly.
Regarding the number of iterations, I would try to keep it below 100, preferably 50, when running transient. It may be better to reduce the timestep size and reach a quicker convergence in that respect.

[amin.z]

Hoom, okay, I'll check it with one way coupling, I was thinking about DDPM too, but I must check one way firts,
Thanks a lot for giving me some idea

[CeesH]

Problem with DDPM is that it makes things even more compicated (hence harder to converge possibly, and certainly longer to run) and based on the stokes number I suspect the effect of parcticles on the fluid will be reasonably small - of course, best to test that. But I would opt for the simpler 1-way before moving to DDPM for sure.

[hwet]

 after each DPM Iteration, the residuals jump and they didn't decrease enough till next one

I suppose this is just transient behavior and is what happens in a transient simulation, the residuals should "jump" at every time step and then converge and then jump again for the next time step.

Also, did you get a converged solution first for the gas phase before injecting in the particles? probably, that is the way to go.

[amin.z]

Originally Posted by CeesH

Problem with DDPM is that it makes things even more compicated (hence harder to converge possibly, and certainly longer to run) and based on the stokes number I suspect the effect of parcticles on the fluid will be reasonably small - of course, best to test that. But I would opt for the simpler 1-way before moving to DDPM for sure.

dear Cees,
I checked the solution using one way coupling but I'm afraid the results was completely wrong! |:
I'm studying the particle distribution after bends and the difference between one way and exp. results is too much,
what do you think? shall I switch to 2-way coupling?
what do you suggest me for convergence problem in 2-way?

[amin.z]

Originally Posted by hwet

 after each DPM Iteration, the residuals jump and they didn't decrease enough till next one

I suppose this is just transient behavior and is what happens in a transient simulation, the residuals should "jump" at every time step and then converge and then jump again for the next time step.

Also, did you get a converged solution first for the gas phase before injecting in the particles? probably, that is the way to go.

actually I'm running it using steady solver, so it's not possible to control the stability and convergence using time step size,

yes, the solution converges using one phase and whilst I ran it using one-way coupling, the residuals converged to 1e-11!

[hwet]

actually I'm running it using steady solver, so it's not possible to control the stability and convergence using time step size,

I cannot make much sense of it so can't summarize what I want to say, but I think you can find the answer to this in section 24.2.2 Steady/transient treatment of particles in the Ansys fluent users guide.

A part of the explanation from the users guide is below:

In the Discrete Phase Model Dialog Box (p. 1998) you have the option of choosing whether you want to
treat the particles in an unsteady or a steady fashion. This option can be chosen independent of the
settings for the solver. Thus, you can perform steady state trajectory simulations even when selecting
a transient solver for numerical reasons. You can also specify unsteady particle tracking when solving
the steady continuous phase equations.

[CeesH]

Hi Amin,

It can of course be the case 1-way coupling does not work, but it is a good test I think for comparison. Another reason why it may not work is that the discrete random walk for turbulence does not work well in wall-bound flows where turbulence is largely non-isotropic. (For more, check papers by Dehbi on continuous random walk for example).

Anyway, when you go for 2-way coupling, make sure the timestep is short enough for convergence!

[amin.z]

Originally Posted by hwet

I cannot make much sense of it so can't summarize what I want to say, but I think you can find the answer to this in section 24.2.2 Steady/transient treatment of particles in the Ansys fluent users guide.

A part of the explanation from the users guide is below:

Thanks dear hwet for the piece of the manual, logic of transient/steady in DPM is pretty complex

[amin.z]

Originally Posted by CeesH

Hi Amin,

It can of course be the case 1-way coupling does not work, but it is a good test I think for comparison. Another reason why it may not work is that the discrete random walk for turbulence does not work well in wall-bound flows where turbulence is largely non-isotropic. (For more, check papers by Dehbi on continuous random walk for example).

Anyway, when you go for 2-way coupling, make sure the timestep is short enough for convergence!

Hi dear friend,

Thanks for the paper, I'll peruse it, I checked the solution with 2-way, and the required time step is too small, around 1e-05, and, you see, it needs too much time for the domain to be steady, I guess it should be solved to at least 30 sec!
I might have to solve the problem steady, but there's no time step for steady solver,
Could you suggest me something if I want to solve steady?
I should mentioned quality of mesh is acceptable, I think good enough, It has more than 500,000 cells.

[CeesH]

I haven't got a lot of experience with steady particle tracking, but it seems to me this would be inherently 1-way coupled. As soon as the particle trajectories start influencing the fluid movement, this problem will become unsteady.

Are your convergence criteria too tight maybe? Do you check the residuals alone or also some global properties, such as average velocities and so. Maybe you don't need as deep convergence as you are striving for now, because I agree the timestep of 10^-5 is too small - and below what would even be necessary for DNS.

[amin.z]

I let the solution to run to 50,000 iterations with time step size of 1e-04, it converged in each time step, the convergence criteria was 1e-03 for each equation, which I believe it's not too tight at all, what do you think?
but the results are awful! dpm concentration is completely wrong! my time step size was small enough and the residual wasn't too big! but it's wrong!

[CeesH]

Well, the residuals are of course just a guideline to see where your simulation is going - they are not an absolute measure of convergence. It depends very much on your geometry and initial guess how much the residuals will drop before reaching satisfactory convergence. So purely on the level '10e-3' I can't conclude a lot, but typically they should indeed reduce more than that. Anyway, it would be good to monitor how, say, the average velocity or so develops throughout a timestep to see if it reaches a (near) steady value already.

Anyway, before drawing any conclusions, let's see where things could go wrong. Did you check the following?
- Did you do a mesh dependency study?
- Did you compare the single phase results with experimental single phase data? Do the velocity profiles agree? Do you have any information on the turbulence experimentally (say from LDA or PIV data) - whether or not turbulence is accurately captured by the SST model will matter a lot for the particle track random motion. So it would be good to know how accurate the single phase solution is.
- What is the turbulent Schmidt number? Do you have any info on that? The constant in the DRW-particle turbulence model (C = 0.15) is based on Sc_t = 0.7; if your Schmidt number changes, so does C.

If you checked all of those things and they do work out well, there is still the option that the physical models associated with tracking don't work out well. As said, the DRW model does not behave properly in non-isotropic turbulence and close to walls (where k and epsilon vanish, particles get no random kick anymore and 'stick' to the wall artificially as their velocity becomes 0). Perhaps the drag force and so are off; are your particles odd-shaped or widely distributed in size in reality?