CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   DPM converging Problem (

Markus Alzon May 29, 2007 02:14

DPM converging Problem

I have a problem in setting up a simple DPM Simulation. The Problem is, that the residuals of the continuity and also of all velocities do not converge.

I read several threads in this forum, but no advice given here could solve my problem.

Very interesting to me was the tutorial about modeling an evaporating liquid spray. After the initial and steady state solution, one was advised the unset the convergence check and do more 200 timesteps. As I did so too, the residuals were growing too and didn't fall towards zero. So, what I'd like to ask now, if it is normal that the residuals do not converge when using a dpm-model (maybe I made something wrong in this tutorial?)?

And is there a standard approach for setting up a liquid spray in a gas phase, to ensure the stability of the calculation? Or in another way: which steps should I first do to solve my converging problem?

I hope you could answer my questions, I am pretty new to Fluent. And I would be glad if you could give me a hint.

Thanks in advance,


A A S May 29, 2007 13:32

Re: DPM converging Problem
I have had problems myself.

My residuals would fall to about an order of magnitude above the convergence criteria and stay there indefinately without changing. If your solution is stable, I suggest doing a mass and heat flux balance and checking grid independance. Those two are sufficient for a "converged solution."

Sujith May 29, 2007 15:20

Re: DPM converging Problem
There will be convergence issues with DPM model as it creates source terms in the continuous phase. After 1 DPM iteration the momentum, energy etc of the particles are exchanged to the continuous phase as the respective source terms. This results in a sudden change in the solution equilibrium and there will be a residual jump. If the source terms are very high, you should increase the number of continuous phase iteration per dpm iteration so that the continuous phase converges after every DPM iteration. If there is still convergence trouble decrease the URF of DPM sources or try with a decreased DPM mass flow rate. Also remember that the DPM model is valid only under some conditions like very low volume loading...

Markus Alzon May 30, 2007 01:06

Re: DPM converging Problem
Hello out there, I changed now my particles from droplets to inert particles (I did this before I read your advices). So by that, evaporation should be excluded (am I right?). And with this, my calculation is now running since yesterday.

So, it seems that you both are right.

About the grid: I have a very simple grid, and of course set the cell-volumes (compared with one droplet of maximum-size) not too low. However, what if in one cell not only one particle comes but, but many, so that they together occupy more than 10% of the cell-volume (or a parcel has too many droplets)? Would be this a break of the rule-of-thumb?

I hope you understand my question.

Thank you for your postings. It helped me to understand the DPM-Concept more.

Greetings from Japan,


Sujith May 30, 2007 14:56

Re: DPM converging Problem

In fluent DPM approach particles are considered as point masses which exchanges property with the continuous phase in the cell in which the particle is currently located. So the volume of particle does not pose a hindrance to the continuous phase flow.

In the above case if the particles are clustered together in a single cell, the volume of particles are definitely going to affect the continuous phase flow and as Fluent neglects this fact, the results wont be as accurate as the actual physics...

But in usual simulations this kind of situations are least expected and the DPM is used if conditions are met in a global sense. The clustering of particles is usually avoided by particle dispersion techniques like discrete random walk model or stochastic tracking etc..


A A S June 5, 2007 14:19

Re: DPM converging Problem
Thanks for the information Sujeth, even though I didn't pose the original question, what you provided is fairly practical for my simulations as well.

Cheers AAS

All times are GMT -4. The time now is 10:31.