Hi

I am running DPM simulation using KE model, segregated solver, two way coupled calculation and Stochastic model.

I have had problems with convergence so have set the Max no. of steps to 10000 and a length scale of 0.00001. Also I have increased the continious phase calculations per DPM to 1000. Is this too high and what are the physical implications (if any) of doing so?

I specify a 1000 particles as a group in the injections menu however when I run fluent it is only recognising half this amount: "Number Tracked=500 Number Escaped= 500......"

and error message: "Unable to locate injection-0, number 500 Unable to locate injection-0, number 501 Unable to locate injection-0, number 502 Unable to locate injection-0, number 503.........."

When I try a surface injection at the inlet it only recognises 2 particles. Does anyone have any suggestions?

Additionaly I have noticed that the residuals increase dramitically at the point of injection and then fall again until the the next one, is there a minimum number of injections that the solution has to process for the result to be accurate as I have had a converged solution after just 1 injection previously.

Thanks in advance

For coupled calculations the mass f/r must be relatively small compared with gas phase (<10%) If higher Fluent recommends to use Multiphase models. The continuous phase per DPM shouldn't be as high as 1000, I actually use 1, although coarse it fits my case.\ Also for group injections you have to define the location of injection at x,y,z.

For surface injections no. of particles = no. face cells on the surface x no. stochastic tries.

If you use R-Rammler distribution in surface, the no. particles increase by the product of the number of diameter bins.

''''I have had problems with convergence so have set the Max no. of steps to 10000 and a length scale of 0.00001. Also I have increased the continious phase calculations per DPM to 1000. Is this too high and what are the physical implications (if any) of doing so?''''

If you specify max no. of steps 100000 and leave length scale as default, it should be fine. Make sure that in any case, you don't have any particle fate with incomplete. As Kiao said, DPM iteration per every 1000 contineus pahse iteration is too high. Also, DPM iteration per every contineous phase iteration may be computationally expensity, however, depends on number of cells you use. But default of DPM iteration per 10 gas phase iteration worked well in my case and should be good. What does it physically mean? It means that you have enabled two way coupling. This way it accounts for the gas phase turbulence on the particle phase and particle phase turbulence dispersion on the gas phase if you have enabled stochastic tracking.

Regards -US

Thanks for your responses, I shall try again with what you have suggested.

Hi again, I have another question; when using the surface injection how can I tell Fluent the number particles that I require in the injection? There doesn't appear to be any option for this but on group injections is available.

Thanks

Hi again, I have another question; when using the surface injection how can I tell Fluent the number particles that I require in the injection? There doesn't appear to be any option for this but on group injections is available.

Thanks

In the case of surface injection you don't explicitely mention the number of particles. Fluent takes number of particles depending on the number of face elements on the injection surface.

When you use single sized particles, No. of particles = no. of face elements on the injection surface

When you use multisize particles,

No. of particles = no. of face elements X no. of bins in your particle size distribution that you input

Now, if you are using two-way coupling and hv enabled stachastic tracking with DRW then,

No. of particles that fluent tracks is,

(No. of particles from any of above two definition)(No. of stochastic tracking)

regards, -US

I'm actually working on injections now and have a problem setting the RRammler distn for surface injection. Initial settings was for a uniform size which worked fine. However when I switch over to R-Rammler distn sizes, the particles don't complete their path and in the report Fluent says they evaporated!! But I didn't set any energy laws. I am using the realizable k-e turbulence with enhanced wall treatment. Is it this??

I set the flow rate of the injection to 1e-6 kg/s for water particles, do i need to "set the scale flow rate by face area" for a distributed set?

Any suggestions please....

Can't tell why the droplets should evaporate.

If the injection surface has different sized elements, then it is a good idea to set the scale flowrate by face area. I am not sure how it would change the evaporation thing.

I used inert particles for my study and don't hv any direct experience with water droplet particles and its physics. So can't really tell about evaporation thing.

Regards -US

Actually i think i resolved it. I changed the mass flow rate. Considering the number of droplets (9600) my flow rate wasn't sufficient to allow that amount of droplets to be released so I increased it to a value above the 9600 particles of water droplets and it worked out!!!

Oh now i have another query. When I go for the coupling solution, I initially solve the continuous phase until it converges. I then define my injections and discrete phase model panel settings. I iterate once more and it converges immediately as i set my coupling with continuous phase = 1.

However if I iterate again, to make sure it really did converge, the residuals jump up and then I see the dpm actually being coupled but it never converges back to where it was.

why is this?

One thing is, you need to run enough iterations for both the gas and discrete phase and that untill you get steady residue. The solution is converged with 1 iteration of DPM is not the message for coupled solution. It is for previously converged gas phase solution. It is normal that residue jumps right when you start your coupled solution. But then it should start converging.Continue coupled calculation untill good residue.

I also had problem of convergence once DPM is activated. It didn't come to the value where only gas phase residue reached. Do you find your residue ups and down consistently between certain range(for coupled solution)? What i understood, it is bcs of contineous momentum exchange between gas and particles through drag term in momentum. Those jumps could be made more smooth with increasing number of particles through more stachastic tries. Finally, make sure that you have statisticaly correct results.

Regards, -US

Thanks for confirming my thoughts. I have been on this problem for days. I was getting fluctuations on the residuals and it wouldn't converge but I changed the mass f/r so that it was equal to no.particles x mass of one particle and this worked (I also increased my stochastic tries from 10 to 20 initially but this didn't help). I think you are right about the continuous momentum exchange because if there is too much mass the momentum exchange calculations are messed up. Thanks for your help.

[NH_Aus]

Originally Posted by kiao
;121597

Thanks for confirming my thoughts. I have been on this problem for days. I was getting fluctuations on the residuals and it wouldn't converge but I changed the mass f/r so that it was equal to no.particles x mass of one particle and this worked (I also increased my stochastic tries from 10 to 20 initially but this didn't help). I think you are right about the continuous momentum exchange because if there is too much mass the momentum exchange calculations are messed up. Thanks for your help.

--
Pls increase the mass flow of particulate slowly

[jalay]

Hello All,
I am making a simulation of hydrogen gas diffusion in lab.to know what will be the region where the hydrogen mass will be floating?
i have a doubt that if give go for injection of gas and give its velocity there by surface, do we have to give mass flow rate in BC? or else it will understand by itself?
And hydrogen gas is not in material list. how can i give hydrogen gas as injection ?