## Fluids

#### DPM or DDPM-DEM to model flow of water and sand particles in pipe ?

• almulhem_900
Subscriber

Hi everyone,

I'm trying to model the flow of water and sand in 3D pipe with three side openings ( perforations) as shown in the following picture. The three holes are marked with the letters (A,B,C) and the other side of the pipe near hole C is plugged. The first objective is to estimate how much sand will escape from each hole.

Case Parameters:

Inlet (velocity-inlet B.C) with velocity = 8.617 ft/sec and reflect DPM B.C

outlet (pressure outlet B.C) with 0 gauge pressure and escape DPM B.C

Sand Injection is at the inlet face at the same velocity of the fluid (8.617 ft/sec) at flow rate of (22.4 lb/sec)

I'm having difficulty to get a converged solution using DPM without DEM collision and with steady particle tracking. Allowing DEM collision and tracking the particle in unsteady mode seems to be easier to get a converged solution but I have not gotten any yet.

Here are some questions I have:

- With such dense particle concentration will the DPM work ? or it is still considered to be a dilute fluid ?

- How can I model this problem using DDPM-DEM ? is the right model to handle such case ?

- Any tips to reach a convergence ( particle time step size, number of time steps, tracking parameters, Parcels, etc.... )

• Karthik R

Hello,

To answer your question in general terms - DPM generally works well when your dispersed phase is dilute (volume loading ~ 10%). In case of DDPM, this volume loading is much larger and the model is preferred for modeling particulate flows. A note of caution - DDPM takes into account particle-particle collision and there are really two different approaches - 1. using kinetic theory of grannular flow (KTGF), and 2. Discrete element modeling. KTGF models particle-particle interaction using an approximate grannular theory while DEM explicitly resolves these particle-particle interactions.

Regarding steady vs. unsteady particle tracking, please take a look at this screenshot below (ref - Fluent Users Guide, R18.2, Chapter 23: Modeling Discrete Phase).

Please use this information to select a modeling approach based on the problem you are attempting to solve.

Thank you.

Best Regards,

Karthik

• almulhem_900
Subscriber

I'm currently trying to run DEM with interaction between fluid and particles and it automatically switches to unsteady tracking. The question is how can I tell Fluent to simulate particles using DDPM? is there any specific button/window to enable it or DDPM is active when DEM collision model is selected? .

Please see below snapshots of an attempt to run DEM for the above problem.It is a very slow simulation. Is that normal for the case parameters? any suggestions/tips to make the case faster and reach convergence ? this case has been running for around 6 hours so far.

• DrAmine
Ansys Employee

To use DDPM you need to enable it under Multiphase Panel (as It a hybrid approach). Then in the injection panel check if the "Discrete Phase Domain" corresponds to the DDPM (secondary) phase

Ansys Employee

Hi,

Here is ddpm option.

Regards,

Keyur

• almulhem_900
Subscriber

Thank abenhadj and kkande for pointing out the DDPM in the Eulerian model.

I forgot to mention that I'm interested to model particles in the Lagrangian approach as indicated in the below table:

• DrAmine
Ansys Employee

Either KTGF or DEM for particle particle interactions within the DDPM  framework. The particles are tracked by solving ODE's as you want.

• almulhem_900
Subscriber

Thanks Amine,

Are both KTGF and DEM with DDPM framework you are referring to are using Lagrangian ? Can you show me where can I specify those models?

Best regards,

Abdul

• Karthik R

Hello,

Yes, both are lagrangian. If you are interested in the difference, please refer to my previous post.

Enabling KTGF: This can be done from the secondary phase. Please see the screenshot below.

Enabling DEM: DEM can be enabled from the Discrete phase options under Models. Select DEM collisions from Physical Models. Please see the attached screenshot.

I hope this helps.

Best Regards,

Karthik

• almulhem_900
Subscriber

Here is a DPM case that I'm trying to solve.

I get a convergence when I use a 0.15 lb/sec mass flow rate as shown below:

When I increase the mass flow rate to 1.5 lb/sec (at iteration 1500), the solution does not converge and I get "floating point exception" as shown below:

This is the way I setup the DPM:

Can someone help me with solving this issue ?

• DrAmine
Ansys Employee

Switch on update DPM source every iteration, increase number of continuous iterations per DPM and reduce DPM Underrelaxation and run for much more iterations: first steps to sort problems out.

ps: even the case at low loading the run is not converging at all from residual perspective

• almulhem_900
Subscriber

Thanks Amine.

This is the status of an ongoing re-run of the high loading particles (1lb/sec) with the parameters you suggested. I'm using a 0.3 underrelaxation for DPM.

it is now around 35k iterations and still there is no convergence. Do you think it needs more iterations to converge ?

The following snapshot is for the early time. 0.15 lb/sec particle flow rate until 2000 iterations. is this still not converged for the low loading using 1e-3 residual criteria ?

Thanks again and best regards,

• DrAmine
Ansys Employee

That is kind of non-converging case. Can you please describe a bit your case and share with us all information regarding boundaries, settings and co?

• almulhem_900
Subscriber

Hello Amine,

The case tries to simulate the flow of water + sand along a pipe that is plugged from the outlet side and perforated on the sides as shown below:

Pipe length: 1 ft

Pipe diameter: 4.3 in

Perforation diameter: 0.38 in

Quadratic Meshing (400k nodes) with program controlled inflation layer as shown below:

BC:

Inlet: velocity inlet with 2 ft/sec. DPM BC: reflect

Holes: outlet vent with 0 gauge pressure . DPM BC: escape

Plug: stationary wall DPM BC: reflect

Coupling:

DPM as shown below:

Let me know if you need additional info

Thanks,

Abdulraof

• DrAmine
Ansys Employee

How big is the particulate volume fraction? Can you make any estimation? Can you obtain a converged case without DPM?

• almulhem_900
Subscriber
It is around 7% volume fraction

I did obtain convergence without introducing particles
• DrAmine
Ansys Employee

So you need to find now a biasing between the DPM Source Terms URF and number of update.

You can run transient for enhanced stability. 7% Volume fraction at high mass loading requires the resolution of particle-particle interaction but you can tackle that stage after you are able to run a fine DPM run.

Are you accounting for buoyancy effects?

• almulhem_900
Subscriber

I'm eventually will use either DEM or DDPM to include particle-particle interaction.

Do you mean transient fluid flow or transient particle tracking ?

I think I'm not accounting for buoyancy yet.

Thanks

• DrAmine
Ansys Employee

Both: Transient flow with transient particle tracking. I guess your continuous flow implies a sort of swirl which affect the particles and the latter start consuming the TKE of the continuous flow and the mean energy.