Particle Deposition using the DPM

Hello everyone, today we will use this pipe geometry to get results of particle deposition. Please do not forget to create the basic name selections.

Now, using the measure tool, you can see the pipe diameter is 200 mm, and if you want to perform a parametric analysis, you can also use the pull tool for the pipe radius. Now let's go through the steps for creating the mesh. Import the geometry; no local sizes in this case.

You can use this set of parameters to create the surface mesh. Check the quality; you see the quality is good. Next, we describe the geometry as a single fluid domain. Update the boundaries, update the regions, now define the inflation layers properly.

And finally, create the volumetric mesh using poly elements. The quality also looks good. If you want to check the element distribution using clipping planes, and now you are ready to transfer the mesh to Fluent. In Fluent, let's begin with the General tab.

Remember to calculate the Reynolds number to choose the proper model in the setup; in this case, it is the default K-Omega SST. Now enable the DPM model. We will use the two-way coupling approach, and please use the shown setup.

This is high resolution; enable the equation model for post-processing, and double-check the tracking methods. Next, create the injection. The particles will be injected from the inlet. They are made of a different material with a uniform size distribution.

For this demo, I'm using that set of values where the flow rate depends on the volume fraction. Enable the dispersion model and type 10 or more for the number of tries. Click on OK and close the window.

In the material sections, you see the water liquid is selected and sand is created for the particles. Double-check that water is the material for the fluid domain. Now it is time for the boundary conditions. The inlet has a velocity profile to account for a fully developed turbulent flow.

You can use an equation that must be created using one or more expressions. Select escape in the DPM tab. The outlet boundary condition has a reference gauge pressure. Keep the defaults and select escape in the DPM tab as well.

For the walls, keep the defaults, but select the trapped boundary condition in the DPM tab. We must use the command line to avoid zeroed particle deposition when using high-order schemes with high-resolution tracking.

By default, Fluent reconstructs wall nodal velocities in a way that removes any velocity components pointing toward the wall. I recommend creating monitors to help define the steady state of the simulation, in addition to the residual plots.

In this case, I created a monitor for the inlet pressure and the average velocity in the domain. You can also create one to track the mass balance. Initialize with the hybrid method and check the velocity at the inlet. You must see the velocity profile. Now run the calculation.

Check the residuals plot and also the monitors you created before. At some point, all will converge to stable values. Once the simulation has converged, you can verify the monitor values are stable. Now generate and review some contour plots.

In this case, check the velocity in the Meridional plane, but focus mainly on the Accretion Rate, as it shows particle deposition. Additionally, you can plot particle tracking, and even create one scene to display multiple plots simultaneously. And that's all for today. Thanks for watching.