The material properties of the sand particles used in the simulation need to be defined. Heat transfer and radiation modeling are not used in this simulation, so the only properties that need to be defined are the density of the sand and the diameter range.

To calculate the effect of the particles on the continuous fluid, between 100 and 1000 particles are usually required. However, if accurate information about the particle volume fraction or local forces on wall boundaries is required, then a much larger number of particles must be modeled.

When you create the domain, choose either full coupling or one-way coupling between the particle and continuous phase. Full coupling is needed to predict the effect of the particles on the continuous phase flow field but has a higher CPU cost than one-way coupling; one-way coupling simply predicts the particle paths during postprocessing based on the flow field, but without affecting the flow field.

To optimize CPU usage, you can create two sets of identical particles. The first set should be fully coupled and around 200 particles will be used. This allows the particles to influence the flow field. The second set uses one-way coupling but contains 5000 particles. This provides a more accurate calculation of the particle volume fraction and local forces on walls. (These values are defined in the inlet boundary definition.)

For this tutorial you will create a "Sand Fully Coupled" boundary condition that has 200 particles moving with a mass flow rate of 0.01 kg/s and a "Sand One Way Coupled" boundary condition that has 5000 particles moving with a mass flow rate of 0.01 kg/s. In both cases the sand density is 2300 [kg m^-3]; particle diameters range from 50 e-6 m to 500 e-6 m, with an average diameter of 250 e-6 m and a standard deviation of 70 e-6 m. You will set a Finnie erosion model with a velocity power factor of 2 and a reference velocity of 1 m/s.

Set up an environment that has water and sand defined in two ways; one in which the sand is fully coupled, and one in which the sand is one-way coupled:

In previous tutorials you have often defined a uniform velocity profile at an inlet boundary. This means that the inlet velocity near to the walls is the same as that at the center of the inlet. If you look at the results from these simulations, you will see that downstream of the inlet a boundary layer will develop, so that the downstream near wall velocity is much lower than the inlet near wall velocity.

You can simulate an inlet more accurately by defining an inlet velocity profile, so that the boundary layer is already fully developed at the inlet. The one seventh power law will be used in this tutorial to describe the profile at the pipe inlet. The equation for this is:

(11–1)

where is the pipe centerline velocity, is the pipe radius, and is the distance from the pipe centerline.

You can create a non-uniform (profile) boundary condition by doing one of the following:

Use a CEL expression to define the velocity profile for the inlet boundary:

Set up the initial values to be consistent with the inlet boundary conditions:

An important consideration in this simulation is erosion to the pipe wall and valve due to the sand particles. A good indication of erosion is given by the Erosion Rate Density parameter, which corresponds to pressure and shear stress due to the flow.

Set the user specified range for coloring to resolve areas of stress on the pipe wall near of the valve:

Default particle track objects are created at the start of the session. One particle track is created for each set of particles in the simulation. You are going to make use of the default object for Sand Fully Coupled.

The default object draws 25 tracks as lines from the inlet to outlet. The Info tab shows information about the total number of tracks, the index range, and the track numbers that are drawn.

The following steps describe how to create a particle tracking animation using Sweep Animation. Similar effects can be achieved in more detail using the Keyframe Animation option, which allows full control over all aspects on an animation.

On the outlet boundary you created in CFX-Pre, you set the Average Static Pressure to 0.0 [Pa]. To see the effect of this:

The geometry was created using a symmetry plane. In addition to the Reflect/Mirror option from the shortcut menu, you also can display the other half of the geometry by creating a YZ Plane at X = 0 and then editing the Default Transform object to use this plane as a reflection plane.

When you have finished viewing the results, quit CFD-Post.