Setting up the Models

Models define the primary variables of the simulation, including pressure, temperature and velocity, and what mathematical formulation will be used to generate the solution. In this example, the flow involves a turbulent, compressible, multi-component gas whose components are reacting chemically. The Segregated Flow model will be used together with the standard K-Epsilon turbulence model and the PPDF reaction model.

Open the Continua node, right-click on the Physics 1 node and select item Select models...

In the Physics Model Selection dialog, select the Stationary radio button in the Motion group box.

Select the Multi-Component Gas radio button in the Material group box.

The Physics Model Selection dialog will guide you through the model selection process by showing only the options appropriate to the initial choices made. Using the same technique as in the previous step:

Select Reacting in the Reaction Regime group box.

Select Non-Premixed Combustion in the Combustion group box.

Select Adiabatic PPDF in the Non-Premixed Combustion group box.

Select PPDF Equilibrium in the Ppdf Reaction group box.

Select Segregated Flow in the Flow group box.

Select Steady in the Time group box.

Select Turbulent in the Viscous Regime group box.

Select K-Epsilon Turbulence in the Turbulence group box.

Select Standard K-Epsilon in the K-Epsilon Turbulence group box.

Select High y+ Wall Treatment in the K-Epsilon High y+ Wall Treatment group box.

The Standard K-Epsilon model is preferable to the default Realizable Two-layer K-Epsilon model for this case because the near-wall mesh is too coarse to resolve the boundary layer properly. Two-layer models are not recommended for meshes without refined near-wall layers.

The Physics Model Selection dialog should look as shown below when you are done.

Note that the color of the Physics 1 node has turned from gray to blue to indicate that models have been activated.

Open the Physics 1 > Models node. The selected models now appear within that node.

In order to keep run times low, the mesh used in this tutorial is rather coarse. As a result, a solution can be obtained much faster if first-order convection term differencing is used for the momentum, PPDF and turbulence equations.

To change the differencing schemes, first select the Segregated Flow node.

In the Properties window, change the Convection property to 1st-order.

Repeat this process for the Adiabatic PPDF and Standard K-Epsilon nodes.

Save the simulation by clicking the

(Save) button.