Workshop 4 Flow Through Porous Media Introduction to CFX

Introduction This workshop demonstrates how to model porous media in CFX. It models a catalytic converter. Nitrogen flows in through the inlet with a uniform velocity of 10 m/s, passes through a ceramic monolith substrate with square shaped channels, and then exits through the outlet. The substrate is impermeable in the X and Y direction, which is modeled by specifying loss coefficients 2 orders of magnitude higher than in the Z direction. Ceramic Monolith Substrate I’d like to remind everyone that some matters that will be discussed during this presentation may constitute forward-looking statements that involve risks and uncertainties, which could cause actual results to differ from those projected. In addition, I would also like to mention that we will not be able to discuss or answer any questions regarding previously provided guidance, as our Company policy is that we only comment on company guidance in a public forum.

Starting CFX-Pre Start Workbench and save the Project as cat_converter.wbpj Drag CFX into the Project Schematic from the Component Systems toolbox and name the system Porous Start CFX-Pre by double clicking Setup When CFX-Pre opens, right-click Mesh and select Import Mesh > ICEM CFD. Select the file catconv.cfx5 Keep the Mesh Units in m

Material Import Right-click Materials and select Import Library Data Select N2 Ideal Gas by expanding the Calorically Perfect Ideal Gases branch Click OK

Fluid Domain Setup Double-click Default Domain For Fluid 1, set the Material to N2 Ideal Gas (note: use the icon) Switch to the Fluid Models tab Set Heat Transfer to Isothermal Set Fluid Temperature to 450 [C] Set Turbulence to k-epsilon Click OK

Setting Up Boundary conditions Insert a boundary condition named Inlet Set Boundary Type to Inlet Set Location to INLET Switch to the Boundary Details tab Set Mass and Momentum to a Normal Speed of 10 [m s^-1] Click OK Insert a Boundary Condition named Outlet Set Boundary Type to Outlet Set Location to OUTLET Enter a Relative Pressure of 0 [Pa]

Setting Up Porous Domain Right-click on Flow Analysis 1 and insert a Domain named Substrate Set the Location to SUBSTRATE Set the Domain Type to Porous Domain Switch to the Porosity Settings tab Set Volume Porosity to 0.5 Set the Loss Model option to Directional Loss For the Streamwise Direction, enter components of 0,0,1 Set Streamwise Loss to Linear and Quadratic Resistance Coefficients Turn on Quadratic Resistance Coefficient and enter a value of 440 [kg m^-4] Set the Streamwise Coefficient Multiplier to 100 and click OK

Domain Interface CFX automatically creates a Fluid-Porous interface between the Default Domain and Substrate. You can double-click Default Fluid-Porous Interface to view the setup, or highlight the Default Fluid Porous Interface Side 1 and Default Fluid Porous Interface Side 2 boundaries in the individual domains to see that that regions are correct.

Output Control Edit Output Control from the Outline tree Switch to the Monitor tab and turn on Monitor Options Click to create a new monitor object, and call it Mass Flow at Outlet Set the Option to Expression Set the Expression Value to massFlow()@Outlet Insert a new object in the same way called Pressure Drop, using the Expression: Click OK Right-click massFlowAve(Total Pressure)@REGION:INLETSUBSTRATEINTERFACE_1 -massFlowAve(Total Pressure)@REGION:OUTLETSUBSTRATEINTERFACE_1

Starting Solver Close CFX-Pre and save the project Double-click Solution to start the Solver Manager When the Solver Manager opens click Start Run At the end of the run, click the User Points tab and click the green line where it flattens out. It reports a pressure drop value of approx 285 Pa across the substrate

Post-processing When the solver finishes, close the Solver Manager Double-click on Results in the Project page to start CFD-Post Once CFD-Post is open, select Location > Plane from the toolbar Set Method to ZX Plane Set Y to 0 [m] Click Apply Turn off Visibility for Plane 1 by disabling the check-box next to its entry in the Outline tree Select Insert > Vector Select Locations to Plane 1

Post-processing Hide the Vector plot created in the last step Select Insert > Contour Set Locations to Plane 1 Set Variable to Pressure Click Apply

Post-processing Select Location > Line from the toolbar Set Point 1 to 0,0,-0.07 Set Point 2 to 0,0,0.07 Click Apply Select Insert > Chart On the General tab enter Pressure in Porous Domain as the Title On the Data Series tab, click to create Series 1 Set Location to Line 1 On the X Axis tab, set Variable to Z On the Y Axis tab, set Variable to Pressure

Post-processing Switch to the Expressions tab Right-click and select New Enter the Name as deltaP and enter the Definition as: massFlowAve(Total Pressure)@Inlet - massFlowAve(Total Pressure)@Outlet Click Apply to evaluate the expression The value should come out to be approximately 300 Pa. Since we know from the solver monitor value that approx. 285 Pa or Total Pressure is lost across the substrate, we can determine that 15 Pa is lost through the rest of the device.