1. Workshop 4 Flow Through Porous Media
Introduction to CFX
Pardad Petrodanesh.Co
Lecturer: Ehsan Saadati

2. 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.

3. 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

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

5. 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

6. 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]

7. 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

8. 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.

9. 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
Insert a new object in the same way called Pressure Drop, using the Expression:
Click OK
Right-click
massFlowAve(Total -massFlowAve(Total

10. 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

11. 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

12. 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

13. 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

14. Post-processing Switch to the Expressions tab
Right-click and select New
Enter the Name as deltaP and enter the Definition as: massFlowAve(Total - massFlowAve(Total
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.