Catalytic Converter Simulation

1. Workshop 11 ANSYS CFX 5.7 Catalytic Converter Simulation

2. Introduction • The catalyst material in the center region is a honeycomb structure upon which reactions take place • The honeycomb structure is too small to resolve in mesh; it is modeled with a flow resistance instead. • Focus: use of CFX to set up a flow simulation in ANSYS Workbench (this workshop is based on imported meshes; second focuses on CFX-Mesh) • Note: this is preview version!!! • Steps: • Preprocess in CFX-Pre, solve in CFX-Solver, and post-process in CFX-Post

3. Catalytic Converter Geometry First start the ANSYS Workbench...

4. Starting the CFX in Workbench • Common starting point for all ANSYS software • New Project – save explicitly to start! • Select New Simulation • Advanced CFD tab will open

5. Starting the CFX-5 Preprocessor • Simulation files have *.cfx extension • Create converter.cfx in your working directory • Click on Save to save the simulation file Copy the following mesh files to your working directory CatConvHousing.msh & CatConvMesh.gtm

6. Importing the Hex Mesh • You will first import a mesh for the central catalyst section (right mouse click) • The hex mesh was created in ICEM CFD Hex • Set the mesh format to ICEM CFD and browse to your working directory • Select CatConvHousing.msh, set the mesh units to cm, and click OK to import the mesh

7. Importing the Hex Mesh

8. Importing the Tet Mesh • You will now import a tetrahedral mesh created for the pipe and flange section • Set the mesh format to CFX-5 GTM file • Select CatConvMesh.gtm, and click OK toimport the mesh.

9. Transforming a Mesh Assembly • The second end section is identical to the first except that it has been rotated by 180 degrees about the center of the housing • You will copy and rotate the flange section you imported by 180 degrees about an axis parallel to the y-axis located at the center of the catalyst housing • In the Mesh Workspace, select Mesh Assembly 2 and right-mouse click to Transform… • This brings up the Mesh Transformation Editor • Ensure that the CFX-Pre working units are set to SI System. (Edit>Options>Common>Units)

10. Mesh Transformation Editor • Set the Transformation to Rotation and set Method to Rotation Axis • In the From boxes enter (0, 0, 0.16) • In the To boxes enter (0, 1, 0.16) • Under Angle, set the Option to Specified and Angle to 180 degrees • In order to prevent the transformed mesh from being deleted, enable the Multiple Copies toggle. Click OK to transform the mesh

11. Completed Transformation Transformed Mesh Original Mesh

12. Defining a Domain • Next we will define the fluid domain • Click Create, Flow Objects and select Domain. • Call the Domain “CatConv” • Click Ok to Edit the Domain

13. Defining a Domain • On the General Options Panel on the Domain form: • Click in the Location box and hold the <CTRL> key down and select all three mesh assemblies (Assembly, Assembly 2, Assembly 3) • Set the Fluids List to Air Ideal Gas • Set the Reference Pressure to 1 atm • On the Fluid Models tab: • Set the Heat Transfer ModelOption to Isothermal and set the Fluid Temperature to 600 K. • Leave all other values at their default and click OK to apply the form

14. Defining a Subdomain • The catalyst-coated honeycomb structure will be modeled using a subdomain with a directional source of resistance. • For quadratic resistances, the pressure drop is modeled as: • To create a subdomain, click on the Subdomain icon from the main toolbar • Set the Name to Catalyst and click OK. • On the Basic Settings Panel, set the Location to Assembly and then click the Sources tab

15. Setting a Quadratic Resistance • On the Sources panel: • Turn on Sources, Momentum Source/Porous Loss, and Directional Loss Model • Under Streamwise Direction, set the Option to Cartesian Components and set: • X Component to 0 • Y Component to 0 • Z Component to 1 • Under Streamwise Loss, set the Option to Linearand Quadratic Coefs • Turn on Quadratic Coefficient and enter a value of 650 kg/m^4 • Click OK to create the subdomain • To create a subdomain, click on the Subdomain icon from the main toolbar • Set the Name to Catalyst and click OK. • On the Basic Settings Panel, set the Location to Assembly and then click the Sources tab

16. Inlet Boundary • Next, we will create inlet and outlet boundary conditions to the fluid domain • Create a boundary condition called “inlet” • Set the Boundary type to Inlet and the location to PipeEnd 2. • On the Boundary Details panel, set the Option to Normal Speed and set a value of 25 m/s. Apply the form.

17. Outlet Boundary • Create a boundary condition called “outlet” • Set the Boundary type to Outlet and the location to PipeEnd. • On the Boundary Details panel, set the Option to Static Pressure (not Average Static Pressure)and Relative Pressure to 0 Pa. Apply the form.

18. Boundary Conditions

19. Domain Interfaces • Domain interfaces are also used to join dissimilar meshes together. You will need to create GGI interfaces between the inlet pipe section mesh and the catalyst housing and between the catalyst housing and the outlet pipe section • Click on the Domain Interfaces iconand set the name to InletSide • On the Basic Settings panel, set the Interface Type to Fluid Fluid. • Set the Side 1 Filter to All Domains and select FlangeEnd 2 in Region List 2 • Set the Side 2 Filter to All Domains and select INLET in Region List 1 Click Ok to apply the form.

20. Domain Interfaces • Similarly create a second domain interface named OutletSide • Set the Side 1 Filter to All Domains and select FlangeEnd in Region List 1. • Set the Side 2 Filter to All Domains and select OUTLET in Region List 2. Click Ok to apply the form.

21. Domain Interfaces

22. Initialisation • Click on the Global Initialisation icon • You will set a guess for the initial velocity based on uniform flow through the catalyst housing. If the inlet velocity is scaled by the ratio of areas between the inlet pipe and housing cross-section, a value of approximately 2 m/s results • Under Cartesian Velocity Components, set the Option to Automatic with Value. Set U and V to 0 m/s and W to –2 m/s (flow goes through in the –z direction) • Toggle on Turbulence Eddy Dissipation and leave the Option as Automatic. Apply the form.

23. Solver Settings • Click on the Solver Control icon • Set a Physical Timescale of 0.04 s and set the Maximum Number of Iterations to 100 • Click Ok to apply the form

24. Writing a Definition File • Select the Write a Solver File icon • Set File Name to converter.def. • Set Operation to Start Solver Manager. • Turn on report Summary of Interface Connections • Press OK • A report of the GGI interfaces you created will be displayed. Click OK in the information window. • Exit Pre and Click Yes on Save Changes window to save the cfx file

25. Defining the Run • When the Define Run formcomes up click the Start Runbutton to start the run.

26. Monitoring Convergence

27. Launching CFX POST • Click on ‘Post Process’ icon • Choose to shut down the Solver Manager and click OK to launch CFX – Post with the current results file

28. Viewing the Domain Interfaces • Turn off visibility of the Wireframe. • Make InletSide Side CatConv Part 1 visible and double-click it in the list.

29. Viewing the Domain Interfaces Under the Render tab, turn on Draw Lines and color the lines red. Turn off Draw Faces and click Apply Repeat these steps for InletSide Side CatConv Part 2 but color the lines green. Orient the view as shown on the next slide to see the interface between the dissimilar meshes clearly. Turn off visibility of the interface boundaries and toggle visibility of the Wireframe back on

30. Viewing the Domain Interfaces

31. Creating a Slice Plane • Click on the Create Plane icon in the main tool bar • Create a ZX plane through Y = 0 and color the plane according to Pressure. You can see the pressure falls steadily through the housing. • Make the plane invisible and create a vector plot on it. The flow through the housing is uniform as expected although there is some separation where the inlet pipe expands into the flange.

32. Creating a Polyline • Make the vector plot invisible • You will create a polyline to plot the pressure as a function of the z coordinate. • Click on the polyline icon from the main toolbar and accept the default name. On the form, set the Method to Boundary Intersection. • Set the Boundary List to CatConv default, inlet and outlet (hold the <CTRL> down for multiple select) • Set Intersect With to Plane 1 • Click on the Color tab and choose a bright color for the polyline. Click on the Render tab and increase the Line Width to 3. Apply the form.

33. Creating a Chart • You will create a chart to plot the pressure as a function of the z coordinate on the polyline you just created. • Click on the chart icon from the main toolbar and accept the default name. • Set the X Axis to Z and the Y Axis to Pressure • Click Apply. • You can see that the pressure drops linearly through the main body of the housing due to the resistance of the catalyst.

34. Exporting Data • From the Main Menu select File/Export. • Make sure that Export Geometry Information is toggled on. This will cause X, Y, and Z values to be sent to the output file. The connectivity information could be used to create a file that you could read back in as a polyline. • Select Pressure in the Select Variable(s) list. • Click the Formatting tab and set the Precision to 3. • Click Save to export the results. The file export.csv will be written to the current working directory. You can view this file in any text editor.