Catalytic Converter Simulation

1
Catalytic Converter Simulation

• Workshop 11
• ANSYS CFX 5.7

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.
(EditgtOptionsgtCommongtUnits)
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
ltCTRLgt 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 Model Option 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 Linear and
Quadratic Coefs Turn on Quadratic Coefficient and
enter a value of 650 kg/m4 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 ltCTRLgt 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.