1. Download SimFlow
SimFlow is a general purpose CFD Software
To follow this tutorial, you will need SimFlow free version, you may download it via the following link:
Download SimFlow
2. Create Case
Open SimFlow and create a new case named catalytic_converter
Go to New panel
Provide name catalytic_converter
Click Create Case

3. Import Geometry
Firstly we need to Download GeometryCatalytic-converter
Click Import Geometry
Select geometry file catalytic-converter.stl
Click Open to import geometry

4. Imported Geometry Units
Since the imported geometry is in STL format, which does not store unit information, we need to confirm the unit in which the model was created. In the selection of unit, we can use the Geometry size label, which displays overall size of the model in each direction. In our case, the model was created in millimeters.
Select mm unit
Press OK button

5. Geometry - Catalytic Converter
After importing geometry, it will appear in the 3D window.
Click Fit View to zoom in on the geometry

6. Split Geometry - Catalytic Converter (I)
The imported geometry is made up of a single surface. We need to split it into multiple faces for further processing.
Expand the Options list for catalytic_converter
Select Split

7. Split Geometry - Catalytic Converter (II)
In order to split original geometry into separate objects, we will disable Create Single Geometry options:
Uncheck Create Single Geometry
Click Split

8. Rename Geometries
To make the resulting mesh boundaries more readable we will rename each geometry face:
Select catalytic_converter_patch00 from the list. The selected face will be highlighted in the 3D graphic window
Double click on the name and change it to match the picture below
catalytic_converter_patch00 \(\rightarrow\) inletRepeat these steps for the remaining geometry components
catalytic_converter_patch01 \(\rightarrow\) outlet
catalytic_converter_patch02 \(\rightarrow\) wall

9. Create Geometry - Cell Zone
In this tutorial, we would like to model a porous zone inside the catalytic converter. To do so we need to define the region where the porous resistance will be applied. For this purpose we will create new box geometry:
Click on Create Box
Set the origin and box dimensions accordingly
Origin \({\sf [m]}\)-0.085-0.06-0.09
Dimensions \({\sf [m]}\)0.1750.120.18

10. Meshing Properties - Catalyctic Converter
In order to create the mesh, we need to specify geometries options used during the meshing process.
Go to Hex Meshing panel
Enable Mesh Geometry on the inlet outlet wall
Enable Create Boundary Layer Mesh on wall geometry
Click on the wall in the listto expand options
Set No. Of Layers to 4

11. Base Mesh - Domain
Now we will define the base mesh. The box geometry determines the background mesh domain. The model is symmetrical on the XZ plane, so we do not need to mesh the whole geometry. Using the box dimensions we will choose only half of the domain.
Go to Base tab
Click on Autosize
Change Max [m] Y to 0
Define the number of divisions
Division1551750

12. Material Point
Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. Since we are considering flow inside the catalytic converter we need to place the material point inside the geometry.
Go to Point tab
Specify location inside the catalytic converter geometry
Material Point0-0.020
You can specify the point location from the 3D view. Hold the CTRL key and drag the arrows to the destination.

13. Start Meshing
Everything is now set up for meshing
Go to Mesh tab
Start the meshing process with Mesh button

14. Mesh
After the meshing process is finished the mesh will appear in the graphics window.

15. Create Cell Zone (I)
Now we will define the cell zone using box_1 geometry.
Expand the Options list next to default region
Select Add Cell Zones

16. Create Cell Zone (II)
Check the box_1
Click on Create Cell Zones

17. Display Cell Zone
The cell zone appears inside the catalytic converter. It is colored on light blue.

18. Boundaries
Change boundary name from boundaries \(\rightarrow\) symmetry
Define boundary types accordingly
inlet Patch
outlet Patch
symmetry Symmetry
wall Wall

19. Select Solver - SIMPLE
We want to analyze internal, incompressible turbulent flow. For this purpose, we will use the SIMPLE (simpleFoam) solver.
Go to SETUP panel
Enable Steady State filter
Filter the solvers by Incompressible flow
Pick SIMPLE (simpleFoam) solver
Select solver

20. Turbulence
For turbulence modeling, we will use the standard \(k-\varepsilon\) model.
Go to Turbulence panel
Select RANS for Turbulence Modeling

21. Transport Properties
We will change the kinematic viscosity to the value of the exhaust gas.
Go to Transport Properties panel
Set the kinematic viscosity
\(\nu\) \({\sf [\frac{m^2}{s}]}\)1.272e-04

22. Cell Zones - Porosity
In order to include porosity to our simulation we have to define porosity for the box_1 cell zone.
Go to Cell Cones panel
Select the box_1 zone
Check Porous Zone
Use default Darcy-Forchheimer model and set its parameters accordingly
d \({\sf [\frac{1}{m^2}]}\)3e-073e-103e-10
f \({\sf [\frac{1}{m}]}\)202000020000

23. Parameters - R, U
SimFlow allows users to create named parameters that can be used instead of numbers. This allows to easily change a single property without the need to edit all inputs where a given property is used. In this tutorial, we will define two global parameters that we will use during further setup.
Go to Parameters panel
Definethe new parameter
Name R Formula 0.025Click Create Parameter
Repeat these steps for the second parameter
Name U Formula 20
The newly created parameters will be shown in the parameters list.

24. Boundary Conditions - Inlet (Flow)
We will set inlet velocity as a parabolic profile. The profile we will define by the formula using U and R parameters. Velocity magnitude near the wall will be equal to zero and the highest value of U will be in the center of the pipe.
Go to Boundary Conditions panel
Select the inlet boundary
Set the Velocity Inlet character
Change the velocity type and value accordingly
U Type Fixed Value
U Value \({\sf [\frac{m}{s}]}\)U*( (R-sqrt(y^2 +z^2 ))/R)^(1/7)00

25. Save Case
To visualize and check velocity distribution we will open ParaView. Firstly we will save the case.
Go to RUN panel
Press Save Case button

26. Check Velocity Profile - ParaView (I)
Run the ParaView from the Postprocessing panel.
Go to POSTPROCESSING panel
Click on Run ParaView

27. Check Velocity Profile - ParaView (II)
We will display a velocity magnitude map on the inlet.
Make sure that catalytic_converter is selected
Press Apply
Uncheck Skip Zero Time
Press Refresh
Press Apply
Select velocity U from the list

28. Boundary Conditions - Inlet (Turbulence)
Back in SimFlow, we will also update the turbulent mixing length for the ε-equation at the inlet.
Go to Boundary Conditions panel
Select inlet boundary
Switch to Turbulence tab
Set the value of Mixing Length to 7% of inlet diameter
\(\varepsilon\) Mixing Length \({\sf [m]}\)0.07*2*R

29. Initial Conditions - Potential
In order to give a better initial guess for velocity and pressure fields, we will use the "Potential" initialization feature. This utility solves pseudo potential flow prior to actual calculations.
Go to Initial Conditions panel
Switch to Potential tab
Check the Initialize Potential Flow
Set No. of correctors to 10

30. Monitors - Boundary
We would like to monitor how results change during computation. We will enable plotting the average pressure at the inlet during the calculation:
Go to Monitors panel
Switch to Boundary tab
Expand Fields list next to inlet boundary
Check the pressure p

31. Monitors - Sampling
We will also display intermediate results on a section plane.
Go to Sampling tab
Add new Slice
Set the normal vector
Normal \({\sf [-]}\)010Expand Fields menu
Choose the pressure p and the velocity U to be sampled on the section plane

32. Run - Time Control
Go to RUN panel
Set the maximal Numbers of Iterations to 300

33. Run - Output
In this tutorial, we run a steady-state simulation. We are only interested in the latest time step. However, it is advised to keep the previous time step result as a backup on the disk. We will make a backup every 50 iterations.
Switch to Output tab
Set the Interval [-] to 50

34. Run - CPU
To speed up the calculation process increase the number of CPUs basing on your PC capability. The free version allows you to use only 2 processors in parallel mode. To get the full version, you can use the contact form to Request 30-day Trial
Estimated computation time for 2 processors: 5 minutes
Switch to CPU tab
Use parallel mode
Increase the Number of processors
Click Run Simulation button

35. Control Inlet Pressure
Go to the p on inlet tab to observe convergence process.
Switch to p on inlet tab

36. Discretization
After preliminary calculation, we will continue with a more accurate algorithm. Change velocity discretization to the Linear Upwind scheme to minimize numerical diffusion affecting results of the simulation.
Go to Discretization panel
Switch to Convection tab
Click on Upwind to extend the list
Select Linear Upwind

37. Run - Continue Simulation
Go to RUN panel
Set the maximal Numbers of Iterations to 2000
Click Continue Simulation button

38. Control Inlet Pressure - New Scheme
Go back to the p on inlet tab and observe convergence process.
Switch to p on inlet tab
Control the convergence of the pressure on the inlet

39. Slice - View Velocity Field
Slices tab appears next to the Residuals tab. Under this tab, we can preview results on the defined section plane.
Change tab to Slices
Select the velocity U
Click Adjust range to data
Click Fit View
Set the XZ orientation View XZ

40. Slice - Final Results
At the end, we will look at the pressure distribution. The Darcy porous model assumes resistance and hence pressure gradient to be proportional to the velocity in the porous zone. We can observe the effect of increased resistance from the porous zone. The pressure builds up in front of the porous zone and then linearly decreases along the flow direction due to resistance.
