Read Time: 20 min
Intended Audience: new-to-Luminary, interested in Porous Media modeling
Simulation Time: ~2 min
Simulation Cost: 2 credits
In This Tutorial
In this Tutorial we focus on internal flow through an exhaust system, where a particular part of the system is modeled using a Porous Media Model (PMM). You will learn:
when or why to use a PMM
geometry requirements to define a PMM
associated parameters of the PMM
and you can use the tutorial to investigate the difference in the solution when the PMM physics modeling is activated vs. not.
Background
A catalytic converter is a vehicle emissions device that converts engine exhaust pollutants into nitrogen, carbon dioxide, and water vapor. Exhaust gasses enter through the inlet, then pass through a complex, honeycomb-shaped substrate made of Platinum, Rhodium, and Palladium to initiate a chemical reaction.
In CFD, the substrate is modeled as porous media due to its complex structure. Geometrically resolving the internal details of the media would require an excessively fine (small length scale, high cell count) mesh that would make such a simulation impractical from a cost perspective. The porous media model framework allows the simulation to impose the required flow restrictions, applied in a bulk fashion on the fluid, in a computationally efficient manner.
This catalytic converter domain is made up of three separate volumes: the inlet, the substrate, and the outlet. As exhaust flows through the inlet, the pressure will drop as it passes through the substrate. You'll apply visualization filters to determine the flow pattern and view the pressure drop.
Let's Get Started
Navigate to the Projects tab and click New Project. From the modal, navigate to the Tutorials tab and select "Catalytic Converter: Porous Media Modeling".
This will create a new project where the mesh described below has been loaded, but no other inputs have been specified. When you enter the project you will be placed in the setup environment:
Assessing the Geometry
Let's first familiarize ourselves with the geometry model. In the Geometry Tree on the left you'll see the three volumes that have been generated:
Additionally there are surface groups for each of these volumes that will be used to define boundary conditions, several of which are used to communicate between the volumes (interfaces):
Set Up the Simulation
In this tutorial, we're going to focus on learning how to set up a porous media model. Upload this settings file into the Project to populate the other settings for you:
Download the above settings file
Note: on mac, right click and select "save link as"
Upload the settings file into your project. Click the three dot (...) menu at the top of the control panel and select Upload Settings, then select the file from your file browser.
Define the Porous Model
In the Setup Checklist, find and expand the Physics section.
Expand Fluid Flow.
Click the + icon to the right of Physical Models and select Porous Model.
Set the Darcy Coefficients to x: 1000, y: 1,000,000, z: 1,000,000.
Set the Forchheimer Coefficients to z: 1000, y: 1,000,000, z: 1,000,000.
Click inside the Volumes box to enter selection mode.
From the Geometry panel on the left, select substrate-domain.
At the top of the control panel, click Run Simulation.
You'll be taken to the simulation tab for this run. Once it's finished running, you'll apply visualization filters to view the results.
Create a Slice
Create a slice to view the pressure distribution throughout the catalytic converter:
In the visualization toolbar at the top of the page, click Add Slice
In the properties panel, set the Display options to:
Color By: Pressure (Pa)
Representation: Surface
Then in the Visualization Input section, set:
Origin: 0.3, -0.2, 0
Normal: 0, 0, 1
Click the check button to create the slice.
In the Geometry panel, click the eye icon to the right of Surfaces to hide all surfaces.
In the upper-right corner of the 3D Viewer, click on the Pressure color bar.
Click Global under the color bar range.
Click Done.
You'll notice pressure increase as air hits the substrate, then drop as it flows through the rest of the device.
Create a Surface LIC
Finally, apply a surface LIC filter to get a better view of velocity distribution through the catalytic converter:
In the visualization toolbar at the top of the page, select Visualizations -> Surface LIC
.In the properties panel, set the Display options to:
Color By: Velocity
Component: Magnitude
Contrast: 1.01
Then in the Visualization Input section, set:
Surface LIC Field: Velocity
Generate LIC On: Plane
Origin: 0.075, -1.4177e-5, -1.3267e-7
Normal: 0, 0, 1
Plane Bounds:
Minimum: -0.2, -0.1, -0.05
Maximum: 0.6, 0.049, 0.05
Click the check button. The surface LIC may take a few seconds to generate.
In the Geometry panel, click the eye icon to the right of Surfaces to hide all surfaces. This will give us the clearest view of the surface LIC.
In the upper-right corner of the 3D Viewer, click on the Velocity color bar.
In the Max box, enter 42.
Click Done.
You'll notice high velocity through the inlet, then the air slows and starts to recirculate as it hits the porous volume. Velocity drops significantly through the substrate before speeding up again at the outlet.