Fill out the form to download

Required field
Required field
Not a valid email address
Required field


Tutorial: Car Park Contamination Simulation

This tutorial will provide a step-by-step tutorial on how to set up a contamination control simulation inside a car park.

Figure 1: Concentration distribution of CO inside a car park


This tutorial will teach you how to:

  • Set up and run car park contamination simulation.
  • Assign boundary conditions, material, passive species and momentum sources to the simulation.
  • Mesh with SimScale’s standard meshing algorithm.

This tutorial will follow the usual SimScale workflow:

  1. Prepare the CAD model for the simulation
  2. Set up the simulation
  3. Create the mesh
  4. Run the simulation and analyze the results

1. Prepare the CAD Model and Select the Analysis Type

First, you should import this project into your workbench.

By importing the tutorial project, a new project containing the tutorial’s geometry:

workbench view with car park model uploaded
Figure 2: Workbench view

As you can see, the jet fans and the car has been included into the model. This will make the simulation setup process easier because we will only need to select these bodies later.

1.1 Create the Simulation

You can follow the steps below to create your simulation:

First of all, to create a new simulation, click on the ‘+’ button next to Simulations in the tree or the ‘Create Simulation’ button on the geometry panel.

geometry dialog box to show user how to start setting up a simulation
Figure 3: Geometry dialog box

Next, select the ‘Incompressible’ analysis type and click ‘Create Simulation’.

simulation list in simscale with incompressible selected and the create simulation button
Figure 4: Simulation list

Doing so creates a new simulation tree, like shown below:

simulation tree in simscale showing the steps on setting up a new simulation
Figure 5: Simulation tree

All setup steps that are already sufficient for initializing a simulation are highlighted with a green check mark. Steps that require some user input are shown with a red circle and those that have a blue circle indicate optional settings.

2. Simulation Setup

In this section, we will be defining the physics of our model for the car park contamination simulation.

2.1 Passive Species

To define a contaminant for our car park contamination simulation, we will need to define a passive species in our simulation. This is done by following the steps below:

general settings of incompressible flow simulation for car park contamination simulation
Figure 6: General settings dialog box
  • After you have selected your simulation type, which is shown in Figure 3, a dialog box will pop up showing the global settings for your simulation. If you ever need to go back to this, you can do it by clicking on your analysis type in the simulation tree.
  • To enable a scalar transport simulation, which we need to calculate the contamination, we have to define the number of passive species that will be simulated. In this simulation, we will assign 1 passive species because we only have one contaminant, which is CO.

Read more:

You can read more about passive species here.

2.2 Geometry

The geometry is automatically assigned to the simulation. If you would upload multiple geometries, you could choose which one to simulate here.

2.3 Model

A scalar transport simulation is highly dependent on two things:

  1. How strong is the transport of mass in the flow (described by the Turbulent Schmidt Number)?
  2. How fast is the rate of diffusion (described by the Diffusion coefficient)?

You can change these values in the Model dialog box in your simulation tree, but for this simulation we will use the default value.

model for car park contamination simulation with turbulent schmidt number defined as 0.7 and difffusion coefficient as 1e-5
Figure 7: Model dialog box

2.4 Material

Air will be assigned as the simulated material in the simulation. To define this, click on the ‘+’ button next to Materials, which opens the SimScale material library:

material list with air selected in SimScale
Figure 8: Material list

Select ‘Air’ and confirm your choice by hitting ‘Apply’. A dialog box showing all the physical parameters of the selected material will show up:

material dialog box showing physical properties of chosen material
Figure 9: Material dialog box

We will select the ‘Car Park’ as the fluid region of the simulation and next, we can confirm the operation by hitting the check box on the top right of the material properties.

You can also just select any material from the library, and change it’s name and properties to define a custom material.

2.5 Initial Conditions

In this section, you are able to modify the initial conditions of the simulation. This simulation is not time-dependent, which means that it will not affect your results, whatever you define here. However, if you already have a correct guess about the end result, adding it here will stabilize the simulation and help the solver to converge faster.

In this case and also if you don’t know the end result, just leave this the initial conditions at their default values.

2.6 Boundary Conditions

This simulation will use three boundary conditions:

  1. Four inlets to define where the air comes in.
  2. A pressure inlet to define the airflow inside the car park.
  3. Three outlets to define where the air will come out of the car park.
overview of boundary conditions
Figure 10: Overview of boundary conditions showing locations of inlets, outlets, ramp, and production of CO
locations of 6 jet fans inside the model
Figure 11: Locations of jet fans

Topological Entity Sets

To make the further boundary condition assignment easier, the faces belonging to the same boundary condition are grouped within a Topologial Entity Set. You can find them on the right side of the workbench in the Geometry panel under Topologial Entity Sets.

The following picture shows how to create them, in case you want to do them yourself.

steps on how to create an entity set for an air inlet of a car park.
Figure 12: Entity sets creation steps
  1. Select the faces that you want to group.
  2. Click the ‘+’ button beside the Topological Entity Sets.
  3. Name the group as ‘Inlets’.

To define the boundary conditions, click on the ‘+’ next to Boundary conditions, which opens the boundary condition library, as shown in the picture below:

list of boundary conditions available in simscale
Figure 13: Boundary conditions

a. Fresh Air Supply: Velocity Inlet

To define the inlets, please create a new Velocity inlet according to Figure 11. Doing so will open the boundary condition panel; assign the properties according to the following picture.

velocity inlet boundary condition used for car park contamination simulation with velocity defined as volumetric flow rate and a value of 5 m3/s
Figure 14: Velocity inlet
  • The value assigned as the (V)Volumetric flow is ‘5 \(m^3/s\)‘.
  • You can directly select the entity set you defined before. The assigned faces will turn blue after being assigned.

b. Opening to Environment: Pressure Inlet

For the remaining inlet we will define a Pressure inlet. Therefore follow the steps from Figure 11. Define the settings as presented in the picture below:

velocity inlet boundary condition used for car park contamination simulation with default values
Figure 15: Pressure inlet
  • Change the Gauge pressure to ‘Total pressure’
  • Leave the default values as they are and assign the face

c. Outlet

Finally, we need to define the location for the outlets. Therefore, create a Velocity outlet according to Figure 11 and define it as presented in the picture below:

velocity outlet boundary condition for outlets for car park contamination simulation with velocity as volumetric flow rate with a value 8 m3/s
Figure 16: Velocity outlets
  • Define the Velocity as ‘Flow Rate‘ and define the Flow rate as ‘(V)Volumetric flow’ and give the value ‘8 \(m^3/s\)’.
  • Select the ‘Outlets’ set you have created before.

2.7 Advanced Concepts

Under advanced concepts, we will define the setup to set Momentum sources to model the fans for the ventilation in the car park and the CO concentrations by defining a Passive scalar source. The jet fans and the car has been included in the model, so there is no need to create any new geometry.

To create a new item of advanced concepts, click on ‘Advanced concepts‘ and hit the ‘+’ button right next to the respective item, like presented in the picture below:

location of advanced concepts in the simulation tree which is below boundary conditions and contains rotating zones, porous media, momentum sources and passive scalar sources.
Figure 17: Advanced concepts list

a. Jet Fans

We will also model the jet fans installed in the car park as the mitigation method to circulate CO out of the car park. To do this, you will need to go to Momentum Sources under Advanced concepts, as presented in Figure 15 in the simulation tree.

settings of the jet fans where the average velocity is 10 m/s in the x-direction
Figure 18: Jet fans settings

Next we will assign the average velocity of the fans which is 8 /(frac{m}{s}/) in the x-direction and select all the fans in the model. You can do this by selecting each one in the model or selecting them in the Geometry tree in the top right of your screen.

b. Car Smoke

We will set a velocity for the CO coming out of the car by following the similar steps above but instead of selecting the fans, we will use the car as the momentum source.

car as a momentum source which has a velocity of 0.8 m/s in the x-direction
Figure 19: Car as a momentum source

The velocity of the CO emitted by the car will be 0.8 /(/frac{m}{s}/) in the x-direction.

c. Passive Scalar Source

Create a Passive scalar source like demonstrated in the picture above. Please define the setup according to the following picture:

passive scalar source defined for car park contamination simulation with flux value of 1 1/(m2/s)
Figure 19: Passive scalar source dialog box
  1. Define the passive scalar source as ‘Volumetric passive scalar source’
  2. Set the Flux as ‘1’ /(1/m^3.s/).
  3. Assign the ‘Car’ as the source and you can do this similar to how the fans were assigned.

Confirm the definition by hitting the check button on the top right of the panel. This will bring you back to the passive scalar source menu. Confirm your setup again to conclude the passive scalar setup procedure.

You can read more about flux here.

2.8 Numerics

The tree item Numerics enables to control numerical settings for the solver. The default values are fine for most simulations, however experts can define whatever numerical settings they want.

For this tutorial, the default values are just fine.

2.9 Simulation Control

The next important tree item is Simulation control which allows to steer the overall simulation settings. For this car park contamination simulation however, we will leave everything as it is.

3. Mesh Setup

In order for you to get an accurate result, a good mesh is necessary. However, the finer the mesh the more core hours will be consumed. It is best to start from a coarse mesh and increase the fineness level if necessary. You can create your mesh by clicking ‘Mesh’ in the simulation tree. This simulation utilizes the Standard meshing algorithm, also keep everything to the default.

mesh settings for car park contamination simulation using default settings
Figure 20: Mesh settings

The next step is to assign the fans and the car as cell zones so that they will be included in the meshing process.

cell zones dialog box where the car and fans are assigned as cell zones
Figure 21: Cell zones dialog box

To do this, you will need to click ‘Cell zones’ under the Mesh settings and assign the car and the fans as cell zones.

Once the mesh is created, it will have 1.5M cells and look like this:

mesh for car park model with 1.8 million cells generated with simscale's standard meshing algorithm
Figure 22: Generated mesh

Now the simulation setup is complete and you’re ready to start your analysis. For this, a simulation Run needs to be created.

A simulation Run calculates the physical situation of the model with the settings just defined.

steps to show how to start a simulation run
Figure 23: How to start a simulation run

In order to create a new Run, click ‘+’ next to Simulation Runs.

dialog box when starting a new run with resource estimation and name of the run
Figure 24: New run dialog box with resource estimates

A dialog box will pop up asking you to name your run. After this, the simulation run will start and you will be notified via e-mail when it is finished.

4. Post-Process Results

After the simulation has finished, you will be able to analyze your results with the built-in post-processor.

steps on how to access the post-processor in simscale
Figure 25: Access to post-processor

You can access the post-processor in two ways, by clicking on ‘Post-process results’ in the Run dialog box or clicking on ‘Solution Fields’ under your simulation run. You will then be redirected to the post-processor.

For this tutorial, we will visualize the areas where there is high concentration of CO in the car park by using Isovolumes. Isovolumes enable us to set a range for the results of the simulation.

settings of isovolumes to determine areas with high co concentration
Figure 26: Isovolumes settings

We can add Isovolumes by clicking the ‘+’ beside Isovolumes and then we can set a minimum and maximum values of the concentration in the Min Iso value and Max Iso value. For this example, we will use 0.25 as the minimum and 2.5 as the maximum value.

concentration of co inside a car park visualized with isovolumes
Figure 27: Visualization of concentration distribution of CO with Isovolumes

You can see from the figure above that the Isovolumes only visualize the concentration range that we have defined before which makes it easier to determine dangerous areas of the car park.

Congratulations! You finished the car park contamination tutorial!


If you have questions or suggestions, please reach out either via the forum or contact us directly.

Last updated: July 30th, 2020

Data Privacy