Garage Ventilation - CFD Simulation CFD Software Tutorial

This tutorial guides you through the process of simulating a garage ventilation system using SimFlow CFD software. You will learn to simulate airflow within the garage, analyze the impact of a car fire, and assess the effectiveness of the ventilation system in removing smoke and reducing temperature over time.

Throughout this tutorial, you will learn how to:

By the end of this tutorial, you will have a solid understanding of how to simulate and evaluate the performance of a garage ventilation system under fire conditions.

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

Open SimFlow and create a new case named garage ventilation

Firstly, we need to download and import the following geometries:

Download GeometriesGarageVent_ductFanFan_wall

In some cases, the imported external geometry may contain multiple parts. SimFlow will ask you whether you want to join all geometries into a single component. If not, each part will be put into separate items.

For the purposes of this tutorial, we will combine all parts within each file into a single geometry.

The imported fan geometry is in STL format, which does not include unit information. Therefore, you need to manually specify the correct unit after import. If you are unsure about the original export unit, you can estimate it based on the total size of the imported geometry, shown next to the Geometry size label in the interface.

In this case, the geometry dimensions are already correctly defined in meters, so no rescaling to SI units is required.

The resulting geometry will be displayed in the graphics window. The geometry components include:

The bottom and top surfaces of the garage are not included, as they will be constrained by the base mesh in later steps.

The imported ventilation duct geometry is used to extract air from the garage. To define where the outlet boundary of the mesh should be created, we will use Face Groups.

In the Geometry Panel, find the new Face Group under the vent_duct geometry. The first group, named default, contains all non-selected surfaces, which will become the duct walls.

The new group represents the exhausts. Rename this group to exhaust. If the face group panel is open, go to point 3 directly.

To create the mesh, we need to specify the meshing options for the given geometries.

For the fan, we will refine the mesh near its faces. Since the fan is represented by a surface geometry, make sure to enable the Create Baffle option. A baffle is a thin internal surface that separates regions without adding physical thickness. It is commonly used for internal walls, fans, or porous surfaces. By duplicating the original surface, it creates two coincident faces—allowing different boundary conditions to be applied on each side (immersed boundary approach).

Repeat the same settings for the fan_wall geometry.

For the garage, we will apply mesh refinement near its surfaces to level 1.

For the vent_duct, we will refine the mesh near its faces to level 2.

Since we are simulating internal flow with an open geometry, the computational domain is bounded by both the geometry itself and the size of the base mesh. For the background mesh, we will use the Box base mesh type, which defines the domain boundaries—limiting the region from the top and bottom.

Now, we need to assign individual names to each side of the base mesh to define different conditions on each side.

The material point indicates which side of the geometry the mesh will be retained on. Since we are simulating airflow inside the garage, the material point must be placed within the garage.

In this step, we will initiate the meshing process.

In the meshing panel, you can indicate how many CPUs you would like to use for this process. Note that if you are using the free version of SimFlow, you may only use serial meshing and cannot create meshes larger than 200,000 nodes.

If you would like to test full version Request 30-day Trial

After the meshing process is finished, the mesh should appear on the screen.

In the mesh setup, we enabled baffle creation for the fan, allowing it to act as a split surface for the internal fan model. Now, we will create a Cyclic Interface on the fan baffle to connect both sides of the internal boundary, enabling airflow through the fan. Note that the cylindrical surface remains split.

To verify the mesh, review the boundary names and types. Then, check the mesh quality.

We want to analyze the transient simulation of the airflow with heat transfer. For this purpose, we will use the Buoyant PIMPLE (buoyantPimpleFoam) solver.

We will run a simulation without taking radiative heat transfer into account.

We are going to use the standard \(k{-}\omega \; SST\) model to resolve turbulence.

To assign specific materials, we will use the built-in database of material properties.

Selecting material from the Material Database will fill all the inputs in the Transport Properties panel. We are still able to overwrite these values at any time.

Air will be used as a fluid material.

We will now specify the model’s boundary conditions. Begin by setting the Pressure Inlet for the garage entrance.

To model the garage ventilation, we will apply an exhaust boundary condition with a predefined mass flow rate.

A fan has been installed in the garage to direct airflow toward the exhaust. In the model, the fan consists of a cylindrical sidewall, with a section where a pressure jump will be applied to drive the flow.

To enforce the airflow through the fan, we will use the Fan boundary condition. This condition allows you to define the relationship between the flow rate and pressure jump using an external file.

You will need to download this file and load it into SimFlow.
Download Fan Curve

Now, load the fan characteristic data from the downloaded file.

In this tutorial, we aim to model a car fire in a simplified way. We will not simulate combustion chemistry, but instead represent the fire as a source of heat and smoke.

To achieve this, we will first create a cell zone in the region of the car fire. This zone defines a group of cells where additional models can be applied.

Next, we will introduce a passive scalar to represent smoke concentration within the garage. This scalar does not influence the physical properties of air but acts as a tracer to visualize the spread of smoke throughout the domain.

The fire source will be modeled using a constant temperature of 550K and a smoke concentration of 1. The buoyancy forces resulting from the heat will drive the motion of hot, smoke-laden air.

We will assume the fire burns for the first 60 seconds of the simulation, after which it is extinguished. The remainder of the simulation will focus on how the ventilation system removes the heat and smoke from the garage.

First, we will create the geometry representing the fire source. Its size will correspond to the volume of the car.

Now we will define the cell zone using car geometry.

Select the geometry within which the cell zone should be created.

We will use a passive scalar to simulate smoke concentration. The passive scalar introduces an additional transport equation into the system of governing equations.

It is important to note that the passive scalar does not affect the flow itself; rather, it serves purely as a marker to trace the movement of smoke within the domain.

The scalar value ranges from 0 to 1, where 0 represents clean air and 1 corresponds to the smoke concentration at the source.

To control how the smoke spreads, we may define a custom diffusivity for the scalar. In this case, it is set to the default value of 1e-05.

To define the heat and smoke source for our simulation, we will use the Fixed Value Constraint option for the designated car cell zone. This option assigns fixed values to specified parameters for all cells within the selected zone. It allows us to set a constant fire temperature, which is useful when the exact firepower (heat release rate) is unknown or cannot be accurately estimated.

During the calculation, we can observe intermediate results using section planes or probe plots. Note that runtime post-processing must be defined before starting the calculations and cannot be modified afterward.

First, we need to specify the variables to be sampled. After that, we will define the section planes.

To add sampling data on a plane, we need to create a slice by defining a normal vector and a point that lies on the section plane. Since the normal vector aligns with the default Z-axis, we only need to specify the point coordinates.

Create a second slice above the first one at a height of 3.3 m to cross-section the vent ducts.

For any simulation, it is very convenient to let the solver automatically determine the proper time step value. To use this option, we need to define time step constraints by providing the initial time step (adjusted by the solver during computations) and maximal time step value. The remaining parameters can be left at their default values.

We can control how often results should be saved on the hard drive. Only this data will be available for post-processing.

To speed up the calculation process, take advantage of parallel computing and increase the number of CPUs based on your PC’s capability. The free version allows you to use only one processor (serial mode). To get the full version, you can use the contact form to Request 30-day Trial

Estimated computation time for serial mode: {time}

When the calculation is finished, we should see a similar residual plot.

During the simulation, the Slices tab appears next to the Residuals . Under this tab, you can preview live results during the simulation on the defined section plane.

Once the computations have been completed, we can perform advanced visualization of the results using ParaView.

Load the results into the program.

Now, import the geometries to visualize the flow pattern in relation to the structure of the garage.

Adjust the geometry display settings to enhance visualization.

In order to display the vector fields, follow these steps:

Now, we will visualize the smoke propagation inside the garage. We will use grayscale color mapping and transparency to make the distribution more visible and intuitive.

Now, enhance the visual appearance using a different color preset and enable transparency.

This concludes the tutorial, covering all the aspects we intended to showcase. For a finely tuned presentation of the results, you may take advantage of the more advanced features.

In ParaView, you can display streamlines, contour plots, vector fields, line or time plots, calculating volume or surface integrals and create animations.

To familiarize yourself with the ParaView capabilities, it’s worth checking out our video tutorial, Paraview CFD Tutorial - Advanced Postprocessing in ParaView, in which we demonstrate some of the most commonly used post-processing techniques.

Paraview CFD Tutorial - Advanced Postprocessing in ParaView