# Garage Ventilation - CFD Simulation

Source: https://help.sim-flow.com/tutorials/garage-ventilation
Last updated: 2026-10-14

[Video](https://help.sim-flow.com/tutorials/images/smoke.mp4)

## 1. Introduction

This tutorial guides you through the process of simulating a garage (car park) ventilation system using [SimFlow CFD software](https://sim-flow.com/download/cfd-simulation-software/). To follow this tutorial, you can download [the free version of SimFlow](https://sim-flow.com/download-simflow/).

You will learn to simulate airflow within an enclosed garage (or underground car park), analyze the impact of a vehicle 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:

- Simulate a garage ventilation system using SimFlow
- Model a source term (thermal and scalar) within a specific region and time range
- Incorporate a simplified fan model into your simulation

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.

## 2. Download SimFlow

To follow this tutorial, you will need the SimFlow free version. You may download it via the following link:
[Download SimFlow](https://sim-flow.com/download-simflow/)

This tutorial is compatible with SimFlow version 5.0.40 or newer. If you are using an older version, please update it using the following link:
[How to update SimFlow](https://help.sim-flow.com/installation/windows/updates)

## 3. Create Case

Open SimFlow and create a new case named *Garage Ventilation*

1. Click **New**
2. Provide name `Garage Ventilation`
3. Click **Create** to open a new case

![simflow-launcher](https://help.sim-flow.com/tutorials/images/launcher-garage_ventilation.png)

## 4. Import Geometry

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

Download Geometries[Garage](https://help.sim-flow.com/tutorials/downloads/garage-ventilation/garage.step)[Vent_duct](https://help.sim-flow.com/tutorials/downloads/garage-ventilation/vent_duct.step)[Fan](https://help.sim-flow.com/tutorials/downloads/garage-ventilation/fan.stl)[Fan_wall](https://help.sim-flow.com/tutorials/downloads/garage-ventilation/fan_wall.stl)

1. Click **Import Geometry**
2. Select geometry files:
   *fan.stl*
   *fan_wall.stl*
   *garage.step*
   *vent_duct.step*
3. Click **Open**

![gv 04 import](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-04-import.png)

## 5. Import Geometry II

In some cases, imported external geometry may consist of multiple parts. SimFlow will prompt you to decide whether to combine all parts into a single component. If you choose not to, each part will be imported as a separate item.

For the purposes of this tutorial, we will merge all parts into one geometry.

Additionally, if the imported geometry is in STL format, be aware that STL files do not include unit information. Therefore, you must manually specify the correct unit after import. If you’re unsure of the original unit used during export, you can estimate it by checking the Geometry size displayed in the interface.

In this case, since the fan geometry is correctly defined in meters, no rescaling is required.

1. Press **Yes** button to merge solids into one item
2. Ensure STL geometry units are set to *meter*
3. Click **OK**

![gv 05 import](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-05-import.png)

## 6. Geometry - Garage

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

- garage walls
- ventilation duct
- two faces of the internal fan:
  - cylindrical fan wall
  - inner cross-section (to specify the pressure jump required to enforce airflow through the fan)

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

1. Click *Fit View* to zoom in the geometry

![gv 07 geometry](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-07-geometry.png)

## 7. Creating Face Group - Exhaust

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*.

1. Select the outlet face by holding `CTRL` key and clicking on the geometry faces in a 3D view. The selection should be marked in red
2. Click on the *Face Group* button in the graphics context toolbar

![gv 08 exhaust](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-08-exhaust.png)

## 8. Rename Face Group

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.

1. Select *vent_duct* geometry
2. Expand *Geometry Faces*
3. Change face group name (double-click on a group name to start editing)
   *group_1* \(\rightarrow\) `exhaust`

![gv 09 face group name](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-09-face-group-name.png)

## 9. Meshing Parameters - Fan

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).

1. Go to *Hex Meshing* panel
2. Select the *fan* component
3. Enable *Mesh Geometry*
4. Set *Refinement* to
   *Min* *2*
   *Max* *2*
5. Mark *Create Baffle*

![gv 10 hex meshing fan](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-10-hex-meshing-fan.png)

## 10. Meshing Parameters - Fan Wall

Repeat the same settings for the *fan_wall* geometry.

1. Select the *fan_wall* component
2. Enable *Mesh Geometry*
3. Set *Refinement* to
   *Min* *2*
   *Max* *2*
4. Mark *Create Baffle*

![gv 11 hex meshing fan wall](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-11-hex-meshing-fan-wall.png)

## 11. Meshing Parameters - Garage

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

1. Select the *garage* component
2. Enable *Mesh Geometry*
3. Set *Refinement* to
   *Min* *1*
   *Max* *1*

![gv 12 hex meshing garage](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-12-hex-meshing-garage.png)

## 12. Meshing Parameters - Vent Duct

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

1. Select the *vent_duct* component
2. Enable *Mesh Geometry*
3. Set *Refinement* to
   *Min* *2*
   *Max* *2*

![gv 13 hex meshing vent duct](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-13-hex-meshing-vent-duct.png)

## 13. Base Mesh - Domain

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.

1. Go to *Base* tab
2. Set the base mesh size:
   *Min \({\sf [m]}\)*`0``0``0`
   *Max \({\sf [m]}\)*`32``46``4`
3. Mark *Lock Cell Size*
4. Define the number of divisions along one axis — the remaining directions will adjust automatically
   *Division*`64``92``8`

![gv 14 base mesh domain](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-14-base-mesh-domain.png)

## 14. Base Mesh Boundaries

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

1. Define boundary names accordingly
   *X-* *inlet*
   *Z-* *bottom*
   *Z+* *top*
2. Define boundary types accordingly
   *Z-* *Wall*
   *Z+* *Wall*

![gv 15 base mesh boundaries](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-15-base-mesh-boundaries.png)

## 15. Material Point

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.

1. Go to *Point* tab
2. Specify location inside garage
   *Material Point*`8``10``2`

![gv 16 material point](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-16-material-point.png)

## 16. Start Meshing

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 the full version, [Request 30-day Trial](https://license.sim-flow.com/trial)

1. Switch to *Mesh* tab
2. Start the meshing process with **Mesh** button

![gv 17 meshing](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-17-meshing.png)

## 17. Mesh

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

![gv 18 mesh](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-18-mesh.png)

## 18. Create Fan Interface

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.

1. Holding the **Ctrl** key, select the following boundaries
   *fan*
   *fan_slave*
2. Select *Create Cyclic Interface*

![gv 19 fan interface](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-19-fan-interface.png)

## 19. Check Mesh

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

1. Make sure the boundaries have the correct names and types
2. Expand the *Options* of the *default* region
3. Select *Check*
4. A summary of the check operation will be displayed in the console window below, along with the checking criteria.

![gv 20 mesh quality](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-20-mesh-quality.png)

## 20. Simulation Type

We want to analyze the natural and forced convection in a garage ventilation system. For this purpose, we will use a transient simulation of the compressible flow with buoyancy and heat transfer.

![Simulation Panel](https://help.sim-flow.com/assets/images/go-to-simulation-panel@2x.png)

![Step 1](https://help.sim-flow.com/assets/images/solvers-selection/buoyantPimpleFoam/01_heat_transfer@2x.png)

![Step 2](https://help.sim-flow.com/assets/images/solvers-selection/buoyantPimpleFoam/02_single_fluid@2x.png)

![Step 3](https://help.sim-flow.com/assets/images/solvers-selection/buoyantPimpleFoam/03_compressible@2x.png)

![Step 4](https://help.sim-flow.com/assets/images/solvers-selection/buoyantPimpleFoam/04_transient@2x.png)

![Step 5](https://help.sim-flow.com/assets/images/solvers-selection/buoyantPimpleFoam/05_apply@2x.png)

## 21. Radiation

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

1. Go to *Radiation* panel
2. Uncheck *Enable Radiation*

![gv 22 radiation](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-22-radiation.png)

## 22. Turbulence

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

1. Go to *Turbulence* panel
2. Select *RANS* modeling
3. Select *\(k{-}\omega \; SST\)* model

![gv 23 turbulence](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-23-turbulence.png)

## 23. Transport Properties - Air

To assign specific materials, we will use the built-in database of material properties. Air will be used as a fluid material.

1. Go to *Thermo* panel
2. Open *Material Database*
3. Select the *air*
4. Click **Apply**

Selecting a 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.

![gv 24 thermo](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-24-thermo.png)

## 24. Boundary Conditions - Inlet

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

1. Go to *Boundary Conditions* panel
2. Select *inlet* boundary
3. Set the *Pressure Inlet* character
4. Switch to *Thermal* tab
5. Configure the thermal settings as follows:
   *T* *Type*`Inlet-Outlet`
   *T* *Inlet Value \({\sf [K]}\)*`300`

![gv 26 bc inlet](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-26-bc-inlet.png)

## 25. Boundary Conditions - Exhaust I

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

1. Select *vent_duct_exhaust* boundary
2. Set the *Mass Flow Inlet* character
3. Switch to *Flow* tab
4. Set the flow type and value accordingly:
   *U* *Type*`Flow Rate Outlet Velocity`
   *U* *Flow Rate \({\sf [kg/s]}\)*`15`

> Please note that after setting the *Flow Rate Outlet Velocity*, the boundary type will change automatically from *Mass Flow Rate* to *Custom*: ![custom icon](https://help.sim-flow.com/tutorials/images/garage-ventilation/custom-icon.png)

![gv 27 bc exhaust flow](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-27-bc-exhaust-flow.png)

## 26. Boundary Conditions - Exhaust II

1. Switch to *Thermal* tab
2. Set the thermal conditions as follows:
   *T* *Type*`Inlet-Outlet`
   *T* *Inlet Value \({\sf [K]}\)*`300`

![gv 28 bc exhaust thermal](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-28-bc-exhaust-thermal.png)

## 27. Boundary Conditions - Fan I

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.

1. Select *fan* boundary
2. Switch to *Flow* tab
3. Set the type for the pressure equation
   *\(p-\rho gh\)* *Type*`Fan`
4. Change the *Jump Table* setting to *table*, then press *Edit Table*

![gv 29 bc fan](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-29-bc-fan.png)

## 28. Boundary Conditions - Fan II

We will load the fan characteristic data from the following file:
[Download Fan Curvefan_curve.dat](https://help.sim-flow.com/tutorials/downloads/garage-ventilation/fan_curve.dat)

1. Click *Load Data From File* and select the *fan_curve.dat* file
2. Once loaded, the table will be filled with the corresponding values
3. Press **Close** to finalize the setup.

![gv 29 bc fan2](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-29-bc-fan2.png)

## 29. Fire Source - Introduction

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.

## 30. Fire Source - Geometry

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

1. Go to *GEOMETRY* panel
2. Select *Create Box*
3. Change geometry name
   *box_1* \(\rightarrow\) `car`
4. Expand *Properties*
5. Set the origin and box dimensions
   *Origin \({\sf [m]}\)*`24``6``0`
   *Dimensions \({\sf [m]}\)*`2``5``2`

![gv 30 car](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-30-car.png)

## 31. Heat Source - Create Cell Zone (I)

Now we will define the cell zone using the *car* geometry.

1. Go to *MESH* panel
2. Expand the *Options* of the *default* region
3. Select *Add Cell Zones*

![gv 31 cell zone](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-31-cell-zone.png)

## 32. Heat Source - Create Cell Zone (II)

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

1. Check the *car*
2. Click on **Create Cell Zones**

![gv 32 cell zone](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-32-cell-zone.png)

## 33. Heat Source - Passive Scalar

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.

1. Go to *Passive Scalars* panel
2. Press **Add new passive scalar Equations** button
3. Change the scalar name
   *scalar1* \(\rightarrow\) `smoke`

![gv 33 passive scalar smoke](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-33-passive-scalar-smoke.png)

## 34. Heat Source - Cell Zone Properties

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.

1. Go to *Cell Zones* panel
2. Mark *Fixed Value Constraints* for the *car* zone
3. Enable *Custom Time Range* for the source
4. Define the time range to:
   *Start Time \({\sf [s]}\)*`0`
   *Duration \({\sf [s]}\)*`60`
5. Expand **Add/Remove** fields
6. Select the following fields:
   *T* temperature
   *smoke* smoke concentration
7. Specify the constant value of the selected parameters
   *T \({\sf [K]}\)*`550`
   *smoke \({\sf [-]}\)*`1`

![gv 34 cell zone source](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-34-cell-zone-source.png)

## 35. Monitors - Sampling

During the calculation, we can observe intermediate results using section planes or probe plots. Note that runtime postprocessing 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.

1. Go to *Monitors* panel
2. Switch to *Sampling* tab
3. Expand *Fields* list
4. Select the following fields:
   *U* velocity
   *T* temperature
   *smoke* smoke concentration

![gv 35 monitors](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-35-monitors.png)

## 36. Monitors - Create Slice (I)

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.

1. Select *Create Slice*
2. Set the origin to
   *Point \({\sf [m]}\)*`0``0``1`

![gv 36 monitors slice1](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-36-monitors-slice1.png)

## 37. Monitors - Create Slice (II)

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

1. Select *Create Slice*
2. Set the origin to
   *Point \({\sf [m]}\)*`0``0``3.3`

![gv 37 monitors slice2](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-37-monitors-slice2.png)

## 38. Run - Time Control

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 the maximal time step value. The remaining parameters can be left at their default values.

1. Go to *RUN* panel
2. Set the *Simulation Time [s]* to `240`
3. Change *Time Stepping* to *Automatic*
4. Set initial and maximum time steps (solver will start computation with the initial value and adjust it in the next iterations, not exceeding the maximum value)
   *Initial \(\Delta t\) \({\sf [s]}\)*`0.01`
   *Max \(\Delta t\) \({\sf [s]}\)*`1`

> Due to the long calculation time, you can reduce the simulation time to 120s.

![gv 38 run time control](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-38-run-time-control.png)

## 39. Run - Output

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

1. Switch to *Output* tab
2. Set the *Interval [s]* to `1`

![gv 39 run output](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-39-run-output.png)

## 40. Run - CPU

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](https://license.sim-flow.com/trial)

Estimated computation time for serial mode: 3 hours

1. Switch to *CPU* tab
2. Click **Run Simulation** button

![run cpu serial](https://help.sim-flow.com/tutorials/images/run-cpu-serial.png)

## 41. Residuals

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

1. Go to *Residuals* tab

![gv 40 residuals](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-40-residuals.png)

## 42. Slice - Velocity Field

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.

1. Change tab to *Slices*
2. Select the velocity *U* field
3. Click *Adjust Range to Data*
4. Play the animation

![gv 41 velocity](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-41-velocity.png)

## 43. Slice - Temperature Field

1. Select the temperature *T*
2. Move the time step to *Start*
3. Click *Play* to run the animation

![gv 42 temperature](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-42-temperature.png)

## 44. Slice - Smoke Concentration Field I

Now, display the smoke concentration and identify areas where the concentration exceeds 20%. To do this, we will define a custom data range.

1. Select the *smoke* field
2. Expand the data range options
3. Choose *Custom range*

![gv 43 smoke 1](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-43-smoke-1.png)

## 45. Slice - Smoke Concentration Field II

1. Set the range to *Min 0* *Max 0.2*
2. Click **OK** to apply
3. Click the *End* button to move to the last time frame

![gv 43 smoke](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-43-smoke.png)

## 46. Postprocessing - ParaView

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

1. Go to *POSTPROCESSING* panel
2. Click on **Run ParaView**

![gv 44 paraview](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-44-paraview.png)

## 47. ParaView - Load Results

Load the results into the program.

1. Make sure you have your case selected *garage_ventilation.foam*
2. Click **Apply** to load results
3. Select coloring variable to *Solid Color*
4. Change the display type to *Feature Edges*

![gv 45 pv load results](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-45-pv-load-results.png)

## 48. ParaView - Import Geometries

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

1. Select **Open**
2. Go to case folder *garage_ventilation*
3. Navigate to folder *constant/triSurface/*
4. Select all geometry files
5. Press *OK*

![gv 46 pv load geometry](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-46-pv-load-geometry.png)

## 49. ParaView - Display Geometries

Adjust the geometry display settings to enhance visualization.

1. Click **Apply** to load the geometries
2. Select *car.stl*
3. Select contour coloring variable to *Solid Color*
4. Set the *Opacity* to `0.3`
5. Set the *Solid Color* for the remaining geometries

![gv 47 pv display geometry](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-47-pv-display-geometry.png)

## 50. ParaView - Display Vector Field

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

1. Select baseline results *garage_ventilation.foam*
2. Select *Glyph*
3. Set the *Scale Array* to velocity *U*
4. Set the *Scale factor* to `1`
5. Specify the number of vectors and their distribution across the domain.
   *Glyph Mode*`Uniform Spatial Distribution (Bounds Based)`
   *Maximum Number Of Sample Points*`7000`
6. Confirm with the **Apply** button
7. Select coloring variable to temperature *T*
8. Play the animation buttons

![gv 48 pv vector field](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-48-pv-vector-field.png)

## 51. ParaView - Display Smoke I

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.

1. Hide the glyphs
2. Select baseline results *garage_ventilation.foam*
3. Change the display type to *Surface*
4. Select coloring variable to *smoke*
5. Select *Edit Color Map*

![gv 49 pv smoke](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-49-pv-smoke.png)

## 52. ParaView - Display Smoke II

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

1. In the *Color Map Editor* panel, set *X Ray* color preset
2. Mark the *Enable Opacity Mapping For Surfaces* to make denser areas more visible through transparency.
3. Play the animation

![gv 50 pv smoke x ray](https://help.sim-flow.com/tutorials/images/garage-ventilation/gv-50-pv-smoke-x-ray.png)

## 53. Advanced Postprocessing with ParaView

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, calculate 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 postprocessing techniques.

[Paraview CFD Tutorial - Advanced Postprocessing in ParaView](https://www.youtube.com/watch?v=5M6VgXyHB60&list=PLy7xPqn9xXckoD2gZgPpv8mrxillJ9PWU&index=21)