# Gas & Pollutant Dispersion - CFD Simulation

Source: https://help.sim-flow.com/tutorials/gas-pollutant-dispersion
Last updated: 2026-10-14

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

## 1. Introduction

This tutorial addresses the modeling of the dispersion of air pollutants, including Lagrangian particles. We will simulate the release of carbon dioxide and ash particles from a chimney into the atmosphere, investigating the dispersion of pollutants in the flowing air.

Throughout this tutorial, you will learn how to utilize species transport to model multiphase solver flow and simulate Lagrangian particles.

## 2. Download SimFlow

SimFlow is a general-purpose [CFD Software](https://sim-flow.com/download/cfd-simulation-software/)

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/)

## 3. Create Case

Open SimFlow and create a new case named *chimney*

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

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

## 4. Create Geometry - Chimney

Firstly, we need to [Download GeometryChimney](https://help.sim-flow.com/tutorials/downloads/chimney/chimney.step)
The geometry will be imported in the same units as it was exported to the STEP format.

1. Click **Import Geometry**
2. Select geometry file *chimney.step*
3. Click **Open**

![ch 02 import geometry](https://help.sim-flow.com/tutorials/images/chimney/ch-02-import-geometry.png)

## 5. Geometry - Chimney

The resulting geometry will be displayed in the graphics window.

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

![ch 03 geometry](https://help.sim-flow.com/tutorials/images/chimney/ch-03-geometry.png)

## 6. Creating Face Group - Inlet

In this simulation, we are dealing with an external flow problem. The imported chimney geometry serves as an airflow obstacle and introduces a second phase into the domain. To define where the boundaries of the inlet mesh should be created, we will use the *Face Groups*.

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

![ch 04 inlet](https://help.sim-flow.com/tutorials/images/chimney/ch-04-inlet.png)

## 7. Rename Face Group

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

The new group represents the contaminant inlet to the domain. Rename this group to *inlet*.

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

![ch 05 face group name](https://help.sim-flow.com/tutorials/images/chimney/ch-05-face-group-name.png)

## 8. Geometry - Refinements (I)

To achieve a denser mesh at the chimney outlet and in the region of contaminant dispersion, we will create two geometries to specify the areas for mesh refinement.

1. Select *Create Cylinder*
2. Rename it to `refinement`
   (double click on the geometry name to start renaming)
3. Set the cylinder origin:
   *Origin \({\sf [m]}\)*`0``0``68`
4. Set the cylinder dimensions:
   *Length \({\sf [m]}\)*`20`
   *Radius \({\sf [m]}\)*`5`

![ch 06 refinement](https://help.sim-flow.com/tutorials/images/chimney/ch-06-refinement.png)

## 9. Geometry - Refinements (II)

1. Select *Create Box*
2. Rename it to `refinement_2`
3. Set the box origin and dimensions:
   *Origin \({\sf [m]}\)*`0``-15``70`
   *Dimensions \({\sf [m]}\)*`80``30``40`

![ch 07 refinement 2](https://help.sim-flow.com/tutorials/images/chimney/ch-07-refinement-2.png)

## 10. Meshing Parameters - Chimney

To create the mesh, we need to specify the meshing options for the given geometry. For the *chimney*, we will refine the mesh near its faces.

1. Go to *Hex Meshing* panel
2. Select the *chimney* component
3. Enable *Mesh Geometry*
4. Set *Refinement* to *Min 2* *Max 2*

![ch 08 hex meshing chimney](https://help.sim-flow.com/tutorials/images/chimney/ch-08-hex-meshing-chimney.png)

## 11. Meshing Parameters - Refinement I

For the refinement geometry, we will set the mesh refinement inside the volume.

1. Select the *refinement* component
2. Enable *Refine Geometry*
3. Set refinement *Level* to `3`

![ch 09 hex meshing refinement](https://help.sim-flow.com/tutorials/images/chimney/ch-09-hex-meshing-refinement.png)

## 12. Meshing Parameters - Refinement II

1. Select the *refinement_2* component
2. Enable *Refine Geometry*
3. Set refinement *Level* to `2`

![ch 10 refinement 2](https://help.sim-flow.com/tutorials/images/chimney/ch-10-refinement-2.png)

## 13. Base Mesh - Domain

As we are considering an external flow, the area under consideration is limited by the size of the base mesh domain. For this purpose, we will use a *Box* base mesh type.

1. Go to *Base* tab
2. Set the base mesh size:
   *Min \({\sf [m]}\)*`-50``-50``0`
   *Max \({\sf [m]}\)*`200``50``150`
3. Define the number of divisions
   *Division*`40``20``30`

![ch 11 base mesh](https://help.sim-flow.com/tutorials/images/chimney/ch-11-base-mesh.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. We will use *symmetry* as a boundary type for simplified slip conditions on the *side* and *top* boundaries.

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

![ch 12 boundaries](https://help.sim-flow.com/tutorials/images/chimney/ch-12-boundaries.png)

## 15. Material Point

The material point indicates on which side of the geometry the mesh is to be retained. We are simulating flow around the chimney, so our material point needs to be located inside the base mesh but outside the chimney.

1. Go to *Point* tab
2. Specify location inside base mesh but outside chimney geometry
   *Material Point*`0``0``120`

You can specify the point location from the 3D view. Hold the `CTRL` key and drag the arrows to the destination.

![ch 13 material point](https://help.sim-flow.com/tutorials/images/chimney/ch-13-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

![ch 14 meshing](https://help.sim-flow.com/tutorials/images/chimney/ch-14-meshing.png)

## 17. Mesh

After the meshing process is finished, the mesh should appear on the screen. To control the mesh quality inside the domain, we can enable the cross-section view.

1. Select *Section View*
2. Mark *Section View*
3. Set section plane normal along *Y* axis
4. Click *Mesh Center* to locate the section plane in the center of the model

![ch 15 mesh](https://help.sim-flow.com/tutorials/images/chimney/ch-15-mesh.png)

## 18. Domain Extrusion - Sides (I)

With SimFlow, you can modify the existing mesh domain by extending the volume through boundary extrusion. This allows the size of successive mesh cells to be graded. For this tutorial, we will extend the domain on each side.

At the beginning, extrude the sides of the boundaries.

1. Expand the *Options* list for the *boundaries*
2. Select *Extrude* option

![ch 16 extrude boundaries](https://help.sim-flow.com/tutorials/images/chimney/ch-16-extrude-boundaries.png)

## 19. Domain Extrusion - Sides (II)

Selected boundaries will be extended by 100 meters in the normal direction. The additional mesh will be split into 10 rows of cells in the extrusion direction with a grading of 1.1.

1. Set the following parameters accordingly:
   *Number of Layers*`10`
   *Expansion Ratio*`1.1`
   *Extrude*`Normal`
   *Thickness*`100`
2. Click *Extrude*

![ch 17 extrude boundaries 2](https://help.sim-flow.com/tutorials/images/chimney/ch-17-extrude-boundaries-2.png)

## 20. Domain Extrusion - Inlet and Top

Next, repeat the extrusion process for the Inlet and Top boundaries using the same parameters as before.

1. Select the *Inlet* boundary and *Extrude* it using the previously defined parameters
2. Repeat the *Extrude* operation for the *Top* boundary

![ch 18 extrude top inlet](https://help.sim-flow.com/tutorials/images/chimney/ch-18-extrude-top-inlet.png)

## 21. Domain Extrusion - Outlet (I)

For the extrusion of the *Outlet* boundary, we will use a different set of parameters.

1. Expand the *Options* list for the *outlet*
2. Select *Extrude* option

![ch 19 extrude outlet](https://help.sim-flow.com/tutorials/images/chimney/ch-19-extrude-outlet.png)

## 22. Domain Extrusion - Outlet (II)

The outlet boundary will be extended by 300 meters, splitting an extra volume into 25 rows of cells with an expansion ratio of 1.05.

1. Set the following parameters accordingly:
   *Number of Layers*`25`
   *Expansion Ratio*`1.05`
   *Extrude*`Normal`
   *Thickness*`300`
2. Click *Extrude*

![ch 20 extrude outlet 2](https://help.sim-flow.com/tutorials/images/chimney/ch-20-extrude-outlet-2.png)

## 23. Mesh Investigation

Using the expansion ratio allows you to significantly enlarge the domain without significantly increasing the number of cells.

Now, we can disable the section view.

1. Uncheck the *Section View* option
2. Close the toolbox by clicking the *Section View* icon

![ch 21 mesh section](https://help.sim-flow.com/tutorials/images/chimney/ch-21-mesh-section.png)

## 24. Simulation Type

We want to analyze a compressible, turbulent flow involving multiple gases and solid particles. For this purpose, we will use a transient simulation with species transport and particle tracking.

![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/reactingParcelFoam/01_multicomponent@2x.png)

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

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

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

## 25. Combustion - Mechanism

We are going to model a dispersion of carbon dioxide in the atmosphere. Therefore, we will need three species to model this: nitrogen, oxygen and carbon dioxide.

1. Go to *Combustion* panel
2. Add the missing species by typing its chemical formula and selecting it from the list:
   *Add Species*`CO2`
3. Check if all necessary species are listed

![ch 23 species](https://help.sim-flow.com/tutorials/images/chimney/ch-23-species.png)

## 26. Discrete Phase - Composition

We will consider a second type of pollutant, which involves solid particles such as ash emitted from the chimney. To initiate this process, we will define the solid phase of the Lagrangian particles in the Discrete Phase panel.

1. Go to *Discrete Phase* panel
2. Expand *Add/Remove* list
3. Check *Solid* phase and uncheck the *Liquid*

![ch 26 composition](https://help.sim-flow.com/tutorials/images/chimney/ch-26-composition.png)

## 27. Discrete Phase - Material

Now, select the ash as a material of particles.

1. Switch tab to *Solid*
2. Expand *Add/Remove* list, check *ash* phase and uncheck the others
3. Set *ash* fraction to `1`

![ch 27 ash](https://help.sim-flow.com/tutorials/images/chimney/ch-27-ash.png)

## 28. Discrete Phase - Properties

Next, define the initial temperature of the particles.

1. Switch tab to *Properties*
2. Define ash temperature
   *\(T_0\) \({\sf [K]}\)*`500`
3. Define devolatilization temperature
   *\(T_{devol}\) \({\sf [K]}\)*`550`

![ch 28 temperature](https://help.sim-flow.com/tutorials/images/chimney/ch-28-temperature.png)

## 29. Discrete Phase - Injection

We will now define the injection of the discrete phase through the chimney inlet boundary. We assume a constant flow rate of 200 kg of ash over 200 s, with the particle velocity equal to the gas velocity escaping from the chimney.

1. Go to *Injection* tab
2. Create *Boundary Injector*
3. Set the total mass of the particles
   *Total Mass \({\sf [kg]}\)*`200`
4. Set the duration of injecting particles
   *Duration \({\sf [s]}\)*`200`
5. Select the boundary to be injected from
   *Boundary*`chimney_inlet`
6. Define the inlet velocity of the particles
   *\(U_0\) \({\sf [m/s]}\)*`0``0``5`

![ch 29 injection](https://help.sim-flow.com/tutorials/images/chimney/ch-29-injection.png)

## 30. Discrete Phase - Distribution

In this step, define the particle size using a normal distribution.

1. Go to *Distribution* tab
2. Set *Distribution* to *Normal*
3. Set distribution parameters accordingly
   *Min \({\sf [m]}\)*`2e-06`
   *Max \({\sf [m]}\)*`3e-04`
   *\(\mu\) \({\sf [m]}\)*`1.1e-04`
   *\(\sigma\) \({\sf [m]}\)*`7e-05`

![ch 30 injection distribution](https://help.sim-flow.com/tutorials/images/chimney/ch-30-injection-distribution.png)

## 31. Discrete Phase - Models

We need to define which models will be used in this simulation. We select the Sphere Drag model to account for the drag force acting on the particles. The Ranz-Marshall heat transfer model is used to consider heat transfer between the particles and the surrounding gas.

1. Switch to *Models* tab
2. Set the drag model as *Sphere Drag*
3. Set the heat transfer model as *Ranz-Marshall*

![ch 31 particles models](https://help.sim-flow.com/tutorials/images/chimney/ch-31-particles-models.png)

## 32. Radiation

We will disable radiation for our simulation.

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

![ch 32 radiation](https://help.sim-flow.com/tutorials/images/chimney/ch-32-radiation.png)

## 33. 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

![ch 33 turbulencepng](https://help.sim-flow.com/tutorials/images/chimney/ch-33-turbulencepng.png)

## 34. Boundary Conditions - Bottom

Now, we will define the boundary conditions. First, we will specify the particle behavior at the bottom boundary as Sticky.

1. Go to *Boundary Conditions* panel
2. Select *bottom* boundary
3. Switch tab to *Particles*
4. Set *Interaction* to *Stick*

![ch 34 bc bottom](https://help.sim-flow.com/tutorials/images/chimney/ch-34-bc-bottom.png)

## 35. Boundary Conditions - Chimney Inlet

For the *chimney_inlet*, we will set a constant CO2 flow rate.

1. Select *chimney_inlet* boundary
2. Set the *Mass Flow Inlet* character
3. Switch tab to *Flow*
4. Set the flow rate
   *U* *Flow Rate \({\sf [kg/s]}\)*`100`

![ch 34 bc chimney flow](https://help.sim-flow.com/tutorials/images/chimney/ch-34-bc-chimney-flow.png)

## 36. Boundary Conditions - Chimney Inlet - Thermal

1. Go to *Thermal* boundary conditions tab
2. Set the temperature: *T* *Inlet Value \({\sf [K]}\)*`500`

![ch 35 bc chimney thermal](https://help.sim-flow.com/tutorials/images/chimney/ch-35-bc-chimney-thermal.png)

## 37. Boundary Conditions - Chimney Inlet - Species

Define the phase fractions of the escaping gas. The sum of all shares must be equal to 1.

1. Switch tab to *Species*
2. Set the inlet phase:
   *O2*`0`
   *N2*`0`
   *CO2*`1`

![ch 36 bc species](https://help.sim-flow.com/tutorials/images/chimney/ch-36-bc-species.png)

## 38. Boundary Conditions - Air Inlet

To model the wind in the atmosphere, we will use a Free Stream condition for the Inlet and Top boundaries.
The remaining parameters are left at the default values for air (Species: 23% of O2 and 77% of N2) with a temperature of 300K.

1. Select *inlet* boundary
2. Set the *Free Stream* character
3. Switch tab to *Flow*
4. Set pressure type to *Fixed Flux Pressure*
5. Define free stream velocity:
   *U* *Freestream Value \({\sf [m/s]}\)*`5``0``0`

![ch 37 bc inlet](https://help.sim-flow.com/tutorials/images/chimney/ch-37-bc-inlet.png)

## 39. Boundary Conditions - Top

For the top boundary, we will use the same Free Stream condition as for the inlet.

1. Select *top* boundary
2. Set the *Free Stream* character
3. Define free stream velocity:
   *U* *Freestream Value \({\sf [m/s]}\)*`5``0``0`

![ch 39 bc top](https://help.sim-flow.com/tutorials/images/chimney/ch-39-bc-top.png)

## 40. Boundary Conditions - Outlet

At the outlet, we will apply an Outflow boundary condition. To prevent reverse flow, we will set an Inlet-Outlet condition that behaves like a zero gradient when air is escaping, and it blocks the reverse flow by imposing zero velocity when entering the domain.

1. Select *outlet*
2. Set the *Outflow* character
3. Change velocity type
   *U* *Type*`Inlet-Outlet`

![ch 38 bc outlet](https://help.sim-flow.com/tutorials/images/chimney/ch-38-bc-outlet.png)

## 41. Initial Conditions

At the initial state, we assume a constant velocity in the domain filled with air.

1. Go to *Initial Conditions* panel
2. Set the initial velocity
   *U*`5``0``0`

![ch 40 initial](https://help.sim-flow.com/tutorials/images/chimney/ch-40-initial.png)

## 42. Monitors - Sampling

During calculation, we can observe intermediate results on a section plane. To sample data on a plane, we need to define the plane and also select fields that will be sampled. Note that runtime postprocessing can only be configured before starting calculations and cannot be changed later on.

1. Go to *Monitors* panel
2. Switch to *Sampling* tab
3. Select *Create Slice*
4. Set slice plane normal vector
   *Normal \({\sf [-]}\)*`0``1``0`
5. Expand *Fields* list
6. Select velocity *U*, temperature *T* and phase *CO2*

![ch 41 monitors](https://help.sim-flow.com/tutorials/images/chimney/ch-41-monitors.png)

## 43. Run - Time Control

In any simulation, it is often convenient to allow the solver to automatically determine the appropriate time step. To use this option, we need to define time step constraints by specifying the initial time step, which the solver can adjust during computations, and the maximum time step value. All other parameters can be left at their default settings.

1. Go to *RUN* panel
2. Set the *Simulation Time [s]* to `200`
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 \(\Delta t\) \({\sf [s]}\)*`0.1`
   *Max \(\Delta t\) \({\sf [s]}\)*`0.5`

![ch 42 run time](https://help.sim-flow.com/tutorials/images/chimney/ch-42-run-time.png)

## 44. 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: 40 minutes

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

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

## 45. Residuals

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

1. Go to *Residuals* tab

![ch 45 residuals](https://help.sim-flow.com/tutorials/images/chimney/ch-45-residuals.png)

## 46. Slice - CO2 Field

The *Slices* tab appears next to the *Residuals* tab. In this section, we will display the CO2 concentration on a defined section plane. We will also adjust the color range to make it easier to visualize regions with low CO2 concentrations, allowing for a more detailed analysis of the dispersion.

1. Change tab to *Slices*
2. Select the phase *CO2*
3. Expand data range options
4. Select *Custom Range*
5. Provide the range to *Min*`0` and *Max*`0.01`
6. Click **OK**

![ch 46 co2 map](https://help.sim-flow.com/tutorials/images/chimney/ch-46-co2-map.png)

## 47. 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**

![ch 47 paraview](https://help.sim-flow.com/tutorials/images/chimney/ch-47-paraview.png)

## 48. ParaView - Load Results

Load the results into the program.

1. Make sure you have your case selected *chimney.foam*
2. Click **Apply** to load results
3. Reduce the opacity to `0.3`
4. Select coloring variable to *vtkBlocksColors*
5. Play the animation using **Play** button
6. Results will be shown in the 3D graphic window

![ch 48 pv load res](https://help.sim-flow.com/tutorials/images/chimney/ch-48-pv-load-res.png)

## 49. ParaView - Extract Particles Block

In order to display the particles in a different scheme, it is necessary to first extract them from the overall results.

1. Select baseline results *chimney.foam*
2. Select *Extract Block*
3. Check *lagrangian* group
4. Confirm with the **Apply** button
5. Double-click on its name and rename it to `particles`
6. Select coloring variable to *mass0*

![ch 49 pv particles](https://help.sim-flow.com/tutorials/images/chimney/ch-49-pv-particles.png)

## 50. ParaView - Slice

We will create a cross-section through the computational domain to display the CO2 distribution.

1. Select the *chimney.foam* from *Pipeline Browser*
2. Select *Slice*
3. Set the plane normal along Y axis using **Y Normal** button
4. Uncheck *Show Plane*
5. Press **Apply**
6. From the drop-down coloring menu, select *CO2*

![ch 50 pv slice](https://help.sim-flow.com/tutorials/images/chimney/ch-50-pv-slice.png)

## 51. ParaView - Rescale

Scale the CO2 results to get a range of up to 1% carbon dioxide contribution.

1. Click on **Rescale to Custom Data Range**
2. Set the range from `0` to `0.01`
3. Confirm by clicking **Rescale**

![ch 51 pv slice rescale](https://help.sim-flow.com/tutorials/images/chimney/ch-51-pv-slice-rescale.png)

## 52. ParaView - Results

Orient the view parallel to the XZ plane and play with the animation buttons to investigate the time history of the flow.

![ch 52 pv final results](https://help.sim-flow.com/tutorials/images/chimney/ch-52-pv-final-results.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)