Chimney - CFD Simulation SimFlow Tutorial

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.

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 chimney

Firstly, we need to Download GeometryChimney
The geometry will be imported in the same units as it was exported to the STEP format.

The resulting geometry will be displayed in the graphics window.

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.

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.

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.

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.

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

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.

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.

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.

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. To control the mesh quality inside the domain, we can enable cross-section view.

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.

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.

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

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

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.c

We want to analyze compressible turbulent flow with lagrangian particles. For this purpose, we will use the Reacting Parcel (reactingParcelFoam) solver.

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.

We are not going to model any chemical reaction. We will disable combustion for our simulation.

We will also disable Chemistry in our analysis.

We will consider a second type of pollutants, 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.

Now, select the ash as a material of particles.

It remained to define the initial temperature of the particles.

We will now define the injection of the discrete phase through the chimney inlet boundary. We assume a constant flow rate of 100 kg of ash over 100 s, with the particle velocity equal to the gas velocity escaping from the chimney.

We will now define a normal distribution of the discrete phase size.

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 droplets. The Ranz-Marshall heat transfer model is used to consider heat transfer between the particles and surrounding gas.

We will disable radiation for our simulation.

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

Now, we will define the inlet and outlet boundary conditions. At the first, we will set constant flow rate of CO2 from the chimney.

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

To model the wind in the atmosphere, we will use a Free Stream condition.
The rest parameters leave by the default as an Air (Species: 23% of O2 and 77% of N2) with a temperature of 300K.

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.

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

At the initial state, we assume a constant velocity on the domain filled by the air.

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, runtime post-processing can only be configured before starting calculations and cannot be changed later on.

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 rest of the parameters we can leave the default.

To speed up the calculation process, we can use parallel mode.

If you are using SimFlow free version (which allows only for 2 CPUs) you can use the contact form to Request 30-day Trial

Estimated computation time for 2 CPUs: 25 minutes

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

Slices tab appears next to the Residuals . Under this tab, we can preview results 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.

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

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

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

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

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