# Spray Combustion

## 1. Create Case

After opening SimFlow, we will create a new case named spray_combustion

1. Go to panel

2. Provide name spray_combustion

3. Click

## 2. Import Geometry

1. Click

2. Select geometry file cylinder.stl

3. Click

## 3. Geometry - Cylinder

After importing geometry, it will appear in the 3D window.

1. Click to zoom in on the geometry.

## 4. Meshing Parameters - Cylinder

In order to create the mesh, we need to enable meshing for the newly imported geometry.

1. Go to Hex Meshing panel

2. Enable Mesh Geometry on cylinder geometry

## 5. Base Mesh - Domain

Now we will define the base mesh. The box geometry determines the background mesh domain. The model is symmetrical on the XZ and YZ planes so we do not need to mesh the whole geometry. Using the box dimensions we will choose only a quarter of a model.

1. Switch to Base tab

2. Click on

3. Change the following parameters accordingly
Min $$\sf{[m]}$$00

4. Define the number of divisions
Division505020

## 6. Base Mesh - Boundaries

We need to assign individual names to each side of the base mesh. This will allow us to apply different conditions to each side.

1. Change the following boundary names
X- symmetry
Y- symmetry

2. Set the types for boundaries accordingly
X- symmetry
X+ wall
Y- symmetry
Y+ wall
Z- wall
Z+ wall

## 7. Material Point

Material Point tells the meshing algorithm on which side of the geometry the mesh is to be retained. Since we are considering flow inside the cylinder we need to place the material point inside the geometry.

1. Switch to Point tab

2. Specify location inside the cylinder
Material Point110.7

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

## 8. Start Meshing

1. Go to Mesh tab

2. Start the meshing process with button

## 9. Examine Mesh

After the meshing process is complete, the mesh should appear in the graphics window. To zoom in or zoom out use the scroll wheel , or move the mouse up or down with pressed RMB (right mouse button).

## 10. Scale Mesh (I)

The model is defined in centimeters unit. We will rescale it to meters.

1. Expand the Options list next to default region

2. Select Scale

## 11. Scale Mesh (II)

1. Check Uniform option

2. Type Scaling Factors as 1e-02 and press Enter

3. Click

## 12. Select Solver - Spray

We want to analyze the transient simulation of spray combustion. For this purpose, we will use the sprayFoam solver.

1. Go to SETUP panel

2. Select the solvers

3. Filter the solvers by choosing Lagrangian models

4. Pick Spray (sprayFoam) solver

5. solver

## 13. Combustion - Mechanism

We will load the chemical kinetic mechanism as well as the thermodynamic properties database. We will consider only the one chemical reaction describing the process which is a simplification in order to decrease the computational cost and calculation time.

After that, import them to the SimFlow.

1. Go to Combustion panel

2. Click mechanism

3. For CHEMKIN Mechanism File select the chem.inp

4. For Thermodynamic Database File select the therm.dat

5. Click

6. Control the listed Species and Reactions

## 14. Combustion - Model

We will select the partially stirred reactor model which is used to simulate combustion.

1. Switch to Combustion tab

2. Select Combustion Model as a PaSR

## 15. Discrete Phase - Composition

We will select the pure heptane as a phase injected into the chamber.

1. Go to Discrete Phase panel

3. Check C7H16 phase and uncheck N2 phase

4. Set the C7H16 mass fraction to 1

## 16. Discrete Phase - Injection

We are going to create a cone injector and define its parameters.

1. Switch to Injection tab

3. Set Total Mass [kg] injection to 1e-04

4. Set Duration [s] injection to 1e-03

5. Set Parcels Per Second to 10000000

6. Set the velocity $$U_{mag} \; [m/s]$$ to 100

## 17. Discrete Phase - Injection Geometry

We need to define the position of the injector and spray outflow direction.

1. Go to Geometry tab

2. Set the position of injector
Position $$\sf{[m]}$$1e-031e-030.013

3. Set the injection direction
Direction $$\sf{[-]}$$110.35

4. Set the outer cone angle $$\Theta_{outer} \; [deg]$$ to 20

## 18. Discrete Phase - Injection Distribution

We will select the Rosin-Rammler distribution model and define the necessary parameters. Models need to define the minimum and maximum spray droplet diameter and size which is the largest probability.

1. Switch to Distribution tab

2. Select the Rosin-Rammler model from drop down list

3. Set the minimal, maximal and nominal droplet diameter:
Min $$\sf{[m]}$$1e-05
Max $$\sf{[m]}$$2e-04
d $$\sf{[m]}$$1e-04

## 19. 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 droplets. We choose the Ranz-Marshall heat transfer model to take into account heat transfer between the spray droplets and surrounding gas. For accounting mass transfer from the droplets to the gas as a result of the evaporation and boiling we use the Evaporation & Boiling model.

1. Switch to Models tab

2. Set the drag model as Sphare Drag

3. Set the heat transfer model as Ranz-Marshall

4. Set the drag model as Evaporation & Boiling

## 20. Turbulence

For the purpose of this tutorial, we will simulate the turbulence phenomenon using the Realizable $$k {-} \varepsilon$$ model.

1. Go to Turbulence panel

2. Select RANS turbulence formulation

3. Select Realizable $$k {-} \varepsilon$$ model

## 21. Solution - PIMPLE

To increase the stability of the simulation we will increase the number of iterations per time step.

1. Go to Solution panel

2. Switch to the PIMPLE tab

3. Set Outer Correctors to 2

## 22. Initial Conditions - Basic

Initially, the entire domain is filled with air. We will set the initial pressure and temperature in the chamber.

1. Go to Initial Conditions panel

2. Set the initial pressure in the chamber P to 5e6 Pa

3. Set the initial temperature in the chamber T to 800 Kelvin

## 23. Monitors - Temperature

In order to measure maximum and minimum temperature, we will use the volume monitor.

1. Go to Monitors panel

2. Expand the Fields for the Minimum volume monitors

3. Select the temperature field T

4. Repeat this step for the Maximum and Average volume monitors.
Selected fields will be visible next to the volume monitor names.

## 24. Run - Time Control

Before running computations, adjust the time controls in order to capture the physical and chemical phenomena that occur during the process.

1. Go to RUN panel

2. Set the Simulation Time [s] to 5e-03

3. Set the Time Stepping $$\Delta \sf{t[s]}$$ to 5e-06

## 25. Run - Output

We can control how often results should be saved on the hard drive. We will write the results at the interval of $$5e-05$$ second. Note, that only saved data will be available during postprocessing.

1. Switch to Output tab

2. Set the Interval [s] to 5e-05

## 26. Run - CPU

This simulation will require high CPU usage and might take several hours to finish the calculation depending on the machine used. To speed up the calculation process increase the number of CPUs basing on your PC capability. We recommend using at least 4 cores for this tutorial. The free version allows you to use only 2 processors in parallel mode. To get the full version, you can use the contact form to Request 30-day Trial

Estimated computation time for 2 processors: 2 hours

1. Switch to CPU tab

2. Use parallel mode

3. Increase the Number of processors

4. Click button

## 27. Results - Temperature

Keep track of the domain’s maximum and minimum temperature. A sudden increase in temperature is a result of the combustion process.

1. Switch tab to T in volume next to the residuals

## 28. Postprocessing - ParaView

After the computation is finished we can do a comprehensive visualization of our results with ParaView.

1. Go to POSTPROCESSING panel

2. Click on Run ParaView

## 29. ParaView - Load Results (I)

Load the results into the program.

1. Select turbidity_current

2. Click to load results into ParaView

## 30. ParaView - Load Results (II)

ParaView skips the initial time step by default, therefore we need to add the zero time to simulation.

1. Uncheck Skip Zero Time

2. Click

3. Click

4. Set the time or time step to 0

5. Select temperature T

## 31. ParaView - Clip

We will slice the domain in the direction of spray combustion.

1. Select Clip options from top menu

2. Define the origin and normal of the clip plane:
Origin000
Normal1-10

3. Click

4. Check the clip in the 3D graphic window

## 32. ParaView - Temperature (I)

Now we will check the temperature distribution during the process.

1. Uncheck Show Plane for better visualisation

2. Select Rescale to data range over all timesteps

3. Confirm choise by clicking

## 33. ParaView - Temperature (II)

1. Play with animation buttons to track the results of the analysis.

## 34. ParaView - Spray Phase

Finally, we will look at the spray particle movement.

1. Select C7H16 (partial) from the list

2. Click Rescale to Custom Data Range

3. Set the range from 0 to 0.1

4. Confirm by clicking

5. Play with an animation buttons to track the results of analysis.