DPM Injection Types in ANSYS Fluent – Direct Methods

Introduction: Understanding DPM Injection Types in ANSYS Fluent

When you work with particles or droplets in ANSYS Fluent, the first question is always: How do I inject these particles into my domain? The answer lies in choosing the right injection type from Fluent’s Discrete Phase Model (DPM).

Whether you’re simulating fuel spray in an engine, powder coating, or particle separation, selecting the proper injection type is crucial. Each injection method has its own purpose and works best for specific applications. For those looking to learn all aspects of DPM simulation, you can explore our comprehensive DPM CFD Simulation Tutorials.

In ANSYS Fluent, you have six main injection types to choose from. Think of these as different ways to introduce particles into your flow field. Some are simple, like releasing particles from a single point. Others are complex, like modeling a real fuel injector with atomization physics.

This guide will walk you through each DPM injection type, explaining when to use it, how to set it up, and what makes it unique. By the end, you’ll know exactly which injection method fits your simulation needs.

Figure 1: DPM injection types selection panel in ANSYS Fluent

Categorizing Injection Types: A Complete Guide

In any Discrete Phase Model (DPM) simulation, the injection is the starting point. It defines how and where particles enter your simulation domain. Getting this right is the most critical step for an accurate result. ANSYS Fluent offers a wide range of DPM injection types, which can seem complex at first. However, they are logically divided into two main categories, based on a simple question: Do you already know the initial state of your particles, or do you need Fluent to calculate it for you?

1. Direct Injection Methods: You use these when you can directly specify the particles’ starting location, size, velocity, and temperature.
2. Atomizer Models: You use these when you have a bulk liquid that breaks up into smaller droplets (a process called atomization). These models simulate the physics of the breakup to determine the initial state of the droplets for you.

The table below provides a complete overview of all the injection types available in ANSYS Fluent, including special cases.

Injection Category	Injection Type	Primary Use Case
Direct Injection	Single	Injecting a single stream of particles from one specific point.
	Group	Injecting multiple particle streams along a defined line.
	Cone (Hollow/Solid)	Creating a conical spray pattern when the spray angle is known. (3D only)
	Surface	Releasing particles from every face on a selected boundary or surface.
	Volume	Filling a cell zone with particles at the beginning of a simulation. (3D unsteady only)
	File	Injecting particles with complex starting conditions read from an external text file.
Atomizer Models	Plain-Orifice	Simulating a solid liquid jet forced through a simple hole (e.g., diesel injectors).
	Pressure-Swirl	Modeling nozzles that use internal swirl to create a hollow-cone spray.
	Air-Blast / Air-Assist	Simulating sprays where a high-speed gas stream helps break up the liquid.
	Flat-Fan	Modeling injectors that create a flat, fan-shaped liquid sheet that then atomizes.
	Effervescent	For super-heated liquids that flash-boil and atomize as they exit the nozzle.
Specialized Injection	Condensate	Modeling the creation of particles due to condensation on a wall film.

In the following sections, we will explore the Direct Injection and Atomizer Model categories in more detail.

Direct Injection Methods: When You Know Your Particle’s Initial State

Single Injection Method

The Single Injection is the most fundamental and straightforward DPM injection type in ANSYS Fluent. As the name suggests, it releases a stream of particles from a single, precise coordinate point in your domain. You should use this method when you need to:

• Trace the path of a single particle to understand its trajectory.
• Simulate a very small, concentrated source of particles, like a tiny nozzle or orifice.
• Perform a simple test to check your DPM settings before running a more complex case.

Figure 2: A single particle being injection and moving through a channel

Key Properties in the Fluent Setup

To set up a single injection, you need to provide the initial state of the particles directly. These are the most important parameters you will define in the “Set Injection Properties”

• Position (X, Y, Z): This is the exact coordinate where the particles are introduced into the simulation.

• Velocity (X, Y, Z): This defines the initial speed and direction of the particles.
• Diameter: The initial size of the particles.
• Temperature: The initial temperature of the particles.
• Flow Rate: The total mass of particles being injected per second (in kg/s).
• Start and Stop Time: For unsteady (transient) simulations, this controls when the injection turns on and off.

Figure 3: Single injection setup panel in ANSYS  showing key parameters

This method gives you complete control over the initial conditions. It is the perfect starting point for learning the Discrete Phase Model because of its simplicity and directness.

 

Group Injection

The Group Injection is a powerful extension of the Single Injection. Instead of releasing particles from one point, it injects multiple particle streams evenly spaced along a straight line. This is extremely useful for simulating things like a rake of injectors or creating a curtain of particles.

Figure 4: Group injection creating multiple parallel particle streams

To set this up, you don’t define just one point; you define the start and end of a line, and Fluent fills in the streams between them.

Here are the unique properties you define in the software for a Group Injection:

• First Point: You set all the initial properties (Position, Velocity, Diameter, etc.) for the first stream in the group, just like a Single Injection.
• Last Point: You set the corresponding properties for the last stream in the group. Fluent will automatically calculate the properties for all the streams in between by smoothly transitioning (interpolating) between the first and last point values.
• Number of Streams: This is a crucial setting where you tell Fluent exactly how many particle streams to create along the line.

Figure 5: The ‘Set Injection Properties’ panel in ANSYS Fluent for a Group Injection. Users define the ‘First Point’ and ‘Last Point’ properties, along with the ‘Number of Streams’ (in this case, 20) to create the particle rake

 

Cone Injection

The Cone Injection is one of the most powerful and frequently used DPM injection types in ANSYS Fluent, especially for spray simulations. You use it when you want to inject particles in a conical pattern and you already know the shape of the spray, such as its angle. This method gives you precise control over the spray’s geometry.

In the software, the “Cone” type is actually a family of four different methods, each defining a different way particles are released.

Figure 6: Cone injection geometry showing spray angle and axis direction

Four Types of Cone Injections

Understanding these four types is the key to using the cone injection effectively.

1. Point-Cone: This is the simplest type. All particle streams originate from a single X-Y-Z point and fan out to form the cone.
2. Solid-Cone: Particles are released from the entire area of a circular disk. This creates a filled, solid spray pattern.
3. Hollow-Cone: Particles are released only from the outer edge (the circumference) of a circular disk. This creates an empty, hollow spray pattern.
4. Ring-Cone: This is a variation of the hollow cone. Particles are released from an annular ring, which has both an inner and outer radius.

Figure 7: Comparison of four cone injection patterns: Point, Solid, Hollow, and Ring

Key Properties in the Fluent Setup

When you set up a cone injection, you need to define these crucial parameters in the panel:

• Cone Type: You must first choose one of the four types listed above (Point, Solid, Hollow, or Ring).
• Position & Axis: The X-Y-Z coordinate for the cone’s apex (or center of the disk) and the vector direction of the cone’s central axis.
• Cone Angle [deg]: This is the half-angle (θ) of the cone. It defines how wide or narrow the spray is. A 30-degree angle creates a spray with a total width of 60 degrees.
• Velocity Magnitude: This is the total speed of the injected particles. Fluent breaks this down into different components to form the spray.
• Outer Radius: Defines the size of the disk for Solid, Hollow, and Ring injections.
• Inner Radius: Used only for the Ring-Cone injection to define the inner boundary of the ring.
• Total Flow Rate: The total mass of particles injected per second (kg/s).

Figure 8: Cone injection configuration panel in ANSYS Fluent

 

Fluent creates the conical shape by calculating the total velocity of each particle stream from its axial, radial, and swirl components. This ensures the particles follow the correct trajectory to form the cone you defined.

The cone injection is not just theoretical; it’s used in serious engineering validation projects. For example, in our study on Evaporative DPM Cooling with Mist Spray, we successfully used the solid-cone injection type. It allowed us to accurately model the mist spray from the nozzles and validate our CFD simulation results against experimental data for evaporative cooling.

Figure 9: Mist spray validation using solid-cone injection for evaporative cooling

 

Surface Injection

The Surface Injection is an incredibly versatile method in ANSYS Fluent DPM. Instead of defining points or shapes, you select an entire surface (like an inlet or a wall), and Fluent releases particles from every single face on that surface. This is the best way to introduce particles over a large, defined area.

This method is ideal for simulations where the particles originate from a wide area rather than a single point. It is the perfect tool for many industrial and environmental applications.

• Cyclone Separators: To model the entry of dust-laden gas, particles are injected across the entire inlet surface. We used this exact method in our Cyclone CFD Simulation validation project.
• Ventilation and Contaminant Spread: To simulate airborne particles like dust or viruses, a surface injection can represent the source. This was crucial in our analysis of Operating Room Ventilation to remove virus particles.
• Seeding a Flow: If you want to see how particles behave throughout your domain, you can seed the entire inlet with them. Our Particles Surface Injection training product covers the setup for this type of problem in detail.

Figure 10: Industrial applications of surface injection in CFD simulations

Key Properties in the Fluent Setup

Setting up a surface injection is straightforward. In the “Set Injection Properties” panel, you will:

1. Change the Injection Type to surface.
2. Select the desired surface from the “Surface” dropdown list.
3. Define the properties for all particles released from this surface, such as their velocity, diameter, temperature, and the total mass flow rate.

Fluent then automatically handles the release of particles from every mesh face on your chosen surface, ensuring an even and realistic distribution.

Figure 11: release of particles from every mesh face on your chosen surface

Figure 12: Surface injection setup panel with boundary selection

Volume Injection

The Volume Injection is a specialized method used for a very different purpose. Unlike other types that inject particles into the domain over time, a Volume Injection instantly fills a predefined cell zone with particles at the start of an unsteady simulation (at time = 0). This method does not inject a flow of particles; it “patches” a region with a certain amount of the discrete phase.

This is the perfect tool for simulations where the domain is already full of particles before the flow begins. It is essential for modeling:

• Fluidized Beds: Where a bed of particles is initially settled at the bottom of a container.
• Hoppers and Silos: Simulating the discharge of grain or powder that is already filling the container.
• Any Unsteady 3D Simulation: Where you need to define an initial state with particles already present in a specific region.

Figure 13: Volume injection creating initial particle distribution in a cell zone

Key Properties in the Fluent Setup

The setup for a Volume Injection is unique, as you can see in the panel below.

• Release From: You must select zone and then choose the specific fluid cell zone you want to fill.
• Parcel Specification: You define the number-of-starting-points, which tells Fluent how many particle parcels to create within the volume. These parcels are then distributed randomly and uniformly throughout the zone.
• Initial Velocity: Often, the initial particle velocities are set to zero or matched to the surrounding fluid velocity at time=0.
• Specifying the Amount: Instead of a Flow Rate, you typically specify the amount of particles using:
  • Total Mass: The total mass of all particles to be placed in the volume.
  • Volume Fraction: You can tell Fluent to fill the zone until a certain particle volume fraction is reached.

The result is a volume that is instantly populated with particles at the start of your simulation, ready for the fluid flow to interact with them.

Figure 14: Volume injection configuration for unsteady simulations

Note that If the injection Stop Time and Start Time are in different fluid flow time steps, then the particles will be injected at once in the Fluid Time Step that includes the middle of the injection time interval.

 

File Injection

The File Injection is the most powerful and flexible injection method in ANSYS Fluent. Instead of using the software’s built-in shapes, you provide a simple text file that contains all the initial data for every particle stream. This gives you complete and total control over the injection process.

You should use this method when your particle starting conditions are too complex for the standard types or when they come from an external source.

• Complex Geometries: When the injection source doesn’t fit a simple point, line, or surface.
• Experimental Data: If you have measured particle data (position, velocity, size) from a real-world experiment, you can format it into a file and use it directly in your simulation.
• Coupling with Other Software: This is a major application. You can use programs like MATLAB or Python to perform calculations and generate a custom particle injection file. This is exactly how we approached our DDPM-DEM simulation of grain drying, where MATLAB was used to create a file defining the initial state of every grain.

Figure 15: File injection workflow from external data to CFD simulation

Key Properties and the File Format

To use this method, you first select file as the Injection Type. Then, you simply select your prepared text file. The real work is in creating this file correctly.

The format is very specific but simple. Each line in the file defines a single particle stream (or “parcel”). For a steady-state simulation, the format is:

( ( x y z u v w diameter temperature mass-flow ) name )

Where:

• (x y z) are the coordinates of the particle’s starting position.
• (u v w) are the components of the particle’s initial velocity.
• diameter is the particle diameter.
• temperature is the particle temperature.
• mass-flow is the mass flow rate for that specific particle stream.
• name is an optional name for the stream.

The most important thing is to get this format exactly right, including the parentheses. Unsteady file formats are similar but include start and stop times for the injection on each line.

Figure 16: File injection panel for importing custom particle data

Conclusion

Understanding DPM injection types in ANSYS Fluent is fundamental for accurate particle-based CFD simulations. Throughout this guide, we’ve explored the seven primary injection types – from simple single injections to complex file injections – each serving specific simulation needs. While this guide covered the fundamental injection types, the world of spray modeling extends further. Atomizers represent the next level of sophistication in DPM simulations, offering advanced breakup models and detailed spray physics for applications requiring high-fidelity droplet dynamics. Ready to enhance your CFD simulations? Explore our DPM tutorials and projects or contact our experts for customized simulation support.