The DPM panel in ANSYS Fluent is the main control center for your particles. It can look complex because it has many options. Every setting in this panel decides how your particles will move and behave in your simulation. If the settings are wrong, your results will be wrong, or your simulation might not finish. This is why understanding the DPM panel settings is so important.
In this guide, we will explain every important option, one by one. You will learn what each button does and when you should use it. We will make these particle tracking options easy to understand. Before we start with the panel settings, you must understand the basic ways to track particles. We explained this in our last guide about the difference between Steady and Unsteady tracking.
If you have not read it, please read it first: Complete Guide to Particle Life Cycle and Motion in DPM. This guide will help you master these settings. To see how these settings are used in real projects, you can explore our library of DPM CFD simulations.
Now, let’s look at the main panel you will be working with.
Figure 1: The main Discrete Phase Model (DPM) panel in ANSYS Fluent.
DPM Interaction Tab: How Particles and Fluid Affect Each Other
The first and most fundamental decision in the DPM panel is to define the relationship between the fluid (the continuous phase) and the particles (the discrete phase). This relationship is called coupling. It determines if the particles are just passive travelers in the flow or if they actively change the flow around them.
One-Way vs. Two-Way Coupling
The main idea of coupling is to decide how the phases exchange momentum and energy.
- One-Way Coupling: In this case, the fluid affects the particles, but the particles do not affect the fluid. This is suitable for simulations where the particles are very small or there are very few of them. The effect of the particles on the main fluid flow is so small that it can be ignored.
- Example: A few specks of dust moving in a large, ventilated room. The air movement dictates where the dust goes, but the dust does not change the airflow in the room.
- Two-Way Coupling: In this case, the fluid affects the particles, AND the particles affect the fluid. This is necessary when the particle phase is dense enough to change the momentum, turbulence, or temperature of the continuous phase.
- Example: A sandblaster. The high-speed air propels the sand particles, but the large mass of sand also slows down the air and changes its flow pattern.
Figure 2: A visual representation of One-Way Coupling (top) where the fluid influences particles, and Two-Way Coupling (bottom) where the fluid and particles influence each other.
In ANSYS Fluent, you control this with a single checkbox.
- To select One-Way Coupling, you leave the “Interaction with Continuous Phase” box unchecked.
- To select Two-Way Coupling, you check the “Interaction with Continuous Phase” box.
Figure 3: The Interaction settings, which control the coupling between the continuous and discrete phases.
Controlling the Update Frequency
When you enable Two-Way Coupling, you must also control how often the particles give their information back to the fluid.
- DPM Iteration Interval: The setting “Number of Continuous Phase Iterations per DPM Iteration” controls this frequency. It tells the solver how many fluid calculations to perform before pausing to get a DPM update.
- A low value (e.g., 1-5) means very frequent communication. This is called “tight coupling” and is more accurate per step but can sometimes be less stable.
- A high value (e.g., 10-20) means less frequent communication. This is called “loose coupling” and is generally more stable. The default of 10 is a good starting point for most cases.
- Update in Unsteady Calculations: The “Update DPM Sources Every Flow Iteration” checkbox is a specific control for unsteady (transient) simulations.
- When this is ON, the particle effects (source terms) are calculated and given to the fluid solver at every single fluid iteration within a time step. This ensures the tightest possible coupling for time-accurate results and is highly recommended for unsteady simulations.
Tracking Tab: How the Computer Finds the Path
The Tracking tab controls how the computer calculates the particle’s path. These settings are very important for getting a correct answer without waiting too long. You are finding a balance between a correct answer and a fast calculation.
Figure 4: The Tracking Parameters section, which controls the numerical integration of the particle trajectory.
Max. Number of Steps:
The “Max. Number of Steps” is a safety control.
- What it is: It is the highest number of steps the computer can use for one particle’s journey.
- Why we need it: Sometimes, a particle gets stuck in the flow, like a leaf caught in a small whirlpool. Without this limit, the computer would try to follow that stuck particle forever. Your simulation would never finish.
- What happens if the number is wrong: If this number is too small, the computer stops tracking a particle too early. The particle’s journey is not finished. In your report, this particle will be called “incomplete.” This is an error. If you see many “incomplete” particles, you must use a bigger number (like 5000 or more).
Step Size: The Most Important Choice Here
The computer moves the particle in many small steps to find its full path. Think of drawing a curve by connecting many tiny, straight lines. Each tiny line is a step. The size of this step is very important.
- Small steps = more correct path, but slow calculation.
- Big steps = fast calculation, but the path can be wrong.
You have two ways to control the step size: “Step Length Factor” or “Specify Length Scale”. You must choose one.
- Step Length Factor (Best for most cases)
- What it is: You give a simple number, like 5.
- How it works: This number tells the computer how many steps to take to cross one cell of your mesh. If the number is 5, the computer takes 5 small steps to move the particle through one cell.
- Why it is good: It is smart. It automatically uses small steps in areas with a small mesh (like near a wall). It uses bigger steps in areas with a big mesh. For almost all simulations, this is the best method. Start with the number 5.
- Specify Length Scale
- What it is: You give a fixed length, in meters (for example, 0.001 m).
- How it works: The computer makes sure that in one step, the particle does not travel more than this length.
- When to use it: Use this only when you know the size of a very small, important feature in your model and you want to be sure the particle path is calculated carefully in that specific area.
‘Unsteady Particle Tracking’ Settings
Sometimes, you need to know more than just where a particle ends its journey. You need to know where it is at every moment in time. For this, you must use Unsteady Particle Tracking.
As we talked about in our blog on steady and unsteady tracking, this method is key for simulations where things change with time. To use these settings, you must first check the “Unsteady Particle Tracking” box. When you check it, new options will appear.
Figure 5: The “Unsteady Particle Tracking” options, which let you control how particles are tracked over time.
This section covers two main situations, just like we discussed in our previous blog:
- Tracking particles over time in a steady fluid flow.
- Tracking particles over time in an unsteady fluid flow.
Case 1: Unsteady Tracking with a Steady Flow
This is a special case. Imagine your fluid flow is stable and not changing (steady). However, you want to see where particles travel over a specific time period.
In this mode, the computer ADVANCES each particle. This means it does not start the particle’s journey over from the beginning. Instead, it continues from where the particle was last. The following settings control this:
- Particle Time Step Size (s): This is the size of each “time jump” for the particle. A small number (like 0.001) means the computer calculates the particle’s position very often, giving you a very detailed history.
- Number of Time Steps: This tells the computer how many of these time jumps to calculate at once. If the “Time Step Size” is 0.001s and the “Number of Time Steps” is 10, Fluent will calculate the particle’s path for the next 0.01 seconds.
Figure 6: Particle Treatment regarding steady flow solver
Case 2: Unsteady Tracking with an Unsteady Flow
This is the most common use. Here, the fluid itself is changing with time, and the particles must react to these changes moment by moment. You have two main ways to control the timing.
Option A: Track with Fluid Flow Time Step (The Simple Method)
This is the easiest and most recommended method. You check the box “Track with Fluid Flow Time Step.”
This tells the particles to use the exact same clock as the main fluid flow. If your fluid simulation takes a time step of 0.01s, the particles also take a time step of 0.01s. There is only one particle step for each fluid step. As a Result: The particle and fluid movements are perfectly synchronized.
Figure 7: unsteady Flow solver + Track particles with Fluid Flow Time Step
Option B: Use a Different Particle Time Step (The Advanced Method)
You use this when the particle’s path changes very quickly, and the main fluid time step is too large to capture that fast motion.
You set a “Particle Time Step Size” that is smaller than your main fluid time step. The computer will then take many small particle steps inside one big fluid step. For example, if the fluid time step is 0.1s and the particle time step is 0.01s, the computer will calculate the particle’s position 10 times to find where it is at the end of the 0.1s fluid step.
Figure 8: Different time step size for continuous and discrete phases
Why is there an “Inject Particles at” option?
This option only appears when you use a different particle time step. It is a very important setting. It does not control the movement of existing particles. Instead, it answers the question: When should the computer add new groups of particles (parcels) into the simulation?
You have two choices:
- Inject at Fluid Flow Time Step: Choose this if you want to add new particles only at the start of each main fluid time step. This is a common choice.
- Inject at Particle Time Step: Choose this if your injection is very continuous, and you want to add new particles at the start of every small particle time step. This creates a smoother, more constant stream of new particles.
Note that, even when you use many small particle steps, Fluent makes sure that the final particle positions always line up with the main fluid clock. This keeps the entire simulation physically correct and synchronized.
Conclusion
In this guide, we have looked at the most important settings in the Fluent DPM panel. These choices control how the solver tracks particles, how they interact with the fluid, and how they move through time. Choosing the right settings is essential for getting an accurate result without wasting calculation time.
To help you make the right decision for your project quickly, use this simple reference table. It summarizes the main tracking methods we discussed.
| If Your Situation Is… | Your Recommended Setting | Why This Is the Best Choice |
| My fluid flow is steady, and I only need to know the final path of the particles. | Use Steady Particle Tracking. (The “Unsteady Particle Tracking” box should be unchecked). | It is the simplest and fastest method. It calculates the entire particle journey in one step. |
| My fluid flow is steady, but I need to see the particle’s position at different moments in time. | Check Unsteady Particle Tracking. Then, set a “Particle Time Step Size” and “Number of Time Steps”. | This gives the particles their own clock. They can move through the frozen fluid flow over time. |
| My fluid flow is unsteady, and the particles must move with the changing fluid. | Check Unsteady Particle Tracking. Then, check the box for “Track with Fluid Flow Time Step”. | This is the easiest and most reliable method. It makes sure the particle and fluid clocks are the same (synchronized). |
This guide covers the fundamental choices for particle tracking. However, every engineering problem is unique. Many simulations involve more complex physics, such as spray atomization, particle erosion, or turbulent dispersion.
If your project requires a detailed and professional DPM analysis, the experts at CFDLAND are here to help. Explore our wide range of DPM CFD Simulation services to see how we can provide you with accurate and reliable results for your specific needs.