DPM Parcel Concept In ANSYS Fluent

Imagine you need to simulate a diesel fuel spray. This spray has millions of tiny droplets. If you try to track each droplet one by one, your computer would need weeks or even months to finish the calculation. This is a common and serious problem in CFD.

The DPM parcel concept in ANSYS Fluent solves this problem. Instead of tracking millions of individual particles, we group them into “parcels.” Each parcel represents many particles that share the same properties. This makes simulations much faster while keeping the results accurate. For anyone working with DPM CFD simulations, this concept is fundamental.

In this complete guide, you will learn:

• What exactly a DPM parcel is.
• Why using parcels can make your simulations over 100 times faster.
• How to calculate the number of particles in each parcel.
• Which parcel release method is right for your specific simulation.

Figure 1: An illustration of the DPM Parcel concept. Instead of tracking each individual particle (small dots), the simulation tracks a single ‘parcel’ (the large blob) that represents a group of particles sharing the same properties.

What is a Parcel in DPM?

So, what exactly is a parcel?

In the simplest terms, a parcel is a single computational “blob” or group that we track in a simulation. This single parcel represents many real particles that all have the same properties.

This means all the particles inside one parcel share the same:

• Size (diameter)
• Speed and direction (velocity)
• Location
• Temperature
•  And other physical properties.

This powerful idea was first introduced by Dukowicz in 1980 to solve the problem of simulating huge numbers of particles. Because all particles in the group are identical, we only need to calculate the path and behavior of the parcel itself. The simulation assumes that every particle within that parcel will behave in the exact same way.

Interestingly, a parcel can represent a non-whole number of particles, like 308.04 particles. This is a mathematical method that ensures the total mass flow rate in the simulation remains perfectly accurate.

Figure 2: A simple diagram showing many small dots (particles) being grouped into a larger circle (parcel)

 

Why Use Parcels Instead of Individual Particles?

The main reason we use the DPM parcel concept is for computational efficiency. It saves a huge amount of time and computer power.

Let’s use a real example from your reference material. A typical diesel fuel spray can contain millions of tiny fuel droplets. A study mentioned in the guide showed that tracking just 5,000 individual particles took 12 hours on a powerful 8-CPU computer cluster. Now, imagine a simulation with 10 million particles. Tracking each one would be practically impossible.

The DPM parcel concept solves this problem. By grouping thousands of identical particles into a single parcel, the computer only needs to track a few thousand parcels instead of millions of particles. This drastically reduces the number of calculations needed. Your simulation can run hundreds or even thousands of times faster, turning an impossible task into a standard one. Here is a simple table to show the difference:

Feature	Tracking Individual Particles	Using DPM Parcels
Computational Cost	Extremely High	Low / Manageable
Simulation Time	Days / Weeks / Months	Hours / Days
Memory Needed	Very Large	Small
Feasibility for Large Problems	Often Impossible	Possible and Practical

In short, the DPM parcel concept is the key that makes large-scale, industrial particle simulations possible in ANSYS Fluent. Without it, many of the complex spray, combustion, and multiphase flow simulations we do today would not be feasible.

 

How to Calculate the Number of Particles Per Parcel

Now for the most important question: How does ANSYS Fluent know how many particles to put in each parcel? You can calculate this yourself to understand and verify your simulation setup. This is especially important for unsteady DPM simulations. The main formula is very simple:

Number of Particles per Parcel = (Mass of one Parcel) / (Mass of one Particle)

   

​

Step 1: Find the Mass of a Single Particle

First, we need to know how much one single particle “weighs.” Since DPM assumes particles are perfect spheres, we use the formula for the volume of a sphere and multiply it by the particle’s density.

Particle Mass = Particle Density * (π/6) * (Particle Diameter)³

Step 2: Find the Mass of a Single Parcel

Next, we calculate the total mass represented by one parcel. This depends on your total injection mass flow rate, how often particles are injected (time step), and how many injection streams you have.

Parcel Mass = (Injection Mass Flow Rate * Particle Time Step Size) / Number of Streams​

Step 3: Put It All Together (A Practical Example)

Given Inputs:

• Injection Mass Flow Rate: 0.0001 kg/s
• Particle Density: 1550 kg/m³
• Particle Diameter: 0.00001 m (or 10 microns)
• Particle Time Step Size: 0.0005 s
• Number of Streams: 200

Calculation:

Particle Mass=1550×6π​×(0.00001)3=8.116×10−13 kg

Parcel Mass=2000.0001×0.0005​=2.5×10−10 kg

Number of Particles per Parcel=8.116×10−132.5×10−10​=308.04

As you can see, the result is 308.04 particles per parcel. It is perfectly normal and correct for this to be a fractional number. It is a mathematical method Fluent uses to ensure the mass in the simulation is perfectly conserved.

         

Figure 3: A comparison showing the input parameters in ANSYS Fluent and the resulting “Particle Number in Parcel” calculated by the software, matching our manual calculation.

Parcel Release Methods in ANSYS Fluent

When you run an unsteady simulation, you need to tell Fluent how to release the parcels into your domain over time. ANSYS Fluent provides four different Parcel Release Methods for this purpose. Choosing the right one depends on your specific simulation needs.

Figure 4: The Parcel Release Method options available in the ANSYS Fluent injection properties panel.

Here is a simple guide to each method:

Release Method	How It Works	Best For
Standard	This is the simplest option. It releases a single parcel stream at each particle time step.	Basic or simple simulations where precise control over the number of parcels is not critical.
Constant Number	You specify the exact number of particles you want in each parcel. Fluent then automatically calculates how many parcels it needs to release to match your total mass flow rate.	Sprays and simulations with a Particle Size Distribution (PSD). This is a very common and recommended method for controlling the simulation’s statistical representation.
Constant Mass	You specify the total mass of each parcel. Fluent uses this to determine the number of particles in the parcel based on their diameter.	Discrete Element Method (DEM) simulations or cases where you need to ensure the parcel size does not become larger than the mesh cells.
Constant Diameter	You specify the diameter of the parcel itself (not the particles inside). This also helps control parcel size relative to the mesh.	Also recommended for DEM simulations and situations requiring strict control over the parcel’s spatial size.

In summary, for most spray and general DPM simulations, the Constant Number method is a great starting point. For specialized simulations like DEM where parcel-mesh interaction is critical, Constant Mass or Constant Diameter are better choices.

Difference Between Particle Parcel and Stream

There is another confusion for users about the definition of a particle stream in DPM (see Fig. 3). The number of streams corresponds directly to the number of locations where parcels are injected. According to the discrete phase model formula, the relationship between stream mass flow rate, injection time interval, and the number of particles in a parcel is clearly defined. The number of particles in each parcel can be fractional, allowing for more precise simulations. However, this definition belongs to the unsteady (transient) simulation. For Steady DPM simulations, the concept slightly differs. Instead of using the number of particles in a parcel, ANSYS Fluent employs “strength,” which represents the number of particles in a parcel per second. This approach allows for continuous particle injection in steady-state simulations.

 ** It’s worth noting that Ansys Fluent’s user documentation often refers to parcels as “particles,” which can sometimes lead to confusion. Understanding these distinctions and relationships is key to effectively utilizing DPM in CFD simulations.

Figure 3: Number of particle stream in DPM Fluent

 

Conclusion

In this guide, we have explained the DPM Parcel concept in ANSYS Fluent from the ground up.

You have learned:

• A parcel is a smart way to group many identical particles into one computational unit.
• We use parcels to make complex simulations with millions of particles run much faster, turning impossible tasks into practical ones.
• How to calculate the number of particles in each parcel using a simple, step-by-step formula.
• How to choose the correct Parcel Release Method for your specific simulation, whether it’s for a spray or a DEM analysis.

The DPM parcel concept is more than just a setting in Fluent; it is the fundamental technique that makes large-scale particle simulation possible. By understanding and using parcels correctly, you can confidently simulate complex systems like fuel sprays, cyclone separators, and pneumatic transport, all while saving significant time and computational resources.

Mastering multiphase flows is a crucial skill for any CFD engineer. If your projects require expert analysis or you need assistance with complex DPM CFD Simulations, the team at CFDLAND is ready to help.