The Eulerian Granular Model is how CFD handles the one problem a standard fluid solver cannot: solid particles that collide, jam, and refuse to be squeezed past their packing limit. Particulate flows like these run through nearly every heavy industry. Engineers constantly use CFD to simulate solid particles moving inside a fluid for oil and gas refineries, chemical processing plants, pharmaceutical factories, food processing facilities, and deep mining projects. In these gas-solid or liquid-solid flows, the small solid particles interact strongly with the surrounding continuous fluid. To resolve these coupled interactions with genuine accuracy, you need to activate this advanced granular model in your simulation software, which is a dedicated extension of the Eulerian multiphase model. If you want to learn how to simulate these particle regimes in the software, you can practice with our step-by-step Multiphase CFD simulation tutorials.
When you start a new particulate flow project, you first need to look at your particle concentration to understand the physical coupling. If your tank has a low number of particles with large empty spaces between them, we call this a dilute flow. In dilute flows, you usually have basic one-way or two-way coupling, which simply means the main fluid pushes the particles, and sometimes the moving particles push the fluid back. However, if your tank contains a massive number of particles packed closely together, we call this a dense flow. In dense flows, you need to calculate four-way coupling because the fluid pushes the particles, the particles push the fluid back, and the particles constantly crash into each other at the same time.
Figure 1: physical regime map showing how increasing the particle volume fraction changes the flow from a simple collision-free state to a dense friction-dominated state
Depending on the total volume fraction of your solids, the mathematical solver will see three different physical particle-particle interactions. In very dilute concentrations, you have a simple collision-free flow because the particles have too much empty space and rarely touch each other. As the particle concentration increases to an intermediate level, the flow changes into a collision-dominated state where fast particles continuously hit and bounce off each other. Finally, when the solid particles are packed very tightly together at the maximum physical limit, the flow becomes friction-dominated because the particles do not have any empty space to bounce, so they just constantly rub against each other.
Granular Flow Regimes
When millions of solid particles move together inside an industrial tank, their physical behavior completely changes based on their speed and how closely they are packed. To accurately simulate these particles, scientists divide this complex movement into three completely different physical categories.
Here are the three distinct granular flow regimes:
- 1. The Quasi-Static Regime (Very Slow Flow): This physical condition happens when the particles are packed tightly together and move slowly, like heavy dirt moving in soil mechanics. Because the particles do not have space to bounce, they just constantly rub against each other. In this slow state, the mathematical solid stress is independent of the flow speed (the strain rate, γ˙). The mathematical equation is written as
- 2. The Intermediate Regime (Medium Flow): This is the middle transition state. The particles start to move a little faster and have a little bit more empty space between them. Because the flow is faster, the mathematical solid stress starts to depend on the physical strain rate. The governing equation relates the stress to the strain rate using a fractional power, written as:
- 3. The Inertial Regime (Rapid Flow): This happens in fast and rapid flows where the particles fly freely and crash into each other. Because the particles hit each other with high kinetic energy, the physical stress depends heavily on the square of the flow speed. The mathematical equation for this rapid regime is written as:
Fluidization Regimes: These three stress regimes appear inside gas-solid reactors as distinct fluidization regimes. As you raise the gas velocity past the minimum fluidization velocity, a fixed bed passes through bubbling, slugging, turbulent, and finally fast-fluidization or pneumatic transport. Each of these fluidization regimes maps onto a different granular stress balance, which is why one universal drag or viscosity setting cannot cover an entire reactor operating range. To set this up properly, you need to match your closures to the specific two-phase flow regime you are simulating.
You must clearly understand these three physical categories because the software uses the advanced Kinetic Theory of Granular Flow (KTGF) to solve the rapid inertial regime, but you must strictly activate different frictional stress equations to correctly solve the slow quasi-static regime.
Figure 2: The granular regime map shows exactly how the physical stresses change from slow friction-dominated movements to rapid collision-dominated flows.
Why We Need the Granular Model
If you attempt to simulate a dense particle bed with a standard two-fluid formulation and no granular closures, the solver returns physically impossible results. That formulation only sees the particles as a simple fluid and allows them to pack together infinitely without any natural resistance. To stop this error, you need the Eulerian Granular Model. This model adds special mathematical equations for solids pressure and granular viscosity, which force the particles to bounce off each other and resist heavy packing.
To completely prove why this advanced model is absolutely necessary, we can look at the main graphical contours from our professional tutorials. Here are three practical examples showing the power of the granular model:
- Gas-Solid Fluidized Bed Hydrodynamics CFD Simulation: In this numerical paper validation, the granular equations perfectly calculate the exact Voidage Profile. This crucial contour represents the empty space (air) in the mixture and accurately shows three distinct zones: a dense lower zone, a transitional region, and a dilute upper region. Because the model calculates the particle collisions correctly, you can clearly visualize the Solid-phase volume fraction and the complex Bubble behavior showing the formation, expansion, and coalescence of bubbles with errors not exceeding 10%. We even extract the Residence Time Distribution (RTD) to validate the highly accurate dynamic behavior against experimental data.
- Biomass Pyrolysis in Conical Spouted Bed Reactor CFD Simulation: In this complex reactor project, the granular physics are strictly required to create the correct flow shape. The main Solid particle volume fraction contour perfectly illustrates the characteristic “spouting” pattern, where a central high-speed jet drives the particle circulation. You can also clearly see the Velocity field driving the circulation and a very stable Temperature contour ranging from 372 K to over 729 K, proving the thermal mixing is highly accurate.
- Sedimentation in Elbow – Granular Multiphase Flow: In this ANSYS Fluent training, we simulate heavy particles moving inside a bent pipe. The primary contour is the volume fraction of the hydrate phase (R11). Because we use the physical granular equations, this contour visually represents exactly how the solid hydrates settle, rub against the walls, and heavily stratify at the bottom of the horizontal section due to gravity and changing viscosity gradients.
You must strictly enable the Eulerian Granular Model whenever your solid volume fraction is high enough for particles to touch or crash into each other, otherwise, your density and volume fraction contours will be completely physically wrong.
Kinetic Theory of Granular Flow (KTGF)
To mathematically calculate how millions of solid particles bounce and crash, the software uses the Kinetic Theory of Granular Flow (KTGF). This advanced framework is based exactly on the famous kinetic theory of gases, but it is modified specifically for solid spheres.
In a normal gas, tiny molecules bounce off each other perfectly without losing any speed. However, real solid particles have non-conservative physical interactions. Every time two real solid spheres collide, some kinetic energy is permanently lost to inelastic deformation and surface friction. The solver quantifies this through the restitution coefficient (ess), a value between 0 and 1 that sets how much rebound velocity survives an impact. A value of 1 means a perfectly elastic bounce; typical fluidized-bed particles sit between 0.9 and 0.99. To accurately solve these complex physics, the KTGF divides the particle movement into two different transport mechanisms:
- 1. Kinetic Transport (Free Flight): This physical mechanism happens when the solid particles fly completely freely through the empty fluid space. During this rapid free flight between the crashes, the moving particles carry their own physical kinetic energy.
- 2. Collisional Transport (The Crash): This physical mechanism happens at the exact moment when two or more particles violently hit each other. During this heavy crash, the particles physically transfer their momentum to each other and immediately lose energy.
Figure 3: The Kinetic Theory of Granular Flow calculates both the free flight of particles (kinetic transport) and the violent crashes between them (collisional transport).
You must strictly use the KTGF equations to correctly calculate this physical energy loss and accurately capture the bouncing particle behavior in high-speed industrial processes.
For a practical example, you can look at our Spouted Bed CFD Simulation using Two Fluid Method (TFM) Training, which is exactly why the two-fluid model (TFM) framework treats the particle cloud as an interpenetrating continuum.
Granular Temperature
In the Eulerian Granular Model, the term “granular temperature” has absolutely nothing to do with real thermal heat. Instead, it is purely a mathematical concept used to measure the random bouncing energy of the solid particles. Just like hot gas molecules move much faster than cold ones, a high granular temperature simply means the solid particles are violently crashing into each other at very high speeds. Mathematically, it is defined as the average of the square of the fluctuating particle velocities, written as 
.
To accurately track this bouncing energy inside your tank, the software solves a special granular temperature equation. This equation balances how the kinetic energy is created, moved, and destroyed during the flow. The full transport equation solved by ANSYS Fluent takes the form:
![\frac{3}{2}\left[\frac{\partial}{\partial t}(\rho_s \alpha_s \theta_s) + \nabla \cdot (\rho_s \alpha_s \vec{v}_s \theta_s)\right] = (-P_s \bar{\bar{I}} + \bar{\bar{\tau}}_s):\nabla \vec{v}_s + \nabla \cdot (k_{\theta s} \nabla \theta_s) - \gamma_{\theta s} + \phi_{ls}](https://cfdland.com/wp-content/ql-cache/quicklatex.com-963221f013104bf7b833b0a6208ebe93_l3.png "Rendered by QuickLaTeX.com")
Reading the terms left to right: the bracketed term is the convection of fluctuating energy. On the right side, the first term is generation by the solid stress tensor. The second is diffusion via granular conductivity (kθs). The third (γθs) is collisional dissipation, energy destroyed by inelastic impacts. The final term (ϕls) is the energy exchange with the fluid phase.
The particle energy naturally increases, called production, when the main fluid strongly pushes and shears the solids. Conversely, the bouncing energy heavily decreases, called dissipation, every single time the hard solid particles crash into each other and lose their physical momentum.
Figure 4: Granular temperature does not represent thermal heat; it is a mathematical equation that accurately calculates the kinetic bouncing energy of the solid particles.
When you set up your granular simulation in ANSYS Fluent, you must choose exactly how to mathematically solve this energy equation. You can choose the algebraic formulation, which solves much faster because it completely ignores how the energy diffuses and spreads out over space. Alternatively, you can choose to solve the full Partial Differential Equation (PDE). This full equation takes more time to calculate, but it tracks the exact transport and diffusion of the kinetic energy everywhere in the domain.
You must strictly select the full Partial Differential Equation (PDE) for granular temperature when your flow is highly rapid and complex, but you can safely use the faster algebraic form for simpler, steady-state flows.
Figure 5: Two main approaches to granular temperature modeling
Leading-Order Granular Temperature: In dense limit conditions, most solvers use the leading-order granular temperature—an algebraic solution obtained when convection and diffusion are dropped, balancing local production directly against local dissipation. This algebraic formulation calculates much faster and is highly accurate for steady-state, collision-dominated flows where you do not need the full Partial Differential Equation (PDE).
Solids Pressure
When you pump a heavy mixture of sand and water into a pipe, the solid sand particles constantly hit the pipe walls and violently crash into each other. This physical pushing force is called Solids Pressure. It is completely different from normal fluid pressure. It is a specific mathematical measurement of how much momentum is transferred when the hard solid spheres fly around and collide.
The software mathematically calculates this solids pressure by combining two different physical actions. The first part is the kinetic contribution, which happens when the particles fly freely through the empty fluid and hit a surface. The second part is the collisional contribution, which happens when the solid particles physically crash directly into one another.
Figure 6: Available Solid pressure models in ANSYS Fluent
There is a very crucial physical rule regarding this pressure. When the solid particles pack completely tightly together, they reach their absolute maximum volume fraction. When the solid particles pack tightly together, they reach their absolute maximum packing limit. At this limit, the granular flow becomes incompressible, like tightly packed dirt. Because the particles cannot squeeze any closer together, the solids pressure mathematically spikes to an extreme level. This massive pressure spike is what pushes the particles apart and stops them from physically overlapping in your simulation. Here is a quick guide table to help you choose the proper model for your specific project:
| Solids Pressure Model | Mathematical Approach | When to Choose This Model |
| Lun et al. | Calculates both the free-flight (kinetic) momentum and the crashing (collisional) momentum. | Best for general cases. Use this for standard fluidized beds where particles rapidly fly freely and crash frequently. |
| Syamlal et al. | Calculates ONLY the crashing (collisional) momentum. It completely ignores the free-flight energy. | Best for very dense flows. Use this when your particles are very heavy and constantly touching, with almost zero free flight. |
| Ma and Ahmadi | Calculates the kinetic and collisional forces, but also includes heavy frictional viscosity effects. | Best for packed beds. Use this for tightly packed geometries where heavy physical sliding and friction dominate the flow. |
| Model | Governing Equation |
| Lun et al. |  |
| Syamlal et al. |  |
| Ma and Ahmadi | ![P_s = \alpha_s \rho_s \theta_s \left[ (1+4\alpha_s g_{os}) + \frac{1}{2} (1+e_{ss})(1-e_{ss} + 2\mu_{fr}) \right]](https://cfdland.com/wp-content/ql-cache/quicklatex.com-3a6556802ec3a496235084fb7f4c4754_l3.png "Rendered by QuickLaTeX.com") |
Radial Distribution Function
In the Eulerian Granular Model, solid particles act very differently when they are flying far apart versus when they are crushed tightly together. When particles get very close to their maximum packing limit, the empty physical space between them almost completely disappears. Because they are forced into such a tight space, the physical probability of them violently crashing into each other increases massively. To accurately calculate this extreme collision rate, the software uses the Radial Distribution Function.
This mathematical concept acts as a powerful statistical multiplier in your governing equations. It automatically corrects the math and drastically increases the probability of particle collisions as the solid volume fraction gets denser. If you ignore this correction factor, your software will completely underestimate how often densely packed particles hit each other. You must strictly use a radial distribution function to mathematically prevent your solid particles from artificially overlapping and to calculate the correct heavy collision forces near the packing limit.
ANSYS Fluent provides four different mathematical models to calculate this exact collision probability. To help you easily choose the best one for your specific engineering project, please use the quick guide table below.
| Radial Distribution Model | Quick Guide for Choosing the Proper Model |
| Lun et al. | The standard and most widely used general-purpose model. It works perfectly for most standard granular flows and is an excellent starting point. |
| Syamlal-O’Brien | The best choice when you are simulating bubbling or settling fluidized beds. It is highly recommended to use this exactly alongside the Syamlal-O’Brien drag model. |
| Ma and Ahmadi | The proper choice for extremely dense and heavy flows. It works perfectly when you also select the Ma and Ahmadi solids pressure model to include high frictional effects. |
| Arastoopour | A great alternative mathematical option for highly dense flows. It provides a very smooth numerical transition as the particles safely reach their absolute maximum packing limit. |
Figure 7: The radial distribution function is a mathematical multiplier that strictly increases the probability of particle collisions as they get dangerously close to their maximum packing limit.
Granular Viscosity
Just like thick honey resists flowing much more than liquid water, a moving mass of solid particles also heavily resists being pushed. This physical internal flow resistance is called Granular Viscosity. The software mathematically calculates this total flow resistance by strictly adding three completely different physical mechanisms together.
The first mechanism is the kinetic viscosity, which measures the resistance created when particles fly freely across the flow streams. The second mechanism is the collisional viscosity, which measures the heavy friction caused when particles directly crash and bounce off each other. The third and final mechanism is the bulk viscosity, which calculates how much the entire cloud of particles physically resists being compressed or expanded as a whole volume. A fourth contribution, frictional viscosity, switches on only once the bed approaches its packing limit. That mechanism is handled separately below.
Figure 8: Available Granular viscosity models in ANSYS Fluent
Inside ANSYS Fluent, you must select exactly how to calculate these viscous forces. Here is a quick guide table to help you choose the proper kinetic granular viscosity model:
| Granular Viscosity Model | Mathematical Approach | When to Choose This Model |
| Lun et al. | Calculates both kinetic and collisional viscosity simultaneously. | Best for standard flows. This is the default and most robust choice for general fluid-solid interactions and bubbling beds. |
| Syamlal et al. | A specialized kinetic viscosity calculation. | Best for uniform math. Use this specifically when you have chosen Syamlal et al. for your other models to maintain numerical stability. |
| Gidaspow et al. | An advanced kinetic viscosity calculation. | Best for dense fluidized beds. Highly recommended for flows where particles frequently alternate between flying freely and packing tightly. |
Frictional Stress Modeling
When solid particles are flowing freely in a dilute mixture, they simply bounce and crash into each other. However, as the particles accumulate at the bottom of a tank or inside a hopper, they eventually run out of empty space to fly.
When the volume fraction of the solids reaches the critical packing limit of 0.63 (for monodisperse spheres), the physical behavior of the flow changes. At this extreme density, the particles can no longer bounce freely. Instead, they are forced into constant physical contact and begin sliding, grinding, and rubbing directly against one another. To capture this grinding motion, the software stops relying on collision physics and activates Frictional Stress Modeling, which calculates the mechanical friction created by the sliding particle surfaces. When your solids volume fraction exceeds the packing limit, the software adds these frictional forces to the total solid stress to prevent the simulation from failing.
This heavy frictional stress is mathematically divided into two parts: frictional pressure and frictional viscosity. When your solids volume fraction exceeds the packing limit, the software strictly adds these massive frictional forces to the total solid stress to prevent the simulation from failing. ANSYS Fluent provides a few specialized mathematical models to accurately calculate this heavy sliding friction. Here is a quick guide table to help you easily choose the exact proper frictional model for your specific dense flow:
| Frictional Model | Mathematical Approach | When to Choose This Model |
| Schaeffer (Coulomb Law) | Calculates pure sliding frictional viscosity based directly on the internal friction angle of the solids. | Best for standard packed flows. Use this as your default choice for hoppers, silos, and deeply settled beds. |
| Johnson and Jackson | A comprehensive model that mathematically calculates both frictional pressure and frictional viscosity. | Best for heavy soil mechanics. Highly recommended when simulating extremely heavy, dirt-like sliding flows where particles are totally locked. |
| Syamlal et al. | Calculates frictional pressure using specific volume fraction curves. | Best for consistent Syamlal setups. Use this specifically to maintain numerical stability if you have already chosen Syamlal for your drag or collision models. |
Frictional physics also governs how the solid phase behaves at the wall. A no-slip condition is rarely correct for a dense bed, since particles slide along the surface while exchanging momentum with it. The Johnson and Jackson boundary condition handles this through a specularity coefficient, where a value near zero produces almost free slip and a value near one approaches no-slip. Getting this coefficient right has a direct effect on predicted bed expansion and near-wall solids circulation.
Drag Models for Gas-Solid Flows
When a fluid flows through a cloud of solid particles, the gas physically grabs the solid spheres. This momentum exchange is handled by a gas-solid drag model—a correlation built specifically for dense clouds of spheres rather than for isolated particles. The correlations below are specific to solid granular phases, where drag depends on the local solids concentration. For bubbly and droplet systems, and for the non-drag contributions such as lift and virtual mass, see our dedicated guide to interphase forces in the Eulerian model. Because of this crowding effect, the software uses specialized correlations that mathematically increase the friction based on how densely the particles are packed. Choosing the proper gas-solid drag model is a critical step to correctly predict terminal velocities in dilute pipes and minimum fluidization velocities in dense beds.
ANSYS Fluent provides several highly specialized mathematical equations to calculate this gas-solid friction. Because drag strongly depends on the particle diameter and concentration, you must select the model that matches your flow regime.
Figure 9: gas-solid Drag models for granular flows in ANSYS Fluent
Here is a quick guide table to help you perfectly choose the exact proper gas-solid drag model for your simulation:
| Gas-Solid Drag Model | Mathematical Approach | When to Choose This Model |
| Wen and Yu | An extension of standard single-particle drag, corrected for slightly crowded spaces. | Best for dilute systems. Use this when your flow is mostly empty gas with light particle dispersion. |
| Gidaspow | Strictly combines the Wen-Yu model for dilute zones and the heavy Ergun equation for densely packed zones. | Best for dense fluidized beds. The most highly recommended standard choice for heavy gas-solid interactions. |
| Huilin-Gidaspow | Uses the exact same equations as Gidaspow but adds a specialized mathematical blending function. | Best for mixed flows. Use this to prevent numerical crashes when your flow rapidly transitions between highly dense and completely dilute. |
| Syamlal-O’Brien | Mathematically adjusts the drag friction based specifically on the terminal velocity of settling particles. | Best for bubbling beds. Highly recommended when you already know your exact minimum fluidization velocity. |
| Gibilaro | Uses theoretical considerations to calculate the pressure drop across moving and expanding beds. | Best for circulating beds. Gives highly accurate predictions for turbulent bed expansion. |
Granular Heat Transfer: The Gunn Model
In a fluidized bed dryer, a biomass gasifier, or a thermal storage column, gas and particles enter at very different temperatures and exchange heat across an enormous interfacial surface area. Granular heat transfer is what sets how quickly that gap closes.
In many multiphase applications, the fluid and solid phases enter the system at completely different temperatures. As they mix and interact, thermal energy is constantly exchanged between them until they reach an equilibrium. This thermal exchange is known as interphase heat transfer. Accurately predicting this temperature shift is essential for simulating complex thermal processes like drying, combustion, or catalytic reactions. You can explore a great example of complex particle dynamics and mixing in our Particle Mixing in a Conical Fluidized Bed CFD Simulation, ANSYS Fluent Training tutorial.
ANSYS Fluent manages this thermal exchange through the Phase Interaction panel. By defining a volumetric heat transfer coefficient, the software can calculate exactly how fast heat moves from the continuous fluid to the dispersed particles, or vice versa. Because different flow regimes and particle types transfer heat at very different rates, Fluent offers a wide variety of empirical models to calculate this coefficient. Choosing the correct model depends heavily on whether you are simulating solid particles, liquid droplets, or gas bubbles.
Below is a quick-guide table detailing the heat transfer coefficient models in ANSYS Fluent that are relevant to granular flows:
| Heat Transfer Model | Description & Best Use Case |
| gunn | The standard choice for Granular Flows. Valid across porosities of 0.35 to 1.0 and particle Reynolds numbers up to 10⁵, covering essentially the full operating range of fluidized beds. |
| ranz-marshall | Best for Droplets/Bubbles. This model is frequently used for Eulerian multiphase simulations that do not involve a granular phase, such as liquid droplets in a gas. |
| hughmark | Best for High-Speed Droplets/Bubbles. This is an extension of the Ranz-Marshall model designed to remain accurate over a much wider range of Reynolds numbers. |
| tomiyama | Best for Slow Bubbles. This model is frequently used for Eulerian multiphase simulations of bubbly flows operating at relatively low Reynolds numbers. |
| constant-htc | Allows you to specify a fixed, constant value for the volumetric heat transfer coefficient if you already know the exchange rate. |
| nusselt-number | Best for Known Empirical Data. This allows you to specify a constant value for the Nusselt number, from which the software will automatically compute the heat transfer coefficient. |
| fixed-to-sat-temp | Best for Simple Phase Change. This models heat transfer when all heat transferred to an interface is used in mass transfer, assuming the destination phase remains at the saturation temperature. |
| two-resistance | Best for Evaporation-Condensation. This opens a secondary dialog box allowing you to independently specify the heat transfer coefficient correlations for both the liquid and gas phases. |
| time-scale (two-resistance sub-model) | Best for Rapid Phase Change. This models the gas-interface heat transfer by assuming the gas phase retains the saturation temperature through rapid evaporation or condensation. |
| zero-resistance (two-resistance sub-model) | Best for Interfacial Equilibrium. When selected for one of the phases, it forces that specific phase’s temperature to be exactly equal to the interfacial temperature. |
| user-defined | Best for Custom Research. This allows you to hook a User-Defined Function (UDF) to implement a custom correlation for the heat transfer coefficient. |
| none | Best for Isothermal Flows. This instructs the solver to completely ignore the effects of heat transfer between the two phases. |
Figure 10: ANSYS Fluent provides a wide variety of heat transfer coefficient models in the Phase Interaction panel to accurately simulate thermal exchange between different phases.
Eulerian Granular Model Setup in Fluent
Setting up a standard two-phase simulation in ANSYS Fluent is straightforward. However, when your solid particles reach high concentrations, you must explicitly instruct the software to activate the complex soil mechanics and kinetic theory equations. To do this, you must navigate to the Phases panel and edit your secondary solid phase. By checking the Granular option inside the secondary phase dialog box, you immediately unlock a completely new set of specialized mechanical properties.
The software will now require you to mathematically define exactly how the particles bounce, slide, flow, and pack together. Instead of just entering a simple density and viscosity, you must carefully assign specific models for the granular temperature, internal friction, and solid pressure.
Failing to define these granular parameters correctly will cause your dense particle bed to either artificially collapse into a tiny volume or explode with numerical instability. To guarantee a successful simulation, you must set up the secondary phase properties correctly.
Packed Bed Simulation
In many heavy chemical engineering applications, such as catalytic reactors, thermal energy storage, or filtration systems, the solid particles do not move at all. Instead, they sit completely stationary in a dense, tightly locked column while the fluid flows rapidly through the tiny gaps between them.
Traditionally, engineers simulate these complex stationary zones using a simplified Porous Media model. We have successfully utilized this macroscopic approach in several of our advanced projects. For example, in our Heat Transfer from Cylinder in Porous Medium CFD Simulation, we treated an entire packed bed as a porous zone using the Darcy-Brinkman-Forchheimer formulation. This simplified the geometry and perfectly validated forced convection without the computationally impossible task of meshing millions of individual particles.
Figure 11: An application of porous media for modeling packed bed
While the porous media approach is excellent for simple flow resistance, ANSYS Fluent also allows you to use the Eulerian Granular model to create a much more detailed, physics-based packed bed. This Eulerian approach is mathematically the absolute best physical representation of stationary particles because it actively calculates the true interphase drag, solids pressure, and local volume fractions.
By using the Eulerian packed bed approach instead of a simple porous zone, you gain full, unrestricted access to the advanced homogeneous and heterogeneous reactions framework to simulate complex surface chemistry.
Setting up an Eulerian packed bed requires a very specific two-step process in the software. First, you must edit your secondary solid phase, enable the Granular option, and explicitly check the Packed Bed box to activate the specialized stationary equations. Second, you must navigate to the Cell Zone Conditions panel and manually set the packed solids velocity components to exactly zero. This effectively freezes the particles in place, forcing the continuous fluid to strictly navigate through the tightly locked solid structure.
Figure 12: Simulating a packed bed using the Eulerian Granular model provides a superior physical representation of stationary particles and unlocks advanced heterogeneous reaction capabilities.
Conclusion
The Eulerian Granular Model is what separates a simulation that merely moves particles around from one that respects how they actually behave—bouncing, dissipating energy, and locking up at the packing limit. We have explored the kinetic theory of granular flow, the granular temperature equation, solids pressure, and the gas-solid drag correlations that hold it together.
Whether you are designing bubbling fluidized beds, circulating reactors, spouted-bed pyrolysis units, or packed catalytic columns, a correctly configured granular model is what separates a converged, defensible result from a diverged mesh.
Frequently Asked Questions (FAQ)
- What is the leading-order granular temperature? It is the simplified mathematical balance you get when the convection and diffusion of fluctuating energy are negligible compared to local production and dissipation. Under that assumption, the transport equation reduces to a local algebraic relation. This is what Fluent solves when you select the algebraic formulation, and it is reliable in dense, collision-dominated beds.
- Should I use the Eulerian Granular Model or CFD-DEM? Use the Eulerian granular model when you care about bulk hydrodynamics (such as bed expansion and pressure drop) and your particle count is in the millions, since the solid phase is treated as a continuum and computational cost is independent of particle number. Choose the CFD-DEM approach when individual particle trajectories, size distributions, or specific contact forces are the actual result you need.
- Why does my granular simulation diverge near the packing limit? This happens because the solids pressure and frictional stress cannot arrest the physical packing fast enough. To fix this, verify the packing limit matches your material, ensure a frictional viscosity model is enabled, drop the volume fraction under-relaxation factor to roughly 0.3, and start with a small time step (near 1e-4 seconds). If your project timeline cannot absorb this tuning phase, our CFD Consultation & Project Ordering service can diagnose and correct the solver setup directly.