LES Implementation in ANSYS Fluent: Step-by-Step Setup, Mesh Requirements & Numerical Settings

Kiarash Kord
Reading time: 13 min

Welcome to the second part of our Large Eddy Simulation (LES) trilogy. In Blog 1, we discussed the physics of turbulence and the mathematical closure problem. Now, we move from theory to practice.

Contents

Setting up an ANSYS Fluent LES case is different from a standard RANS simulation. It requires specific steps to ensure stability and accuracy. If you try to run LES CFD immediately on a standard mesh, the solution will likely fail or give incorrect results. This guide serves as a quick guide to setting up les type simulations, ensuring you avoid common mistakes.

For practical examples of the setups we will discuss, you can explore these complete tutorials from our shop:

In this blog, we will guide you through the complete workflow, starting with the essential first step: The Precursor RANS Simulation.

Figure 1: Two examples of high-fidelity ANSYS LES Model simulations from our CFD Shop

Pre-LES Setup: RANS Initialization & Assessment

Many users make the mistake of selecting the LES model immediately. This is not the correct way. A successful LES ANSYS Fluent simulation always starts with a steady-state RANS (Reynolds-Averaged Navier-Stokes) simulation.

We use this “Precursor RANS” simulation for three critical tasks:

To provide a converged initial flow field (initial condition).
To calculate the Integral Length Scale ( $l_0$ ) of the turbulence.
To assess if our mesh is fine enough for LES simulation.

Step 1: Choosing the Right RANS Model

Before switching to Large Eddy Simulation ANSYS Fluent, run your simulation in steady-state. You must choose a RANS model that provides good turbulence data.

According to best practices, avoid the Spalart-Allmaras (1-equation) model for this step because it does not calculate the turbulence length scale directly. Instead, use a 2-equation model.

RANS Model	Suitability for Pre-LES	Reason
Standard k-epsilon	Good	Robust and provides and to calculate length scales easily.
SST k-omega	Best	Excellent for wall-bounded flows and widely used in LES Fluent tutorials.
Spalart-Allmaras	Poor	Does not solve for or , making length scale estimation difficult.
Reynolds Stress (RSM)	Overkill	Usually too expensive just for initialization, unless the flow has strong swirl.

Figure 2: The first stage was a steady-state simulation using a RANS turbulence model on a structured grid of 20 million cells.

Step 2: Calculating the Integral Length Scale

In Large Eddy Simulation vs RANS, the main difference is that LES resolves the large eddies. To do this, your mesh cells must be smaller than these large eddies. But how big are they? The Integral Length Scale ( $l_0$ ) represents the physical size of the largest energy-carrying eddies in your flow. In a valid LES simulation, your grid cells must be much smaller than .

We can visualize this concept using the diagram below. The largest circle represents the Integral Length Scale ( $l_0$ ). This contains the most energy. To capture this energy, our mesh (represented by the smaller grid lines) must be fine enough to fit multiple cells inside this large eddy.

Figure 3: Mesh Resolution Strategy: The grid size ( $\Delta$ ) must be significantly smaller than the Integral Length Scale to resolve energy-carrying eddies.

We can estimate the size of the largest energy-containing eddies (the Integral Length Scale, ) using data from the RANS simulation.

If using k-epsilon, $l_0 = k^{1.5}/\varepsilon$
If using k-omega, $l_0 = k^{0.5}/(C_\mu \cdot \omega) \text{ (where } C_\mu \approx 0.09\text{)}$

You do not need to calculate this manually. In ANSYS Fluent, you can create a Custom Field Function to plot this across your domain. We performed the same process before modeling the LES simulation of NACA 6409 that you can read more about it. This is an experimental validation study, proving the methodology was done properly.

Figure 4: Contour of the Integral Length Scale around an NACA airfoil calculated using a custom field function in ANSYS Fluent.

Mesh Requirements & Grid Generation for LES

The difference between Large Eddy Simulation vs RANS is the role of the mesh. In RANS, the mesh only needs to resolve the gradients of the mean flow. In LES ANSYS eddy simulation, the mesh determines the quality of the physics. If the mesh is too coarse, the “filter” is too large. The simulation will fail to resolve the eddies, and the SGS model will try to model too much energy. This leads to inaccurate results. We must check two specific requirements: the Grid Resolution ( $l_0/\Delta$ ) and the Near-Wall Resolution.

Grid Resolution Check

The primary goal of LES is to resolve at least 80% of the turbulent kinetic energy (TKE). The remaining 20% is handled by the SGS model.

To achieve this 80% resolution, the grid size ( $\Delta$ ) must be significantly smaller than the integral length scale ( $l_0$ ).

The Rule: You need at least 5 to 10 cells across the size of the integral eddy.
The Grid Size ( $\Delta$ ): This is typically defined as the cube root of the cell volume: .

We check this by plotting the ratio of the eddy size to the cell size. Create a Custom Field Function in Fluent:

Ratio < 5: The mesh is too coarse. You are resolving less than 80% of the energy. The results will be poor.
Ratio > 5: The mesh is acceptable.
Ratio > 10: The mesh is good (resolving ~90% of energy).

Look at the image below. This shows the ratio on the same airfoil. The Red areas in the wake show a ratio greater than 10. This means the mesh is fine enough to capture the turbulence behind the wing. The Blue areas far away show a low ratio. This is acceptable in the “far field” where there is no turbulence, but if you see blue in the wake or near the wall, you must refine your mesh.

Figure 5: Grid Resolution Check: Plotting the ratio of Integral Length Scale to Grid Size ( $l_0/\Delta$ ). Red areas (>10) indicate a high-quality LES mesh.

Near-Wall Resolution ( y+ and Aspect Ratio)

If your LES fluent tutorial involves walls (like a pipe, airfoil, or car), the mesh near the wall must be extremely fine.

y+ Requirement: In RANS, we often use wall functions with y+>30 . In LES simulation, we typically use “Wall-Resolved LES.” This means we must resolve the viscous sublayer directly.
- Target: The first cell height must result in $y^+ \approx 1$ .
Aspect Ratio Requirement: This is a common error. In RANS, it is standard practice to use long, thin prism cells near the wall (high aspect ratio, e.g., 100:1). This saves cell count. In LES CFD, turbulence is 3D and chaotic. Highly stretched cells cannot capture isotropic (cube-like) eddies.
- Rule: The aspect ratio in the boundary layer should be low. Ideally, $\Delta x$ (streamwise) and $\Delta z$ (spanwise) should be small.
- Target: $\Delta x^+ \approx 40 \text{ and } \Delta z^+ \approx 20.$

The image below clearly shows the difference. Left (RANS Mesh): You can see long, thin cells. This is “Conventional grid compression.” It saves cell count but is bad for LES. Right (LES Mesh): You can see the mesh is adapted. The cells are cut into smaller blocks (Nested Adaptation). The goal is to keep the aspect ratio low (close to 1). The cells look more like cubes.

Figure 6: Comparison of high aspect ratio cells used in RANS versus isotropic adapted cells required for Large Eddy Simulation.

Hybrid Options (DES & WMLES)

Meeting the and aspect ratio requirements leads to massive mesh counts for high Reynolds numbers. If the computational cost is too high, you should use a Hybrid RANS-LES model.

Detached Eddy Simulation (DES): This model uses RANS inside the boundary layer and LES in the detached flow (wake). Because it uses RANS near the wall, you can use high aspect ratio cells there, significantly reducing the mesh count.
Wall-Modeled LES (WMLES): This approach models the inner wall layer completely, allowing for a coarser mesh near the wall (y+ can be > 1).

By strictly following these mesh checks ( $l_0/\Delta > 5$ and proper wall resolution), you ensure your simulation is physically accurate.

Activating LES and Choosing a Sub-Grid Scale (SGS) Model

In the previous sections, we prepared our simulation by running a precursor RANS case and validating our mesh. Now, we are ready to switch the physics from RANS to Large Eddy Simulation (LES). This is a critical step where we tell Fluent to resolve the large eddies and model the small ones. To enable LES, you must open the Viscous Model panel. Here, you will switch from your RANS model (e.g., SST k-omega) to the LES model.

As shown in the image below, you simply select the Large Eddy Simulation (LES) radio button. When you do this, Fluent automatically switches the solver to “Transient” mode, because LES simulation must be unsteady.

Figure 7: The Viscous Model panel in ANSYS Fluent. Here we activate LES and select the WALE sub-model.

After selecting LES, you must choose a Subgrid-Scale Model. But what is this?

In LES, our mesh acts as a filter. We only have enough cells to “resolve” or see the large eddies. The small eddies are smaller than our cells, so they are “unresolved.” The SGS model is the mathematical formula that represents the effect of all these small, unresolved eddies. Its main job is to remove the correct amount of energy from the flow, just like real small eddies do through viscosity. This process is called “dissipation.” If we do not have an SGS model, the energy from the large eddies cannot dissipate correctly and the simulation will be wrong.

Fluent offers several SGS models. Here are the most common choices:

Smagorinsky-Lilly: This is the original and simplest SGS model. It is a simple algebraic formula that calculates an “eddy viscosity” for the small scales. Its main weakness is that its constant (Cs) is not universal and it does not behave correctly near walls without a special damping function.
WALE (Wall-Adapting Local Eddy-Viscosity): This is a very popular and robust choice for general-purpose LES CFD. The WALE model is an algebraic model (like Smagorinsky) but it is designed to behave correctly near solid walls. It automatically gives zero eddy viscosity in pure shear flows, which is physically correct. For most applications, WALE is an excellent starting point.
Dynamic Smagorinsky-Lilly: This is an “intelligent” version of the Smagorinsky model. Instead of using a fixed constant, it dynamically calculates the constant based on the resolved flow field. This makes it more accurate for a wider range of flows, especially flows that are changing from laminar to turbulent.
Kinetic-Energy Transport: This is a more advanced model. It solves one extra transport equation for the kinetic energy of the sub-grid scales (). Because it solves a transport equation, it can account for the history and transport of the small eddies, which can be important in complex, non-equilibrium flows. It is more computationally expensive than the algebraic models.
WMLES (Wall-Modeled LES): This is a hybrid approach. It is designed for high Reynolds number flows where it is too expensive to have a very fine mesh near the wall (). The WMLES model uses a RANS-like model for the very inner part of the boundary layer and switches to LES for the rest of the flow.

Numerical Settings & Solver Configuration

Once the mesh is generated and checked, we must define the physics of time. LES simulation is inherently transient (unsteady). This means we calculate the flow evolution over tiny fractions of a second. The accuracy of an LES CFD simulation depends heavily on choosing the correct time step size ( $\Delta t$ ) and the correct mathematical schemes. If these settings are wrong, the simulation will either crash or produce results that look like a low-quality RANS simulation.

Calculating the Time Step Size

In LES simulation, you cannot simply guess a time step size. The time step is strictly linked to your mesh size and flow velocity. We must satisfy the CFL Condition (Courant–Friedrichs–Lewy).

The Courant Number (C) represents how many cells a fluid particle passes through in one time step. For a stable and accurate LES, a particle should ideally stay within one cell during one calculation step.

$C = \frac{U \cdot \Delta t}{\Delta x} \leq 1$

$U = \text{Local Flow Velocity}$

$\Delta t = \text{Time Step Size}$

$\Delta x = \text{Local Cell Size}$

If your Courant number is greater than 1, the simulation might miss the high-frequency turbulence, leading to incorrect results. For a detailed explanation of this concept and its importance in CFD, you can read our comprehensive blog about Courant Number (CFL Number).

To find the correct time step for your simulation, you can use the data from your Precursor RANS simulation. You rearrange the formula to solve for $\Delta t$ :

$\Delta t \approx \frac{\Delta x}{U}$

You should look for the region in your domain where the cells are smallest ( $\Delta x$ ) and the velocity is highest (U). This gives you the limiting time step.

Spatial Discretization (Momentum)

The next step is selecting the “Discretization Scheme.” This setting controls how Fluent calculates the flow values between the centers of the cells.

In standard RANS simulations, we typically use Second Order Upwind. This scheme is very stable, but it introduces “numerical diffusion.” This means it acts like artificial viscosity and blurs the solution. In LES CFD, this blurring is dangerous because it dampens (kills) the small eddies we are trying to resolve.

The Solution: Bounded Central Differencing For LES ANSYS eddy simulation, you should use the Bounded Central Differencing (BCD) scheme for the Momentum equation.

Central Differencing (CD): This scheme is very accurate and preserves the sharp shape of turbulent eddies. However, it can be unstable and cause non-physical oscillations (wiggles) in the solution.
Bounded Central Differencing (BCD): This is the recommended default in Fluent. It combines the accuracy of Central Differencing with a special damping method that prevents instability.

The image below compares these schemes. On the left, the “Upwind” scheme blurs the vortex, losing its detail. On the right, the “Central Differencing” scheme keeps the vortex sharp and defined.

Figure 8: Comparison of Upwind versus Central Differencing schemes showing how BCD preserves vortex structure in LES simulations.

Solver Algorithm (Pressure-Velocity Coupling)

Finally, we must choose how the solver handles the pressure and velocity equations. LES fluent tutorial cases require thousands of time steps, so speed is essential.

ITA (Iterative Time Advancement): Algorithms like SIMPLE or SIMPLEC are iterative. They are very robust but perform many calculations per time step, making them slow.
NITA (Non-Iterative Time Advancement): This method is designed specifically for transient flows like LES. It performs fewer calculations per time step, making the simulation 2x to 4x faster.

Recommendation: For incompressible flows (liquids or low-speed gas), use NITA with the Fractional Step Method (FSM). For compressible flows (high-speed aerodynamics), NITA might be unstable. In these cases, use PISO or SIMPLEC (ITA).

Conclusion

In conclusion, setting up a reliable Large Eddy Simulation is a strict, step-by-step process that demands more care than a standard RANS simulation. This blog has provided a complete workflow: we began with a precursor RANS simulation to initialize the flow and validate the mesh, then moved to activating the LES model and selecting an appropriate SGS model like WALE. Finally, we configured the precise numerical schemes and time step required for a time-accurate simulation. By following this guide, you build a solid foundation for a physically meaningful ANSYS Fluent LES simulation.

In our final post of this trilogy, Blog 3, we will answer that question by exploring the advanced Hybrid RANS-LES models. We will explore powerful techniques like DES, SAS, and WMLES that combine the efficiency of RANS with the accuracy of LES, making scale-resolving simulations practical for complex engineering challenges.

Frequently Asked Questions (FAQ)

What is the difference between RANS and LES? RANS averages all turbulence, giving a steady result. LES ANSYS Fluent resolves the large unsteady eddies directly, providing much higher accuracy for mixing and acoustics.
How fine should my mesh be for LES? Your mesh should be fine enough to resolve 80% of the turbulent energy. A good rule is that the cell size should be at least 5 to 10 times smaller than the Integral Length Scale ().
Which SGS model is best for beginners? The WALE model is the best starting point. It is robust, handles walls correctly, and does not require complex tuning like the Dynamic model.
Why is my LES simulation unstable? Instability usually comes from a Time Step that is too large (CFL > 1) or a mesh that is too coarse. Try reducing the time step or using Bounded Central Differencing.

LES Implementation in ANSYS Fluent: Step-by-Step Setup, Mesh Requirements & Numerical Settings