Imagine you want to simulate air flowing slowly through a room or water moving inside a pipe. For these cases, the Pressure-based solver in ANSYS Fluent is a good choice because it handles low-speed flows well. But what if you want to simulate air rushing at high speed around a jet engine or a rocket nozzle? Then, the Density-based solver is better because it can capture fast changes like shock waves. These two solver types use different methods to solve the flow and heat transfer equations, and choosing the right one is key to getting accurate and fast results in your simulations.
Figure 1: A general guide to what is covered to choosing a solver.
Introduction to Pressure-Based and Density-Based Solver Types in ANSYS Fluent
The pressure-based solver was traditionally used for incompressible or mildly compressible flows. It works by solving the pressure first, then adjusting velocity to conserve mass. This solver uses two main algorithms: the segregated algorithm, which solves each equation one after another, and the coupled algorithm, which solves momentum and pressure equations together for faster convergence but needs more memory.
The density-based solver, on the other hand, was originally designed for high-speed compressible flows. It solves the continuity, momentum, energy, and species equations all at once. It has two formulations: implicit, which is faster and more stable but uses more memory, and explicit, which uses less memory but can be slower and less stable. The density-based solver is better at handling shock waves and rapid density changes.
Figure 2: Left: Density-based solver works best for high-speed, compressible flows such as air over a jet wing. Right: Pressure-based solver is ideal for low-speed, incompressible flows like water in pipes.
Overview of Pressure-Based and Density-Based Solvers
In ANSYS Fluent, you can choose between two main solver types: the pressure-based solver and the density-based solver. Both solvers are powerful tools. They can solve many types of fluid flow, heat transfer, and species transport problems. However, they use different methods to solve the main equations of fluid flow: continuity, momentum, energy, and species equations.
The pressure-based solver works by solving the pressure and velocity fields together. This approach is called pressure-velocity coupling. It first solves the momentum equations and then adjusts pressure to make sure the flow follows the rule of mass conservation (continuity). The pressure-based solver has two main algorithms: the segregated algorithm and the coupled algorithm. The segregated algorithm solves each equation one after another, which saves computer memory but takes more time. The coupled algorithm solves momentum and continuity equations at the same time, making the solution faster but using more memory.
This solver is mostly used for low-speed flows and incompressible or mildly compressible flows. For example, it works well for water flow in pipes or slow-moving air in rooms. It also supports many physical models like multiphase flows, combustion, and radiation.
The density-based solver solves the continuity, momentum, energy, and species equations all at once. This is called density coupling. It works well when the fluid speed is high and the density changes a lot, such as in compressible flows around airplanes or rockets. The density-based solver has two formulations: implicit and explicit. The implicit solver is more stable and faster for steady flows but uses more memory. The explicit solver uses less memory but can be slower and less stable.
This solver is best for high-speed compressible flows, including transonic, supersonic, and hypersonic flows. It can better capture flow features like shock waves. However, it supports fewer physical models than the pressure-based solver. For example, the wet steam multiphase model is only available with the density-based solver.
Figure 3: Overview of Pressure-Base and Density-Based solver methods in ANSYS Fluent.
Detailed Explanation of the Pressure-Based Solver
The pressure-based solver in ANSYS Fluent uses a method called the projection method to solve fluid flow problems. This method ensures that the flow follows the rule of mass conservation, also called the continuity equation. The solver does this by solving a pressure equation that corrects the velocity field.
The pressure equation is derived from the continuity and momentum equations. Because these equations are nonlinear and connected, the solver solves them many times in a loop. Each time, it updates the values until the solution becomes stable and accurate. This process is called iteration.
There are two main algorithms under the pressure-based solver:
Pressure-Based Segregated Algorithm
The segregated algorithm solves the governing equations one by one, separately. For example, it solves the velocity in the x-direction first, then y-direction, then pressure, and so on. Because the equations are solved separately, the algorithm uses less computer memory. This makes it good for simulations with limited memory.
However, since the equations are solved separately, the convergence to the final solution can be slower. The solver goes through these steps in each iteration:
- Update fluid properties like density, viscosity, and turbulence variables based on the current solution.
- Solve the momentum equations one after another using the latest pressure and mass flow data.
- Solve the pressure correction equation to ensure mass conservation.
- Correct the velocity and pressure values using the pressure correction.
- Solve any additional equations for temperature, species, or turbulence.
- Update source terms from interactions between phases, if any.
- Check if the solution has converged; if not, repeat the steps.
This loop continues until the solution reaches the desired accuracy.
Figure 4: Overview of the Pressure-Based Segregated Algorithm methods in ANSYS Fluent.
Pressure-Based Coupled Algorithm
The coupled algorithm solves the momentum equations and the pressure equation together at the same time. This means the solver handles these equations as a system rather than separately. Because of this, the solution converges much faster than with the segregated algorithm.
The trade-off is that the coupled algorithm needs more computer memory — about 1.5 to 2 times more than the segregated algorithm. This is because the solver must store all momentum and pressure equations together during the solution.
Despite using more memory, the coupled algorithm is very useful for steady or slowly changing flows and when faster convergence is important.
Figure 5: Overview of the pressure-based solver methods in ANSYS Fluent.
Detailed Explanation of the Density-Based Solver
The density-based solver in ANSYS Fluent solves the main fluid flow equations (continuity, momentum, energy, and species transport) all at the same time. This means it solves these equations in a coupled way, unlike the pressure-based solver which often solves them one by one. Because the equations are nonlinear and linked, the solver repeats a solution loop many times until the answers stop changing and the solution is converged.
How the Density-Based Solver Works
Each iteration of the density-based solver follows these steps:
- Update fluid properties (like density and viscosity) based on the current solution.
- Solve the continuity, momentum, energy, and species equations simultaneously.
- Solve equations for additional scalars (such as turbulence or radiation) one after another, using the updated flow variables.
- Update source terms when multiphase interactions occur (for example, particles affecting the flow).
- Check if the solution has converged. If not, repeat the loop.
This process continues until the solution meets the convergence criteria.
Figure 6: Overview of the density-based solver solution loop in ANSYS Fluent
Implicit and Explicit Formulations
The density-based solver offers two main ways to solve the coupled equations:
- Implicit formulation:
In this method, the solver uses information from both the current and neighboring cells to calculate the flow variables. This leads to a system of equations that must be solved all together. This method is more stable and converges faster, especially for steady-state problems. However, it requires more computer memory. - Explicit formulation:
Here, the solver calculates flow variables in each cell using only information from the current or previous steps. The equations can be solved one cell at a time, which uses less memory but can be slower and less stable. This method uses a multi-stage solver called Runge-Kutta and optionally a full approximation storage (FAS) multigrid to speed up convergence.
Comparison of Pressure-Based and Density-Based Solvers
Choosing the right solver in ANSYS Fluent is important for getting accurate and fast results. The pressure-based solver and the density-based solver differ in many ways. The table below summarizes the key differences between them.
| Feature | Pressure-Based Solver | Density-Based Solver |
| Governing Equations Treatment | Solves momentum and continuity equations using pressure-velocity coupling. Often solves equations sequentially (segregated) or together (coupled). | Solves continuity, momentum, energy, and species transport equations simultaneously (density coupling). |
| Solver Algorithms and Coupling | Uses segregated algorithm (equations solved one by one) or coupled algorithm (momentum and pressure solved together). | Uses implicit or explicit formulations, solving all flow equations together. |
| Memory and Computational Cost | Segregated algorithm uses less memory but converges slower. Coupled algorithm converges faster but needs more memory (1.5–2× segregated). | Can be memory-intensive due to solving large coupled systems. Implicit formulation uses more memory than explicit. |
| Applicable Flow Regimes | Best for incompressible and low-speed compressible flows (Mach number < 0.3). Coupled algorithms can handle moderate compressibility. | Best for high-speed compressible flows, including transonic, supersonic, and hypersonic flows. |
| Model Availability and Limitations | Supports many physical models: multiphase flows (VOF, Eulerian), combustion (premixed, non-premixed), radiation, and more. | Limited model availability; some multiphase and combustion models are not available. Wet steam model only in density-based. Can struggle with rapidly changing properties without fine mesh. |
Practical Guidelines on Solver Selection
- Flow Speed and Compressibility:
Use the pressure-based solver for low-speed, incompressible flows such as water in pipes or slow airflows. Choose the density-based solver for high-speed compressible flows like airflow over aircraft wings or rocket nozzles, where shocks and rapid density changes occur. - Physical Models Required:
If your simulation needs complex physical models such as multiphase flow (VOF, Eulerian) or combustion (premixed or non-premixed flames), the pressure-based solver is usually the only choice. The density-based solver supports fewer such models. - Computational Resources:
The pressure-based segregated algorithm uses less memory but may be slower to converge. The coupled pressure-based solver is faster but uses more memory. The density-based solver generally requires more memory, especially for implicit formulations. - Convergence and Stability:
The coupled pressure-based algorithm improves convergence for incompressible and mildly compressible flows. The density-based solver is stable and efficient for compressible flows with shocks. For incompressible flows, pressure-based solvers are often more reliable. - Mesh Quality and Resolution:
Density-based solvers need fine meshes to accurately capture shocks and rapid changes in flow properties. Pressure-based solvers can work with coarser meshes for low-speed flows.
Solved Example and Practical Comparison
To understand the difference between the pressure-based solver and the density-based solver, let’s look at two real examples from the CFD-Land tutorials. We will see why one solver is better for a specific problem than the other.
Density-Based Solver Example: Hypersonic Shock Wave
For our first example, we look at the Hypersonic Shock Wave CFD: A Tutorial on Bluff Body Analysis. In this case, air flows at a very high speed (hypersonic, Mach > 5) around an object.
- Why the Density-Based Solver is Used: This is a classic high-speed compressible flow. The air density, temperature, and pressure change very suddenly when a strong shock wave forms in front of the object. The density-based solver is the best choice here because it solves the continuity, momentum, and energy equations all at once. This helps it capture the sharp changes at the shock wave very accurately.
- Expected Results:
- Pressure and Temperature Contours: The images would show a very clear, strong shock wave standing in front of the body. Behind this shock, the pressure and temperature would be extremely high.
- Velocity Contours: The velocity of the air would drop suddenly after passing through the shock wave.
- Convergence and Cost: For this difficult problem, the implicit formulation of the density-based solver provides a stable and robust solution. It needs significant computer memory and power (high computational cost), but it can reach a converged solution reliably.
Figure 7: Pressure contour from a hypersonic simulation using the density-based solver. The sharp red line in front of the object is a strong shock wave, which this solver captures very well.
Pressure-Based Solver Example: Supersonic Flow
For our second example, we consider the Shock Wave In Supersonic Flow CFD Simulation | ANSYS Fluent Tutorial. In this case, air flows at supersonic speed (Mach > 1) and creates weaker shock waves.
- Why the Pressure-Based Solver Can Be Used: While the density-based solver is the traditional choice for any supersonic flow, the modern coupled pressure-based solver can also handle these cases. It solves the momentum and continuity equations together, making it strong enough for some compressible flows with weaker shocks. Using it here shows how powerful the pressure-based solver has become.
- Expected Results:
- Mach Number Contours: The images would show the flow speed dropping from supersonic to subsonic after the shock wave.
- Pressure Contours: The pressure would increase across the shock wave, but the change would be less extreme than in the hypersonic case.
- Convergence and Cost: The coupled algorithm in the pressure-based solver helps the simulation converge faster than the segregated algorithm. For this case, the computational cost might be lower than the density-based solver, but getting a stable solution can sometimes be more challenging and require careful setup.
Figure 8: contour from a supersonic simulation using the coupled pressure-based solver. This solver can also capture shock waves, showing its capability for compressible flows.
Pressure-Based Solver Example 2: B-2 Spirit Aerodynamic CFD Simulation
The B-2 Spirit Aerodynamic CFD Simulation studies the complex airflow around the B-2 Spirit stealth bomber, which has a unique flying wing design.
- Why the Pressure-Based Solver is Used: This is a high subsonic speed flow where the pressure-based solver’s capability to handle incompressible and mildly compressible flows is ideal. The solver helps analyze lift, drag, and stealth characteristics by solving the flow equations sequentially or coupled.
- Expected Results:
- Mach number and pressure Contours: Mach number contours around B2 Spirit showing supersonic flow regions and shock wave formation and pressure gradient contour colored showing high pressure zones on aircraft surfaces
- Convergence and Cost: The solver handles the complex geometry efficiently with moderate computational cost.
Figure 9 : Mach number contours around B2 Spirit showing supersonic flow regions and shock wave formation, B2 Spirit pressure gradient contour colored by pressure showing high pressure zones on aircraft surfaces.
Pressure-Based Solver Example 3: Missile Aerodynamics CFD: Inviscid Flow Simulation of Shock Waves
The fourth example is the Missile Aerodynamics CFD: An Inviscid Flow Simulation of Shock Waves. This simulates shock waves around missile shapes at various speeds.
- Why the Pressure-Based Solver is Used: Although this involves shock waves, the flow is modeled as inviscid and at relatively lower Mach numbers where the pressure-based solver still performs well. This example highlights the solver’s ability to analyze pressure distributions and wave drag.
- Expected Results:
- Mach number: The Mach number contour shows the consequences of these shocks on the airflow. The air, initially at a high Mach number, abruptly slows down as it passes through the bow shock.
- Pressure Distribution: The pressure gradient contour acts like a map of these shocks. The intense white and red area at the very front is the bow shock, where the air is hit and compressed almost instantly.
- Convergence and Cost: The pressure-based solver provides efficient and accurate results for this inviscid flow case.
Figure 10: The Mach number contour shows the consequences of these shocks on the airflow, The pressure gradient contour acts like a map of these shocks.
Conclusion and Recommendations
In this article, we explained the two main solver types in ANSYS Fluent: the pressure-based solver and the density-based solver. Both solvers solve the key fluid flow equations—continuity, momentum, energy, and species transport—but they do so using different methods.
The pressure-based solver uses pressure-velocity coupling and is best for incompressible and low-speed compressible flows. It offers two algorithms: the segregated algorithm, which is memory-efficient but slower, and the coupled algorithm, which converges faster but uses more memory. This solver supports many physical models like multiphase flows, combustion, and radiation, making it very flexible for many engineering problems.
The density-based solver uses density coupling by solving all flow equations simultaneously. It is designed for high-speed compressible flows, such as transonic, supersonic, and hypersonic flows where shock waves and rapid density changes occur. The solver has implicit and explicit formulations, with the implicit being more stable but more memory-intensive.
Choosing the right solver is very important for both accuracy and efficiency in CFD simulations. Using the wrong solver can lead to slow convergence, inaccurate results, or excessive computational cost.
Best Practices for Solver Selection in ANSYS Fluent
- For low-speed, incompressible flows (Mach number less than 0.3), use the pressure-based solver. It is stable, efficient, and supports many physical models.
- For high-speed compressible flows with shocks, use the density-based solver to capture flow physics accurately.
- For mildly compressible or supersonic flows with weaker shocks, the coupled pressure-based solver can be a good balance between accuracy and computational cost.
- Always consider your physical models, mesh quality, and available computer memory when choosing the solver.
- Use the Case Check utility in ANSYS Fluent to get recommendations for solver settings and models.
Further Reading and Resources
To learn more about solver selection and practical CFD simulations in ANSYS Fluent, visit these valuable resources:
- CFDLand Tutorials: Explore detailed tutorials like Hypersonic Shock Wave CFD, Shock Wave in Supersonic Flow, B-2 Spirit Aerodynamic CFD Simulation and Missile Aerodynamics CFD that show solver applications in real problems.
Figure 11: CFDLand Tutorials ,Hypersonic Shock Wave CFD, Shock Wave in Supersonic Flow, B-2 Spirit Aerodynamic CFD Simulation and Missile Aerodynamics CFD simulations in ANSYS Fluent
- ANSYS Fluent Official Documentation: The comprehensive User’s Guide and Theory Guide provide in-depth explanations of solver algorithms, discretization methods, and physical models.
By understanding the strengths and limitations of each solver type, you can make informed decisions that improve the reliability and speed of your ANSYS Fluent simulations.