As we know, Computational Fluid Dynamics (CFD) depends on numerically solving the Navier–Stokes equations along with related transport equations. Since exact analytical solutions exist only for simplified cases, numerical discretization techniques are applied to transform the governing partial differential equations (PDEs) into algebraic systems solvable by computers. ANSYS Fluent, one of the most widely used CFD solvers, employs the Finite Volume Method (FVM) as its primary discretization framework. However, depending on the mathematical characteristics of individual terms in the conservation equations, different numerical schemes are required. This study focuses on reviewing Pressure–Velocity Coupling Methods, highlighting their distinctions and specific implementations in ANSYS Fluent.

Pressure–Velocity Coupling Methods in CFD

In CFD, solving the Navier–Stokes equations requires accurate coupling between pressure and velocity to satisfy the continuity equation. This is particularly challenging in incompressible and weakly compressible flows, where pressure does not appear as a separate conservation equation. Instead, it must be obtained indirectly through iterative schemes. Several pressure–velocity coupling algorithms have been developed to address this challenge, with ANSYS Fluent providing four widely used methods: SIMPLE, SIMPLEC, PISO, and the Coupled Scheme. This study reviews these methods in an example, highlighting their principles, advantages, limitations, and applications in CFD simulations.

Figure 1- Types of Pressure–Velocity Coupling Methods in ANSYS Fluent

Table 1 summarizes the main pressure–velocity coupling methods available in ANSYS Fluent, highlighting their key features and suitable application ranges for different flow conditions.

Table 1- Comparison of Pressure–Velocity Coupling Methods in ANSYS Fluent

Method	Features	Suitable For
SIMPLE	– Sequential solving between pressure and velocity. – Relatively fast and stable for steady-state problems.	– Calm flows or cases with minimal temporal changes. – Steady-state problems with sufficient accuracy.
SIMPLEC	– Corrects pressure-velocity relations to reduce prediction errors. – Fewer steps compared to SIMPLE for convergence.	– Steady-state problems with coarse grids – When requiring faster convergence.
Coupled	– Uses a large matrix solver for pressure and velocity. – Fast convergence, especially for pressure and velocity dependence.	– Compressible flows – For cases with high Mach numbers or shock flows.
PISO	– Multiple pressure-correction steps within each time step – High stability without the need for strong under-relaxation	– Transient flows (e.g., rapidly varying or oscillating flows) – LES models and time-dependent flow simulations requiring high temporal accuracy

Figure 2 provides a comparative overview of four algorithms commonly used in CFD for solving pressure–velocity coupling: SIMPLE, SIMPLEC, PISO, and Coupled. ANSYS Fluent provides several pressure–velocity coupling algorithms tailored to different flow conditions.

Figure 2- Comparison of Pressure–Velocity Coupling Algorithms in CFD

The SIMPLE method serves as the basic and default approach for steady-state simulations and may also be applied to transient cases with reduced under-relaxation coefficients. The SIMPLEC algorithm, an enhanced version of SIMPLE, modifies the momentum correction terms to improve pressure–velocity coupling and achieve a higher convergence rate, though it is generally less suitable for transient problems without careful accuracy adjustments. The Coupled scheme solves the pressure and momentum equations simultaneously, offering rapid convergence but requiring greater computational resources. The PISO algorithm, optimized for transient or unsteady simulations, employs multiple pressure-correction steps within each time step to enhance temporal accuracy, though it tends to be slower than SIMPLE in steady-state cases. Overall, each method provides a balance between accuracy, convergence speed, and computational efficiency, depending on the nature of the simulation.

Comparison of Pressure–Velocity Coupling Methods in ANSYS Fluent

To conduct a fair and systematic comparison between the four pressure–velocity coupling algorithms—SIMPLE, SIMPLEC, PISO, and Coupled—within ANSYS Fluent, we decided to analyze a single representative case study where all governing conditions, such as boundary conditions, mesh resolution, and initial conditions, are kept identical. The only variable that changes between simulations is the numerical solution method itself.

Case Study

Consider steady, incompressible turbulent flow of a fluid inside a circular pipe of diameter D. The pipe wall is exposed to external irradiation that supplies a uniform radiative heat flux to the wall. Heat is transferred from the wall to the flowing fluid by a forced convection while the wall temperature is maintained (or measured) at a known value. Figures 3 and 4 illustrate the computational domain geometry of the internal flow and the structured grid generated using the ANSYS ICEM CFD pre-processing software, respectively.

The computational domain was discretized using a structured mesh consisting primarily of hexahedral elements to ensure accuracy and stability in the numerical solution. The generated mesh contained a total of 1,106,400 nodes, 49,134 quadrilateral surface elements, and 1,081,195 hexahedral volume elements, providing sufficient resolution to capture the flow and thermal gradients within the pipe.

Figure 3- Computational domain geometry of the turbulent pipe flow.

Figure 4- Structured Grid Generated for Internal Flow Simulation Using ANSYS ICEM CFD

Moreover, Table 2 presents the geometrical and physical parameters of the turbulent pipe flow employed in the present analysis, including the pipe diameter, mean velocity, fluid thermal conductivity, applied wall heat flux, and wall temperature.

Table 2- Geometrical and physical parameters of the turbulent pipe flow

Parameter	Symbol	Value	Unit
Pipe diameter	D	0.05	m
Density	ρ	1000	kg/m³
Dynamic Viscosity	μ	0.001	Pa·s
Mean flow velocity	U	0.20	m/s
Specific Heat at Constant Pressure	Cp	4182	J/kg·K
Fluid thermal conductivity	k	0.60	W/m·K
Wall heat flux	q”	50,000	W/m²
Wall temperature (in fully developed state)	Twall	342.5189	K
Average temperature across the pipe cross-section	Tbulk	302.799	K
Convective heat transfer coefficient	h= q”/ (Twall-Tbulk)	966.63324	W/m2.K

It is worth mentioning that the last three parameters—wall temperature (T_wall), average temperature across the pipe cross-section (T_bulk), and convective heat transfer coefficient (h)— are outputs of the ANSYS Fluent simulation and correspond to the region where the flow is fully developed.

Hydrodynamic and Thermal Characteristics

The hydrodynamic and thermal behavior of the turbulent pipe flow is characterized by a set of derived parameters that provide insight into the flow regime and heat transfer performance. Key dimensionless numbers, including the Reynolds number (Re), Prandtl number (Pr), and Nusselt number (Nu), are evaluated to quantify the relative importance of inertial, viscous, and thermal effects within the flow. The turbulence intensity (T.I.) also show that an estimate of the velocity fluctuations inherent to turbulent flow. These parameters collectively allow for a comprehensive assessment of the flow’s hydrodynamic and thermal performance, providing the basis for subsequent analysis and optimization.

Reynolds Number

The Reynolds number is used to characterize the flow regime of a fluid, whether it is laminar or turbulent. It is defined as:

Re = (U × D × ρ) / μ

For the fluid properties of water-liquid in this analysis which are set as Table1, Reynolds number is equal to   , which corresponds to turbulent flow conditions.

Turbulent Intensity

This parameter quantifies the level of turbulence in the flow and can be calculated using the following formula:

T.I = 0.16 × Re^(-1/8)

For Re=10,000, the calculated turbulent intensity corresponds to T.I = 5.06%.

Prandtl number

The Prandtl number (Pr) is a dimensionless parameter that represents the ratio of momentum diffusivity (viscous effects) to thermal diffusivity, defined as:

Pr = (μ × Cp) / k

In fact, the Prandtl number indicates how fast heat diffuses compared to momentum in a fluid. In the presented problem, the Prandtl number is equal to Pr = 6.97.

Nusselt Number

For fully developed turbulent flow inside smooth circular pipes, the Nusselt number (Nu) is determined using empirical correlations based on the Reynolds number (Re) and the Prandtl number (Pr). The most widely used correlation for moderate Prandtl numbers  is the Dittus–Boelter equation. Based on this equation the Nusselt number can be written as follow:

 

Nusselt Number (for heating): Nu = 0.023 × Re^(0.8) × Pr^(0.4)

Nusselt Number (for cooling): Nu = 0.023 × Re^(0.8) × Pr^(0.3)

It should be noted that for the turbulent pipe flow being heated, the Nusselt number is calculated as Nu=79.254.

 

ANSYS Fluent: General Setting for All Methods

Fig.5 highlights the Fluent Launcher and Solution Initialization panels for setting up our simulation. In the launcher, Double Precision is enabled to ensure numerical accuracy, while 16 solver processes are selected for efficient parallel computation on an 11th Gen Intel® Core™ i7-11800H processor. The Solution Initialization panel shows the use of Hybrid Initialization, a robust method combining iterative and algebraic approaches for faster convergence and reliable starting conditions in complex combustion cases. Options like Patch and Species allow flexibility in defining initial conditions and species concentrations. These consistent settings across all pressure–velocity coupling algorithms (SIMPLE, SIMPLEC, PISO, and Coupled) ensure a fair and accurate comparison of solver performance.

Figure 5- Fluent Launcher Settings and Solution Initialization for our simulation

The standard k-ε turbulence model is employed for turbulent flow dynamics, ensuring robust performance for combustion modeling. It should be noted that since the Yplus(Y+) is about 5 for the current problem, the Enhanced Wall Treatment approach is activated.

Figure 6- Viscous Model Settings for Turbulent Flow Simulation

Discretization Settings

Figure 7 showcases the Solution Methods panel in ANSYS Fluent for comparing four pressure–velocity coupling algorithms: SIMPLE, SIMPLEC, PISO, and Coupled, as applied to our case study. Each column represents the settings for a specific algorithm, with consistent governing conditions across all simulations.  These settings ensure uniform computational conditions, enabling a fair comparison of solver efficiency, robustness, convergence rate, computational cost, numerical stability, and solution accuracy.

Figure 7- Solution Methods and Spatial Discretization Settings for SIMPLE, SIMPLEC, PISO, and Coupled Algorithms in ANSYS Fluent

Result and Discussions

First of all, the Nusselt number obtained from ANSYS Fluent is 80.55, while the analytical calculation using the full Dittus–Boelter correlation gives 79.25, resulting in a relative error of approximately 1.64%. The close agreement between the numerical and analytical results demonstrates that the empirical correlation accurately captures the convective heat transfer for fully developed turbulent flow in a smooth circular pipe. The small discrepancy arises from simplifications in the analytical model, such as assuming constant fluid properties and neglecting minor three-dimensional effects, whereas Fluent solves the full coupled momentum and energy equations, accounting for the actual flow and temperature development along the pipe.

Secondly, the presented graph (Fig.8) provides a comparative analysis of the CPU time and convergence iterations associated with four different pressure-velocity coupling methods used in computational fluid dynamics (CFD): Coupled, SIMPLE, SIMPLEC, and PISO. The graph is organized with the x-axis representing the different algorithms and the y-axis showcasing two distinct measurements: CPU time (in seconds) and the number of convergence iterations required for each method. This dual representation allows for a nuanced understanding of the computational efficiency and effectiveness of each algorithm.

Figure 8- Performance Comparison of Pressure-Velocity Coupling Methods in ANSYS Fluent

Starting with the CPU time, it is evident that the Coupled method exhibits the lowest computational demand, requiring just over 200 seconds for the simulation. In contrast, the PISO method requires significantly more time, approaching 900 seconds. SIMPLE and SIMPLEC fall in between these two extremes, with SIMPLE at around 400 seconds and SIMPLEC slightly higher. This indicates that the Coupled method is the most efficient in terms of time consumption, potentially making it a preferable choice for applications where computational resources are a concern.

Conversely, when examining the number of convergence iterations, the graph illustrates a different trend. The PISO method requires approximately 600 iterations to converge, which is higher than the other methods, suggesting that it may be more complex or less stable under the tested conditions. SIMPLEC shows a similar number of iterations, while SIMPLE requires fewer iterations than both PISO and SIMPLEC. The orange line connecting the iteration points indicates a gradual increase in the number of iterations from the Coupled method through SIMPLE, SIMPLEC, and finally to PISO. This relationship suggests that while the Coupled method is computationally efficient, it may also converge more quickly than its counterparts.

 

Conclusion

This study focused on reviewing Pressure–Velocity Coupling Methods, highlighting their distinctions and specific implementations in ANSYS Fluent. The comparative study of SIMPLE, SIMPLEC, PISO, and Coupled algorithms in ANSYS Fluent for turbulent flow of a fluid inside a pipe shows that, despite their different numerical approaches, all methods ultimately produce nearly identical physical results when the simulations are properly converged.  For our problem, the Coupled method shows the least CPU time, around 200 seconds, while PISO takes the longest at nearly 900 seconds. In terms of iterations, PISO also requires the most, around 600 iterations, indicating a correlation between longer computation times and more iterations needed for convergence across the methods. Besides, with a Nusselt number of 80.55 from ANSYS Fluent versus 79.25 from the full Dittus–Boelter correlation, the simulation agrees with the analytical benchmark to within 1.64 %—a difference that underscores the high accuracy of the CFD solution. Overall, this analysis emphasizes the importance of selecting appropriate numerical techniques to achieve reliable and precise results in fluid dynamics simulations.

FAQs

1. Do these four algorithms give different physical results?

No, when fully converged under the same conditions, they yield nearly identical physical solutions (temperature, velocity, and species).

2. Why do we need different methods if the results are the same?

The difference lies in efficiency, stability, and convergence speed. Some methods are faster or more stable depending on whether the case is steady, transient, or highly coupled.

3. What is the SIMPLE method used for?

SIMPLE is the default solver for steady-state flows, offering fast and stable convergence, and can be applied to transient cases with reduced under-relaxation.

4. How does SIMPLEC differ from SIMPLE?

SIMPLEC improves pressure–velocity coupling by modifying momentum correction terms, converges faster than SIMPLE, and works well for steady-state problems, but requires care for transient flows.

5. When should the Coupled solver be used?

Coupled solves pressure and momentum simultaneously, giving rapid convergence for strongly coupled or compressible flows, though it demands more computational resources.

6. What is PISO best suited for?

PISO excels in transient or unsteady simulations, using multiple pressure-correction steps per time step to enhance temporal accuracy, though it is slower in steady-state cases.