Solve Case

Abstract

Chapter 5 presents the final universal form of the discretized governing equations for all flow conservations (e.g., mass, momentum, energy).

Appendices

Practice-8: Fast CFD Modelling

Example Project: Semi-Lagrangian-based PISO method for fast and accurate indoor modelling.

• Background:

The demand for fast engineering modeling has led to various means and efforts to reduce the cost of CFD techniques. Some of these efforts include: developing simplified turbulence models such as zero-equation models (Chen and Xu 1998); reforming solution algorithms for pressure-velocity decoupling such as Pressure Implicit with Splitting of Operator (PISO) (Issa 1986) and projection methods (Chorin 1967); utilizing coarse grids (Mora et al. 2003; Wang and Zhai 2012); and employing computer hardware technology such as Graphics Processing Unit (GPU) (Cohen and Molemake 2009) and parallel/multi-processor supercomputers. Although the rapid development of computer hardware provides more powerful computing capacity, it does not address the challenge fundamentally.

Fast fluid dynamics (FFD) is a method widely used in weather prediction and atmospheric flow study (Robert 1981; Staniforth and Côté 1991). It solves the Navier-Stokes (NS) equations with a time-advancement scheme and a semi-Lagrangian (SL) scheme. For instance, Foster and Metaxas (1996, 1997) implemented the projection method (Chorin 1967) to simulate the 3D motion of hot, turbulent gas using a relatively coarse grid. Stam (1999) proposed using semi-Lagrangian advection and fast Fourier transformation to speed up the computation to a real-time or faster-than-real-time level. Zuo and Chen (2009) first applied this operator splitting algorithm to 2-D indoor environment modeling, improved the sequence of operators, tested higher orders of differencing schemes, and evaluated the accuracy levels. Zuo et al. (2010, 2012) further improved the accuracy of FFD by using the finite volume method, mass conservation correction, and a hybrid interpolation scheme. Jin et al. (2012, 2013, 2015) extended FFD to the solution of three-dimensional airflow. Liu et al. (2016) implemented FFD in OpenFOAM (2007) with unstructured mesh, enabling the practical application of the algorithm. Even though FFD significantly accelerates the computation, its accuracy is still far from satisfaction. This study attempts to combine the semi-Lagrangian scheme with a PISO solver with the goal to increase the computation speed of PISO but without losing the accuracy (Xue et al. 2016).

• Simulation Details:

• (1) Semi-Lagrangian Advection

A fully implicit algorithm is unconditionally stable and has no Courant–Friedrichs–Lewy (CFL) restriction (Issa 1986), thus it is commonly used in CFD. However, in solving the momentum equations numerically, the advection term is fundamentally different from others because it brings significant non-linearity. Semi-Lagrangian scheme (Courant et al. 1952) shows potential for resolving the dilemma. The idea of semi-Lagrangian scheme was originated from the advection of scalar, but it can be directly applied to vector as well.

The Lagrangian method treats the continuum as a particle system. Each point in the fluid is labeled as a separate particle. From the perspective of such particles, the observed value of (i.g., density, temperature, etc.) will remain the same within the lapse of time. The semi-Lagrangian scheme follows the procedure as described in Fig. 8.5 to obtain the observed value of next time step. An existing velocity field of current time step t provides the velocity at (any) point A of the grid. To predict point A’s value of next time step $t + \Delta t$, the semi-Lagrangian method traces back to point A’s upstream location B $(\overrightarrow {AB} = - \vec{v} \cdot \Delta t)$ using the current velocity. This location B may not necessarily match an exact grid node. The surrounding values of current time step will be used to interpolate the value at this specific location. This value will then be kept and assigned to point A as its observed value of next time step. Since there is no CFL condition restriction, the time step and grid size used in a semi-Lagrangian scheme are usually large, which introduces large truncation error. Higher order numerical schemes can be used to improve the accuracy in the interpolation of the method.

Fig. 8.5

Procedure of semi-Lagrangian scheme

• (2) Semi-Lagrangian PISO Algorithm

An algorithm integrating semi-Lagrangian advection with the PISO algorithm is proposed as follows.

• Step 1: Semi-Lagrangian Advection: Velocity

Use the semi-Lagrangian advection ((x, −t)) to obtain a first intermediate velocity field.

$$\frac{{u^{*} - u^{n} }}{\Delta t} = - \left( {u^{*} \cdot \nabla } \right)u^{*} \Rightarrow u^{*} = u^{n} \left[ {P\left( {x, - \Delta t} \right)} \right]$$

(8.57)

• Step 2: Predictor Step: Velocity

Intermediate velocity field u^* and initial pressure field pⁿ are used in the solution of the implicit momentum Eq. (8.58) to yield a second intermediate velocity field u^**

$$\frac{{u^{**} - u^{*} }}{\Delta t} = v\nabla^{2} u^{**} - \frac{1}{{\rho^{n} }}\nabla p^{n} + S^{u}$$

(8.58)

Since this is using pⁿ instead of p^**, ^** will not satisfy the continuity equation.

• Step 3: First Corrector Step: Pressure

An approximation of the velocity field u^*** together with the corresponding new pressure field p^*** are sought that satisfy the continuity equation

$$\nabla u^{***} = 0$$

(8.59)

The momentum equation is then taken as

$$\frac{{u^{***} - u^{*} }}{\Delta t} = v\nabla^{2} u^{**} - \frac{1}{{\rho^{n} }}\nabla p^{***} + S^{u}$$

(8.60)

Equation (8.60) subtracting Eq. (8.58) yields

$$\frac{{u^{***} - u^{**} }}{\Delta t} = - \frac{1}{{\rho^{n} }}\left( {\nabla p^{***} - \nabla p^{n} } \right)$$

(8.61)

Take divergence for both sides of Eq. (8.61), the velocity increment Eq. (8.61) becomes the pressure increment equation to solve p*** − pⁿ field

$$\nabla^{2} p^{***} - \nabla^{2} p^{n} = \frac{{\rho^{n} }}{\Delta t}\nabla \cdot u^{**}$$

(8.62)

• Step 4: First Corrector Step: Velocity

The updated pressure field (or pressure increment field) can be substituted into Eq. (8.60) or Eq. (8.61) to update the velocity field and produce the velocity field u***.

• Step 5: Second Corrector Step: Pressure

A replication of Step 2 is conducted using the updated result from Step 3 u*** and after advection of the initial value u*, with the newest pressure field p****, yields an updated velocity field

$$\frac{{u^{n + 1} - u^{*} }}{\Delta t} = v\nabla^{2} u^{***} - \frac{1}{{\rho^{n} }}\nabla p^{****} + S^{u}$$

(8.63)

where the explicit scheme in $v\nabla^{2} u^{***}$ is taken to operate on the $u^{***}$ field. Then $u^{****}$ corresponding with $p^{****}$ satisfies the continuity equation

$$\nabla u^{****} = 0$$

(8.64)

Equation (8.63) subtracting Eq. (8.60) produces

$$\frac{{u^{****} - u^{***} }}{\Delta t} = - \frac{1}{{\rho^{n} }}\left( {\nabla p^{****} - \nabla p^{***} } \right) + \left( {v\nabla^{2} u^{***} } \right) - \left( {v\nabla^{2} u^{**} } \right)$$

(8.65)

After taking the divergence of both sides of Eq. (8.65), together with the continuity equation $\nabla u^{****}$ and $\nabla u^{***}$, the velocity increment, Eq. (8.65), yields the pressure increment equation to solve the p^**** − p^*** field:

$$\nabla^{2} p^{****} - \nabla^{2} p^{***} = \rho^{n} \nabla \cdot \left[ {\left( {v\nabla^{2} u^{***} } \right) - \left( {v\nabla^{2} u^{**} } \right)} \right]$$

(8.66)

• Step 6: Second Corrector Step: Velocity

The updated pressure field (or pressure increment field) can be plugged into Eq. (8.63) or Eq. (8.65) to update the velocity field and produce the velocity field u^****. More corrector steps can be used. However, the accuracy of two corrector steps is often adequate to approximate the exact solutions uⁿ⁺¹ and pⁿ⁺¹.

The temperature field is solved separately from the velocity field, in the PISO algorithm, although the procedure is similar. Considering the coupling between the temperature and velocity, the current study used the state equation of ideal gases to update the density of air, as shown in the steps below.

• Step 7: Semi-Lagrangian Advection: Temperature

Use the semi-Lagrangian advection ((x, −t)) to obtain a first intermediate temperature field.

$$\frac{{T^{*} - T^{n} }}{\Delta t} = - \left( {u^{n} \cdot \nabla } \right)T^{*} \Rightarrow T^{*} = T^{n} \left[ {P\left( {x, - \Delta t} \right)} \right]$$

(8.67)

• Step 8: Corrector Step: Temperature

Intermediate temperature field T^* is used in the solution of the implicit energy Eq. (8.68) to yield the temperature field Tⁿ⁺¹

$$\frac{{T^{n + 1} - T^{*} }}{\Delta t} = a\nabla^{2} T^{n + 1} + S^{T}$$

(8.68)

• Step 9: Update of Density

Update the density of air with the state equation of ideal gases.

$$\rho^{n + 1} = \frac{{p^{n + 1} M}}{{RT^{n + 1} }}$$

(8.69)

The proposed semi-Lagrangian PISO algorithm, without the corrector steps (Step 5 and Step 6), is similar to FFD except that it takes into consideration the pressure field from the previous time step. The FFD algorithm neglects the influence of pressure from the previous time step and assumes pressure is solely determined by the velocity field under the continuity restriction. In FFD, the advection term is completely separated from the rest of the momentum equation and is solved by using the semi-Lagrangian algorithm, which is faster and more stable compared to the conventional method of directly solving the advection equation. But the accuracy of PISO, theoretically and practically, has more advantages over FFD. The integrated algorithm (SLPISO) is expected to improve the accuracy of FFD without sacrificing much computing speed. The semi-Lagrangian advection algorithm is anticipated to largely reduce the computing cost of the direct solving of the advection term in the original PISO algorithm.

• (3) Simulation Cases

It is critical to evaluate the performance of the developed algorithm for both steady and unsteady problems. A lid-driven cavity flow case and a mixing convection case in a confined space are used to evaluate and illustrate method performance. Figure 8.6 shows the lid-driven cavity laminar flow under isothermal condition (Ghia et al. 1982). Figure 8.7 shows a 2-D mixing convection case (Blay et al. 1992) with temperature impacts.

Fig. 8.6

Lid-driven cavity flow under isothermal condition

Fig. 8.7

2-D mixing convection case with heated floor

• Results and Analysis:

• (1) Lid-driven cavity flow

The study compares the performance of four algorithms: SIMPLE, PISO, FFD and SLPISO. The mesh size is 50 × 50 and the time step size is 0.005 s. Figure 8.8a shows the predicted V_y at line Y = 0.5 m. The results of PISO and SLPISO are almost identical. SIMPLE provides similar velocity magnitude while FFD obtains considerably different results. The results in this case reveal that SLPISO shares the same accuracy as PISO, with a slight deviation from experimental data. All of them provide better results than FFD. Figure 8.8b compares the computing costs. SIMPLE requires much more time. SLPISO has a similar speed as FFD. However, both of them are slower than PISO in this case, which will be explained later.

Fig. 8.8

Predicted results and computing costs of the lid-driven cavity case

• (2) 2-D mixing convection flow

The study evaluates the algorithm with a 2-D mixing convection case (Blay et al. 1992) that includes the temperature field. Experimental results were obtained from the literature, which were measured in a laboratory chamber of 1.04 m × 1.04 m × 0.7 m (x × y × z) equipped with a 18 mm wide inlet slot and a 24 mm wide outlet slot. The experiment produced a fairly good 2-D flow at the central plate. The experiment measured wall temperatures and supply air conditions, respectively, as T_roof = T_walls = 15 °C, T_floor = 35.5 °C, T_inlet = 15 °C, V_inlet = 0.57 m/s (normal to the inlet slot), as well as temperature, V_y at the ten points along the middle line on the central plate (as shown in Fig. 8.7). This study uses the constant effective kinematic viscosity and heat transfer coefficient, namely one hundred times of the physical values, to consider the turbulence impact. The mesh size is 80 × 80 and the time step size is 0.005 s. Results in Fig. 8.9 demonstrate that the SLPISO algorithm provides similar results as the PISO method. FFD has a large disparity in temperature prediction. SLPISO has similar computational speed as FFD, while they are still slower than PISO.

Fig. 8.9

Predicted results and computing costs of the mixing convection case

When the study increases the grid number from 80 × 80 to 300 × 300, and further to 1000 × 1000, the computational cost performance for these algorithms changes as shown in Fig. 8.10a, b. As the number of grid increases, SLPISO and FFD are faster than PISO. The reason for this is the inherent characteristic of the semi-Lagrangian scheme. As the grid number increases, the computing cost of the traditional solvers, such as SIMPLE and PISO, demonstrates exponential growth trend, while the semi-Lagrangian scheme shows a linear growth as revealed in Fig. 8.10c (the influence of correction steps makes the calculation cost growth of FFD and SLPISO not exactly the linear).

Fig. 8.10

Computational cost comparison of different solvers with different grids

The comparison of simulation speed above is under the situation of using the same time step. However, the stability analysis shows that SLPISO can tolerate a larger time step than PISO. The study uses the mixing convection case with mesh size of 1000 × 1000 to check the actual calculation speed of different solvers with different time steps. Figure 8.11 shows the computing time with the largest time step that each solver can handle. To reach stable and acceptable results for this case, the largest time steps are, 0.02 s, 0.005 s, 0.08 s, and 0.1 s, for SIMPLE, PISO, SLPISO and FFD, respectively. The shadowed columns in Fig. 8.11 show the relative computing cost with the time step size of 0.005 s for all the solvers, using SIMPLE as the benchmark. The black columns show the relative computing cost using their own largest time step. While the predicted results for velocity and temperature are similar to Fig. 8.9a, b, the modeling speeds of SLPISO and FFD with larger time steps are significantly increased.

Fig. 8.11

Computational cost comparison with different time steps

• (3) Transient 2-D mixing convection flow

To evaluate the transient simulation accuracy of SLPISO and FFD, a transient flow in the 2-D mixing convection case is simulated. Since no transient experiment results exist for this case, the SIMPLE algorithm results are used as the reference for comparison. The “experimental” data is taken every five seconds from the SIMPLE prediction at the middle point of the test chamber. The study uses the mesh size of 80 × 80. The time step is varied from 0.005 to 0.08 s. As the time step increases, the transient results and the steady state results of SLPISO and FFD deviate, where SLPISO outperforms FFD in general (Fig. 8.12). FFD must use smaller time steps to obtain similar results as SLPISO.

Fig. 8.12

Accuracy comparison with different time steps for transient simulation with SLPISO and FFD (“Exp” is from SIMPLE)

The increasing deviation of the SLPISO results is attributed to the false diffusion of the time term. Compared to the original equation, the discretization of the time term leads to an additional false diffusion $\frac{{u^{2} \varDelta t}}{2}\nabla^{2} u$ that is related to the time step size. The increase of the time step enlarges the false diffusion, so that the transient simulation result is less responsive than the reference curve, to the transient velocity. If the constant effective kinematic viscosity is adjusted according lower, compensating for the larger time step used, the results of SLPISO with the time step of 0.08 s can be similar to the results with the time step of 0.005 s, as verified by the numerical tests.

• (4) Discussions

Because of the inherent characteristics of the semi-Lagrangian scheme, SLPISO and FFD may not provide significant computing saving than the conventional CFD algorithms when the number of grid is relatively small. They gain their advantages when the number of grid is increased. Most engineering problems require more than one-million grids to reach solutions of grid-independence, and thus FFD and SLPISO show great potential of fast simulation for these applications. This potential is further enhanced with the advantage of being able to use larger time steps for both SLPISO and FFD. SLPISO is slightly slower than FFD but with a higher accuracy especially for transient cases. SLPISO can adopt larger time steps than PISO and FFD to obtain accurate steady state results.

Assignment-8: Simulating Microenvironment Around Thermal Manikin

• Objectives:

This assignment will use a computational fluid dynamics (CFD) program to simulate the benchmark case of a computer-simulated person (CSP) under a mixing ventilation condition (Fig. 8.13).

Fig. 8.13

Test of mixing convection around a thermal manikin

Key learning points:

• Indoor airflow and heat transfer simulation

• Simplification of indoor object (person)

• Comparison of simulation with experimental data.

• Case Descriptions:

• (1) 3D computational domain with dimensions of X × Y × Z = 2.44 × 1.2 × 2.46 m.

• (2) Air is supplied through the full cross-sectional area at one end of the channel and leaves through two circular openings at the opposite end.

• (3) The circular exhaust openings have a diameter of 0.25 m and are located 0.6 m from the floor and the ceiling, respectively.

• (4) The CSPs are located 0.7 m from the inlet, centered on the x-axis.

• (5) The geometry of the CSP is based on an average-sized woman with a standing height of 1.7 m. When seated, the CSP has a height of 1.38 m. The surface area of the CSP is 1.52 m². Pick up a reasonable body size.

• (6) A uniform velocity profile of U = 0.2 m/s and T = 22 °C is applied to the opening. Inlet turbulence intensity k and dissipation rate ε values can be calculated based on the literature (ISSN 1395-7953 R0307).

• (7) A convective heat flow rate of 38.0 W is prescribed for the CSP corresponding to an activity level of approximately 1 Met (sedentary work).

• (8) Steady state w/o contaminant.

• (9) Other surfaces are adiabatic.

• (10) More case details and experimental data can be found at: http://homes.civil.aau.dk/pvn/cfd-benchmarks/csp_benchmark_test/.

• Simulation Details:

• (1) Turbulence model: Re-Normalization Group (RNG) k − ε model (Yakhot and Orszag 1986).

• (2) Convergence criterion: 0.1%.

• (3) Iteration: at least 1000 steps.

• (4) Grid: local refined grid with different total grid numbers.

• Cases to Be Simulated:

• (1) KERNG model with at least three different orders of grid numbers (e.g., 30 × 15 × 30, 45 × 23 × 45, 70 × 35 × 70).

• Report:

• (1) Case descriptions: descriptions of the cases.

• (2) Simulation details: computational domain, grid cells, convergence status.

  • Figure of the best grid used (on X–Z and X–Y planes);

  • Figure of a typical convergence process recorded.

• (3) Result and analysis (only present the best results except for the 1st item).

  • Grid-independent solution: use one vertical pole at X = 1.69 m to compare and show the predicted velocity differences with different grids;

  • Figure of velocity contours at the middle height of the CSP;

  • Figure of airflow vectors at the middle height of the CSP;

  • Figure of temperature contours at the middle height of the CSP;

  • Figure of velocity contours at the central plane cross the CSP;

  • Figure of airflow vectors at the central plane cross the CSP;

  • Figure of temperature contours at the central plane cross the CSP;

  • Comparison of velocities along the three tested vertical poles at the central plane cross the CSP (experiment-dot; simulation-solid line).

• (4) Conclusions (findings, CFD experience and lessons, etc.)