Select Equations to Be Solved

Abstract

Fluid mechanics mainly applies three conservation laws of mass, energy, and momentum to the fluid flow (called governing equations of flow) and predicts the flow characteristics and the interactions among fluids as well as with solids.

Appendices

Practice-3: Indoor Airflow and Heat Transfer

• Example Project: Air distribution inside a hospital operating room (OR)

• Background:

The goal of the air distribution inside a hospital operating room (OR) is to protect the patient and staff from cross-infection while maintaining occupant comfort and not affecting the facilitation of surgical tasks. However, a source of contamination bypasses HEPA installations in every OR, this source being the surgical staff themselves and the particles stirred up by their movement (Cook and Int-Hout 2009). Therefore, air motion control must be used to maximize air asepsis.

In hospital ORs, using HEPA-filtered air and vertical (downward) laminar airflow is typical. ASHRAE Standard 170-2008 (ASHRAE 2008) requires that ventilation be provided from the ceiling in a downward direction concentrated over the patient and surgical team. The area of the primary ventilation air diffusers must extend at least 305 mm beyond each side of the surgical table. It also requires that air is exhausted from at least two grilles on opposing sides of the room near the floor. It requires the use of non-aspirating, Group E outlets that provide a unidirectional flow pattern in the room (aka laminar flow diffusers). This study applied a computational fluid dynamics (CFD) tool to predict the flow pattern in a representative OR environment with standard air flow settings (Zhai and Osborne 2013).

• Simulation Details:

The CFD model was built according to the full-scale laboratory experiment. The same diffuser specifications and air change rate per hour (ACH) as tested in the experiment were used in the CFD model, as well as the same room and equipment and occupant conditions, as shown in Table 3.4 and Fig. 3.14. These objects and heat gain values were chosen based on detailed on-site OR studies and measurements (Zhai et al. 2013). The equipment thermal loads as well as temperature of the patient’s wound and skin can be seen in Table 3.5. Table 3.6 indicates the sizes of all of the objects in the room.

Table 3.4 Laboratory experiment specifications

Fig. 3.14

Base CFD model setup

Table 3.5 Laboratory thermal loads

Table 3.6 Room object dimensions

• (a) Geometry Generation:

Melikov and Kaczmarczyk (2007) discussed the importance of detailed indoor objects such as human body on indoor airflow characteristics and indicated the local impacts of most details of indoor objects. Focusing on the general indoor airflow patterns and interactions between patient and medical staffs, this study simplified the simulation of indoor subjects such as human bodies and equipment as rectangular geometries (except the surgical lighting) with exact heat sources as tested. This practice facilitates the generation of high-quality meshes and therefore improves both speed and accuracy of the simulations.

• (b) Mesh Generation

The example OR case was modeled using a rectangular Cartesian grid, which maps well to typical OR geometry. Local grid refinement was implemented near critical spaces and objects such as walls, inlets and persons. The results of a CFD simulation are highly dependent on the quality of the computational grid. The grid refinement study was conducted on the following grids: 70 × 58 × 45 (180 k cells), 87 × 73 × 57 (362 k cells), 106 × 91 × 70 (675 k cells), 124 × 111 × 86 (1.2 M cells), 155 × 142 × 108 (2.4 M cells). Figure 3.15 demonstrates the finest grid distribution.

Fig. 3.15

Grid refinement case: 2.4 M cells

Fig. 3.16

CFD grid refinement measurement locations in central cross-sectional plane (1. center of room; 2. interior edge of diffuser; 3. midpoint of diffuser; 4. exterior edge of diffuser; 5. midpoint of outer region of room)

• (c) Solver and Models

Both RANS and LES CFD methods were tested for this example case. While advanced CFD modeling techniques such as Large Eddy Simulation (LES) provide substantial benefits, the currently available RANS technologies have proven to be adequate for modeling the steady-state characteristics of the hospital operating room air distribution. In the RANS CFD solution methodology, the RNG k − ε turbulence model (Yakhot and Orszag, 1986) was employed as suggested by Zhang et al. (2007). Details about these models will be introduced in Chap. 4 “Select Turbulence Modeling Method”.

• (d) Boundary Conditions/Object Modeling

Most indoor objects such as persons and equipment were specified straightforwardly using the standard wall/block boundary condition methods. Inlet boundary condition modeling is critical to accurate CFD modeling of indoor environments, as the inlet boundary condition is the primary source of momentum that is responsible for the overall room air distribution pattern. Srebric and Chen (2002) performed a comprehensive analysis of diffuser boundary conditions to determine appropriate simplified boundary conditions, and the box and momentum method have been determined to be the most appropriate models for the diffusers that were applied in this study. The momentum method was used in this example since it was recommended by Chen and Srebric (2002) for the grille diffuser that is similar to the non-aspirating diffuser type.

• Results and Analysis:

• (a) Convergence/Grid Independence

The simulation was considered converged when the sums of residual errors in the mass, momentum, energy, and turbulence-model equations, respectively, reach a pre-defined level (i.e., 0.1%). The grids of different sizes were evaluated using the normalized root mean squared error (NRMSE) of the CFD model results with different grids (Wang and Zhai 2012) that will be described in Chap. 9 “Analyze Results”. Figure 3.17 shows the NRMSE of the predicted U and W direction velocity at the four measure poles (1–4) across the center axis of the room (2.88 m) (shown in Fig. 3.16), between the 180 K (and 362 K) meshes and the 675 K mesh. It reveals that there is generally a great improvement in error with the 362 K mesh, and the computational error is typically below 10%, and absolutely below 30%. Based on these, and in order to minimize the simulation time, the 362 K mesh could be used for various engineering parametric simulations.

Fig. 3.17

NRMSE comparison between 180 and 362 K meshes and 675 K mesh

• (b) Model Validation

The simulation replicates the airflow pattern as observed in the lab experiment (Zhai et al. 2013): an inward curvature of the airflow to the center of the jet stream, as seen in Fig. 3.18. This behavior reduces the overall coverage area and could pose a contamination risk to the patient.

Fig. 3.18

Velocity vectors and contours at the central cross section with 675 K grid

The quantitative comparisons of simulation and experimental results were plotted in Figs. 3.19 and 3.20, for U (X) and W (Z) velocity component, respectively. Figures 3.19 and 3.20 show that the CFD simulations closely follow the experimental results, with a few exceptions (e.g., right above the patient body at Pole 1). It also appears that there is, in general, a large difference between the experimental results and the 180 K mesh, but a smaller difference between the 362 and 675 K meshes.

Fig. 3.19

Comparison of U-velocity in X direction

Fig. 3.20

Comparison of W-velocity in Z direction

• (c) Discussion of Results

This example was used to demonstrate the applicability of using CFD for modeling and analysis of the surgical environment air flow. While CFD can be accurately used for modeling indoor air distribution in operating rooms, CFD user must be extremely careful in implementing these models to insure accurate simulation of air flow. The sensitivity of air flow to thermal characteristics of the indoor environment makes the model sensitive to heat gain input parameters. The heat gain and inlet boundary conditions must be carefully selected to ensure that the resulting air distribution patterns are correct.

The general indoor environment conditions place the operating room indoor air distribution in the mixed convection regime, but high cooling loads can lead to a strongly buoyancy-driven flow that is verified by the parametric study of the Archimedes number of supply air jet in the OR. The study reveals that the dependence of the room air distribution on the Archimedes number of supply air jet, instead of face velocity of supply diffuser, is of significant importance.

Assignment-3: Simulating Wind Flow Pattern across an Urban Environment

• Objectives:

This assignment will use a computational fluid dynamics (CFD) program to model the wind-driven airflow distribution over an urban environment.

Key learning point:

• Urban wind simulation with appropriate domain sizes

• Wind profile input.

• Simulation Steps:

• (1) Build a (few) block(s) of buildings to represent a realistic community site (You may use map tools such as Google Earth to find some info);

  • a. For those of you familiar with SketchUp (free tool), you may also consider to download building block models from Google SketchUp 3D warehouse for some specific real location in the world;

  • b. You need to convert the SketchUp model into a certain suitable format that can be recognized and imported into the CFD software. Cleaning work is needed most of time to correctly use SketchUp models in CFD tools.

• (2) Select appropriate outdoor domain sizes to be modeled;

• (3) Study local weather data and identify representative wind conditions (directions, speeds, changes, frequencies, etc.);

• (4) Establish corresponding boundary conditions, particularly the wind profile [iso-thermal case only: no temperature];

• (5) Select a turbulence model: the standard k-ε model;

• (6) Define convergence criterion: 0.1%;

• (7) Set iteration: at least 1000 steps for steady simulation;

• (8) Determine proper grid resolution with local refinement: at least 400,000 cells.

• Cases to Be Simulated:

• (1) Steady flow of wind over the building complex.

• Report:

• (1) Case descriptions: description of the case

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

  • Figure of the grid used (on X-Z, X-Y planes);

  • Figure of simulation convergence records.

• (3) Result and analysis

  • Figure of airflow vectors at the middle plane of the buildings;

  • Figure of pressure contours at the middle plane of the buildings;

  • Figure of velocity contours at the middle plane of the buildings.

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