Computational Fluid Dynamics Analysis of Butterfly Valve Performance Factors

Adam Del Toro
Utah State University

Abstract
Computational Fluid Dynamics Analysis of Butterfly Valve Performance Factors
by
Adam Del Toro, Master of Science
Utah State University, 2012
Major Professor: Dr. Robert E. Spall
Department: Mechanical and Aerospace Engineering

Butterfly valves are commonly used in industrial applications to control the internal flow of both compressible and incompressible fluids.

A butterfly valve typically consists of a metal disc formed around a central shaft, which acts as its axis of rotation.

As the valve’s opening angle, θ, is increased from 0 degrees (fully closed) to 90 degrees (fully open), fluid is
able to more readily flow past the valve. Characterizing a valve’s performance factors, such as pressure drop, hydrodynamic torque, flow coefficient, loss coefficient, and torque coefficient , is necessary for fluid system designers to account for system requirements to properly operate the valve and prevent permanent damage from occurring.

This comparison study of a 48-inch butterfly valve’s experimental performance factors using Computational Fluid Dynamics (CFD) in an incompressible fluid at Reynolds numbers ranging approximately between 105 to 106 found that for mid-open positions (30-60 degrees), CFD was able to appropriately predict common performance factors for butterfly valves.

For lower valve angle cases (10-20 degrees), CFD simulations failed to predict those same values, while higher valve angles (70-90 degrees) gave mixed results.

Butterfly valves are commonly used to control fluid flow inside of piping systems.

A butterfly valve typically consists of a metal disc formed around a central shaft, which acts as its axis of rotation. As a butterfly valve is rotated open, fluid is able to more readily flow past the valve. A butterfly valve’s design is important to understand and is commonly characterized by its own performance factors.

How a butterfly valve will perform, while in operation at different opening angles and under different types of flow, is critical information for individuals planning and installing piping systems involving the valve.

Performance factors common to a butterfly valve include the following: pressure drop, hydrodynamic torque, flow coefficient, loss coefficient, and torque coefficient.

While these values can usually be obtained experimentally, it is sometimes not feasible or possible to calculate the performance factors of some butterfly valves.

Another method wherein butterfly valve performance factors can be obtained is by using Computational Fluid Dynamics (CFD) software to simulate the physics of fluid flow in a piping system around a butterfly valve. This study sought to compare experimental and simulated CFD performance factors of a 48-inch diameter butterfly valve for various valve openings and flow conditions in order to determine the validity of using CFD to predict butterfly valve performance factors.

It was found that for mid-open butterfly valve positions (30-60 degrees), CFD was able to appropriately predict common performance factors for butterfly valves.

For lower valve angle cases (10-20 degrees), CFD simulations failed to predict those same values, while higher valve angles (70-90 degrees) gave mixed results.

Introduction

Butterfly valves are commonly used in industrial applications to control the internal flow of both compressible and incompressible fluids.

A butterfly valve typically consists of a metal disc formed around a central shaft, which acts as its axis of rotation.

As the valve’s opening angle, θ, is increased from 0◦ (fully closed) to 90◦ (fully open), fluid is able to more readily flow past the valve.

Butterfly valves must be able to withstand the stresses and forces that results from high Reynolds number flows.

Characterizing a valve’s performance factors, such as pressure drop, hydrodynamic torque, flow coefficient, loss coefficient, and torque coefficient, is necessary for fluid system designers to account for system requirements to properly operate the valve and prevent permanent damage from occurring to the valve.
This study seeks to compare a 48-inch butterfly valve’s experimental performance factors to those obtained using Computational Fluid Dynamics (CFD) and to assess the feasibility of using CFD to predict performance factors of butterfly valves.

Chapter 1 will contain a literature review regarding the research done on butterfly valves, its current state-of-art, and its connection to this study.

A brief overview of butterfly valve attributes, nomenclature, features, and performance factors will also be highlighted.
Chapter 2 will describe the experimental setup carried out by the UWRL for this study, including instrumentation, experimental results, and the uncertainty of the experimental results.

Chapter 3 will present a short overview of CFD theory and use.

Chapter 4 will provide details regarding the meshing process and setup used on the butterfly valve simulations, including geometry import and tessellation, boundary conditions, meshing models
and options, Chapter 5 will cover the physical models used and their corresponding options.

Chapter 6 will contain results from the executed CFD simulations, including descriptions of
the flow field such as pressure and velocity, predicted performance factors, and demonstrated grid convergence.

Chapter 7 will draw upon results of the experiment and simulations and provide conclusive remarks.

1.1 Literature Review

One the earliest and most comprehensive pieces of research on the flow characteristics and performance of butterfly valves was performed by Cohn [1].

Using data provided by previous authors, Cohn attempted to parameterize torque and flow coefficients based on thickness to diameter ratio for numerous butterfly valve geometries, most of which were symmetrical.
McPherson [2] studied various blade variations of single eccentric butterfly valves in incompressible turbulent flow subject to free, submerged, and continuous piping discharge arrangements.

McPherson found that for a given type of installation, the flow characteristics were not significantly influenced by either the shape of the blade or by the closing angle except for the near-open and closed positions, respectively.

Using a two dimensional setup of different symmetric butterfly valve blades, cavitation was also predicted.
Sarpkaya [3] also studied the torque and cavitation characteristics of idealized twodimensional and axially symmetrical butterfly valves by considering an idealized case of laminar uniform flow through a symmetrical lamina (representing the butterfly valve) between two infinite walls.

Using these assumptions, Sarpkaya was able to extend approximate solutions to hydrodynamic torque, cavitation, and flow coefficients for three dimensional butterfly valves using semi-empirical equations.

Addy et al. [4] conducted several small-scale compressible flow experiments with sudden enlargement configurations for butterfly valve models to predict mass flowrate and overall pressure characteristics. In addition, a full size butterfly valve was built and tested.

The sudden enlargement configurations were classified as three different types of nozzles:
contoured converging, conical converging and sharp-edge orifice.

It was concluded that the performance characteristics of the valve can be predicted if the valve flow coefficient is known for a specified operating pressure ratio.

Eom [5] building off the work of Cohn [1] and McPherson [2], studied the performance of butterfly valves as a flow controller.

Eom compared the flow characteristics of perforated and non-perforated butterfly valve disks and found their performance to be in good agreement with one another, except at low blade (opening) angle values of about 10 degrees.

He also studied the effect that blockage ratios (area of disk to area of pipe or duct) had on butterfly valves as throttling devices. Furthermore, Eom was able to predict loss coefficients sufficiently well from blockage ratios at Reynolds numbers in the range of 104.

Kimura et al. [6] and Ogawa and Kimura [7] used free-streamline and wing theory to model symmetric butterfly valves between infinite parallel walls in two dimensions and used correction equations to compensate for pipe wall conditions.

The correction equations also required a corrected opening angle and thickness of the disks, and uniform velocity. Using the given two-dimensional models, torque characteristics, pressure loss, and cavitation of three-dimensional experiments were predicted and analyzed.

While the general pattern of torque coefficients followed the experimental data, the difference between the predicted and actual values were large.

In more recent years since Kimura and Ogawa, scientific and engineering communities in the field of fluid dynamics and valve research have placed more emphasis in Computational Fluid Dynamics (CFD), especially with the advent of commercial CFD software in the 1990s.

Huang and Kim [8] were some of the first to use commercial CFD software to investigate three dimensional flow visualization of a symmetric butterfly valve (modeled as a thin flap valve disk). Huang used CFD code FLUENT to simulate a steady incompressible flow with k- turbulence modeling. Valve positions were simulated at openings of 30, 45, 60, 70, and 90 degrees.

Huang also investigated the length downstream of the valve in which flow would return to fully developed conditions. Due to computational restrictions, a relatively coarse mesh of a maximum of 25,000 cells was used in the CFD calculations.

Huang also compared his numerical results with the experiments carried out by Blevins [9]. The 45 degree case was found to be the most agreeable with the experimental data, while the rest lacked agreement.

Lin and Schohl [10] used commercial CFD software FLUENT to predict drag coefficients for a symmetric coin shaped butterfly valve at opening angles in an infinite flow field with results obtained experimentally by Hoerner [11].

Sensitivity of the results to turbulence model selection, accuracy of discretization schemes, grid quality, and grid dependence were studied as part of the validation. Lin compared k-, k-ω, and k-ω SST turbulence models and opined that the later model was preferred for resolving the Reynolds-averaged Navier-Stokes equations and that use of a 1st order discretization for the flow domain led to predictions significantly higher than those from the 2nd order schemes.

Flow coefficients aligned well with experimental data overall, however it should be noted that exact modeling comparisons between the experimental setup and the numerical model were difficult to match. Lin also modeled a 3.66 meter diameter butterfly valve within a pipe at valve openings of 20, 40, 50, 60, 70, 80, and 90 degrees with cavitation free conditions and incompressible flow using CFD.

A computational mesh size included about 1.5 million tetra and hexa-elements. Pressure drop across the valve was calculated and predicted flow coefficients matched relatively well with experimental data provided by the United States Army Corps of Engineers (USACE) for a similarly shaped disc butterfly damper.

Song et al. [12] performed a structural analysis of large butterfly valves, in addition to validating three-dimensional experimental data of a butterfly valve’s pressure drop, flow coefficient, and hydrodynamic torque coefficient using general purpose CFD code CFX [13].

The k- turbulence model was selected by Song since it does not involve the complex nonlinear damping functions required by other models. A mesh of nearly one million cells was used with a domain extending eight pipe diameters upstream from the valve and approximately ten pipe diameters downstream.

Cases were run for disk opening angles of 5 to 90 degrees in increments of 5 degrees. Generally, good results were obtained except when the valve opening angle was less than 20 degrees. In the 20 degree case, differences between experimental and simulation data were found to be nearly 50%.

Leutwyler and Dalton [14, 15] performed a CFD study in two and three dimensions for symmetric butterfly valves in compressible fluids at various angles and over a range of of pressure ratios.

The general purpose CFD code FLUENT was used with the following turbulence models: Spalart-Allmaras, k-, and k-ω. Leutwyler favored the k- turbulence model for its well rounded capabilities and moderate computational costs. In addition to examining grid refinement, coefficients for lift, drag and torque were validated against experimental values.

Henderson et al. [16] measured torque and head loss of a symmetrical butterfly valve installed in a hydro-electric power generating scheme for steady flow at Reynolds numbers of order 106. This was done for valve opening angles of 10 to 80 degrees in 10 degree increments.

The general purpose CFD software ANSYS CFX was validated using collected experimental data. In the experiment, Henderson used anti-vacuum valves downstream in a penstock tunnel to prevent severe cavitation. The CFD flow domain extended from about 58 diameters (D) upstream and 15D downstream to ensure fully developed flow conditions.

Tetrahedral elements were used on the valve face to best model the butterfly valve features. Consequently, the number of cells in the domain ranged from 2.2 million to 220 million.

Henderson favored the Shear Stress Transport (SST) turbulence modeled and found that for valve angles greater than 20 degrees, the flow downstream from the valve was dominated strongly by unsteady vortical disturbances.

An estimated eddy shedding frequency of about 1.3 Hz was estimated. Cases were run in which the CFD models had a symmetrical boundary to improve solution time and one in which the whole model was used for a steady and transient solution, respectively.

The main difference manifested between the full and symmetry models was that the whole model was able to show the eddy shedding alternate between sides, while the torque coefficients and flow patterns remained unchanged overall.

While the overall pattern of the predicted torque characteristics are similar to the experimental data, they differ by over 25% in many mid-valve positions.

Henderson concluded that better field measurements, including the flow rate, could improve the modeling of the CFD boundary conditions.

Cheiworapuek et al. [17] investigated incompressible turbulent flow past a butterfly valve at 15, 30, 45, 60 and 90 degree opening angles.

The CFD code FLUENT was used to validate experimental data for butterfly valves having diameters of 150 and 300 mm. The number of elements used in the simulation ranged from 1.1 million to 1.4 million. The k- turbulent model was used.

For the experiment, pressure taps were located 1D upstream and 14D downstream. Cheiworapuek observed that vortices were found near the tips of the butterfly valve and became larger as the valve disk was oriented at more closed positions.

The loss coefficient was generally unaffected by a change in inlet velocity for a given disk orientation. Large differences between the experimental data and simulation results were on the order of 50% for loss coefficients and torque.

Feng et al. [18] used a general purpose CFD code with a k- turbulence model to study cavitation and flow characteristics of a 1.2 meter diameter double eccentric butterfly valve.

A hybrid mesh of quadrilateral and triangular elements were used. The flow domain extended from five diameters upstream to about ten diameters downstream.

Feng found that a double eccentric structure had improved dynamic response and self-sealing in comparison with a single or no offset butterfly valve.

While many have researched butterfly valves over the years, the following comparison study will seek to contribute insight into the use of CFD to predict butterfly valve performance factors, especially in specifying the level of agreement that can be expected at various valve opening angles, and discuss meshing methods to improve results.

1.2 Butterfly Valve Attributes

Many butterfly valves have asymmetrical features and thus their direction of installation, commonly referred to as a seating direction, typically affect the valve’s flow characteristics. Butterfly valves can be installed in one of two directions: seated upstream and seated downstream.

Seated upstream signifies that the valve seat, where the valve seals off flow when fully closed, is upstream of the valve disk shaft or axis of rotation.

Seated downstream signifies that the valve seat is downstream of the valve disk shaft or axis of rotation. A layout of the butterfly valve for the present configuration (seated downstream) and opening angle definition, θ, can be seen in Fig. 1.1.

The port diameter of a seated downstream butterfly valve is defined as the diameter of the main valve body as it leaves the main valve body and enters into the pipe diameter in which it is installed. Figure 1.2 further shows the main features and components of the butterfly valve used in this paper.

Components that are considered dynamic and move with the rotation of the main disk body are the following listed in Fig. 1.2: bottom and top shaft, rubber seal, seal ring retainer, and retainer bolts.

The rest are static components. Epoxy bonds the seating ring onto the main valve body.

The top and bottom sleeves help secure their corresponding shafts to the main valve and disc body.

The rubber seal is fastened tight onto the main disc body by means of the seal ring retainer and corresponding bolts. The rubber seal ensures a tightly closed valve when fully closed.

1.3 Butterfly Valve Performance Factors

Characterizing a butterfly valve typically involves evaluating the most common performance factors such as: pressure drop across the valve, hydrodynamic torque, flow coefficient loss coefficient, and the torque coefficient.

These performance factor standards have been widely published by Bosserman and AWWA [19] and will be described in subsequent paragraphs.

1.3.1 Pressure Loss

Pressure loss across a valve is often attributed to disruptions caused in the flow field such as obstruction, flow separation and mixing. For butterfly valves, pressure losses vary depending on the disk angle configuration, θ, and flow rate, Q.

The pressure loss is represented by the absolute pressure differential between the measured pressure upstream, Puθ and the measured pressure downstream, Pdθ, as given in Eqn. 1.1 below:

∆Pθ = Puθ − Pdθ (1.1)

For a given flow rate, pressure losses will generally decrease as the valve’s opening angle increases due to less interference in the flow. In this study, the upstream and downstream pressures were measured at a point two diameters upstream and six diameters downstream, respectively, per AWWA guidelines [19].

It should also be noted that this pressure loss represents a gross measurement instead of net measurement.

This means that head losses due to pipe friction length between measurement points (which are minimal), are included in the ∆Pθ measurements, and thus affect other performance factors to be discussed.

1.3.2 Hydrodynamic Torque

The sign convention used in this study is for torque around the valve shaft (axis of rotation) to be positive when flow acts to close the valve, such that a positive torque is required to keep the valve open.

Measurement of hydrodynamic torque requires measuring the total opening and closing torque, Ttoθ and Ttcθ, respectively, as demonstrated below and described later in the experimental setup section.

Total Opening and Closing Torque

The total opening and closing torques can be defined as follows in equations 1.2 and 1.3:

Ttoθ = Tdθ + Tbθ + Tcgθ + Tp , (1.2)

Ttcθ = Tdθ − Tbθ − Tcgθ − Tp, (1.3)

where Tdθ is the hydrodynamic torque, Tbθ is the bearing torque, Tcgθ is the center of gravity torque, and Tp is the packing and hub torque. These various torques will be briefly described below.

Bearing Torque (Tbθ)

The bearing torque, Tbθ, in a butterfly valve is the frictional resistance to rotation imposed on the valve shaft by the bearings. Its value is highest at the near-closed position because of the high differential pressure when the valve is nearly closed. Bearing torque reduces to nearly zero as the valve reaches the fully open position and always acts in the opposite direction to the valve’s movement. It is defined in Eqn. 1.4:

where Dd is the disk diameter, ∆Pθ is the pressure drop while at the disc angle θ, ds is the shaft diameter, and Cf is the coefficient of friction between the shaft and bushing.

Center of Gravity Torque (Tcgθ)

Center of gravity torque, Tcgθ, is caused by the offset center of gravity of the disc and occurs when the valve shaft is located in or near the horizontal plane.

This torque is often assumed as insignificant, which in the case of this study is deemed valid since the stem is in the vertical position. Center of gravity torque is defined in Eqn. 1.5 as:

Tcgθ = ScWdCg cos(θ + γ), (1.5)

where Sc is the sign convention variable, Wd is the weight of valve disc, Cg is the valve disc center of gravity distance from the shaft centerline, θ is the valve opening position angle where closed=0 degrees and fully open=90 degrees, and γ is the center of gravity offset angle in non-symmetric disc designs [19].

Packing and Hub Torque (Tp)

The packing and hub torque is due to friction between the shaft seal and the valve shaft, and the friction between the disc and/or shaft and the body hub seal where the shaft penetrates the pressure boundary.

The packing and hub torque always acts in the opposite direction to the valve’s movement and is defined below in Eqn. 1.6:

Tp = Cpckds, (1.6)

where Cpck is a packing coefficient [19], and ds is the valve shaft diameter.

Hydrodynamic Flow Torque (Tdθ)

The hydrodynamic flow torque is due to the effects of the internal fluid media (water in this case) or gravity acting on the valve at any given opening angle, θ.

Hydrodynamic flow torque is necessary to compute flow characteristics and the torque coefficient for the valve, and in determining motor requirements for operating the butterfly valve.

1.3.3 Flow Coefficient

The valve flow coefficient, Cvθ is a measure of the flow rate of water through a valve at 60◦ F at a pressure drop of 1 psi (lb/in2) and is customarily presented in units of gpm/psi1/2 as seen in Eqn. 1.8 below:

where Q is the flow rate in gpm, SG is the specific gravity of the fluid in use, and ∆Pθ is the pressure drop across the valve in psi. The valve flow coefficient is useful to manufacturers and users in understanding the flow capacity of valves.

1.3.4 Loss Coefficient

The flow resistance coefficient, commonly known as the loss coefficient, Kθ, is a dimensionless value commonly used in the design of thermal fluid systems to predict head losses present due to the presence of various components.

The loss coefficient is shown below in Eqn. 1.9:

where ∆Pθ is the pressure loss measured across the points previously described, and ρ is the density of the fluid in use.

1.3.5 Torque Coefficient

The torque coefficient, Ctθ, is a dimensionless quantity used by manufacturers and users to determine the torque and power requirements of valves scaled relative one to another.
Torque coefficient is defined in Eqn. 1.12 as:

Experimental Setup and Results

Utah State University (USU) was contracted to conduct performance tests at the Utah Water Research Laboratory (UWRL) on a 48-inch butterfly valve.

The valve was installed in the seated downstream position in a 47.25 inch internal diameter steel pipe line as seen in Fig. 2.1.

A flowchart regarding the experimental setup can be seen in Fig. 2.2. Flow was regulated upstream using a control valve to ensure a fully developed flow profile before traveling a length of 15 diameters (D) to encounter a 48-inch Venturi flowmeter, which was used to measure the volume flow rate, Q.

Further downstream an additional 15D from the Venturi flowmeter, a pressure tap was installed. The pressure tap was used to measure the pressure, Puθ, 2D upstream from the butterfly valve which was configured with linear strain gages.

During the experiment, the butterfly valve was opened and closed under each set of flow conditions in order to measure the total opening and closing torques, Ttoθ and Ttcθ, using the installed strain gages. Six diameters downstream from the butterfly, another pressure tap was installed to measure the pressure, Pdθ. Beyond the downstream pressure tap, the flow line extended an additional 15D before reaching another control valve, and then out to atmospheric conditions.

The temperature of the water used in the experiment varied little at an average of 48.6 ◦F, which gives the following fluid properties: SG = 1.0007 for the specific gravity, and ν = 1.45 ∗ 10−5
ft2/sec for the kinematic viscosity.

Using these values combined with the five directly measured values of Q, Puθ, Pdθ, Ttoθ, and Ttcθ, the following flow performance factors from section 1.3 were calculated for the butterfly valve: pressure drop (∆Pθ), hydrodynamic torque (Tdθ), flow coefficient (Cvθ), loss coefficient (Kθ), and the torque coefficient (Ctθ).

These values and performance measurements were performed and calculated for nine different valve degree angle openings, from θ = 10 degrees to θ = 90 degrees in 10 degree increments. The instrumentation used to take the measurements will be briefly described, followed by a review of the instrumentation uncertainty of directly measured values and the uncertainty of the flow performance factors.

2.1 Instrumentation

Using the setup previously described, five flow configuration properties were directly measured using instrumentation installed in the experimental system: a venturi flowmeter, pressure taps, and strain gages. These will now be briefly discussed.

Venturi flowmeters are considered to be very accurate flowmeters. They are generally characterized by their gradual contraction and expansion, which prevents flow separation and swirling. They only suffer frictional losses on the inner wall surfaces and cause very low head losses. Figure 2.3 shows a cross-section of a Venturi flowmeter.

By using the assumptions of the Bernoulli and continuity equations [20], Venturi flowmeters can measure the volume flow rate. The relative uncertainty of the 48-inch Venturi flowmeter used in this experiment was UQ/Q = 0.25%.

Pressure taps are commonly used in piping systems to take differential measurements of pressure. This is done by drilling prescribed holes through the pipe wall and welding the tap fittings into the drilled hole such that the tapped fitting is flush to the interior of the pipe wall, so as not to interfere significantly with the fluid flow. Once this is done for another pressure tap, a pressure transducer is connected to both pressure taps, allowing the transducer to take a differential measurement of the two. The relative uncertainty of the pressure transducer used in this experiment was U∆Pθ/∆Pθ = 0.25%.
Torque strain gages are used by installing thin strain gages onto cylindrical surfaces that will undergo torsion. Using the stress-strain relationship of a known material and calibrating the strain gages, the torque can be calculated. For this experiment, calibrated linear strain gages were installed on the butterfly valve shafts. For each set of flow conditions associated with the valve degree opening, an actuator cycled the butterfly valve to completely open and closed positions numerous times in order to measure the total opening and closing torques.
The relative uncertainty of these measurements using the strain gages was UTtoθ /Ttoθ = UTtcθ /Ttcθ = 3%.

2.2 Experimental Results

Results for the described experiment were provided by the UWRL. The directly measured flow values are provided in Table 2.1. The calculated flow performance factors are provided in Table 2.2 along with Reynolds numbers for each respective flow.

2.3 Uncertainty of Experimental Results

Knowing the uncertainty in the direct measurements and the calculated flow performance factors is vital to understanding the range within which to expect errors arising from systematic and random uncertainties. Uncertainty analysis of the experimental data and calculated results provide important information regarding the possible overlap between the experiment itself and the CFD simulations. For example, if large relative uncertainties are discovered for the experimental data and if large disparities exist between the experimental and simulation results, it could be difficult to quantify the level of agreement between the two.
A common method for carrying out a general uncertainty analysis involves using the Taylor Series Method (TSM) for propagation of uncertainties [21]. This usually involves considering a result, r, as a function of several variables

r = r(X1, X2, …, XN ). (2.1)

The combined standard uncertainty at 95% confidence interval, U95, is given as

where bXi and sXi are the systematic and random standard uncertainties, respectively.
A detailed general uncertainty analysis has been carried out in Appendix A for all the performance factors listed in Table 2.2. The experimental relative uncertainties are provided in Table 2.3.

CFD Setup

Using general purpose CFD software STAR-CCM+1, the previously described experiment was modeled in an attempt to simulate and predict the measured butterfly valve performance factors. The overall approach to simulating the experimental model consisted of: using a computer aided design model of the butterfly valve with appropriate cylindrical parts added to simulate pipe flow upstream and downstream of the valve, properly meshing and applying physical models to the simulation, creating appropriate flow conditions to match the experiment, such as mass flow rate, fluid properties, valve angle opening, etc., ensuring iterative and grid convergence and time independent results, and recording the
predicted flow performance factors and overall flow properties. Simulations were evaluated for nine different valve degree openings from θ = 10 to 90 degrees in ten degree increments, and two additional simulations for the 10, 50, and 90 degree cases with coarser meshes to investigate grid refinement.
According to Versteeg and Malalasekera [22], a large source of uncertainty in CFD modeling can result from poor representation of boundary conditions, particularly the inlet and outlet conditions for internal flow. While the outlet conditions are of less concern as discussed later on, the inlet boundary condition deserves special consideration. In order to ensure the fully developed flow conditions listed in Table 2.1 for each valve opening case, a periodic flow simulation was setup prior to simulation of the butterfly valve case and was used as the upstream boundary condition.
The periodic flow simulation for this study allowed rapid development of fully developed flow conditions by forcing a short internal turbulent flow simulation to match a specified pressure drop. By iterating the pressure drop several times, the fully turbulent flow conditions of each simulation case can match the experimental flow conditions found in 2.1. The turbulent kinetic energy, turbulent dissipation rate, and velocity vectors for the periodic flow cases are then extracted and used as the necessary inlet boundary conditions of the valve simulations. This allows for exceptional representation of the inlet boundary
condition values, eliminates the need for a long upstream entry length cylinder region to simulate the development of fully developed flow prior to passing into the butterfly valve, and effectively decreases the amount of time needed to iterate over a larger domain valve simulation. More details regarding the procedure can be found in Appendix B.
A brief discussion regarding computational fluid dynamics will now be presented, followed by a description in the next chapter of how butterfly valve simulations were setup using STAR-CCM+.

3.1 Computational Fluid Dynamics

Governing equations of fluid dynamics commonly referenced for incompressible isothermal fluids in CFD include the Navier-Stokes equations [23] given in conservative form using index notation as seen in Eqn. 3.1. The Navier-Stokes equations are a simplification of the conservation of momentum equations and the constitutive equations that define the relationship between shear and strain for a newtonian fluid.

While many laminar solutions (low Reynolds number flows) are possible using Eqn. 3.1, nonlinearities and instability arise due to turbulence. Turbulence is often characterized as irregular and random flow, with three-dimensional vortical fluctuations. Most methods of analyzing turbulence results in more unknowns than available equations, and thus results in an equation closure problem. Some techniques used include focusing on the mean flow and the effects of turbulence on mean flow properties by using what are called the unsteady Reynolds-averaged Navier-Stokes (RANS) equations [22] as given in Eqn. 3.2 using index notation:

where ´τij is the Reynolds stress tensor that attempts to describe the diffusive nature of turbulence as defined in Eqn. 3.3 .

However, in order to compute turbulent flows with the RANS equations, it is necessary to develop turbulence models to predict the Reynolds stresses and have closure.
Some of the most common turbulence models include: mixing length, Spalart-Allmaras, k-, k-ω, algebraic stress, and Reynolds stress. While each turbulence model has its strengths, weaknesses, and variations, this study will focus on using the k- model only.
Reasons for choosing the k- turbulence model include the following: simple turbulence model to use for which only initial and/or boundary conditions need to be supplied, excellent performance for many industrially relevant flows, and well established as the most widely validated turbulence model [22]. Since the initial and/or boundary conditions are only required, they can be easily extracted from the periodic flow cases with ease as mentioned earlier in this chapter.
While many variations of the k- turbulence model are commonly used, they all derive from the standard k- model. The standard k- model uses the following transport equations for the turbulent kinetic energy, k, and turbulent dissipation rate, , respectively:

where C1, C2, Cµ, σk, and σ are empirical constants and µt , the turbulent viscosity, is modeled as

Versteeg and Malalasekera provide additional information regarding the formulation and calculation of these transport equations [22].

Meshing

In order to numerically solve the RANS equations from Chapter 3, it is necessary to discretize or partition a normally continuous medium into discrete volumetric cells, which consist of vertices and faces. A vertex is a point in space defined by a position vector as seen in Fig. 4.1. A number of vertices can be used to define a feature curve or a face. A feature curve in its most basic terms consists of two vertices that define a line in two dimensional space. A face defines a surface in three-dimensional space with four or more faces being used to define a three-dimensional cell. All of the volumetric cells combined are what is
called a volume mesh.
In a numerical simulation, a volume mesh represents the mathematical description of the space or geometry of the problem being solved. In this study using CFD, the volume mesh represents the entire simulated flow field inside the experimental continuum previously described in Chapter 2. By solving the RANS equations using CFD, flow properties existent at each discrete volumetric cell such as the velocity, pressure, turbulence, etc. will attempt to simulate the experimentally measured values individually and as a whole. As the mesh is refined to better represent more discrete cells in the flow domain, the ability of CFD to simulate and predict the real life conditions improves. However, the trade off of a larger
amount of cells to compute is often undesirable due to a lack of computational resources.
The meshing process in STAR-CCM+ involves creating a mesh continua for the continuum that one is attempting to model, selecting correct meshing models, making any changes to mesh sizing parameters and/or attributes globally and/or locally, setting volumetric controls, and running the surface and volume mesh generators. Checking the quality of the mesh by inspection and diagnostic tools usually follows as well as some iterations to get the correct sizing parameters for the specific simulation.

4.1 Geometry Import and Tessellation

After being provided with the appropriate computer aided drafting (CAD) model of the butterfly valve used in the experiment, as seen in Fig. 1.2, the CAD model was imported into STAR-CCM+ and re-tessellated with a very fine level of surface refinement as seen in Fig. 4.2. Tessellation is the process in which the surfaces of three-dimensional models are represented using triangles. A coarse tessellation level for complex geometries will typically produce a poor representation of the curved and intricate features of any CAD model. A finer level of tessellation will typically preserve the desired surface curvatures and features of a CAD model with a trade off of requiring more triangles to represent it.
After tessellation, CAD model components were assigned as parts. Two cylindrical parts, representing the piping upstream and downstream in the experiment, were added to each end of the valve. The seated downstream position for the butterfly valve was used to match the experiment. Each cylinder has an inner diameter of 47.25 inches to match the nominal inner diameter of the steel pipe used in the experiment. One cylinder extends approximately two and a half times the inner diameter (2.5D) upstream from the valve.

This significantly shortened upstream entry length, prior to reaching the valve, is justified by using a periodic flow simulation to determine the appropriate fully developed flow conditions that should be existent at the inlet face before approaching the butterfly valve in the pipe line. Upon convergence and correct matching of volume flow rates between the periodic simulations and the measured experiments of Table 2.1, the necessary values for the inlet boundary conditions of this study, such as the velocity, turbulent kinetic energy, and turbulent dissipation rate, were extracted from the periodic simulations and mapped onto the inlet for the 2.5D long upstream cylinder. Additional information regarding the
periodic simulation technique used in this study can be found in Appendix B.
Another cylinder extends approximately 6.5D downstream from the valve. The downstream domain extends an additional 5.5D approximately by using a meshing extrusion technique which will be discussed later on. This brings the total length of the downstream domain from the valve to nearly 12D. This length downstream from the valve was chosen to ensure that the assumed boundary conditions of a fully developed flow outlet were as valid as possible as will be later discussed.
Next, each cylinder’s combined surfaces were split into three surfaces: side, top, and bottom, where the side represents the interior walls of the pipe, and the top or the bottom could be the mating surface connecting into the butterfly valve geometry or the inlet or outlet. In order to have a flow domain from an inlet connect into the upstream cylinder to the valve and then to the downstream cylinder leaving to an outlet, a top or bottom surface was removed with its opposite side connecting into the valve for each cylinder. Figure 4.3 shows an example of an upstream cylinder connecting into a butterfly valve in the seated downstream position. The face connecting to the valve has been removed, and the dark colored face on the left represents the inlet boundary for the domain. The downstream cylinder was manipulated in similar fashion. After all of the aforementioned parts were defined and created, they were assigned to a region continuum.

4.2 Boundary Conditions

In three dimensions, boundaries are surfaces that completely surround and define a region. Each boundary has its own properties and can be given custom configurations such as meshing surface size, or how it should behave relative to other surfaces. The main boundary types chosen were the following: wall, internal interface, velocity inlet, and flow outlet. These boundaries and their corresponding chosen surfaces for this study, will now be discussed.

4.2.1 Wall

A wall boundary represents an impermeable surface. For simulations with viscous flow such as this one, it also represents a no-slip boundary. All of the following surfaces were chosen as wall boundaries except: the upstream inlet face, the downstream outlet face, and the interface connecting the downstream cylinder to the extruded cylinder portion as seen in Fig. 4.4. All valve faces were assumed to be smooth by inspection at the time of the experiment, and therefore required no modifications to surface roughness. All other walls, constituting the interior walls of the upstream cylinder and all connected downstream
cylinders were modified with a rough wall surface specification and roughness height of 0.0024 inches to match the steel pipe conditions of the experiment. All other wall roughness parameters were left as default.

4.2.2 Internal Interface

The internal interface joins two regions within the same continuum and can be used to combine together separate regions from the same continuum for in-place or periodic interfaces. When the extrusion process takes place, an internal interface boundary is automatically created between the outlet of the original 6.5D downstream cylinder and the inlet of the newly extruded 5.5D cylinder portion. This internal interface will cause the two sections to behave as one continuous flow region with no interruption in the fluid flow.

4.2.3 Velocity Inlet

A velocity inlet boundary represents the inlet of a duct at which the flow velocity is known. The upstream cylinder inlet face was selected as such. For the velocity inlet boundary, the velocity must be specified by the user, as well as the turbulent dissipation rate and the turbulent kinetic energy when using the k- turbulence model, which was the case in this study. These values were extracted from the periodic flow simulations previously discussed and were mapped onto this boundary using their corresponding coordinates.

4.2.4 Flow Split Outlet

The flow split outlet boundary represents the outlet of a duct and can allow flow split fractions in which the user can specify the percentage of flow leaving multiple ducts.
In this study, that value is set to unity for the downstream outlet face of the extruded cylinder. Additionally, flow properties such as velocity, turbulence qualities, etc. are forced to have zero gradients normal to the outflow face. In order to properly apply this boundary condition, the pipe length downstream from the installed butterfly valve must be long enough that the flow has become fully developed so as not to prematurely force the flow to a zero gradient condition.

For instance, most flow manufacturers recommend installing their flow meters 10D to 20D downstream of any valve because swirling turbulent eddies generated by valves largely disappear and the velocity flow profile returns to fully developed [20]. Huang [8] compared how flow profiles changed for CFD simulation by forcing the zero gradient condition on the outlet for a butterfly valve simulation for different exit lengths. It was observed that in changing the exit length of the pipe downstream from 8D to 9D, a 2% difference was recorded. For this study, no significant differences were observed between simulation cases run initially with 15D exit lengths compared to 12D exit lengths. Consequently, a length of approximately 12D was used in order to simplify the flow model and computational requirements.

4.3 Meshing Models and Options

Once the region continuum and boundaries are setup correctly, the meshing models can be set. The main meshing models selected were the following: polyhedral mesher, extruder, prism layer mesher, surface wrapper, and the surface remesher. An explanation of each meshing model as well as selected parameters and options for this study will be described.
Further explanations can be found in Appendix C and also in the STAR-CCM+ user’s manual [24].

4.3.1 Polyhedral Mesher

The polyhedral mesher is a core volume mesh model that dictates the main aspects of the entire mesh to be constructed. Polyhedral cells created typically have an average of 14 cell faces and provide a balanced solution. A large advantage that the polyhedral meshing model has compared to tetrahedral meshes is that they are relatively easy and efficient to generate, and contain approximately five times fewer cells than a tetrahedral mesh, thus alleviating computational burdens. Figure 4.5 shows an example of what polyhedral cells look like in a typical volume mesh. The run optimizer option for the polyhedral mesher was also enabled.

4.3.2 Extruder

As previously mentioned, an extruded portion of the downstream cylinder extending approximately 5.5D beyond the original downstream cylinder was to be constructed during the meshing process as illustrated in Fig. 4.4. The extruder mesher model allows a boundary located in a region continuum to be extended beyond its originally constructed bounds. This is particularly useful since the extended domain can be produced as orthogonal extruded cells which are ideal in steady flows such as internal flow in a pipe. By creating orthogonal extruded cells in a significant portion of the domain, the computational expenses are much less in comparison to using a polyhedral mesher to construct the same region. The frozen boundaries and check validity options were also selected to prevent the extruded boundary from shifting and to error check problems with the extrusion. Before meshing, the extrusion parameters at the boundary of extrusion must be chosen. The following parameters were selected: average normal extrusion, 80 layers of extrusion, stretching extrusion magnitude of six, and a magnitude of 260 inches (≈ 5.5D), with a new region being created for the extrusion as part of the continuum.

4.3.3 Prism Layer Mesher

The prism layer mesher model is used to generate orthogonal prismatic cells next to wall boundaries. This layer of cells helps resolve the boundary layer and improve the accuracy of the flow solution. By default, they are created only on wall boundary types. The default options that were selected for the prism layer mesher include: geometric progression for the stretching function, stretch factor for the stretching mode, a gap fill percentage of 25%, a minimum thickness percentage of 10%, a layer reduction percentage of 50%, a boundary march angle of 50 degrees, a concave angle limit of zero, a convex angle limit of 360 degrees, a near core layer aspect ratio of 1, and the improve subsurface quality option selected.

4.3.4 Surface Wrapper

The surface wrapper is typically used to provide a closed, manifold, non-intersecting surface and is used for imported surfaces that include the following: multiple intersecting parts, missing data in the form of holes and gaps, surface mismatches, double and internal surfaces, and overly complex geometry with too much detail. The curvature and proximity refinement options were also selected. The resulting surface quality from the surface wrapper is not optimal so it is commonly used with the surface remesher to provide a high quality starting surface for the core volume mesher. Because the CAD geometry of the butterfly valve involves multiple parts with narrow gaps, such as between the valve and the disc, the
surface wrapper was chosen to help alleviate meshing issues.
Figures 4.6 and 4.7 show the undesirable intersection that can occur between the butterfly valve main body and the disk after meshing. Figure 4.7 shows a close up view of the intersection. Such intersections in narrow gaps misrepresent the valve’s geometry. In particular, this misrepresentation could cause a higher predicted pressure drop and affect the flow simulation results. Figures 4.8 and 4.9 demonstrate a proper application of using the surface wrapper with no unintended intersections. Setting the surface wrapper involves first adding a contact prevention set under the fluid continuum’s mesh values node. Once a contact prevention set is added, two sets of boundaries for which to prevent intersection
must be set, including a search floor. For the first set of boundaries, the following regions were selected: epoxy, main body, ring body seat. The second set of boundaries including the following regions: main disc body, ring retainer, and rubber seal, shaft top, and shaft bottom. The search floor was set to 0.001m.

4.3.5 Surface Remesher

The surface remesher model is used to retriangulate surfaces as needed to improve the overall quality of an existing surface and optimize it for the volume mesh models. It is also typically used for remeshing surfaces that are produced by the surface wrapper model, which is the case in this study. The following options were selected for the surface remesher model: curvature, proximity, and compatibility refinement, retain geometric features, create aligned meshes, minimum face quality of 0.1, and enable automatic surface repair.

4.3.6 Reference Values

Once the meshing models have been selected with their given parameters and options, reference values based off those models need to be set. Reference values apply to all meshing parameters on a global level and can be set to apply to all boundaries and surfaces in a region continuum. Custom values can also be selected for each boundary inside the continuum.
Furthermore, most reference values can be set as absolute quantities or as a percentage relative to the base size. The meshing reference values were set as seen in Table 4.1.
It should also be noted that the base size reference value was the same for all results presented in Chapter 6, and were only modified to investigate grid refinement at two coarser levels each carried out for the 10, 50, and 90 degree open cases which will be later discussed.
Once all the options and parameters were set for the core mesh, local refinement using volumetric controls was carried out.

4.4 Localized Refinement

In CFD simulations, it is common to enable localized refinement in areas that are of most interest, and/or require greater detail in order to appropriately resolve existent behavior. In STAR-CCM+, volumetric controls (VC) can be enabled to allow the user to make predefined volumes from generic and custom geometries to refine the mesh as desired within those volumes. Custom parameters were enabled inside each VC for the following: custom base size relative to the reference base size value in Table 4.1, number of prism layers, prism layer stretching, and prism layer absolute thickness. Three different VCs were
enabled and labeled as: coarse, fine, and disc, as seen in Figs. 4.10 and 4.11. The mesh accordingly becomes more refined as the butterfly valve is approached from either side of the general domain into the VC regions until reaching its finest VC closest to the disc. This will ensure that computational burdens are not excessive due to refining unnecessary parts of the whole mesh, and that meshing resources are placed in the area of interest and likely instability. Table 4.2 shows the custom values used for each VC. Regions not within a VC maintain the same parameters and options as found in Table 4.1.
The coarse volumetric control extends 1.75 m in both directions away from the butterfly valve as a large cylinder that encompasses the flow domain within its length. The fine volumetric control extends 0.85 m in both directions away from the butterfly valve as a large cylinder that encompasses the flow domain within its length. The disc control volume is modeled as a thick disk that encompasses the dynamic disc components of the butterfly valve. This disc volumetric control has a radius of 0.75 m with a total thickness of 0.5 m centered along the butterfly valve shaft and perpendicular to the axis of flow. While the
coarse and fine volumetric controls remain stationary, the disc volumetric control has the same alignment as the valve degree opening. Sizes of the volumetric controls in Figs. 4.10 and 4.11 have been embellished to distinguish the overlap between each volumetric control.
After meshing, the difference between the volumetric control regions is easily identified, due to the progression of refinement of the mesh as the butterfly valve is approached as seen in Figs. 4.12 and 4.13.

4.5 Grid Refinement

A vital part of using numerical methods such as CFD, is estimating the contribution of discretization errors. In order to investigate this, it is necessary to carry out grid refinement and/or coarsening of the discretized domain one is trying to solve in order to see the behavior of the solution as more or less resolution is provided by the corresponding mesh. For this study, three different disk angle opening cases were coarsened to estimate the discretization error. The three different disk angle openings investigated were the following: 10, 50, and 90 degrees open.
The recommended method for discretization error estimation is the GCI method [25], which is based on the Richardson extrapolation (RE) method.

Results

All of the CFD simulations discussed were carried out using the criteria previously mentioned in Chapters 4 and 5. The flow fields generated by the simulations were studied, including visualizations of flow field streamlines, velocity vectors, and pressure fields.
These visualizations are shown in Figs. 6.1 – 6.29 and will be discussed accordingly. Additional figures are provided in Appendix E. The performance factors were also calculated and tabulated for comparison with the experimental results as shown in Tables 6.1 – 6.5.
Additionally, Figs. 6.30 – 6.34 show plots of these results, including the relative difference of the simulation results from the experiment (Erel). An outline of these results will be discussed in this chapter, followed by the results of the grid refinement study for the 10, 50, and 90 degree open cases.

6.1 Visualization of the Results

A common characteristic of the simulated flow in all of the valve degree openings is the development and eventual dissipation of a pair of swirling vortices that form after passing around the butterfly valve as seen in Fig. 6.1 and 6.2. The absolute pressure and velocity scalar bars represent the disk surface and streamlines, respectively. The top streamline view in Fig. 6.1 shows some steady streamlines along the larger opening between the valve disk and the pipe wall. Streamlines along the butterfly valve disk separate from the valve disk and cause a large amount of turbulent and swirling behavior. Henderson et al. [16] also noted this behavior and the presence of a strong pair of vortices behind butterfly valves as
seen in Fig. 6.2.
Visualization of the flow field for the absolute pressure and the velocity vectors is presented along two planes intersecting the flow domain: one perpendicular to the angle of rotation, and another parallel to the angle of rotation for the butterfly valve, referred henceforth as the top and side views, respectively. These visualizations can be seen in Figs. 6.3 – 6.29. Detailed views of the region surrounding the valve are also given in the mentioned figures, in order to allow greater clarity regarding the characteristics of the flow.

For the 10 degree open cases, high pressure is observed in the small gap between the valve disk and the pipe wall as shown in Fig. 6.3. A large pressure drop across the valve is also observed. The velocity vectors in Fig. 6.4 show swirling and rotational flow behind the valve disk, with large eddies present. The velocity vectors for the side view in Fig. 6.5 show a pair of eddy regions symmetrically across from one another.
For the 20 degree open case, distinct areas of high pressure are seen on the larger gap opening between the butterfly valve disk and the pipe wall as seen in Fig. 6.6. A much smaller pressure drop across the valve is present in comparison to the 10 degree case. The velocity flow field is similar to that of the 10 degree case with exception to a more concentrated eddy region directly behind the valve disk as seen in Fig. 6.7.

The 30 degree open case shows a more gradual drop in pressure from the top view of Fig. 6.8 in the larger gap region between the valve disk and the pipe wall. Figure 6.9 shows more flow moving along the pipe wall after passing the butterfly valve instead of recirculating into the strong eddy region behind the butterfly valve. The eddy regions from the side view in Fig. 6.10 appear to have moved closer towards each other near the centerline of the pipe.
In the 40 degree open case, the region of highest pressure distinctly appears at the point where the upstream flow first makes contact with the valve disk’s rotating edge as seen in Fig. 6.11. In the earlier cases considered, this distinction was not observed, as the main flow maintained a higher region of pressure prior to passing through the gap between the disk and pipe wall. The concentrated eddy behind the disk from the top view appears to have moved closer to the valve axis of rotation than earlier cases as seen in Fig. 6.12. The flow passing through the gap between the disk and pipe wall also seems to be less inclined to participate in the rotating flow behind the disk. From the side view in Fig. 6.13, an interesting elliptically shaped eddy recirculation region is formed approximately one diameter length downstream.

The 50 degree open cases also exhibits the same behavior as the 40 degree case for the distinct region of high pressure at the disk’s rotated edge as seen in Fig. 6.14. In Fig. 6.15, the amount of recirculation and swirling behind the valve has decreased due to a larger area available in the relatively smaller gap between the disk and the pipe wall. This ultimately allows the flow to separate less as it comes around the valve. The elliptically shaped eddy observed in the 40 degree case has increased in magnitude of velocity as observed in Fig. 6.16.
For the 60 degree open case, the high pressure region at the rotated edge of the disk becomes less distinct. Figure 6.17 shows a more gradual pressure drop as the flow moves past the valve disk. Figure 6.18 shows the circulation region behind the valve moving even closer to the cavity portion of the disk since more flow is able to stay attached longer down the disk edge. While this occurs, the side view in Fig. 6.19 shows an even more increased amount of circulating flow in the eddy region previously described.

The 70 degree open case, shows a similar pattern in the decrease of the high pressure region at the rotated edge of the disc in Fig. 6.20. The side view in Fig. 6.21, shows high regions of pressure in the pockets on the convex side of the butterfly valve disk as the flow becomes more perpendicular to the valve opening angle. The recirculation from the top view in Fig. 6.22 has become practically contained inside the concave side and feature of the butterfly valve disk. In Fig. 6.23, highly concentrated velocity vectors can be seen approximately one diameter downstream from the valve with less recirculation present.
The 80 degree open case shows agreement with the pattern seen in the top view of the 70 degree open case. For the side view, the regions of high pressure are present in the first set of pockets on the convex side of the butterfly valve disk as seen in Fig. 6.24. Two recirculating areas opposite from one another in Fig. 6.25 appear to have formed near the pipe walls and disk, downstream from the valve. These eddy regions appear to dissipate quickly downstream due to the highly dominant flow in the direction downstream from the valve.

In the 90 degree open case, the pressure gradients are quite gradual with a small amount of pressure distinctness at the leading edge of the disk in Fig. 6.26. The high pressure values in the pockets, appear to have lessened in the side of view of Fig. 6.27. Figure 6.28 shows a largely unobstructed flow and small amounts swirling due to the high opening valve angle in the flow. Like the 80 degree case, effects from the eddy regions in Fig. 6.29, appear to dissipate quickly downstream as the flow is dominated by a high velocity flow.