Master’s Thesis
Pressure Effects in Orifice Cavitation Modeling
Supervisor:
Eric Lillberg Examinator:
Krister Wiklund
Author:
Henrik Sjöholm
November 19, 2020
In this thesis computational models for cavitating flows around orifice plates has been studied and compared. The goal was to fit a model with experimental data and this was done with some success, although problems with numerical stability, long calculation times and geometry overfitting remain. Cavitation is a complex fluid phenomenon that can occur in pressurized liquid flows. It starts when the liquid pressure is lowered below the boiling pressure and water that undergoes cavitation forms vapor which later implodes violently. This process can cause problems such as noise, vibrations and corrosion in piping systems.
Loud noise is a nuisance, however powerful vibrations and corrosion can have serious consequences for the structural integrity of pipes. The for example less- ened performance, leakages or even failure. Therefore the minimization of cav- itation is often a goal in orifice and piping design. Vattenfall AB, together with Forsmark and Ringhals nuclear plants have studied cavitating flows around ori- fice plates used for flow limitation. A set of data from laboratory tests made by Vattenfall was used as the basis of analysis. Existing computational models in OpenFOAM were tested and evaluated based on their ability to model the experimental data accurately, as well as their computational performance and stability. The cavitation phenomenon was difficult to simulate using established methods so a new method was created and verified. It is based on the Kunz cavitation model together with Large Eddy Simulations, but with turbulence as a predictor of cavitation. The new computational model will serve as a tool for knowing how to design orifices in the future, so that laboratory experiments will not have to be conducted for each new piping design.
I detta examensarbete så har beräkningsmodeller för kavitation runt strypflän- sar studerats och jämförts. Målet var att matcha en modell med experimentella data och detta kunde åstadkommas relativt lyckat. Men problem med numerisk stabilitet, långa beräkningstider och geometriberoende finns kvar. Kavitation är ett komplext flödesfenomen som kan uppstå i trycksatta vätskeflöden. Det sker då vätsketrycket faller under koktrycket och vatten som genomgår kavitation bildar ånga som sedan imploderar våldsamt. Denna process kan skapa problem såsom ljud, vibrationer och korrosion i rörsystemet. Oljud är irriterande, men kraftiga vibrationer och korrosion kan ha allvarliga konsekvenser för rörsys- temets integritet. Till exempel förlorad verkningsgrad, läckage eller till och med att röret går sönder. Därför är det minimering av kavitation ofta målet i stryfläns- och rördesign. Vattenfall AB har tillsammans med Forsmarks och Ringhals kärnkraftverk, studerat kavitationsflöden runt strypflänsar som an- vänds för flödeskontroll. En samling experimentella resultat användes som grund för analysen. Redan existerande beräkningsmetoder i OpenFoam testades och utvärderades baserat på deras förmåga att matcha experimentella datat, samt deras beräkningshastighet och stabilitet. Kavitationsfenomenet var svårt att simulera med etablerade metoder så en ny metod togs fram och verifierades.
Den är baserad på Kunz kavitationsmodel med Large Eddy Simulations men använder turbulens för att prediktera kavitation. Beräkningsmodellen ska an- vändas som grund för framtida analys och design av strypflänslösningar så att man slipper utföra experiment för nya rördesigner.
I want to personally thank my supervisors Eric Lillberg and Nicolas Edh for their patience, skill and guidance. Both of them answered my questions with much knowledge and experience. This project would not have been possible without their help. I consider myself lucky that Vattenfall gave me this opportunity to learn. A big thank you also goes to my parents and my girlfriend who supported me along the way, and kept me motivated throughout the pandemic.
1 Introduction 1
2 Theory 3
2.1 Cavitation . . . 3
2.2 Cavitation in orifice flows . . . 4
2.3 Navier Stokes Equations . . . 6
2.4 Turbulence Modeling . . . 6
2.5 Rayleigh-Plesset Equation . . . 8
2.6 Approaches to Numerical Modeling . . . 9
2.6.1 Kunz Model . . . 10
2.6.2 Schnerr-Sauer Model . . . 11
2.7 Local Pressure Effects. . . 11
3 Method 13 3.1 Experiments at Älvkarleby. . . 13
3.2 Software & Modeling . . . 16
3.3 Geometry & Boundary Conditions . . . 16
3.4 Solvers . . . 17
3.4.1 Compressible - cavitatingFoam . . . 17
3.4.2 In-compressible - interPhaseChangeFoam . . . 17
3.4.3 In-compressible - modifiedPressureSolver . . . 18
4 Results 19 4.1 Compressible Solver . . . 19
4.2 Unmodified In-compressible Solver . . . 19
4.3 Modified In-compressible Solver . . . 24
5 Discussion 26 5.1 Compressible Solver . . . 26
5.2 In-compressible Solvers . . . 27
5.3 The Modified In-compressible Solver . . . 28
6 Conclusions 30
7 References 31
Appendix 35
iv
Introduction
Cavitation is a widely studied phenomenon in fluid mechanics. It is the creation of vapor bubbles in a fluid due to large local pressure fluctuations and it occurs in various engineering and industrial applications [1]. It occurs at low pressure points in the flow, and water that undergoes the cavitation process boils, despite its relatively low temperature. It is the local (in both space and time) change in pressure that causes the boiling. The creation and subsequent destruction of cavitation bubbles is a violent process and it can happen on short timescales [2, 3]. It can also cause significant problems such as noise [4], vibrations [5] and corrosion [6, 7, 8]. The tear of cavitation corrosion is due to microscopic jet streams that are formed when cavitation bubbles collapse near the surface [9].
In various pipe systems, there are throttles for flow limitation that cause drops in pressure. These come in various types, the simplest one is a plate with a circular hole in it, while other more complex have many plates, many holes or a combination of the two [10]. Figure 1.1 shows a schematic of how the pressure changes when a flow passes an orifice, at the orifice, and after it there is risk of cavitation.
Figure 1.1– Schematic of the pressure and risk of cavitation in a pipe with a single orifice plate. The red region is the high pressure region and the blue region has lower pressure. The white dotted lines indicate where cavitation bubbles might form.
Vattenfall AB has studied orifice cavitation, making tests and developing pre- ventive mechanisms [11] together with Forsmark and Ringhals nuclear power plants. There has also been attempts at implementing Computational Fluid Dy- namic (CFD) models using various techniques [12]. Vattenfall AB wants to find a method that minimizes cavitation in orifice flows. The development of a func- tioning, efficient and accurate computational model would greatly help in this
1
effort. Experiments on cavitation onset and different preventive mechanisms such as other piping geometry have been made [11]. This includes having many orifices in a row instead of just one and orifices with many holes instead of just one. This year (2020) Ringhals switched their orifice design after experimental tests but the interest in a computational model remains. This thesis deals with the computational modeling of cavitation in a pressure orifice. A set of data from a laboratory test has been made available as well the earlier CFD work.
The project has the aim of studying and testing existing solvers, and if necessary the development of a new solver. The computational model should fit the exper- imental data and ideally it should be both resource efficient and accurate. When finished the solvers that have been studied should be able to be used in studies for orifice design, so that the need for laboratory test is reduced. This would save money and time. In figure 1.2 a photograph of single-orifice cavitation is shown. It was taken using a high speed camera and the white cloud are small vapor bubbles.
Figure 1.2 – Photograph showing the amount of cavitation that can form in an orifice flow. The local pressure is low enough for the water to turn into water vapor, seen as the white cloud on the black background.
Existing cavitation simulations are varied in their use; for example injection noz- zles in engines [13], ship propellers [7] and medicine [14]. They use a great variety of software and numerical techniques [15]. The orifice cavitation prob- lem is complex and there exists no definitive solution method [16]. Many factors play into this; experimental cavitation is hard to quantify and directly measure.
On the computational side it is difficult to model unsteady flows where acoustic effects interplay with the phase model [4]. It requires a very fine mesh, and due to the scale of the geometry as many as 1 to 10 million cells are needed. One also has to use very small time steps, from 50µs to 500ns. To mitigate this a computational cluster with 320 cores was used. This project is centered around OpenFOAM (Open-source Field Operation and Manipulation) which is a C++
based application and numerical solver [17].
Theory
2.1 Cavitation
Cavitation is the phenomenon were a liquid evaporates due to low pressure, despite having a low temperature. What differentiates the cavitation process from boiling is the change in pressure causing the phase change, instead of a change in temperature [18]. The process can occur in a flow on an edge where there is a sudden pressure drop, or in a free flow. In its simplest form the liquid changes into gas when its local static pressure ps is lower than the vaporization pressure Pvap. The process is not instantaneous due to the internal forces of the fluid, such as its viscosity and tensile strength [19]. The bubbles formed in a liquid are called cavities and they implode if the pressure rises above Pvap. The length scale of the cavitation is important. Macroscopic cavitation bubbles are known to form around foils such as ship propellers [7, 8] as seen in figure 2.1. This is called sheet cavitation [20]. Another type of cavitation is cloud cavitation. It is characterized by small spherical cavitation bubbles that form a haze or cloud, hence the name [21]. An example of cloud cavitation can be seen in figure 1.2 where no large bubble structures are seen, but there are still vapor bubbles.
Figure 2.1 – Cavitation bubbles forming in the low pressure regions of a boat propeller. The cavitation bubbles are ring-like structures that remain for a while after the propeller blade. Image borrowed from TU Delft [22].
3
Cavitation can cause problems in industrial and engineering applications. The process of vapor cavitation is violent and the creation and dissipation of small bubbles generate a lot of noise [4]. Cavitation bubbles that collapse onto a boundary surface can be corrosive. This is due to the microscopic jet streams of liquid water hitting the surface [9]. For cavitation bubbles to grow there has to already exist gas nuclei in the liquid. In an ideal fluid with no impurities a liquid would remain a liquid despite low pressure due to the tension between the molecules [23]. This does not happen in reality since there are impurities and boundary effects. Cavities made of water vapor is called vapor cavitation and those made of mainly non-condensable gases (for example air) are called gaseous cavitation. There is no defined boundary between the two types, although due to the prevalence of solved gases in most water, cavitation near atmospheric pressure is gas cavitation [24]. For highly purified water the cavitation pro- cess is more violent. This is due to the dampening effects from expanding and contracting gas absorbing the pressure fluctuations. Gaseous cavitation is less corrosive than vapor cavitation due to the fact that non-condensable cavities that collapse, produce less jet streams since they collapse slower [25]. The process of adding extra non-condensable gases is sometimes used to make the cavitation less violent [26], although this process is not an alternative at Vattenfall.
2.2 Cavitation in orifice flows
Cavitation in orifice flows has been studied for a long time due to its importance in industrial applications [27, 28]. In recent years computational models have been developed in order to predict the phenomenon. The models are narrow in scope and there are flaws in accuracy. Many models often come at a high computational cost. For a single orifice flows there are a few empirically known relationships between the ratio of up- and downstream pressure, orifice to pipe diameter ratio and when one can expect cavitation onset. The ratio between the width of the pipe and the width of the single hole orifice is defined β = d/D and figure 2.2 shows the conceptual setup for studying orifice flows. The flow rate Q(l/s) is constant such that a velocity U is reached.
Figure 2.2 – Schematic of a typical single orifice pipe system. Water flows with an initial velocity U into the orifice were it speeds up to its top velocity Ujet. The lower graph shows the ambient pressure in the center of the pipe. It falls to a lowest value Pmin a short distance after the orifice.
The difference in upstream and downstream pressure is defined ∆P = P2−P1
with pressure loss coefficient
ξ(β) = ∆P
0.5ρU2, (2.1)
describes the pressure loss depending on flow velocity U. The cavitation number σ = pmin−psat
∆P , (2.2)
describes how close the flow is to cavitation onset [29]. The onset or initialization of cavitation is described by
σi =1.55+4.88CD +5.66CD2 +1.95C3D, (2.3) such that σi =1.55+4.88CD+5.66C2D+1.95C3D < 1 indicates onset and where CD = (ξ −1)−12 [30]. In applications there are a variety of methods used for the control of cavitation. This equation is used in orifice design when Q or P2 cannot be modified, allowing one to pick a orifice with correct diameter. Other methods for minimizing cavitation are for example using a multi-hole orifice or many orifices in series [31] or forcing air into the fluid [32].
2.3 Navier Stokes Equations
Fluid mechanics and computational fluid mechanics is centered around the un- derstanding of Navier-Stokes equations. They govern how a fluid element moves through a flow and how forces act upon it. The equations are
ρ DUj
Dt =µ ∂
2Uj
∂xi∂xi
− ∂P
∂xj
−ρ∂Ψ
∂xj
, (2.4)
where the element moves with velocity U, density ρ and viscosity µ. Ψ is the effect from gravity and xi, xj are the Cartesian coordinates. The pressure P is rewritten to the hydro-static pressure pstat where the gravity is discounted using gravitational potential ρgh:
pstat =P+ρΨ, (2.5)
which simplifies2.4 to
DU
Dt = −1
ρ∇pstat+v∇2U, (2.6)
where v=µ/ρ is the kinematic viscosity [33]. The continuity equation
∂ρ
∂t + ∇ · (ρU) =0, (2.7) describes mass conservation for infinitesimal volume elements. For incompress- ible flows this simplifies to
∇ ·U=0, (2.8)
since ρ is constant in space and time [34]. In this thesis the Finite Volume Method was used, with either compressible or incompressible flow. Compressible flow can model sound propagation where incompressible cannot. However it is more computationally expensive.
Using a Direct Numerical Simulation (DNS) one can solve the Navier-Stokes equations numerically. In a DNS all the force equations on each fluid element is calculated and there is no need for a turbulence model. DNS simulations approximate the flow accurately if the mesh is fine enough but they are incredi- bly computationally expensive. Therefore DNS is not usually used in industrial applications. Turbulence models are instead used to simplify numerical approx- imations of the Navier-Stokes equation [35].
2.4 Turbulence Modeling
Turbulence and eddies are important concepts that both elude simple defini- tions. Turbulent flow is by nature chaotic in regards to velocity and pressure.
It is composed by eddies that are parcels (or small volumes) of the fluid that
generally move in a coherent manner. Within a turbulent flow the eddies exist on different length scales l. The largest are the size of the entire flow, and the smallest are smaller than what the human eye can observe [36]. Reynolds Aver- age Navier Stokes (RANS) and Large Eddy Simulations (LES) are two commonly used methods for solving Navier-Stokes equation numerically [35]. They model turbulence in different ways. RANS takes a time average of each term in the Navier-Stokes equation and uses Reynolds decomposition that separates each physical quantityΦtotinto a average and fluctuation termΦtot =Φ+Φ0. It does this for all scales of the flow [37]. The largest flow scales are of the size of the geometry, and down to the dissipation range which will be explained later. LES on the other hand model all physics below a certain scale and directly solves Navier-Stokes equations for the larger scales [38]. The concept is seen in figure 2.3where κ =1/l is the length scale of each separate flow.
Figure 2.3 – The Turbulence Scale shows the energy E(κ)of eddies in turbulent flow for different length scales κ.
In turbulent flows many physical processes and forces take place on different size scales at once. Meaning that a large body of liquid within the flow can ex- hibit a certain flow behavior, but within that larger flow there can be other move- ments also occurring. The flow is therefore separated into three scale ranges.
The energy range is the largest scale, macroscopic flow directly computed by LES. The dissipation range is the small and in the Kolmogorov scale energy k is converted into heat, called dissipation. The Kolmogorov scales are
η =v
3
e
1/4
, (2.9)
τη =v e
1/2
, (2.10)
uη = (ve)1/4, (2.11)
for length, time and velocity respectively. e is the average dissipation rate of energy per mass, ν is the viscosity. The Kolmogorov scales vary within a flow due to local changes but when modeling it is set as constant [39]. The changes occur in the Reynolds number (Re)
Re = uL
ν , (2.12)
which is a measurement of the ration between internal and viscous forces. It can be used to predict whether flow will be turbulent or laminar. High Reyonolds Numbers is correlated with turbulence and low indicates laminar flow.
The energy of each eddy always dissipates towards the Kolmogorov scale in a phenomenon called the energy cascade. This is due to the inherent instability of larger eddies [40]. As seen in figure2.3, LES computes the energy spectrum down to somewhere before the dissipation range. A fine mesh will include more of the inertial subrange. Making the magnitude of k bound to the mesh size [41].
The RANS method models the entire spectrum, and uses time averaging, there- fore in simulations, its k-value tend to be more diffused. The k−emodel can be used to close the time averaged Navier Stokes equations in RANS. This model calculates production and dissipation (e) of the turbulent kinetic energy k and assumes that the turbulence fluctuations are locally isotropic. It is the simplest turbulence model where only initial and boundary conditions are needed. The model is well tested and it is known that k−e overestimates the spread of the turbulence, and that it cannot model flows with large pressure gradients accu- rately [35].
2.5 Rayleigh-Plesset Equation
The Rayleigh-Plesset Equation is directly derived from Navier-Stokes equation [42] and it describes how the radius R of a gas bubble changes over time. It has assumptions that apply locally for each bubble; constant temperature T over the
bubble, constant fluid density ρl (liquid) and ρv (vapor) and constant dynamic viscosity µland µv. The temperature and pressure inside and around the bubble is homogeneous. The equation states
Rd2R dt2 +3
2
dR dt
2
+4ν R
dR dt + 2γ
ρlR+ ∆P(t) ρl
=0, (2.13)
where γ is the surface tension of the interface between the two phases. ∆P(t) is the difference in pressure inside and outside of the bubble [43].
2.6 Approaches to Numerical Modeling
Cavitation modeling is based on the continuity equation equation (2.7) and has two or more phases. Cavitation models are put on top of ordinary multi-phase solvers of the Navier-Stokes equations. They have an extra term that translates one phase to another, given some condition. This condition is connected to the pressure or temperature of a phase. In this thesis the growth of the gaseous phase is determined by a interpretation of the Rayleigh-Plesset equation (2.13).
One category of solvers are the Volume of Fluid (VOF) methods. They are Eu- lerian mass transfer models that calculates a ratio between two pre-described media within a cell. The ratio of liquid to gas in a two phase model is denoted as α = [0, 1]. Were 0 is the total absence of liquid, and 1 is total absence of gas.
In this report, liquid water and water vapor are used. For the vaporization and condensation process one is therefore interested in the rate of phase change, dαdt. This is often rewritten as dmdtα = m˙α to indicate how much mass flow there is between the two phases [44]. The physical meaning of the ratio α is of great importance. Each model have different assuptions of what any given value of α represents. For example if α = 0.1, this could represent many small bubbles with a combined volume of 10% gas or is it one large one. The model also have to account for the assumed shape of each bubble. These assumptions are re- lated to the surface area of the bubble, where one spherical gas bubble would minimize the surface area and many small ones would maximize it. This has implications for the diffusion rate of a bubble since the surface tension γ in the Rayleigh-Plesset equation is directly tied to that physical property [45].
A different branch of cavitation modeling describes each cavity as a La- grangian particle. These are called Lagrangian Particle Tracking methods (LPT).
Each cavitation bubble is simulated and has its own radius, velocity and mass and it flows through the liquid. This method is often used for cavitation corro- sion models due to its ability to see where cavitation bubbles reach a vulnerable surface. It is also used when simulating a bubble flowing to the surface. There has been attempts at uniting the two methods [46].
Figure2.4 shows a comparison between the two approaches as well as differ- ent approaches within the VOF methods. Each small box represents a mesh grid
cell, and the number inside represents the percentage of gas in that cell. The cells without a number does not have any gas. Figure 2.4a is a representation of sheet cavitation as seen in figure2.1, Many of the cells are either all liquid or all gas. In this case the surface tension model used will be important. Figure 2.4b is also a Volume of Fluid representation but the gas is diffused. In this case the surface area modeling will be essential [21] due to its importance in the Rayleigh-Plesset equation. Figure2.4cshows a Lagrangian representation of gas bubbles, all with exact values for their radii and velocities.
re
(a) (b) (c)
Figure 2.4 – Each black square represents a mesh cell, here simplified to 2D. (a) and (b) are Volume of Fluid and (c) is Lagrangian Particle Tracking. White colored boxes are just liquid water, while the ones with coloring are a percentage gas. The red line indicates conceptually were the bubble structure has its border in a cavity sheet.
2.6.1 Kunz Model
There are many VOF methods available today [44,47]. Merkle et al. developed a fundamental computational VOF model in 1998 and it was meant to model sheet cavitation [48], seen in figure 2.4a. In sheet cavitation modeling there are large bubble structures covering many cells. The Kunz model was developed from the Merkle method but allowed for dispersed liquids (ρl) and gases (ρv), as well as turbulence transport. The model is capable of assessing super cavitation and sheet cavitation with three phases (air, vapor and liquid water). The problems before Kunz were high density fluctuations in space and time, as well as inter- faces. These cannot be solved with a single phase model [49]. The Kunz model is one of the most widely used methods [44]. Its Eulerian transport equations describe the change of volume fraction α:
∂(αρl)
∂t + ∇ · (αρlU) + ∇ · [αU(1−α)] = Rc−Re, (2.14)
were Re represents the evaporation source term:
Re =Cν
ρνα
t∞(1/2ρl)U∞2 , (2.15) and Rc is the condensation source term:
Rc =Ccρνα2(1−α)
t∞ , (2.16)
where U∞ represents the steam velocity (inlet), t∞ the mean flow time scale is L/U∞. L is the nozzle length. Cv and Cc are empirical coefficients.
2.6.2 Schnerr-Sauer Model
The Schnerr-Sauer model [50] uses a two-phase VOF approach. It also assumes homogeneous nucleation and homogeneous temperature and pressure at a lo- cal level. The method uses the Rayleigh-Plasset equation 2.13 to calculate the growth and shrinking of cavitation bubbles. What differentiates the Schnerr- Sauer model from Kunz [49] its way of modeling sub-grid cavities. The small cavities form a cloud inside each cell and are assumed to all be of the same size, as a function of the volume fraction α. This method defines it as
α = n0
4 3πR3 1+n03
4πR3, (2.17)
were n0 is a preset homogeneous nuclei-density. The change in volume fraction is calculated using convection to
∂α
∂t +∂(αUx)
∂x +(∂αUy)
∂y = n0 1+n043πR3
d dt
4 3πR3
, (2.18)
using cartesian coordinates x and y. The Schnerr-Sauer model has been used successfully on hydrofoils, showing cloud cavitation behavior [50].
2.7 Local Pressure Effects
Cavitation onset at ps < pvap is an idealized view. In many cases the measured static pressure is much higher than the vaporization pressure, but there is still cavitation. There are many possible reasons for this discrepancy, such as the effect from the Reynolds number, solved gases as mentioned before, and the tensile strength of the liquid [51]. The temperature could be a factor but most models for cavitation onset in water are developed for temperatures lower 300◦C [52]. So that is not a factor in this study. Models using the enthalpy have also been suggested [53].
A connection to turbulence and shear layers has been suggested [51] and this thesis focused on this hypothesis in particular. A way to model a hypothetical connection to turbulence k would be to model it like sound pressure. The sound pressure prms is a component of the absolute pressure so that pabs = ps ±prms and it can be related to the turbulence
prms =0.58ρu02 =0.58· 2
3ρk=0.39ρk, (2.19)
since k = (u02+v02+w02) = 32u02 if isotropic turbulence is assumed [54]. The authors claim no certainty in the factor 0.58 and also use 0.70. This value would instead yield prms =0.47ρk. Rearranging the equations in terms of a new vapor pressure, or phase-change pressure padj one gets
padj = pvap+prms, (2.20)
thus making the pressure needed for cavitation highwe. Singhal et al. used this framework for modifying the vaporization pressure using the turbulent kinetic energy. In their model the phase change is expressed in terms of
padj = pvap+p0turb/2= pvap+Cρk/2, (2.21) with the coefficient C = 0.39 and with no further motivation of 1/2 [55]. Since the original coefficient 0.39 is derived from a normal distribution [54] however no further reasoning was given.
Method
3.1 Experiments at Älvkarleby
A test-rig was constructed at the Vattenfall owned laboratory at Älvkarleby. It had the capacity to control the inward water flow rate Q and downward pres- sure P2 (see figure 2.2) while trying out different pressure orifices. Its sensors measured the flow velocity U with±0.5% accuracy before and after the orifice.
The tap water used was 18◦ C ±0.1◦C and its density ρ = 998kg/m3 (±0.1%).
The setup included a Plexiglas section directly after the orifice for visualization of the flow [11]. Figure 3.1a shows the experimental setup. The water flow Q comes from the left side and travels past P1 through the Plexiglas section to P2. The pressure can be measured at both points and the flow rate before and af- ter the glass section. A type of single hole orifice can be seen in figure 3.1b.
Equation2.3was used for different values of ξ as described in equation 2.1
(a) (b)
Figure 3.1– Figure (a) shows the experimental setup. A Plexiglas section was put in the pipe in order to observe the cavitation. The arrow indicates the direction of flow and the orifice was located at P1. The flow rate Q and downward pressure P2were changed to modify the amount of cavitation for a given orifice. In (b) is a single-hole orifice used in the experiments can be seen.
The experimental results from Älvkarleby showed how the cavitation was formed, and how it was structured. The type of cavitation was cloud cavitation it started at the orifice ring. The bubbles then traveled down the Plexiglas section and disappeared. The cavitation was irregular (not following a geometric pattern) and spread throughout the Plexiglas region sideways. It also varied with time in
13
bursts. A typical burst can be seen in figure3.2. Cavitation onset was character- ized by sudden bursts of cavitation clouds of different size. They were formed in the vicinity of the orifice and disappeared before reaching the end of the glass.
When decreasing the downstream pressure P2 the cavitation became constant and it filled up the chamber more as the pressure was decreased further. This is shown in figures3.3a and 3.3b.
Figure 3.2– Cavitation burst seen at cavitation onset. The orifice is seen to left and the water is flowing into the Plexiglas section of the pipe to the right. The white mist around the center of the cylinder is the cavitation bubbles cloud.
(a) (b)
Figure 3.3– The cavitation cloud growing as the downstream pressure was de- creased between (a) and (b). In (a) the cavitation is stable and covers much of the chamber. In (b) the entire pipe is fill with bubbles and the process creates very loud noise and vibrations.
When performing a time-average using many photos a pattern emerges as seen in figure 3.4a. The cavitation bubbles were centered in a ring protruding from the orifice downstream. Figure3.4bshows how the bubbles originated from the orifice edge.
(a) (b)
Figure 3.4 – (a) shows the time average of constant cavitation (figure 3.2). The more white, the more bubbles. (b) shows cavitation at the orifice. The bubbles are formed on the inside of the orifice edge.
Figure 3.5– Photograph showing the scale of the cavitation a bit after onset. The photograph was taken using a high speed camera against a dark background. The white mist is made of cavitation bubbles.
3.2 Software & Modeling
OpenFOAM is a C++ based multi-physics software. This thesis used OpenFOAM- v1912 [56] for the simulations and the visualizations were made using ParaView (version X). A cluster was made available with up to 320 cores. Non-fixed time- steps were used with standard OpenFoam implementation around acoustic and non-acoustic Courant numbers cn [57]. It is a Finite Volume Method solver and the goal of all tested models was to replicate the behavior seen in the experi- ments. This included, the pressure profile, measured velocities, shape and be- havior of the cavities as well as when cavitation was formed.
3.3 Geometry & Boundary Conditions
Several geometries were modeled, all with static mesh. The single hole orifice was modeled as a pipe with diameter 102.3 mm and length is 1400 mm, with the orifice 400 mm after the inlet. The orifice had width 31 mm giving β = 0.0775.
Extra fine mesh was used around the orifice and downstream at least six inner diameter lengths, 186mm. There was also extra computational space added to avoid effects from the boundary conditions. The finer mesh around the orifice can be seen in figure 3.6. The mesh of the bulk and at the boundaries is in the appendix: figures 7.3, 7.2 and 7.1. For the turbulence model fine mesh at the boundaries was used, it was trimmed such that y+ < 30, which could be accomplished in almost all of the geometry. A total of 3.1 million cells was used, most of them hexahedras. Coarser meshes (down to around 100 000 cells) was used for initial tests. The size of the mesh was critical in the LES simulation as mentioned in section 2.4. In the finest mesh used, the smallest cells in the bulk had wall-to-wall distance of around 0.64mm, and the largest cells had wall-to- wall distance of around 4.5mm.
Figure 3.6– Fine mesh used in the single hole orifice.
A variety of boundary conditions were tested with the different solvers. The
turbulent kinetic energy at the inlet was set to X in the bulk and Y at the bound- ary. The inlet k value was Z. These are standard values in OpenFoam. In order to reach the fully developed flow, the inlet velocity was steadily increased and the simulation was left running until the pressure field, velocity and turbulent kinetic energy was stable before measurements were taken. The velocity profile was homogeneous at the inlet, The inlet and outlet pressure were set constant and back-flow was allowed.
Note from the author: Due to the sensitivity of the studied systems and the data that was collected, the exact experimental values have been removed.
3.4 Solvers
3.4.1 Compressible - cavitatingFoam
Compressible solvers can model the sound waves propagating through the sys- tem, which makes an audio-study and possible when using LES [58]. The used compressible solver is called cavitatingFoam [59]. It is a VOF solver and many mass transfer models can be used. Kunz or Schnerr-Sauer was used for all the simulations when testing cavitatingFoam. cavitatingFoam has the following equa- tions of state:
Dρm
Dt =ΨDP
Dt, (3.1)
and
γ = ρm−ρl,sat
ρν,sat−ρl,sat, (3.2)
directly derived from equation2.4, as well as mixture equilibrium
ρm = (1−γ)ρ0l + (γΨν+ (1−γ)Ψl)Psat+Ψm(P−Psat), (3.3) from equation2.7. The solver also has the continuity equation
∂ρ
∂t + ∇ · (ρU) =0, (3.4) and the momentum equation
∂ρU
∂t + ∇ · (ρUU) = −∇P+ ∇ ·µe f f(∇U+ (∇U)T), (3.5) where µe f f is the effective viscosity and ρm is the density of the mixture of the two phases.
3.4.2 In-compressible - interPhaseChangeFoam
In-compressible solvers are unable to resolve audio chock-waves propagating the fluid, as well as the density fluctuations at the surface in a cavitation model.
The incompressible that was used solver is called interPhaseChangeFoam [60] and it has the continuity equation:
∂ρm
∂t + ∇ · (ρmU) =0, (3.6) and the momentum equation:
∂ρmU
∂t + ∇ · (ρmUU) = −∇P+ ∇ ·µe f f(∇U+ (∇U)T)+ fσ, (3.7) where fσis the surface tension force and the transport equation for the solver is
∂(αρl)
∂t + ∇ · (αρlU) = −∇P+ ∇ · αUc(1−α)= Rc−Re, (3.8) where Uc is the so called artificial compression term. interPhaseChangeFoam is also a VOF solver where Kunz and Schnerr-Sauer can be used.
3.4.3 In-compressible - modifiedPressureSolver
A modified version of interPhaseChangeFoam was developed, the modifiedPres- sureSolver. The purpose was to take into account the effect on the local pressure by the turbulent kinetic energy k as described in section 2.2. It was modified according to equation (2.21) and the modified code is the appendix (7). The phase change-pressure was modified so that for high values of k, the threshold pressure for phase change was lowered locally. Values of k >250 were deemed nonphysical so those values were capped at 250 J/kg. The adjusted vaporization pressure was then applied to the Kunz solver. The coefficient C was tested for different values, starting with the ones described in [54] and [55]. In order to tune the C parameter the cavitation onset values of Q and P2 were used.
Results
4.1 Compressible Solver
Tests with cavitatingFoam were performed using both RANS and LES turbulence models. Figure4.1 shows how the pressure field became chaotic, with high cell- to-cell differences. The pressure fluctuations are spread throughout the entire geometry. The compressible solver modeled propagating waves at a 10−8s time scale. It was only numerically stable with those time steps. Cavitation did form but it was not centered around the orifice, rather spread where the mesh grid changed. Using the fine mesh it took 0.2 to 2.0s to calculate a single time step.
Figure 4.1 – Compressible pressure fluctuations spread out homogeneously throughout the geometry. The cloud seen inside the entire geometry is cavita- tion. It exhibits nonhpysical behavior.
4.2 Unmodified In-compressible Solver
interPhaseChangeFoam was able to take time steps ∆t ≈ 5·10−5s and remain stable. The upstream and downstream pressures concur with equation2.1using the different experimental values. The typical interPhaseChangeFoam behavior for Uis seen in figure 4.2 when using RANS. The gradients in U are small and the highest velocities are in the center of the pipe inside the orifice. In figure4.3the
19
behavior for k is seen. Its gradients are also small and the highest values are centered around the edges of the orifice. RANS did not form cavitation bubbles when testing using the equation for cavitation onset (equation2.3), nor with the values from the experiments that gave much cavitation.
Figure 4.2 – Velocity profile U using RANS and an incompressible solver. The blue regions have low flow velocity, whereas the red region has high velocity. The flow is travelling to the right. A fine mesh was used.
Figure 4.3 – Turbulent kinetic energy k using RANS. The red regions have high turbulence and the blue ones low turbulence. High turbulence was observed on the orifice edge. This was done using the fine mesh.
Using LES the velocity profile can be seen in figure 4.4. The velocity grows at the entrance of the orifice and forms a jet stream that collapses after a few orifice diameter lengths. The stream forms circular vortexes that dissipate. The kinetic turbulent energy k is centered around the shear layer of the flow as seen in figure 4.5. Its peak values are at the orifice entrance at the boundary. The pressure can
be seen in figure 4.6. The pressure is high before the orifice and low after it.
There are vortexes flowing downstream.
Figure 4.4– Velocity field U using LES and the fine mesh. A jet streams from the left to the right with high velocity, as the red indicates.
Figure 4.5 – Typical LES k field using fine grid and no-slip boundary condition.
The highest k-values are found on the edge of the geometry and around the jet, in its sheer layer.
Figure 4.6 – The pressure using LES and the fine mesh. The highest pressure is observed before the orifice. After the orifice the pressure becomes lower and the pattern of paired circles that are seen in this region are vertexes.
When testing the incipient cavitation values for Q and P2 from the experiments, only a little cavitation was formed when using the established cavitation models.
The cavitation was centered on the cells on the rim (figure 4.7) and did not spread downstream. Mesh analysis confirmed this by showing that with even extremely small cells on the rim, only the inner most layer had α < 1, meaning the presence of some gas. This held true for both RANS and LES turbulence models, as well as Kunz and Schnerr-Sauer cavitation models.
Figure 4.7– Cavitation seen (the circle at the orifice) when using LES and Kunz with the fine mesh.
For much lower downstream pressures tests showed cavitation in the bulk of the flow, away from the boundary. This was tested using the different turbu- lence models. When testing LES, cavitation eventually forms when the down- stream pressure is significantly lowered. In the experiments reality pressure this low makes the entire glass chamber full of bubbles. The bubbles observed us- ing interPhaseChangeFoam were not of the nature seen in the experiments. They
were large bubble rings, seen in figure 4.8. The bubble structures were cen- tered around vortexes moving downstream. Further analysis showed that they only formed when large pressure waves formed at the orifice edge, caused by the changing boundary conditions. The same behavior was observed for the Schnerr-Sauer model: large bubble structures in the shear layers of large vor- tices. The cloud structures described in figure2.4bwere not seen.
Figure 4.8– Cavitation using LES and Kunz at lower downstream pressure. The large structures are around the vortexes flowing downstream.
4.3 Modified In-compressible Solver
The new solver was implemented and its coefficient found for a single hole orifice. When testing RANS there was no cavitation for low values of C. When increased the onset was so powerful that much of the bulk became gas, and time steps became very small (≈10−8s). The solver was only numerically stable using LES when the coefficient took high values. In figure4.9 the final turbulent kinetic energy field. It was used as the test case when tuning C. When using LES time steps of ≈ 10−5s were possible. For certain coefficient values the cavities spread around the geometry in small clusters as seen in figure4.10.
Figure 4.9– Turbulent kinetic energy k (foreground) and pressure p (background) that was used when tuning the coefficient C.
Figure 4.10 – Cavitation using inception values for Q and P2 when using one coefficient value C.
Later verification of the determined coefficient was made with higher velocities from the experimental values. The tests showed that the pressure difference∆P followed equation 2.1. The tests showed resulted in more cavitation 4.11. This cavitation filled much but not all of the geometry.
Figure 4.11– Much cavitation forming when the flow rate is higher.
Tests using multi-hole orifices confirmed that the new model also predicted less cavitation when using it as seen in figure4.12. Using the same coefficient as seen in figures4.10 and 4.11barely gave any cavitation at all.
Figure 4.12– Small cavities can be seen on the multi-hole-orifice edge. The values for k are smaller when using a multi-hole orifice.
Discussion
The boundary conditions and initial conditions for k and e were set to standard OpenFOAM values. Tests using higher values were made but they proved to have little effect on the results due to how low they were compared to the values of k at the orifice. Using Slip condition or No-slip condition on the pipe bound- ary was also tested and it did not have any effect on the cavitation or the velocity profile of the flow. In figure 4.5 no-slip was used and this caused high values of k on the boundary. For faster computational speeds, the Slip-condition was used in most simulations. The velocity profile at the inlet did also not matter to the results due to all the liquid being forced into the orifice. There the original velocity profile disappeared at that point. Back-flow through the outlet had to be permitted otherwise numerical instability became a problem. This was due to when the cavitation bubbles collapsed there was always some back-flow due to the reduced volume in the system.
There were problems when studying the cavitation in the experiments. Be- yond the observation that the type of cavitation formed was cloud cavitation, it was difficult to draw further conclusions. For example the cavitation seen in figure 3.5 is small and spread out. But observations cannot tell the size of each cavitation bubble, or if they are made of solved gases. The numerical construct α cannot be tested or verified yet. The bulk pressure could be measured, as well as the flow rate, but the line between different amounts of cavitation remain subjective. Further tests measuring vibrations and a time average comparison as seen in figure3.4a between different cavitation numbers σ would have helped.
5.1 Compressible Solver
When testing cavitatingFoam the calculations were heavy and numerical stabil- ity was an issue, as well as checker-boarding. For that reason low (cn ≈ 0.01) Courant numbers were necessary. Time steps of around 10−7s were achieved but when using the fine mesh calculation times of around 0.2 – 2.0s were com- mon. This was when more than 100 cores were used. This results in calculation times of several days or weeks for usable results. The computational load was trimmed by removing extra mesh grid cells and by pre-calculating a fully de- veloped flow with an in-compressible solver. Despite the attempts made, once cavitation started the chock-waves of bubbles collapsing led to an cascade of nu- merical errors forcing the time-step further down to 10−9s. Physics taking place
26
on this time scale was not unexpected since audio recordings showed sounds at that frequency. A functioning compressible solver would have been useful for studying the frequency spectrum and the loudness of the system. The noise caused by cavitation is a studied phenomenon [4] and could be the key to un- derstanding the cavitation process better.
5.2 In-compressible Solvers
The existing in-compressible solver interPhaseChangeFoam proved more stable than the compressible solver. Tests using RANS and LES showed different be- havior as expected. If cavitation can be connected to the kinetic turbulent energy k LES is more promising than RANS. The behavior of k using RANS seen in fig- ure 4.3 does not look like the experimental behavior seen in figures 3.3a and 3.3b. Nor does it look like figure3.4a since the k-field is high in the center of the flow. However both turbulence models show good behavior for predicting ∆P as predicted by the equation2.1.
The behavior of k in LES models looks more like the cavitation clouds in the experiments. For example when comparing figure 4.5 to figure 3.2 the resem- blance is clear. A large part of the bulk has high values of k and they are spread irregularly. Both LES and RANS it did not produce sufficient cavitation as seen in figure 4.7. Once cavitation was formed (by artificially reducing the down- stream pressure) the behavior resembled macroscopic sheet cavitation seen in other contexts, for example propellers as seen in figure 2.1. The behavior can be seen in figure 4.8. This phenomenon can have many explanations, such as the numerical effects from changing pressure boundary conditions and the fact that the vapor inside each cavity is not in-compressible, making its structure more rigid. The behavior could also be come from the Kunz models’ inability to model the effects of turbulence and acoustic pressure on the vaporization pres- sure. Thus the simulations showed nonphysical behavior for a system where the turbulence is such a large factor.
There are other VOF methods not studied here for example the Zwart-Belamri model [61]. Zwart-Belamri counts in the effects from the turbulent viscosity µ, however it does not seem to have a LES implementation. Quick tests using it and RANS show that it produces about the same behavior at the inception cav- itation parameters that were tested using Kunz. There are also unified theories that tries to find a balance by combining existing methods [44]. Further study is needed for these models. The Schnerr-Sauer [50] was tested but surprisingly did not yield very different results from the Kunz model. It was supposed to have the ability to model cloud cavitation seen around propellers, and the cir- cumstances around an orifice could be similar with sharp edges and large shear stresses. The reasons for its inability to yield the same results remains unknown.
A possible hypothesis is that both cavitation models can model the creation of cavitation well, however not its transportation. A behavior seen in many simula-
tions is the creation of a ring of bubbles on the orifice but none in the bulk of the pipe. The models could be unable to properly move the cavitation bubbles or, their method of modeling the collapse of the bubbles is wrong. Thus destroying the cavities immediately after leaving the creation-zone at the boundary. The existence of solved gases, and them making up the rest of the seen cavitation could be the cause. However this is for the moment impossible to test with an experiment.
5.3 The Modified In-compressible Solver
The modified solver was somewhat flawed from the beginning. Quick calcula- tions around equation2.21 show that when using RANS the coefficient C has to be very large in order to force cavitation, given reasonable values for k in the bulk and the ambient pressure. Values of k>250 J/kg start to become non-physical, so even with LES (where k is large locally), large coefficients are needed. There was a recurring problem around the cavitation onset when trying out high C- values. The first creation of a cavity would cause an immediate pressure drop on the entire space, sometimes leading to a cascade. This is counter intuitive, since by making the vaporization pressure locally different, the affected region would experience more cavitation than in the standard Kunz model. These pro- cesses remain largely not understood. Despite the flaws of the new model, it did not act in a very non-physical manner. The behavior seen in figure4.10 shows bubbles in the bulk of the Plexiglas section using the onset parameters. However due to our inability to directly measure the amount of cavitation present in the system its spread throughout the pipe was the only way to approximate whether the coefficient was tuned or not. Cavitation increased when the inputs Q and P2
were changed according to the experiments, as seen in figure4.11and changes in geometry led to changes in the result. The multi-orifice design however did not give much cavitation after tuning, implying that the coefficient either is wrong in the single hole design, or that the coefficient is geometry dependent. The biggest flaw with the new model is its over-reliance on the tuning of C, which have to be tuned for each geometry, thus diminishing the models usability, and the lack of understanding of the physics that happens on a micro-scale for each cavitation bubble.
The orifice cavitation phenomenon remains a difficult problem to tackle. De- spite many of the practical processes are well known, such as onset and pressure behavior on a macro scale [45], the numerical modeling has many structural difficulties. The scaling effects and mesh analysis around the LES model has been thoroughly studied. Since the cavitation seen in the experiments almost always is on a smaller scale than the computational cells, a greater understand- ing around this is needed. There has been studies around this also showing the need for further studies [47]. The Lagrangian cavitation models could be a way, however existing models only look at the growth, change and collapse
of already existing bubbles, not the creation of new ones [46]. If such a model was developed it could bridge the gap and give further understanding on the experimental results.
Conclusions
In this thesis existing models of orifice cavitation flows were tested and evalu- ated. The compressible solver was deemed too flawed for further use. In the future, with more reliable numerical models and faster computation times a compressible solver should be the chosen due to its ability to correctly model the densities ρl and ρv at the phase boundary. It would also be able to test vibrations and noise in order to compare with experiments.
Established in-compressible solvers were unable to match the experimental data but proved more stable and easy to work with. Therefore a modified solver was developed and tested. It showed the capacity to adequately model cavitation in a single hole orifice and was verified using other boundary conditions and geometries as well. However the solvers built-in coefficient C remains bound to the geometry that is tested and poorly understood. Further study of the cavitation models used is needed in order to create better and more universal tools for cavitation prediction.
Using the new solver cavitation can be predicted in orifice flows in the piping used by Vattenfall AB. The data generated from computational simulations can be used in order to minimize noise, vibrations and make sure no damage is caused to critical systems.
30
References
[1] Christopher Earls Brennen. Cavitation and bubble dynamics. Oxford Univer- sity Press, 1995, pp. 217–218. isbn: 0-19-509409-3.
[2] Batuhan Aktas and Dmitriy Ponkratov. “Time accurate numerical cavita- tion erosion prediction of multiphase flow through a venturi”. In: Sympo- sium of Marine Propulsion (2017).
[3] Tibor Juhasz, George A. Kastis, Carlos Suárez, Zsolt Mor, and Walter E.
Bron. “Time-Resolved Observations of Shock Waves and Cavitation Bub- bles Generated by Femtosecond Laser Pulses in Corneal Tissue and Wa- ter”. In: (1995).
[4] P. Testud, P. Moussou, A. Hirschberg, and Y. Aurégan. “Noise generated by cavitating single-hole and multi-hole orifices in a water pipe”. In: Journal of fluids and structures (2007).
[5] Sulo Lahdelma and Esko K. Juuso. “Vibration Analysis of Cavitation in Kaplan Water Turbines”. In: The International Federation of Automatic Control (2008).
[6] Anne Boorsma and Stewart Whitworth. “Understanding the Details of Cavitation”. In: Second International Symposium on Marine Propulsors (2011).
[7] Dmitriy Ponkratov and Alejandro Caldas. “Prediction of Cavitation Ero- sion by Detached Eddy Simulation (DES) and its Validation against Model and Ship Scale Results”. In: Fourth International Symposium on Marine Propul- sors (2015).
[8] B V.Hubballi and V. B. Sondur. “‘A Review on the Prediction of Cavitation Erosion Inception in Hydraulic Control Valves”. In: International Journal of Emerging Technology and Advanced Engineering. Volume 3, Issue 1 (2013).
[9] B. H. T. Goh, S. W. Ohl, E. Klaseboer, and B. C. Khoo. “Jet orientation of a collapsing bubble near a solid wall with an attached air bubble”. In:
Physics of fluids. 26th ser. (2014).
[10] Werner Sölken. Orifice Plates for Flow Measurement and Flow Restriction. url:
http://www.wermac.org/specials/orificeplate.html. (accessed: 2020- 10-09).
[11] Angele K. “Prediction of cavitation in orifice plates - a novel and simple rule-of-thumb”. In: Experimental and Computational Multiphase Flow (2020).
31
[12] P. Veber, N. Edh, E. Lillberg, K. Angele, D. Edebro, H. Lindqvist, and H.
Sjöholm. “Experimental and numerical analyses of cavitation in orifices plates for flow limitation in nuclear applications”. In: (2020).
[13] Weixing Yuan, Jürgen Sauer, and Günter H. Schnerr. “Modeling and com- putation of unsteady cavitation flows in injection nozzles”. In: Éditions scientifiques et médicales Elsevier SAS (2001).
[14] Ehsan Badfar and Mahdi Alinaghizadeh Ardestani. “Utilizing sliding mode control for the cavitation phenomenon and using the obtaining result in modern medicine”. In: Springer Nature Applied Sciences (2019).
[15] Si Huang, Yifeng Wei, Chenguang Guo, and Wenming Kang. “Numerical Simulation and Performance Prediction of Centrifugal Pump’s Full Flow Field Based on OpenFOAM”. In: Processes (2019).
[16] Chao-Kun Huang. “Turbulence and cavitation : applications in the NSMB and OpenFOAM solvers”. In: (2018).
[17] OpenFOAM. doi:https://openfoam.org/. (accessed: 2020-10-09).
[18] Christopher Earls Brennen. Cavitation and bubble dynamics. Oxford Univer- sity Press, 1995, p. 21. isbn: 0-19-509409-3.
[19] K. A. Mørch. “Cavitation inception from bubble nuclei”. In: É. Interface Focus (2015). doi:http://dx.doi.org/10.1098/rsfs.2015.0006.
[20] Christopher Earls Brennen. Cavitation and bubble dynamics. Oxford Univer- sity Press, 1995, pp. 233–237. isbn: 0-19-509409-3.
[21] Mahamadou Adama Maiga, Olivier Coutier-Delgosha, and Daniel Buisine.
“A new cavitation model based on bubble-bubble interactions”. In: Physics of Fluids, American Institute of Physics (2018).
[22] Cavitation on Ship Propellers - Vortex Cavitation. 2012. doi: https : / / ocw . tudelft.nl/wp-content/uploads/Chapter_9.pdf. (accessed: 2020-11-01).
[23] J. Paul Tullis. Cavitation Guide for Control Valves. Office of Nuclear Regula- tory Research, 1993, pp. 121–122.
[24] J. W. Holl. “An Effect of Air Content on the Occurrence of Cavitation”. In:
American Society of Mechanical Engineers (1960).
[25] Hamed Sadeghi and Masoud Darbandi. “The Effect of Gas Diffusion on the Nuclei Population Downstream of a Cavitation Zone”. In: American Society of Mechanical Engineers (2009).
[26] G. E. Reisman, M. E. Duttweiler, and C. E. Brennen. “Assessment of Cavi- tation Models in the Prediction of Cavitation in Nozzle Flow”. In: American Society of Mechanical Engineers (1997).
[27] James A. Stares. “Control Valve Cavitation, Damage Control”. In: Dresser Masoneilan (2007).
[28] J. Paul Tullis. Cavitation Guide for Control Valves. Office of Nuclear Regula- tory Research, 1993, pp. 2–12.
[29] J. Paul Tullis. Cavitation Guide for Control Valves. Office of Nuclear Regula- tory Research, 1993, pp. 13–17.
[30] J. Paul Tullis. Cavitation Guide for Control Valves. Office of Nuclear Regula- tory Research, 1993, p. 74.
[31] J. Paul Tullis. Cavitation Guide for Control Valves. Office of Nuclear Regula- tory Research, 1993, pp. 79–85.
[32] J. Paul Tullis. Cavitation Guide for Control Valves. Office of Nuclear Regula- tory Research, 1993, pp. 101–104.
[33] Stephen B. Pope. Turbulent Flows. 1st Edition. Cornell University, 2000, pp. 17–18.
[34] Stephen B. Pope. Turbulent Flows. 1st Edition. Cornell University, 2000, pp. 14–15.
[35] ANSYS Inc. Modeling Turbulent Flows. 2006. doi:https://www.southampton.
ac.uk/~nwb/lectures/GoodPracticeCFD/Articles/Turbulence_Notes_
Fluent-v6.3.06.pdf.
[36] Stephen B. Pope. Turbulent Flows. 1st Edition. Cornell University, 2000, pp. 184–188.
[37] Markus Uhlmann. ATurbulent flows and their modelling. 2008. doi: http : //www- cfd.ifh.uni- karlsruhe.de/uhlmann/VORLESUNG/turbmod/ws08/
talk8_ho.pdf.
[38] Stephen B. Pope. Turbulent Flows. 1st Edition. Cornell University, 2000, pp. 335–336.
[39] Stephen B. Pope. Turbulent Flows. 1st Edition. Cornell University, 2000, p. 183.
[40] Stephen B. Pope. Turbulent Flows. 1st Edition. Cornell University, 2000, pp. 183–185.
[41] H. Choi and P. Moi. “Grid-point requirements for large eddy simulation:
Chapman’s estimates revisited”. In: Center for Turbulence Research (2011).
[42] T.G. Leighton. “Derivation of the Rayleigh-Plesset Equation in Terms of Volume”. In: Institute of Sound and Vibration Research (2007).
[43] Christopher Earls Brennen. Cavitation and bubble dynamics. Oxford Univer- sity Press, 1995, pp. 47–50. isbn: 0-19-509409-3.
[44] Michael Kinzel, Jules W. Lindau, and Robert Francis Kunz. “A Unified Homogenous Multiphase CFD Model for Cavitation”. In: American Society of Mechanical Engineers (1997).
[45] Christopher E. Brennen. An Introduction to Cavitation Fundamentals. 2011.
[46] Aurélia Vallier. “Eulerian and Lagrangian cavitation related simulations using OpenFOAM”. In: (2010).
[47] Dorien O. Villafranco, Huy K. Do, Sheryl M. Grace, Emily M. Ryan, and R. Glynn Holt. “Assessment of Cavitation Models in the Prediction of Cav- itation in Nozzle Flow”. In: American Society of Mechanical Engineers (2018).
[48] Merkle, J. C. L. Feng, and Buelow. “Computational Modeling of the Dy- namics of Sheet Cavitation”. In: 3rd International Symposium on Cavitation (1998).
[49] Robert F. Kunz, Brett W. Siebert, W. Kevin Cope, Norman F. Foster, Steven P. Antal, and Stephen M. Ettorre. “A Coupled Phasic Exchange Algorithm for Three-Dimensional Multi-Field Analysis of Heated Flows with Mass Transfer”. In: (1998).
[50] Gunter H. Schnerr and Jurgen Sauer. “Physical and Numerical Modeling of Unsteady Cavitation Dynamics”. In: International Conference on Multi- phase Flow (2001).
[51] Christopher Earls Brennen. Cavitation and bubble dynamics. Oxford Univer- sity Press, 1995, p. 36. isbn: 0-19-509409-3.
[52] Christopher Earls Brennen. Cavitation and bubble dynamics. Oxford Univer- sity Press, 1995, pp. 27–28. isbn: 0-19-509409-3.
[53] Gert-Jan Meijn. “Physical modeling of cavitation using an enthalpy based model”. In: (2015).
[54] M. V. Lowson and George C. Marshall. “Pressure fluctuations in turbu- lence boundary layers”. In: (1965).
[55] Ashok K. Singhal, Mahesh M. Athavale, Huiying Li, and Yu Jiang. “Math- ematical Basis and Validation of the Full Cavitation Model”. In: Journal of Fluids Engineering (2002).
[56] OpenCFD Release OpenFOAM v1912. 2019. doi:R https://www.openfoam.
com/releases/openfoam-v1912/. (accessed: 2020-10-14).
[57] Guilherme Caminha. The CFL Condition and How to Choose Your Timestep Size. 2019. doi:https://www.simscale.com/blog/2017/08/cfl-condition/.
[58] Barı¸s B˙IÇER. “Implementation of Transport Model into CavitatingFoam to simulate the Cavitation in Diesel Injector Nozzle”. In: (2014).
[59] cavitatingFoam.C File Reference. doi:https://openfoam.com/documentation/
guides/latest/api/cavitatingFoam_8C.html. (accessed: 2020-10-09).
[60] Martin Andersen. “A interphaseChangeFoam tutorial”. In: (2011).
[61] Philip J. Zwart, Andrew G. Gerber, and Thabet Belamri. “A Two-Phase Flow Model for Predicting Cavitation Dynamics”. In: International Confer- ence on Multiphase Flow (2004).
This section shows some of the finer meshes used. The meshes were generated using the OpenFOAM functions blockMesh in combination with snappyHexMesh.
Figure 7.1– Fine mesh used for the pipe. This is a cross section of the pipe after the orifice. Notice the finer mesh on the edge of the surface.
Figure 7.2– Fine mesh used for the geometry. In the center of the pipe a coarser mesh was used.
35
Figure 7.3– Fine mesh used. This is the center of the pipe seen from the side. The mesh is finer around the orifice and around the edge.
Figure 7.4– This is the fine mesh that was used for the multi whole orifice. The mesh was made finer around orifice and particularly on the edge of the geomen- try.
This section shows the code used in the modified solver.
interPhaseChangeFoam.C
# i n c l u d e " fvCFD .H"
# i n c l u d e "CMULES.H"
# i n c l u d e " subCycle .H"
# i n c l u d e " i n t e r f a c e P r o p e r t i e s .H"
# i n c l u d e " phaseChangeTwoPhaseMixtures_my .H"
# i n c l u d e " t ur bu le nt Tr an spo rt Mo de l .H"
# i n c l u d e " pimpleControl .H"
# i n c l u d e " fvOptions .H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
int main (int argc , char ∗ argv [ ] ) {
# i n c l u d e " p o s t P r o c e s s .H"
# i n c l u d e " addCheckCaseOptions .H"
# i n c l u d e " s e t R o o t C a s e L i s t s .H"
# i n c l u d e " c r e a t e T i m e .H"
# i n c l u d e " createMesh .H"
# i n c l u d e " c r e a t e C o n t r o l .H"
# i n c l u d e " c r e a t e F i e l d s .H"
# i n c l u d e " c r e a t e T i m e C o n t r o l s .H"
# i n c l u d e " CourantNo .H"
# i n c l u d e " s e t I n i t i a l D e l t a T .H"
t u r b u l e n c e−>v a l i d a t e ( ) ;
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
I n f o << "\ nStarting ␣ time ␣ loop \n" << endl ; dimensionedScalar k_max_value
(
" k_max_value ", dimensionSet ( 0 , 2 ,−2 , 0 , 0 , 0 , 0 ) , s c a l a r ( 2 5 0 . 0 ) ) ;
while ( runTime . run ( ) ) {
# i n c l u d e " readTimeControls .H"
# i n c l u d e " CourantNo .H"
# i n c l u d e " s e t D e l t a T .H"
++runTime ;
I n f o << " Time ␣=␣" << runTime . timeName ( ) << n l << endl ;
37
