Internati onal seminar on ejector/jetpump technol ogy and applicati ons
Louvain-la-Neuve, Belgium
September 7-9, 2009
Paper No. 34
MULTIDIMENSIONAL MODELING OF CONDENSING TWO-PHASE EJECTOR FLOW
Davi d Schmi dt and Michael Colarossi
University of Massachusetts Amherst
Mark J. Bergander
Magnetic Development Inc.
ABSTRACT
Condensing ejectors utilize the beneficial thermodynamics of condensation to produce an exit ing static pressure that can
be in excess of either entering static pressure. The phas e change process is driven by both mixing and interphase heat
transfer. The co mp lete details of the flu id flow are not well understood and cannot be calculated directly. However, semi emp irical models could be used in conjunction with computational flu id dynamics (CFD) to gain some understanding of
how condensing ejectors should be designed and operated. The current work describes the construction of a preliminary
mu ltid imensional simu lation capability that is built around an Eulerian pseudo -fluid approach. The transport equations for
mass and mo mentum t reat the two phases as a continuus mixture. The rate of mass transfer is assumed to be limited by
heat transfer, and a modified form of the Ho mogenous Relaxation Model (HRM) is employed. This model was originally
intended for representing flash-boiling, but the authors hypothesize that with suitable modification, the same ideas could
be used for condensing flow. The co mputational flu id dynamics code is constructed using the open -source OpenFOAM
lib rary, wh ich facilitates object-oriented fluid flow calculations. The resulting code is a transient, finite-volu me code that
can operate in either two or three dimensions, though two -dimensional calculat ions appear to be much more nu merically
stable. The simulat ions are parallelized using a standard message passing interface (MPI) co mbined with domain
decomposition. The simulat ion can use general polyhedral cells, for flexibility in geo metry. Fluid properties are evaluated
using the REFPROP database from NIST , which includes many common fluids and refrigerants. Development is
currently underway for handling multi-co mponent fluids. The results of the simulat ions will allow the study of the flow
within the two-phase condensing ejectors. Of particular interest are the stability of the condensation process and the
permissible boundary conditions. The model can also be used to study flow separation and consequent diffuser stall that
may occur in the diverging portion of the ejector. Due to the strong adverse pressure gradients that coincide with
condensation, extreme care is warranted in avoiding such recirculations.
NOMENCLATURE
Θ
Timescale (s)
ρ
Density (kg/ m3 )
h
Enthalpy (J/ kg)
p
Pressure (Pa)
τ
Stress tensor (Pa)
p crit
Critical pressure (Pa)
φ
Mass flu x (kg/ m2 *s)
p sat
Saturated pressure (Pa)
ψ
Dimensionless pressure difference
t
Time (s)
U
Velocity (m/s)
x
Vapor mass fraction
Equilibriu m vapor mass fraction
α
Vapor volu me fraction
INTRODUCTION
The main objective of this project is to model the flow
inside a condensing ejector, including the condensation
shock that occurs, when the vapor phase is quickly
condensed onto the liquid stream, producing rapid
transformation fro m two-phase into single-phase flow
with a resulting rise in pressure.
Figure 1. Princip le of a condensing ejector
The condensing ejector is a two-phase jet device in
which a sub-cooled fluid in a liquid state is mixed with
its vapor phase, producing a liquid stream with a
pressure that is higher than the pressure of either of the
two inlet streams. Figure 1 above presents the predicted
behavior of a condensing ejector. The high relative
velocity between vapor and liquid streams produces a
high value of heat transfer and the rate of condensation
of the vapor phase is high. This condensed vapor adds to
the mo mentum flu x of liquid stream. The remaining
vapor and liquid jet (original plus condensed vapor)
enter the constant area mixing section where a
condensation shock may occur such that a completely
liquid state exists downstream of the shock. The
pressure rises due to lowering the velocity of the stream
and the mass flow balance is maintained by a sudden
change of density (condensation).
A computational fluid dynamics (CFD) analysis was
emp loyed to overcome the limitat ions of a conventional
control volume analysis and to provide an input to
design methodology of the condensing ejector. The
simu lation method is needed to predict the behavior of
the condensing ejector in various operating conditions
and for different refrigerants. This provides the basis for
establishing fundamentally new engineering and design
methods for a broad spectrum of equip ment operating on
two-phase flow, not only condensing ejectors but also
pumps, heat exchangers, jet compressors, supersonic
nozzles and diffusers.
MODELING APPROACH
For a condensing flow simulat ion, the basic laws of
conservation are followed as for a single fluid. This is
known as the “pseudo-fluid” approach. The equations
for the conservation of mass, mo mentum, and energy are
given below. In these equations, is the mass flu x and
is the stress tensor.
0
t
U
(U ) p
t
h
U p
(h)
t
t
(1)
(2)
(3)
These three equations are not a closed system. For a
flu id in single -phase, an equation of state would be
necessary.
In the case of two-phase flow, the
condensation process involves mixing and heat transfer
between the phases, and there is no direct method to
calculate this. Also, the two-phase mixture is not in
thermodynamic equilibriu m. To bring the mixture
towards equilibriu m, a modified form o f the
Ho mogenous Relaxation Model (HRM) is used. The
model was originally used for flash-boiling cases, but
with some modificat ions the same idea can be applied
for condensing flow.
The Homogeneous Relaxation Model is based on a
linearized expansion proposed by Bilicki and Kestin [1].
The equation for the total derivative of quality, the mass
fraction of vapor, is shown below. The derivative shows
the relaxation of the quality, x, co mpared to the
equilibriu m quality, , over the timescale Θ.
Dx x x
Dt
(4)
The formula suggested by Downar-Zapolski et al. [2]
for the timescale, Θ, is shown below in Eqn. 5.
o a b
(5)
The values for Θ0 , a, and b were determined by best-fit
values to flashing experiments [2]. The values are Θ0 =
6.51 10-4 [s], a = -0.257, and b = -2.24. The variable α
is the vapor volume fraction and the variable is a
dimensionless pressure difference represented in Eqn. 6.
Though the current application is far beyond the
intended use of this empiricism, it serves as a starting
point for further investigation.
p sat p
p crit p sat
x ,h
Dp
Dt x
p ,h
Dx
Dt h
p,x
Dh
Dt
(7)
As shown in the above equation, density is a function of
pressure, quality, and enthalpy [1]. The first and last
terms on the right-hand side of Eqn. 7 are currently not
included.
The HRM model is an empiricis m that has been tuned to
represent flash boiling. The current application to rapid
condensation represents a stretch of the model beyond
its original intent, and quite possibly, beyond its validity.
One should certainly expect that some adjustment of the
model is required. In the current application, the
following changes were made to the HRM model:
A turbulent mixing model based on a single
length scale was added to the transport
equations for mo mentum, energy, and density
(Eqn. 7) [3]
An extra term was added to Eqn. 5 to provide
symmetry of phases. According to Eqn. 5, the
timescale of phase change becomes infinite at
zero void fraction. This behavior represents the
effect of nucleation. A similar behavior should
be present for the case of unity void fraction.
The timescale was bounded, both above and
below, in order to avoid numerical instability
and floating point exceptions.
By subtracting the conservation of mass, Eqn. 1, fro m
Eqn. 7, the left side gives an expression for the velocity
divergence at the new time step.
U
p
x ,h
Dp
Dt x
a pU p H U p
(6)
The HRM model solves for the pressure that satisfies the
chain rule and utilizes the continuity equation. Because
a non-equilibriu m fluid is being considered, the chain
rule takes the place of an equation of state. In the chain
rule, the pressure reacts to the change in compressibility
and density caused by the phase change. Eqn. 7
describes the chain rule as a total derivative of density.
D
Dt p
To make an equation for pressure, a discretized form of
the momentu m equation is coupled with the chain rule.
A generalized form of the mo mentum equation is shown
below in Eqn. 9, where a p is the coefficient term of the
matrix o f velocity equations and H represents
convection and diffusion as discretized equation
coefficients multip lied by neighboring velocities. The
pressure equation, Eqn. 10, does not include the
neglected terms fro m Eqn. 7.
p ,h
Dx
Dt
(8)
H
1 p
ap
x
ap
p ,h
(9)
Dx
0
Dt
(10)
A benefit of this pressure equation is that most of the
terms are linear in relation to pres sure. In the case of
constant density, an incompressible form is established.
Schmidt et. al [4] used this idea in a two-step projection
method on a staggered mesh approach. This method
was used for their two-d imensional structured grid
solver. In order to apply this model to a threedimensional solution and for an unstructured, general
polyhedral mesh, a collocated variable approach is used.
The numerical details can be found in Gopalakrishnan
and Schmidt [5].
Flu id properties are obtained using REFPROP
(Reference Flu id Thermodynamic and Transport
Properties Database) fro m the NIST (National Institute
of Standards and Technology) database. Given two
thermodynamic inputs, REFPROP calls its necessary
subroutines to calculate the thermodynamic and
transport properties requested by the user. The user
selects the two thermodynamic properties to use as
inputs and selects an appropriate range and step size.
The properties calculated at these specified points are
arranged in a table format. Properties can be calculated
for many flu ids, including mixtures; in this case the
working fluid is water.
Typically, five to ten PISO/secant iterations are
emp loyed, and the solution of the pressure equation is
necessary for every iteration. For the full pressure
equation, a diagonal incomp lete LU preconditioned
biconjugate gradient is used. Once the pressure equation
is solved, the pressure field is used to correct the flu xes
and the time step is fin ished.
The structure for solving these equations is provided by
OpenFOAM, wh ich allows rapid construction of CFD
codes in an object-oriented framework [6]. OpenFOAM
also provides a message passing interface (MPI) that can
run decomposed cases in parallel.
LEVY-B ROWN CONDENS ING EJ ECTOR
The nozzle being modeled in the CFD simu lations is one
that has been used in experiments by E.K. Levy and G.
A. Brown [7], and is shown below in Figure 2.
Wall
Gas inlet
Li qui d
inlet
Outflow
Centerline axis
Figure 2: Two-dimensional representation of nozzle used by Levy and Brown [7]
This nozzle acts as a condensing ejector for twodimensional flo w of a flu id. In the figure above, the
image can be mirrored around the centerline axis.
For these simulations, saturated vapor enters through the
annular channel and saturated liquid enters near the
centerline. As the saturated liquid and saturated vapor
flow past the splitter, the two streams should start to
mix. Around the diverging part of the nozzle there is a
shock wave that leads to more mixing and circulation of
the two streams. The location and size of the shock
wave is difficu lt to determine at this time. Due to the
unstableness of the flow that occurs during
condensation, the validity and accuracy of the mixing
prediction both before and after the throat are in
question.
Choosing appropriate boundary conditions are essential
to running a meaningful simu lation. Because of the
strong pressure gradients and general instability of the
flow, find ing acceptable boundary conditions can be
difficult. The velocity at the gas inlet is set to a value
much lower than what was used in Levy and Brown [7];
75 meters per second compared to approximately 472
meters per second in the experiments. Zero pressure
gradient boundary conditions and specified densities , 0.5
kg/m3 at the gas inlet and 996.7 kg/ m3 at the liquid inlet,
are used at the inlets. At the outlet, a specified pressure
is imposed at an arbitrary distance, creating a partially
non-reflection boundary condition. The outlet boundary
condition on velocity is zero gradient. A ll walls are
adiabatic.
RES ULTS
The simulat ions were run for over 0.3 s of simu lated
time. During this period, the flow never achieved a
steady state due to diffuser stall. Vortices were created
due to flow separation, as shown in Fig. 3. These
vortices create oscillations in pressure and convolute the
condensation shock.
The upper half of Fig. 3 shows that, by the beginning of
the diffuser section, the high enthalpy of the gas mixes
with the lo w enthalpy of the liquid. This mixing
predisposes the vapor to condense by lowering its
temperature. In Fig. 4, the mass fraction of vapor
declines just after the end of the high enthalpy zone.
Pressure shows a modest increase, as shown in the upper
half of Fig. 4. However, the vortices created by the flow
separation cause locally low pressures that reduce the
effectiveness of the condensing ejector. This separation
is exacerbated by the strong adverse pressure gradient in
this part of the flow.
Figure 3. The enthalpy near the diffuser is shown in the top half of the figure. In a mirror image, the streak lines,
indicating the instantaneous velocity field, are shown in the bottom half of the figure.
Figure 4. The pressure field in the co mputational domain is show in the top half of the figure wh ile the mass fraction of
vapor is mirrored in the bottom half o f the figure.
Figure 5. The velocity magnitude in the computational do main is show in the top half of the figure while the time
derivative of mass fraction of vapor is mirrored in the bottom half of the figure.
Figure 5 shows the deceleration that accompanies the
pressure increase and condensation shock. As can be
seen in the upper half of the figure, the shock is oblique.
Locally low pressures, corresponding to the locations of
vortices, are visible in the diffuser section. The bottom
half of Fig. 5 shows the high rate of condensation in the
shock. Though not clearly visible in the figure, small
amounts of liquid can vaporize in the high-shear zone
near the inlet.
Though, in these images, the condensing ejector is
producing the desired static pressure increase, the
strongly oscillatory nature of the flow caused very large
transient variations in pressure. Depending on the time
considered, the static pressure at the exit could be below
the upstream pressures. Further investigations will
include
time-averaging
of
performance
and
investigations of the acoustic reflect ivity of various exit
boundary conditions.
CONCLUS IONS
The idea embodied in the Ho mogenous Relaxation
Model was used to construct a CFD model of
condensing ejectors. Though further model adjustment
and experimental validation is likely required, it is an
encouraging early result. To date, the authors are
unaware of any existent CFD simu lations of condensing
ejectors. The current imp lementation benefits from the
flexib ility of the OpenFOAM libraries and is fully
parallelized.
The preliminary results show the potential for a
condensation shock to occur at the beginning of the
diffuser section of the condensing ejector, triggering
diffuser stall. The separated flo w causes a highly
unstable flow field and interferes with ejector efficiency.
The shed vortices produce locally low pressures and
contribute to the oscillations.
Continuing work will use experimental validation to
adjust the model to improve its accuracy and check the
overall applicability to predicting condensation shocks.
It is also likely that a more sophisticated model of
interphase turbulent mixing will be required, since the
mixing rate strongly affects the performance of the
ejector. These areas will be exp lored in future work.
ACKNOWLEDGEMENT
This material is based upon work supported by the
National Science Foundation, STTR Phase II Project
No. 0822525 and by the Depart ment of Energy, under
Award Nu mber DE-FG36-06GO16049
DISCLAIMER
This report was prepared as an account of work
sponsored by an agency of the United States
Govern ment. Neither the United States Government nor
any agency thereof, nor any of their employees, makes
any warranty, express or implied, or assumes any legal
liab ility or responsibility for the accuracy, completeness,
or usefulness of any information, apparatus, product, or
process disclosed, or represents that its use would not
infringe privately owned rights. Reference herein to any
specific co mmercial product, process, or service by trade
name, trademark, manufacturer, or otherwise does not
necessarily constitute or imply its endorsement,
recommendation, or favoring by the United States
Govern ment or any agency thereof. The views and
opinions of authors expressed herein do not necessarily
state or reflect those of the United States Govern ment or
any agency thereof.
REFERENCES
[1]
Bilicki Z., Kestin J.: Physical Aspects of the
Relaxation Model in Two-Phase Flo w, Proc.
Roy. Soc. London A., 428(1990), 379-397.
[2]
Downar-Zapolski P., Bilicki Z., Bo lle L.,
Franco J.: The Non-Equilibriu m Relaxation
Model for One-Dimensional Flashing Liquid
Flow, IJMF, 22(1996), No. 3, 473-483.
[3]
Prandtl, L.: About Fully-Developed Turbulence
(Über d ie ausgebildete Turbulenz), Z. Angew.
Math. Mech., 5(1925), 136-139.
[4]
Schmidt D.P., Corradin i M.L., Rut land C.J.: A
Two-Dimensional, Non-Equilibriu m Model of
Flashing Nozzle Flo w, 3rd ASME/JSM E Joint
Flu ids Engineering Conference, 208(1999), No.
616.
[5]
Gopalakrishnan S., Sch midt D.P.:
A
Co mputational Study of Flashing Flow in Fuel
Injector Nozzles, SA E Int. J. Engines 1(2008),
No. 1, 160-170.
[6]
Weller H.G., Tabor G., Jasak H., Fureby C.: A
Tensorial
Approach
to
Computational
Continuum Mechanics Using Object-Oriented
Techniques, Computers in Physics, 12(1998),
No. 6, 620.
[7]
Levy E.K., Bro wn G.A.:
Liquid-Vapor
Interactions in a Constant-Area Condensing
Ejector, Journal of Basic Engineering,
94(1972), No. 1, 169-180.