Article

Design Optimization of an Oil-Air Catch Can Separation System

Abstract and Figures

The Positive Crankcase Ventilation (PCV) system in a car engine is designed to lower the pressure in the crankcase, which otherwise could lead to oil leaks and seal damage. The rotation of crankshaft in the crankcase causes the churn up of oil which conducts to occurrence of oil droplets which in turn may end in the PCV exhaust air intended to be re-injected in the engine admission. The oil catch can (OCC) is a device designed to trap these oil droplets, allowing the air to escape from the crankcase with the lowest content of oil as possible and thus, reducing the generation and emission of extra pollutants during the combustion of the air-fuel mixture. The main purpose of this paper is to optimize the design of a typical OCC used in many commercial cars by varying the length of its inner tube and the relative position of the outlet from radial to tangential fitting to the can body. For this purpose, CFD parametric analysis is performed to compute a one-way coupled Lagrangian-Eulerian two-phase flow simulation of the engine oil droplets driven by the air flow stream running through the device. The study was performed using the finite volume method with second-order spatial discretization scheme on governing equations in the Solid Works-EFD CFD platform. The turbulence was modelled using the k-ɛ model with wall functions. Numerical results have proved that maximum efficiency is obtained for the longest inner tube and the tangential position of the outlet; however, it is recommended further investigation to assess the potential erosion on the bottom of the can under such a design configuration.
Content may be subject to copyright.
Journal of Transportation Technologies, 2015, 5, 247-262
Published Online October 2015 in SciRes. http://www.scirp.org/journal/jtts
http://dx.doi.org/10.4236/jtts.2015.54023
How to cite this paper: Abilgaziyev, A., Nogerbek, N. and Rojas-Solórzano, L. (2015) Design Optimization of an Oil-Air Catch
Can Separation System. Journal of Transportation Technologies, 5, 247-262. http://dx.doi.org/10.4236/jtts.2015.54023
Design Optimization of an Oil-Air Catch Can
Separation System
Anuar Abilgaziyev, Nurbol Nogerbek, Luis Rojas-Solórzano
Department of Mechanical Engineering, School of Engineering, Nazarbayev University, Astana, Kazakhstan
Email: a.abilgaziyev@gmail.com
Received 30 June 2015; accepted 24 October 2015; published 27 October 2015
Copyright © 2015 by authors and Scientific Research Publishing Inc.
This work is licensed under the Creative Commons Attribution International License (CC BY).
http://creativecommons.org/licenses/by/4.0/
Abstract
The Positive Crankcase Ventilation (PCV) system in a car engine is designed to lower the pressure
in the crankcase, which otherwise could lead to oil leaks and seal damage. The rotation of crank-
shaft in the crankcase causes the churn up of oil which conducts to occurrence of oil droplets
which in turn may end in the PCV exhaust air intended to be re-injected in the engine admission.
The oil catch can (OCC) is a device designed to trap these oil droplets, allowing the air to escape
from the crankcase with the lowest content of oil as possible and thus, reducing the generation
and emission of extra pollutants during the combustion of the air-fuel mixture. The main purpose
of this paper is to optimize the design of a typical OCC used in many commercial cars by varying
the length of its inner tube and the relative position of the outlet from radial to tangential fitting to
the can body. For this purpose, CFD parametric analysis is performed to compute a one-way cou-
pled Lagrangian-Eulerian two-phase flow simulation of the engine oil droplets driven by the air
flow stream running through the device. The study was performed using the finite volume method
with second-order spatial discretization scheme on governing equations in the Solid Works-EFD
CFD platform. The turbulence was modelled using the k-ɛ model with wall functions. Numerical
results have proved that maximum efficiency is obtained for the longest inner tube and the tan-
gential position of the outlet; however, it is recommended further investigation to assess the po-
tential erosion on the bottom of the can under such a design configuration.
Keywords
CFD, Oil Catch Can, Positive Crankcase Ventilation, Motor Oil Droplets, Mesh Refinement,
Two-Phase Flow, Lagrangian-Eulerian
1. Introduction
Manufacturers of motor vehicles design their products in accordance with external factors such as government
A. Abilgaziyev et al.
248
and industry standards. These standards are related to aspects such as safety, performance, price through taxes
and the most important to this research: emissions.
In the operation of an internal combustion engine, the crankshaft and the connecting rod act as a blender mix-
ing the air and lubricating oil into a mist. In the 4-stroke process, the piston is forced down by the ignition of a
mixture of compressed air and fuel that takes place inside the combustion chamber. The pumping action from
the pistons pressurizes the crankcase, thus further mixing the air and oil. At the same time, a small amount of
that ignited mixture leaks through the piston ring seals and ends up in the crankcase. This leakage is often men-
tioned as blow-by” (see Figure 1 and Figure 2). In addition to the air-fuel mixture, there exists a large possi-
bility of appearance of condensation and oil droplets [1].
Figure 1. Schematic diagram of PCV system [2].
Figure 2. Schematic diagram 4-stroke engine process [5].
A. Abilgaziyev et al.
249
This mixture of oil mist and hydrocarbons needs to be released and vented from the crankcase; otherwise a
positive pressure will occur due to expansion, caused by heating of gases. Thus, gas-droplets mixture pressure
inside the crankcase becomes higher than atmospheric pressure and if not taken care of, the mixture may diffuse
onto the crankcase oil, contaminating it or else, it could return back to the intake manifold. In order to avoid or
minimize this potential issue, engines are regularly equipped with breathers that would allow excess of crank-
case pressure to be vented. However, the damage from not eliminating all gases out results in a reduced life of
engine. In the end of 1950s, General Motors started to investigate the relationship between the hydrocarbons
from gasoline engines and the environment (Filter Manufacturers Council, n.d.). Thus, the Positive Crankcase
Ventilation (PCV) was developed and integrated to their cars by 1963 [3].
According to Ding [4], the main function of the PCV is to extract the mixture of gas-droplets from the crank-
case by drawing fresh clean air in. The mechanism of operation is simple: air passes through the oil drain back
passages to the crankcase below, displacing the dirty air-oil mist and hydrocarbons to the PCV valve. However,
the PCV system is not perfect and it allows some of the oil mist back into the intake manifold, which will in-
crease the level of carbon solids and reduce the octane level of the combustion fuel. For instance, for boosted
setup with turbo and supercharger, the breather/PCV will not capture some of oil droplets. Thus, some of these
oil droplets will recirculate from the intake to intercooler again and again. It will lead to reduction of heat ex-
change efficiency, since fume with oil droplets will coat the inside of the intercooler with oil. In addition, there
exist other uncontrolled related issues such as the detonation or “knock” that occurs when oil is introduced into
the combustion chamber triggering the action of the knock sensors pick-up and pull timing to protect the engine
from damage, and thus reducing power. Another result is the carbon build-up on the valves and piston tops,
which also results in decreased performance and less efficient performance. The main purpose of separating oil
catch can (OCC) is to trap and remove these oil droplets from the gases before they will continue on through the
intake and get burnt and consumed. Therefore, the OCC is placed in the PCV system, between PCV valve and
intake manifold [6].
The OCCs are usually devised as an aftermarket device. The reason of it is that cars that need the separator
come with individual built-in ones and not all cars necessarily need them. Thus, the only way OCCs could be
publicly evaluated is by the amount of after-use oil found in the reservoir after a period of time of operation
since the last oil change to the engine. The designs of OCCs in the market vary from a simple empty container
with two pots to complex ones filled with some filters (see Figure 3). Therefore, this paper aims to obtain the
most efficient design of an OCC by making some design modifications, ranging from the most common existing
unit, with radial outlet, to a unit with fully tangential exit, depicted in Figure 4(a) and Figure 4(b), respectively.
Figure 3. Schematic diagram of the oil catch can [7].
A. Abilgaziyev et al.
250
(a) (b)
Figure 4. Physical generic CAD model of the OCCs. (a)
Radial outlet; (b) Tangential outlet.
The independent parameters to be varied in the optimization process are the length of inner tube and the rela-
tive position of outlet pipe respect to can axis. The main hypothesis behind the use of those parameters is that
these are simple changes that could be implemented with low expenses and would affect the travel-time of
droplets and the exposure to surface contact which should portray an optimal configuration to maximize oil re-
tention by the device.
The analysis here presented is based on CFD tools using a Lagrangian-Eulerian framework with one-direction
coupling between phases, assuming the low volume fraction of the droplets compared to the airflow. Following
a design of experiments approach with sampling of scenarios and construction of a surrogate model, the final
optimal design is obtained based on the maximization of the collection efficiency, used as objective function.
The next sections are devoted to the following stages of the CFD study:
Prescription of governing equations and respective boundary conditions.
Description of verification of the discretization or Mesh Sensitivity Analysis.
Validation of the numerical tool (SolidWorks-EFD solver and physical models).
Preliminary results based on the analysis of the performance of most popular Oil Catch Can currently in the
market.
Parametric study varying the input variables of interest in the optimization to validate the hypothesis.
Analysis and discussion, and concluding remarks.
2. Background
Nowadays, with the development of manufacturing industry, the fabrication of OCCs has also evolved and there
exist various designs of cans [8]. For instance, some cans have pretty simple designs that consist of simple
empty housing, inlet and outlet tube. In-deep background research of catch can was conducted and it was found
that most companies use two main approaches for catch can design. The basic design is a simple can with hoses
attached [8]. The more advanced designs include internal baffling, which provides more surface area for the oil
to be collected, e.g. baffled OCC made by Mishimoto [9]. Though both of these approaches work, the simpler
design is much less efficient than the complex unit.
One of the most popular companies manufacturing the OCCs is Mishimoto [9]. According to the Mishimoto
Technical Specs [9], their aim is to design a high-end oil/air separator that is universal and can be installed in
any vehicle. At the same time Mishimoto engineers pursue a design with exceptional functionality and still
looking aesthetically pleasing. Unfortunately, they did not publish the official results of their research, but indi-
cate in their company’s web site that they created a new MMBCC-UNI model that claims to be the most effec-
tive oil catch can today on the market. However it should be understood that different motor vehicles have dif-
ferent type of engines and, therefore, each company manufacturing oil catch cans creates its own design for a
specific type of engine or specific car make.
Thus, the design that was used as a base case in this work was based on the design that according to Mishi-
moto Technical Specs [9] is the most efficient and universal currently in the market. Since the goal of this paper
is to develop a design optimization of the geometry of the oil catch can, the device was simplified and none of
A. Abilgaziyev et al.
251
regular inner filters were included, but instead the numerical model will artificially capture all droplets hitting
the can walls, as if they were naturally attached and drained out.
3. Numerical Model Set-Up
The OCC models, with inlet on the top part and outlet with two positions on the top part of the cylinder, are
shown in Figure 4.
As it was mentioned before, all parameters of the can were taken from one of the most efficient and universal
OCCs that are designed by Mishimoto Company. The CAD drawings with dimensions of the two main models
of OCC, according to exit pipe, are shown in Figure 5.
Thus, two parameters, the length of inner tube from top to bottom and the position of the outlet, were taken
into account for the analysis. The length of the inner tube is represented by X variable (the range is [30; 130]
mm), whereas the position of the outer tube is Y (the range is [0, 35.5] mm) (see Figure 6).
(a) (b)
Figure 5. Schematic multi-view drawings of the oil catch can with two
critical types of outlet tube. (a) Radial outlet; (b) Tangential outlet.
Figure 6. Demonstrating figure of Xo and Yo distances.
A. Abilgaziyev et al.
252
3.1. Mathematical Model
The setup of the mathematical model is performed using the CFD workbench SolidWorks-FloEFD (SW-FloEFD)
v.2013-14. The main premises are: steady state, Newtonian fluid, compressible and turbulent flow. Therefore,
the following favré-averaged governing equations and boundary conditions were prescribed: (a) mass conserva-
tion; (b) Navier-Stokes (momentum conservation) equations; (c) energy conservation; (d) constitutive relations
between p, T and H; and (f) k-ɛ turbulence model with wall functions. These equations for the air are shown as
follows:
( )
0
i
i
u
tx
ρρ
∂∂
+=
∂∂
(2.1)
( )
( )
; 1, 2, 3
R
ii j ij ij i
j ij
up
uu S i
t x xx
ρρ ττ
∂ ∂∂
+ =−+ ++ =
∂ ∂ ∂∂
(2.2)
with:
2
3
j
ik
ij ij
ji k
u
uu
xx x
τµ δ

∂∂
= +−


∂∂ ∂

(2.3)
(Newtonian fluid constitutive equation to turn the momentum equations into Navier-Stokes equations).
(2.4)
(Boussinesqs assumption for the Reynolds-stress) where, δij is the Kronecker delta function, μ is the dynamic
viscosity, μt is the turbulent eddy viscosity and k is the specific turbulent kinetic energy.
The energy transport equation for the fluid in terms of the enthalpy:
( )
( )
RR
ii
j ij ij i ij i i
ii j
uH u
Hp
u q Su
t xx tx
ρ
ρτ τ τ ρε
∂∂
∂∂ ∂
+ = + ++− ++
∂∂ ∂∂
2
2
u
Hh= +
(2.5)
The Ideal Gas state equation is prescribed to compute the air density as a function of pressure and tempera-
ture:
air
p
RT
ρ
=
with:
universal
air Air_Molecular_Mass
R
R=
(2.6)
For the oil droplets trajectories within the fluid (air), the solver assumes spherical liquid particles (droplets) in
a steady-state air flow field. Only fluid-to-particle interaction is allowed, thus the model is limited to dilute par-
ticles only, which is in general valid for bulk mass ratio of particles to fluid of less than 20% - 30%, as in this
case. The particles drag is calculated using Henderson’s formula [10], which accounts for laminar/transitional/
turbulent flow regimes and temperature difference between particles and carrier fluid. The particle/fluid heat
transfer is computed according to Carlson and Hoglund [11] formula and since each particle mass is assumed
constant, the size may change accordingly, as they are cooled or heated by the surrounding air. The gravity is
included in the analysis and the walls are treated as adiabatic with full absorption of any particle that hits them.
The additional k-ɛ transport equations for the specific turbulent kinetic energy and dissipation respectively
are:
( )
t
ik
i i ki
kk
uk S
tx x x
µ
ρρµ
σ


∂∂ ∂
+ =++



∂∂ ∂


(2.7)
A. Abilgaziyev et al.
253
( )
t
i
ii i
uS
tx x x
ε
ε
µ
ρε ε
ρε µ σ


∂∂ ∂
+ =++



∂∂ ∂


(2.8)
where, the source terms are defined as:
Ri
k ij t B
j
u
S P
x
τ ρε µ
= −+
(2.9)
2
1 1 22
Ri
ij t B B
j
u
S C f CP C f
kx k
εε ε
ε ρε
τµ

= +−



(2.10)
where, PB represents the turbulent production due to buoyancy forces and is given by:
1
i
BBi
g
P x
ρ
σρ
= −
(2.11)
with gi = (gx, gy, gz) the gravity vector, the constant σB = 0.9 and constant CB = 1 when PB > 0, and 0 otherwise.
Whereas:
( )
3
2
12
0.05
1 and 1 exp
T
f fR
f
µ

=+ =−−



(2.12)
The constants Cμ, Cɛ1, Cɛ2, σk, σɛ are obtained from typical fitting experiments as:
12
0.09, 1.44, 1.92, 1, 1.3
k
CCC
µε ε ε
σσ
= = = = =
(2.13)
The diffusive heat flux is defined as:
Pr
t
ici
h
qx
µ
µ
σ

= +


(2.14)
with the constant σc = 0.9, Pr is the Prandtl number and α is the thermal diffusivity.
And the relation between k, ɛ and μt is given by:
2
t
Ck
f
µ
µ
ρ
µε
=
(2.15)
and fμ is a turbulence damping factor to consider the laminar-turbulent transition as a function of distance from
the wall, defined by the expression:
( )
2
20.5
1 exp 0.025 1
yT
fR
R
µ


=− − ⋅+



(2.16)
where:
2
and
Ty
k ky
RR
ρρ
µε µ
= =
(2.17)
and y is the distance from the wall.
3.2. Boundary Conditions
The following boundary conditions are prescribed on the governing equations:
Inlet air volume flow rate is 5 cfm (~2.35 × 103 m3/s) [12].
Inlet static pressure and temperature are 7 bar and 700˚C, respectively. Since inlet flow was obtained from
the combustion chamber with high rpm motor, the inlet air is assumed with same pressure and temperature
of average parameters (pressure and temperature) of the combustion chamber. The average values are ob-
tained from the graph shown in Figure 7.
Outlet static pressure and temperature are 1 bar and 20˚C, respectively. These values are obtained from the
A. Abilgaziyev et al.
254
graph of pressure and temperature against crank angle in the combustion chamber (Figure 7). It is assumed
that the outlet has the thermodynamic conditions as the air in the intake stroke (approximately in the range
[270, 90] degrees of crank angle) since other end of blow-by-gas line is connected to intake air for re-
combustion (Figure 8).
Figure 7. Pressure and temperature behaviour in the combustion chamber of a 4-stroke engine [13].
Figure 8. Schematic diagram of the principle of how OCC works [14].
A. Abilgaziyev et al.
255
The properties for the motor oil are listed below:
Density (ρ) = 895 kg/m3 [15].
Kinematic viscosity (ν) = 1.01 × 105 m2/s (= 10.1 cSt) [15].
Dynamic viscosity (μ) = 0.01 Pa·s (found by the formula μ = ρν using previous parameters).
Specific heat = 1900 J/(kg·K) [16].
Thermal conductivity = 0.2 W/(m·K) [16].
The mass flow rate of the oil is 2.89 × 107 kg/s. The value is estimated by knowing the volume of the oil
caught when a car is driven for approximately 2400 m (1500 miles) from a video in YouTube Channel:
newagemuscle 2010 ss [17]. Taking average velocity of the car as 30 km/h [18], we can obtain approximate
volume flow rate of the oil to finally get the mass flow rate of oil flowing into the catch can, which as expected,
is much smaller than the mass flow of air as expected. For the modelling, the sizes of droplets are so small that
the droplets of the oil are considered as perfect spheres. For the simulation, the diameter of the droplets is taken
as 1.5 µm [19].
The inner wall is set to absorb oil droplets hitting it. Some particles will not be caught by the wall which will
leave the can with the air stream. Thus, the lower the number of particles leaving the can, the higher the OCC
efficiency. Hence, the efficiency of the OCC is calculated by the formula:
100%
io
i
NN
N
ε
= ⋅
where Ni is the number of droplets at inlet and No is the number of droplets at outlet. Assuming the velocity of
droplets at inlet is equivalent to the velocity of the air, number of droplets at inlet would be approximately 200
for this study.
3.3. Discretization and Mesh Sensitivity Analysis
In order to ensure proper and acceptable accuracy of the results, the discretization mesh has to undergo a Mesh
Sensitivity Analysis (MSA), in which density of cells is gradually increased, with special attention to region of
largest gradients, and the solution must be re-assessed until results demonstrate sufficient independence on grid
size.
For the MSA, the catch can model with Y = 35.5 mm and X = 130 mm specifications is selected, since this
corresponds to the most critical configuration due to the expected helical motion of the air stream carrying the
droplets.
The discretization of the geometry was performed according to the following mesh parameters: initial coarse
mesh with total number of cells equal to 27,381. Mesh refined by the range of 50% - 65% with total of 43,725,
and this was repeated until results converged satisfactorily. The mesh refinement process stopped when the dif-
ference in overall pressure drop between consecutive meshes was less than 1%, which occurred for mesh with
112,525 cells. This level of error was acceptable given the complexity of the two-phase flow model and its dif-
ficulty to obtain full convergence. The main generated computational grids during the MSA are presented in
Figure 9 and results are summarised in Table 1.
The set of governing equations are discretized and solved using the finite volume (FV) method on a spatially
rectangular computational mesh refined locally at the solid/fluid interfaces and in specified fluid regions where
high gradients are expected. The FV method grants a conservative discretization of the governing equations,
(a) (b) (c) (d)
Figure 9. Side and front views for meshes during MSA. (a) 27,381 cells; (b) 43,725 cells; (c) 71,405 cells; (d) 112,525 cells.
A. Abilgaziyev et al.
256
Table 1. Summary of MSA.
Cell size Number of cells Pressure drop (Pa) Error (%)
Mesh 1 Nx = 8, Ny = 18, Nz = 12 27,381 112.00
Mesh 2 Nx = 16, Ny = 36, Nz = 24 43,725 80.04 28.54
Mesh 3 Nx = 30, Ny = 68, Nz = 45 71,405 89.49 11.81
Mesh 4 Nx = 36, Ny = 81, Nz = 54 112,525 91.70 2.47
Mesh 5 Nx = 44, Ny = 99, Nz = 66 176,989 91.79 0.098
with spatial derivatives (fluxes) approximated with second-order upwind on the implicitly treated modified
Leonard’s QUICK (Quadratic Upstream Interpolation of Convective Kinematics) [20] and a Total Variation
Diminishing (TVD) method [21].
An operator-splitting technique [22]-[24] to efficiently resolve the problem of pressure-velocity decoupling,
following a SIMPLE/like approach [25] is used.
The resulting linearised algebraic system of equations is solved by iteration on the LU-factorization precondi-
tioned matrix using the generalized conjugate gradient method [26]. The stop criterion is reached when the dif-
ference between consecutive iterations for global mass flow conservation is met at less than 0.001% of inlet
flow rate (~2.82 × 108 kg/s).
3.4. Computational Resource
The simulations were carried out using a PC with CPU Intel(R) Core(TM) i7-3517U @ 1.90 GHz, 2.40 GHz
and 8.00 GB RAM characteristics. The time taken for every simulation with the finally chosen mesh to fully
convergence starting from previously converged results in coarser mesh was approximately 1 hour.
3.5. Validation of SW-FloEFD Model
Transportation of small particles and their trajectories in uniform flows were already validated for SW-FloEFD
[27]. Two different type of validations were presented: (a) trajectories of massless particles initially injected
perpendicular to uniform flow are numerically predicted in excellent agreement with theoretical trajectories; (b)
trajectories of the particles in similar conditions but including gravitational effects are also numerically calcu-
lated in very good agreement with theoretical results. Detailed information may be found in the references.
Moreover, SW-FloEFD has been validated for laminar and turbulent flows in pipes [28]. The longitudinal
pressure gradient along a pipe and the fluid velocity profile at the pipe exit at various Re were calculated in ex-
cellent agreement with theoretical solution for laminar flow and experimental data for turbulent regime. Further
details may be found in the references.
4. Methodology
The optimization proceeded with the independent two parameters Xo and Yo already described, using a second
order two-variable “multivariate nonlinear regression analysis” (MNRA) in the form of quadratic equation with
two variables. The physical ranges were Xo: [30, 130] mm and Yo: [0, 35.5] mm, respectively, but were normalised
as (x, y) with range of [0, 1] each one to facilitate the manipulation of data and minimise round-off errors during
the operations. Therefore, the objective function is described by
( )
22
1 2 3 45 6
,fxy cx cy cxycxcyc= + + +++
where f(x, y) is the OCC efficiency.
At first, the second-order equation, representing a surrogate of the real complex model described by govern-
ing equations and boundary conditions, is found by the regression analysis with 9 input pair of data points. After
that, the critical point (i.e. the highest efficiency) is found by maximizing the surrogate function. Afterwards, a
random pair of data points is chosen and its efficiency is evaluated using CFD simulation. Once the result is ob-
tained, this new point is integrated to the MNRA and a new surrogate is derived. From this new surrogate func-
tion, the critical point is found and its efficiency (maximum) is compared to the maximum from previous surro-
gate (iteration). If the comparison is not satisfactory, a new pair of data points is randomly drawn and the proc-
ess is repeated until the maxima between consecutive iteration differ less than ~1%.
A. Abilgaziyev et al.
257
5. Numerical Results
The initial 9 chosen different OCCs configuration are simulated and the efficiencies were obtained as shown in
Table 2.
Then, MNRA led to 6 coefficients of the surrogate function. All results are shown in Table 3 for 5 consecu-
tive iterations. Four random points with respective efficiency for each, as obtained are shown in Table 4, in-
cluding the points with maximum efficiency.
On the 5th iteration, the error is reduced to 1.23%. The best fit equation of the efficiency behaviour is shown
below:
22
0.2317 0.0511 0.0504 0.4344 0.1366 0.4452.
x y xy x y
ε
=− − +++
The final critical point for maximum efficiency is (x, y) = (0.8369, 0.9243), which is equivalent to (Xo, Yo) =
(113.69, 32.8127) in mm. At this point, the efficiency is 0.69 (69%).
After this numerical analysis, it is observed that when x and y are approximately in the range of [0.5, 1],
higher efficiency of the OCC is obtained (see Figure 10).
Trajectory lines of particles are shown in Figure A1 (see Appendix I). Colours on trajectory lines depict the
fluid pressure at each location along the lines, for reference purposes.
Regarding to the length of the inner tube, it is observed that the pressure at the stagnation (see Figure A2(a),
Appendix II) bottom dramatically increases with increase of the inner tube’s length since the jet impinges more
directly and less lateral diffusion is permitted (Figure A2). It is also noticed how the tangential outlet permits a
more ordered exhaust and therefore the velocity recovery as the flow approaches the exit is more gradual than
for the radial exhaust for all inner tube lengths. Figure A2 shows the positive relationship between the inner
tube’s length which, when enlarged, increases the absorption of oil droplets and efficiency of the OCC.
Table 2. Efficiency results of initial 9 points.
Yo = 0 mm Yo = 17.75 mm Yo = 35.5 mm
Xo = 30 mm 0.46 0.47 0.54
Xo = 80 mm 0.62 0.65 0.67
Xo = 130 mm 0.63 0.72 0.66
Table 3. Obtained coefficients of the quadratic equation.
Trial # c1 c2 c3 c4 c5 c6
1 0.2667 0.0667 0.0500 0.4178 0.1450 0.4453
2 0.2679 0.0735 0.0511 0.4721 0.1529 0.4454
3 0.2299 0.0520 0.0510 0.4316 0.1362 0.4464
4 0.2283 0.0503 0.0517 0.4308 0.1352 0.4459
5 0.2317 0.0511 0.0504 0.4344 0.1366 0.4452
Table 4. Results from trial equation.
Trial equation # Random point (x, y) Efficiency at point via CFD Critical point (x, y) @ Max_Effic. Effic. error (%)
1 Base case Base case 0.8109, 0.7834 ----
2 0.127, 0.6324 0.57 0.8085, 0.7588 2.47
3 0.5469, 0.2785 0.61 0.8392, 0.8987 14.3
4 0.2576, 0.2922 0.57 0.8412, 0.9128 1.42
5 0.706, 0.8235 0.69 0.8369, 0.9243 1.23
A. Abilgaziyev et al.
258
Moreover, the results show that the efficiency, when the outlet is located close to tangent (i.e., largest y-value) to
the can, would be higher than the conventional radial outlet can (y = 0 mm). The main reason is that in the tangen-
tial outlets the particle trajectories have a rotational motion that permits to have longer time in potential contact
with the wall or filters, and therefore it increases the possibility to capture more droplets by the filters or walls.
6. Sentivity of CFD Results
In order to assess how sensible are the numerical results to changes in boundary conditions that may have an in-
trinsic level of uncertainty, i.e., mass flowrate of droplets and number of droplets injected through the inlet
stream, a final sensitivity assessment was performed. The configuration Xo and Yo at their intermediate value, i.e.,
[80, 17.5] mm was used for this purpose, comparing the efficiency of the base case conditions, i.e., 200 droplets
and 2.89 × 107 kg/s of oil at inlet flow stream with the efficiency obtained for ±20% variations of both parame-
ters. Table 5 shows the comparison.
Results of sensitivity analysis demonstrate the low dependence of the predicted numerical results with respect
to a moderately larger or smaller number of droplets and mass flowrate through the inlet of the catch can. In
Table 5. Sensitivity of CFD results to droplets flow and size.
Configuration Number of droplets at inlet stream
Xo = 80 mm, Yo = 17.75 mm 160 (80%) 200 (100%) 240 (120%)
Oil mass flow
120% (3.468 × 107 kg/s) 0.645
100% (2.89 × 107 kg/s) 0.644 0.645 0.650
80% (2.312 × 107 kg/s) 0.645
Figure 10. Efficiency against height of inner tube (x) and position of the outlet tube (y).
A. Abilgaziyev et al.
259
essence, the larger the amount of oil introduced in the catch can, the larger the amount of oil captured, at least
within the 20% range variation around the level of oil inflow used for the optimization analysis. For that range
variation, indeed, the predicted efficiency did not change more than 1%, supporting the robustness of the design
obtained from the optimization analysis.
7. Concluding Remarks
A classical design of OCC is here optimized using CFD techniques and a Multivariable Nonlinear Regression
Analysis to build a surrogate function which afterwards permits to maximize the droplet collection efficiency
based on length of inner tube, x, and location of outlet tube respect to radial position, y. The results show that the
efficiency is higher when the outlet is located tangentially to the can. Moreover, it is observed that more droplets
are absorbed when the longer-inner-tube configuration is used, reaffirming the fact that the flow has more direct
impact on walls and particles are more likely to get captured by walls leading again to a higher efficiency.
However, caution should be paid since the closer the inner tube is to the OCC bottom, the larger the potential
erosion and abrasion might be. This particular potentially negative effect deserves further study.
Acknowledgements
We would like to acknowledge the support of the School of Engineering at Nazarbayev University for giving us
open access to its computer laboratory.
References
[1] Digsy (2005) Blow-By Breather SystemsPart One. [Online].
http://www.106rallye.co.uk/members/dynofiend/breathersystems.pdf
[2] AutoZone (n.d.) Schematic of the Positive Crankshaft Ventilation (PCV) System Air Flow in V6 and V8 Engines.
[Online].
http://www.autozone.com/repairinfo/repairguide/repairGuideContent.jsp?pageId=0900c1528007db66
[3] Filter Manufactures Council (n.d.) Positive Crankcase Ventilation. Technical Bulletin 94-2R1, Motor & Equipment
Manufacturers Association, Washington DC. [Online].
http://www.baldwinfilter.com/literature/english/10%20TSB's/94-2R1.pdf
[4] Ding, G. (2011) Study on Extenics Information Fusion Method. International Journal of Engineering and Manufac-
turing, 1, 13-19. http://dx.doi.org/10.5815/ijem.2011.01.03
[5] Bhatt, E.V. (2013) 4-Stroke Engine. [Online]. http://www.makingdifferent.com/2-stroke-engine-and-4-stroke-engine/
[6] Bolduc, J., Wentworth, F., Matthew, D. and Mackenzie, D. (2013) Oil-Air Vapor Separator. Capstone Project, Univer-
sity of Maine, Orono.
[7] Bowman, C. (n.d.) 1999-2004 Mustang Catch Can Uses & Explanations. [Online].
http://www.americanmuscle.com/94-catch-me-if-you-can-99-04-mustangs.html
[8] Michael, J. (2013) Oil Catch CansWhat You Should KnowHow They Work. The Torque Post. [Online].
https://torquepost.wordpress.com/2013/05/06/oil-catch-cans-what-you-should-know-how-the-work
[9] Mishimoto (2013) Mishimoto Baffled Oil Catch Can. Technical Spec, Mishimoto Research and Development, New
Castle. [Online]. http://www.mishimoto.com/mishimoto-baffled-oil-catch-can.html
[10] Henderson, C.B. (1976) Drag Coefficients of Spheres in Continuum and Rarefied Flows. AIAA Journal, 14, 707-708.
http://dx.doi.org/10.2514/3.61409
[11] Carlson, D.J. and Hoglund, R.F. (1964) Particle Drag and Heat Transfer in Rocket Nozzles. AIAA Journal, 2, 1980-
1984. http://dx.doi.org/10.2514/3.2714
[12] Vann, D.L. (1997) Crankcase Breating. [Online]
http://nortonownersclub.org/support/technical-support-commando/crankcase-breathing
[13] Ha, D. (2015) Pressure and Temperature Behavior in the Combustion Chamber of a 4-Stroke Engine. [Online]
http://www-mat.ee.tu-berlin.de/research/sic_sens/sic_sen3.htm
[14] Oil Catch Cans. What Are PCV Oil Catch Cans? Accessed on 16 April 2014. http://oilcatchcan.com/
[15] Nabi, N., Akhter, S. and Rahman, A. (2013) Waste Transformer Oil as an Alternative Fuel for Diesel Engine. Procedia
Engineering, 56, 401-406. http://dx.doi.org/10.1016/j.proeng.2013.03.139
[16] Lam, S.S., Russell, A.D., Lee, C.L., Lam, S.K. and Chase, H.A. (2012) Production of Hydrogen and Light Hydrocar-
A. Abilgaziyev et al.
260
bons as a Potential Gaseous Fuel from Microwave-Heated Pyrolysis of Waste Automotive Engine Oil. International
Journal of Hydrogen Energy, 30, 5011-5021. http://www.sciencedirect.com
http://dx.doi.org/10.1016/j.ijhydene.2011.12.016
[17] Newagemuscle2010ss (2014) Elite Engineering Catch Can. Results @ 1500 Miles. [Online Video]
https://www.youtube.com/watch?v=JHol59_IeV4
[18] Guilford, G. (2014) A Big Reason Beijing Is Polluted: The Average Car Goes 7.5 Miles Per Hour. Quartz. [Online]
http://qz.com/163178/a-big-reason-beijing-is-polluted-the-average-car-goes-7-5-miles-per-hour/
[19] Smith, B.J. and Holness, M.H. (2005) Oil Mist Detection in the Atmosphere of the Machine Rooms. Marine Propul-
sion Conference. Bilbao, January 2005. http://www.oilmist.com/bilbao-paper.pdf
[20] Roache, P.J. (1998) Technical Reference of Computational Fluid Dynamics. Hermosa Publishers, Albuquerque.
[21] Hirsch, C. (1988) Numerical Computation of Internal and External Flows. John Wiley and Sons, Chichester.
[22] Glowinski, R. and Tallec, P.L. (1989) Augmented Lagrangian Methods and Operator-Splitting Methods in Nonlinear
Mechanics. SIAM, Philadelphia.
[23] Marchuk, G.I. (1982) Methods of Numerical Mathematics. Springer-Verlag, Berlin.
[24] Samarskii, A.A. (1989) Theory of Difference Schemes. Nauka, Moscow. (In Russian)
[25] Patankar, S.V. (1980) Numerical Heat Transfer and Fluid Flow. Hemisphere, Washington DC.
[26] Saad, Y. (1996) Iterative Methods for Sparse Linear Systems. PWS Publishing Company, Boston.
[27] Dassault Systemes (2013) Technical Reference. SolidWorks Flow Simulation 2013. (2-82-2-88).
[28] Dassault Systemes (2013) Technical Reference. SolidWorks Flow Simulation 2013. (2-17-2-22).
Nomenclatures
Cb: constant of the turbulent model
fµ: turbulence damping factor
gi: gravity vector
h: enthalpy
k: specific turbulent kinetic energy
p: static pressure
Pr: Prandtl number
R: specific gas constant
Si: gravity force per unit volume
T: static temperature
t: time
ui, uj, uk: velocity components in x, y and z directions, respectively
α: thermal diffusivity
γ: specific ratio
βij: Kronecker’s delta function
ε: turbulent energy dissipation rate
µ: dynamic viscosity
µt: turbulent eddy viscosity
ρ: density
τij: shear stress tensor
A. Abilgaziyev et al.
261
Appendices
Appendix I
(a) (b) (c)
(d) (e) (f)
(g) (h) (i) (j)
Figure A1. Trajectory lines of particles of initial 9 chosen oil catch cans: (a) Xo = 30 mm, Yo = 0 mm; (b) Xo = 30 mm, Yo =
17.75 mm; (c) Xo = 30 mm, Yo = 35.5 mm; (d) Xo = 80 mm, Yo = 0 mm; (e) Xo = 80 mm, Yo = 17.75 mm; (f) Xo = 80 mm, Yo
= 35.5 mm; (g) Xo = 130 mm, Yo = 0 mm; (h) Xo = 130 mm, Yo = 17.75 mm; (i) Xo = 130 mm, Yo = 35.5 mm; (j) Numerical
contour scale.
A. Abilgaziyev et al.
262
Appendix II
(a) (b) (c)
(d) (e) (f)
(g) (h) (i) (j)
Figure A2. Pressure contours of initial 9 chosen oil catch cans on YZ plane: (a) Xo = 30 mm, Yo = 0 mm; (b) Xo = 30 mm, Yo
= 17.75 mm; (c) Xo = 30 mm, Yo = 35.5 mm; (d) Xo = 80 mm, Yo = 0 mm; (e) Xo = 80 mm, Yo = 17.75 mm; (f) Xo = 80 mm,
Yo = 35.5 mm; (g) Xo = 130 mm, Yo = 0 mm; (h) Xo = 130 mm, Yo = 17.75 mm; (i) Xo = 130 mm, Yo = 35.5 mm; (j) Numeri-
cal contour scale.
... The intersection of these planes defines the set of rectangular cells that form the base mesh. In the next stage of the process, the geometry inside the computational domain, i.e., the PAT system, is captured [16]. The program crosses the mesh cells sequentially and for each cell it parses the geometrical configuration inside the cell. ...
... Additionally, the refinement level of the cell is the number of times it has been refined relative to the initial cell in the base mesh. In SolidWorks Flow Simulation the maximum number of refinement levels is limited to seven, so that the smallest cell size is 1/128 of the original cell in the base mesh (level 0) [16]. ...
... To ensure a proper and acceptable accuracy of the results, the discretization mesh undergo a Mesh Sensitivity Analysis (MSA), in which the density of cells is gradually increased and the solution must be re-assessed until results demonstrate sufficient independence on the mesh size [16]. The discretization of the mesh was performed by assuming an initial coarse mesh with the total number of cells equal to 25,668, followed by a mesh refinement process. ...
Article
Full-text available
Velocity profiles originated by a pump as turbine (PAT) were measured using an ultrasonic doppler velocimetry (UDV). PAT behavior is influenced by the velocity data. The effect of the rotational speed and the associated flow velocity variations were investigated. This research focuses, particularly, on the velocity profiles achieved for different rotational speeds and discharge values along the impeller since that is where the available hydraulic power is transformed into the mechanical power. Comparisons were made between experimental test results and computational fluid dynamics (CFD) simulations. The used CFD model was calibrated and validated using the same conditions as the experimental facility. The numerical simulations showed good approximation with the velocity measurements for different cross-sections along the PAT system. The application of this CFD numerical model and experimental tests contributed to better understanding the system behavior and to reach the best efficiency operating conditions. Improvements in the knowledge about the hydrodynamic flow behavior associated with the velocity triangles contribute to improvements in the PAT concept and operation.
... The generation of the mesh begins with the definition of a rectangular computational domain automatically built, enclosing the solid body with the orthogonal boundary planes to the specified axes of the Cartesian coordinates system, according to [30]. Following [30], the intersection of these planes defines the set of rectangular cells that creates the base mesh. ...
... The generation of the mesh begins with the definition of a rectangular computational domain automatically built, enclosing the solid body with the orthogonal boundary planes to the specified axes of the Cartesian coordinates system, according to [30]. Following [30], the intersection of these planes defines the set of rectangular cells that creates the base mesh. The software crosses the mesh cells sequentially and for each cell, it parses the geometrical configuration inside the cell, followed by a refinement criterion [30]. ...
... Following [30], the intersection of these planes defines the set of rectangular cells that creates the base mesh. The software crosses the mesh cells sequentially and for each cell, it parses the geometrical configuration inside the cell, followed by a refinement criterion [30]. Hence, for each cell, a refinement value is calculated individually according to an algorithm that controls the type of refinement. ...
Article
Full-text available
Micro-hydro systems can be used as a promising new source of renewable energy generation, requiring a low investment cost of hydraulic, mechanical, and electrical equipment. The improvement of the water management associated with the use of pumps working as turbines (PATs) is a real advantage when the availability of these machines is considered for a wide range of flow rates and heads. Parallel turbomachines can be used to optimize the flow management of the system. In the present study, experimental tests were performed in two equal PATs working in parallel and in single mode. These results were used to calibrate and validate the numerical simulations. The analysis of pressure variation and head losses was evaluated during steady state conditions using different numerical models (1D and 3D). From the 1D model, the installation curve of the system was able to be defined and used to calculate the operating point of the two PATs running in parallel. As for the computational fluid dynamics (CFD) model, intensive analysis was carried out to predict the PATs′ behavior under different flow conditions and to evaluate the different head losses detected within the impellers. The results show system performance differences between two units running in parallel against a single unit, providing a greater operational flow range. The performance in parallel design conditions show a peak efficiency with less shock losses within the impeller. Furthermore, by combining multiple PATs in parallel arrangement, a site’s efficiency increases, covering a wide range of applications from the minimum to the maximum flow rate. The simulated flow rates were in good agreement with the measured data, presenting an average error of 10%.
... An analysis of the development of a liquid film in an upwelling (swirling) flow due to the action of centrifugal and gravitational fields in a cyclone chamber of a distribution system was discussed. The dynamics of the liquid film flow was analyzed with the help of three-dimensional and unsteady numerical simulations, and it was found that the flow fluctuations become smaller when the thickness of the liquid film is small, and the flow becomes homogeneous at the outlet of the device [8]. In gas turbine engine transmission systems, shaft-bearing lubrication and cooling is typically provided by oil injected into bearing chambers sealed by pneumatic labyrinth seals. ...
... It can be confirmed that a vortex was generated on the central axis of the tank and extended to the outflow pipe. device [8]. In gas turbine engine transmission systems, shaft-bearing lubrication and cooling is typically provided by oil injected into bearing chambers sealed by pneumatic labyrinth seals. ...
Article
Full-text available
Abstract The purpose of this study is to improve the gas–liquid separation performance of an oil tank and to establish a design method to enable gas–liquid separation only in an oil tank. Since it is difficult for conventional oil tanks to completely remove bubbles remaining in the hydraulic oil, it is essential to introduce a technology to actively separate and remove bubbles from the oil. Therefore, the bubble removal performance was improved even under the condition of added lateral acceleration by appropriately generating a swirl flow. First, an acrylic model of an oil tank was used to verify the accuracy by performing numerical analysis using various turbulence models. Then, the parameters of the bubble remover, such as the size of the oil tank, were studied. In addition, the bubble removal performance under the condition of added lateral acceleration was examined.
Article
Full-text available
The current study investigates the suitability for using waste transformer oil (WTO) as an alternative fuel for compression ignition (CI) engine. For this purpose different properties of the WTO were determined. The different properties include density, kinematic viscosity, cetane number, calorific value, flash and fire points, fourier transform infra-red (FTIR). The investigation includes two parts. In the first part of the investigation, different properties and engine performance were conducted. In the latter part of the investigation WTO was refined by well know transesterification process and again different fuel properties and engine performance were conducted. In the text, the refined waste transformer oil is designated as RWTO. All fuel properties with WTO and RWTO were compared with those of conventional diesel fuel (DF). All properties were close to those of DF. FTIR results revealed that the WTO is a diesel like hydrocarbon. The engine performance with WTO and RWTO was much better than that of DF. Based on the findings, WTO and RWTO are suggested to be alternative fuels for CI engine.
Article
In this paper, we have studied the traditional Positive Crankcase Ventilation (PCV) valve equipment. Then we have improved the system by adding ventilation equipment. We have applied this kind of connection equipment on gas engine which has no PCV. This can determine the engine fuel-air ratio and make the engine get the best power performance, economical efficiency and emission behavior. Because emission amount is based on input air amount, so how to control the input air amount is the basis of the whole system. On the basis of traditional inlet manifold MVEM, we have considered the affection of PCV system, and we have simulated the actual input air process by getting improved module’s input air amount and inlet manifold pressure parameters. So the fuel-air ratio precision can be increased greatly. We also have prompted some improving directions about traditional inlet manifold. So we can ensure that engine can get a compact structure and good response on the all operation states.
Article
You may be aware MCA and IMO, together with other Societies, are very concerned about the number of fires that start in machine room spaces. Figures produced suggest that up to 65% of machine room fires are the result of oil mist. Now IMO have published a circular No.MSC1086 June 2003 to try and overcome this problem.
Article
Presents introductory skills needed for prediction of heat transfer and fluid flow, using the numerical method based on physical considerations. The author begins by discussing physical phenomena and moves to the concept and practice of the numerical solution. The book concludes with special topics and possible applications of the method.
Article
An empirical expression for the drag coefficient of a spherical particle in flow regimes such as occur in solid propellant rocket exhausts is presented. In these flows, typical particle Mach numbers will be below 2, and particle Reynolds numbers will range from less than 10⁻¹ to greater than 100. Also, available heat-transfer relationships are applied to the gasparticle nozzle flow case. The effects of these relationships on computed particle velocities and temperatures are shown. In the cases considered, inertial and compressibility effects dominate for large particles and high chamber pressures, causing the thermal and velocity lags to be less than those predicted under a Stokes flow assumption. However, for small particles and low chamber pressures, rarefaction effects dominate, and the Stokes flow assumption leads to low estimates of particle lag. © 1964 American Institute of Aeronautics and Astronautics, Inc., All rights reserved.
Article
Preliminaries basic concepts of the theory of difference schemes homogeneous difference schemes difference schemes for elliptic equations different schemes for time-dependent equations with constant coefficients stability theory of differenceschemes symbols concluding remarks.
Article
This patent describes an oil/air separator apparatus. It comprises a cylindrical wall; a first channel wall within the tank, substantially axially aligned with the cylindrical wall, the first channel wall having a bend portion therein, the first channel wall also having a cap portion normal thereto and interconnecting the first channel wall with the cylindrical wall, the first channel wall further having a first end and a second end each of which spaced from the cylindrical wall; a second channel wall within the tank, the cylindrical wall; the second channel wall, the first channel wall being a means for redirecting a first portion of the mixture in the first flow pattern through a second passageway, separated from the first passageway and into a second flow pattern separated from the means for admitting and separated from the cylindrical wall, and for redirecting a second portion of the mixture in the first flow pattern through the second passageway and into a third flow pattern separated from the means for admitting and adjacent the cylindrical wall.