CFD modelling for parametric investigation of flow through the inlet valve of a four-stroke engine.
As the development of Internal Combustion (IC) engines is more and more driven by emission regulations, an improved understanding of the thermo and fluid dynamics of the in-cylinder processes is becoming increasingly important. The in-cylinder flows of internal combustion engines are highly turbulent and are subject to density variation, separation, recirculation and stagnation. The complexity of engine flows presents a challenge to engine modelers. The inlet charge mass controls the combustion process that in turn depends on the inlet port and valve configuration.
A number of studies indicating the search for optimum intake valve configuration have been carried out using hot wire anemometry and Laser-Doppler anemometry. But because of the restrictions such as the interference of probes for hot wire anemometry and limitations for optical access for LDA, and point wise result of these techniques make it difficult at the flow restriction area. Andreas Maier, Terry H. Sheldrake and Dennis Wilcock [1,2] using an axisymmetric inlet port assembly model with scaled up dimensions under steady flow conditions have carried out investigations inside the port.
In the present work, single cylinder constant speed production engine configurations have been used. The flow through the inlet valve discharges into the cylinder as a jet that separates from the seating faces of valve and seat for specific lift conditions . Such areas of flow separation have to be reduced for optimum volumetric efficiency. The inlet valve discharges into the cylinder sometimes separating from the seating face producing velocity gradients, which are detrimental to the volumetric efficiency of the engine. This paper identifies the sensitivity of the inlet valve geometry to the flow characteristics through CFD that has evolved as a "third approach" synergistically complementing the pure theoretical and computational approach . For the computational domain, a two-valve geometry model without dwell is considered. The inlet valve configuration at various lift conditions and parametric changes have been analyzed and brought out. However this simulation with identical boundary conditions can be applied to any four-stroke CI engine.
The flow separation regions and the occurrence of different flow patterns in axisymmetric models have been previously identified in a number of investigations [3,5]. Based on the literature survey, three flow regimes:
Low lift regime (L/D = 0.05)
Intermediate lift (L/D = 0.12) and
Maximum lift regime (L/D = 0.24) was considered for the study (Fig 1).
[FIGURE 1 OMITTED]
Valve Geometry Model
The valve geometries selected are from production engines with the following specification (Fig 2).
Engine and Computational Details Model 1 Engine Type : Kirloskar Bore : 87.5 mm Stroke : 110 mm Compression ratio : 17.5:1 Rated speed : 1800 rpm Power at rated speed : 5.9 kW Diameter of the inlet valve (mm) : 34 Model 2 Engine Type : Field Marshal Bore : 114.3 mm Stroke : 139.7mm Compression ratio : 16:1 Power at rated speed : 7.35 kW Rated speed : 1000 rpm Diameter of the inlet valve (mm) : 36
[FIGURE 2 OMITTED]
The valve opening and closing were taken to be 20[degrees] before TDC and 40[degrees] after BDC. The lift to diameter ratios were calculated and found that both had the same value of 0.235. The parametric investigation had to be carried out on a relevant range to cover the practical inlet valve designs and hence the following combinations were selected. The three influential parameters, seat angle (30[degrees], 35[degrees], 45[degrees]), cone angle (0[degrees], 10[degrees], 20[degrees]) and fillet radius to diameter ratio (0.2, 0.3) were varied and the combinations were analyzed. This resulted in analyzing eighteen models at three different flow regimes, low, intermediate and high for the parametric study.
Based on the available realistic valve profile, the ramp and main lift parameters were fixed for simulation . The ramp lift as considered being fifty percent of the total lift and the dwell period was considered to be absent.
The Computer Code
CFD codes are structured around the numerical algorithms that can tackle fluid flow problems. The computer software code used for solving the conservation equations for mass, momentum and energy is Fluent 6.2.18 which is control volume based on finite difference method . Ideal gas law is used for density calculations. In this study, RNG k-[epsilon] turbulence model derived by Yakhot and Orszag (1986)  capable of accounting for flow compressibility is used. The RNG k-[epsilon]model is derived using a rigorous statistical technique called renormalization group theory. It is similar to the two-equation model k-[epsilon]in which the solution of two separate transport equations, permit the turbulent velocity and length scales to be independently determined. It has the following refinements over the standard k-[epsilon]model .
* The RNG model has an additional term in its [epsilon]-equation that significantly improves the accuracy for rapidly strained flows
* The effects of swirl on turbulence is included in the RNG model enhancing accuracy for swirling flows
* The RNG theory provides an analytical formula for turbulent prandtl numbers and it also provides an analytically derived differential formula for effective viscosity that accounts for low Reynolds effects.
Compared to the k-[epsilon]model, the k-equation remains the same in the RNG version. However an extra term R appears in the [epsilon]-equation. R is small for weakly strained turbulence, such as a homogenous shear flow, and is large in the rapid distortion limit when [eta] approaches infinity. This feature of the RNG k-[epsilon] model makes it capable of modelling separated flows.
Transport Equations for the RNG k-[epsilon] Model
[MATHEMATICAL EXPRESSION NOT REPRODUCIBLE IN ASCII]
R = [v.sub.T] [S.sup.3] (1 - [eta]/[[eta].sub.0])/1 + [beta][[eta].sup.3]
and [eta] = S [bar.k]/[bar.[epsilon]] is the ratio of the turbulent to mean strain-time scale, S = [square root of (2 [S.sub.ij] [S.sub.ij])] is the magnitude of the mean strain [S.sub.ij] = 1/2 ([partial derivative][bar.[u.sub.i]/[partial derivative][x.sub.j] + [partial derivative][bar.[u.sub.j]/[partial derivative][x.sub.i]) and v = [v.sub.0] + [v.sub.T]. The model constants are given as [C.sub.[mu]] = 0.0845, [C.sub.1] = 1.42, [C.sub.2]=1.68, [[alpha].sub.k] = [[alpha].sub.[epsilon]] = 1.39, [[eta].sub.0] = 4.38 and [beta] = 0.012.
The above model was used in order to overcome the problems faced by J.C. Dent  such as underestimation of turbulence dissipation rate near the walls and the standard k-[epsilon]turbulence model not responding to adverse pressure gradients. A turbulence intensity of 4% and a length scale of 17% of the inlet valve diameter were specified for turbulent kinetic energy k and its dissipation rate [epsilon].
The equations are solved using PISO algorithm with second order upwind differencing scheme. The valve and the required engine configurations were modeled with IDEAS software and then imported to fluent. Meshing was carried out with GAMBIT, the preprocessor and boundary conditions were initialized and solved with Fluent.
In order to solve the governing equations numerically, approximations to the partial differential equations were introduced. In the finite volume approach, flux balance forms are obtained by integrating the governing equations over discrete sub domains. Replacing derivatives by differential expressions in turn approximates the fluxes. The resulting approximate algebraic equations are subsequently solved for all the discrete sub domains. Such a process of creating discrete sub domains are called Grid generation. It could essentially be a structured or unstructured one.
For this study, the governing equations are discretized on an unstructured TGrid (Fig. 3). TGrid mesh consists primarily of tetrahedral mesh elements. However they may also contain hexahedral, pyramidal and wedge mesh elements too. Highly concentrated grid cells were located at the vicinity of the valve.
The 3-D mesh was built and it comprised of 1,79,886 grid cells. This was arrived at after performing grid sensitivity tests, by increasing the number of cells in steps of order of 20%. The grid count at which the results were the same except for the time taken for convergence was identified and considered for analysis. Hence a grid independent mesh model was established.
[FIGURE 3 OMITTED]
The boundary conditions used for this study are as mentioned below:
The boundary condition used here is the pressure inlet condition normal to the boundary. The stagnation temperature of 300 K is considered. Velocity is computed for each face in that zone, and this velocity is used to compute the fluxes of all relevant solution variables into the domain.
In any flow, the Reynolds number of flow becomes very low and turbulent fluctuations are dampened considerably near the walls. Due to this, the laminar viscosity starts to play a significant role. In this case walls are assumed to be adiabatic.
Turbulent flows are significantly affected by the presence of walls. The near-wall modeling significantly impacts the fidelity of numerical solutions, in as much as walls are the main source of mean vorticity and turbulence. After all, it is in the near-wall region that the solution variables have large gradients, and the momentum and other scalar transports occur most vigorously. Therefore, accurate representation of the flow in the near-wall region determines successful predictions of wall-bounded turbulent flows
The Enhanced wall treatment, a near-wall modeling method that combines a two-layer model with enhanced wall functions is used. The viscosity-affected near-wall region is completely resolved all the way to the viscous sub-layer. The entire domain is subdivided into a viscosity-affected region and a fully turbulent region. The demarcation of the two regions is determined by a wall-distance-based, turbulent Reynolds number, [Re.sub.y], defined as [Re.sub.y] = [rho]y[square root of (k)/[mu] where y is the normal distance from the wall at the cell centers.
Near-wall mesh fine enough to be able to resolve the laminar sub layer are used since in- cylinder flows are complex involving separation, reattachment, and impingement where the mean flow and turbulence are subjected to severe pressure gradients and change rapidly.
Pressure outlet boundary conditions are applied with specification of an exit plane at the piston cylinder. Normal gradients at the outflow surface are taken to be zero.
Dynamic Mesh Modeling
In prismatic mesh zones, dynamic layering is carried out to add or remove layers of cells adjacent to a moving boundary, based on the height of the layer adjacent to the moving surface. In the dynamic mesh model [Fig. 4] an ideal layer height is specified on each moving boundary. The layer of cells adjacent to the moving boundary (layer j) is split or merged with the layer of cells next to it based on the height (h) of the cells in layer j.
[FIGURE 4 OMITTED]
If the cells in layer j are expanding, the cell heights are allowed to increase until [h.sub.min] > (1 + [[alpha].sub.s][h.sub.ideal] where [h.sub.min] is the minimum cell height of cell layer j, [h.sub.ideal] is the ideal cell height, and [[alpha].sub.s] is the layer split factor. When this condition is met, the cells are split based on the specified layering option of either constant height or constant ratio. With the constant height option, the cells are split to create a layer of cells with constant height [h.sub.ideal] and a layer of cells of height ideal h - [h.sub.ideal]. If the cells in layer j are being compressed, they can be compressed until [h.sub.min] < [[alpha].sub.c] [h.sub.ideal] where [[alpha].sub.c] is the layer collapse factor. When this condition is satisfied, the compressed layer of cells is merged into the layer of cells above the compressed layer; i.e., the cells in layer j are merged with those in layer i.
The valve profile was plotted and the instantaneous piston location was calculated as a function of crank angle given by
[P.sub.l] = l + A/2 (1 - cos([[theta].sub.c])) - [square root of ([l.sup.2] - [A.sup.2/4 [sin.sup.2]([[theta].sub.c]))]
Results and Discussion
The influence of the combination of the geometric parameters such as seat angle and cone angle to valve diameter ratio on the valve flow characteristics were investigated. Fig. 5 indicates the region of separation at the valve seat. Back flow if present will reduce the volumetric efficiency of the engine since the volume available to the intake charge is less and hence this aspect with respect to the change in the parameters considered was also studied.
[FIGURE 5 OMITTED]
Influence of Valve cone angle
The valve cone angles considered are 0[degrees], 10[degrees] and 20[degrees], which are in the range of practical usage. The discontinuities in flow are represented by change over points in the slope of the mass flow rate graph [Fig 6,7,8] when plotted against the valve lift to diameter ratios.
The mass flow rate was calculated for non-dimensional valve lifts ranging from 0.02 to 0.24, which covered the range of practical valve operations for the three cone angles 30[degrees], 35[degrees] and 45[degrees] seat angles. For the 0 deg cone angle, Fig 6 shows a first change in slope at about L/D=0.11 in the plot that shows the variation in the mass flow with valve lift plot. The 10 and 20 deg cone angle continued the effective value of flow rate up to L/D = 0.14. However, the 10 deg cone angle showed an immediate change in slope at L/D= 0.16. This suggests that the flow separated from the valve seat face at L/D=0.14, with the effective flow area remaining constant over a small range of lift. At L/D=0.19, the flow is reattached to the valve face. The results for a 20 deg valve cone angle suggested that the separation process from the valve and seat face was a continuous one in the lift range between L/D=0.125 and 0.16. There is no reattachment seen and this may be a result of increased axial flow momentum induced by a large cone angle. The 0 deg valve cone angle directed the flow in a more radial direction and produced the largest separation area from the valve face.
The cone angle of the valve affected the flow characteristic over the full range of lifts. A large cone angle, which directed the flow in an axial direction in the low lift region had the opposite effect and caused separation in the medium and higher lift regime.
Therefore a small valve cone angle is advantageous in directing the flow towards the cylinder head, that suppressed flow separation from the seat face and resulted in a superior performance in the medium to higher lift range. This behaviour was consistent for all seat angles investigated in both the models. However, the separation and reattachment effect is significant as the valve seat angle was increased and the flow separation from the valve seat face was most pronounced for large seat angle configurations as seen in Fig. 7 and Fig. 8.
[FIGURE 6 OMITTED]
[FIGURE 7 OMITTED]
[FIGURE 8 OMITTED]
Influence of Fillet Radius
Two fillet radius to diameter ratio's R/D=0.2 and 0.3 were investigated and their influence on the flow behaviour were examined for the various valve seat and valve head configurations. The valve configuration for a 30[degrees] seat angle did not show change in separation area at high and medium lifts with change in fillet radius.
Results for the 35[degrees] seat angle, a small influence was noted in the low lift zone (L/D=0.08) and a larger fillet radius resulted in better performance since it directed the flow in downward direction suppressing the flow separation as seen in Fig. 9 and Fig. 10.
For 0[degrees] cone angle, the effect of fillet radius had showed more influence for the 45[degrees] seat geometry. A large fillet radius resulted in an improved flow performance in the L/D range smaller than 0.05 with the influence almost diminishing in the medium to high lift range 0.10< L/D<0.25. The reasoning is that a large fillet radius did not induce as much radial momentum in the flow as a small fillet radius, resulting in a decreased flow separation from the upper valve face corner as shown in Fig. 11. A reduction in flow velocity was seen at the valve stem-seat area for 0.3 fillet radius to diameter ratio and is shown as Fig. 12.
[FIGURE 9 OMITTED]
[FIGURE 10 OMITTED]
[FIGURE 11 OMITTED]
[FIGURE 12 OMITTED]
Influence of Valve seat angle
The seat angles considered were 30[degrees], 35[degrees] and 45[degrees] for 0, 10[degrees] and 20[degrees] cone angles. At low lifts, a 30[degrees] seat angle the flow was almost nozzle shaped and showed better performance as compared with other seat geometries. The small separation formed at the upper valve face corner for the 30[degrees] seat geometry decreased as the cone angle increased as seen in Fig. 13 and Fig. 14.
A sudden decrease in flow was experienced at L/D = 0.05 which is caused due to the early flow separation at the seat face. This separation did not reattach and thus resulted in poor performance in the medium to high lift range for this valve configuration as indicated in Fig. 15. The transition of flow occurred from flow regime 1 to flow regime 3. Hence this 30[degrees] valve seat can be used in engines that operate at low lifts for a longer duration. The range of effective operation of the 30[degrees] seat configuration was from L/D=0.01 to L/D=0.05.
For the 35[degrees] seat angle drop in flow parameters were experienced at L/D=0.08 at cone angle 20[degrees]. The occurrence of early flow separation as identified in the 30[degrees] profile was delayed and hence better performance was found as cone angle was increased.
An increase in performance in the medium lift range was observed only for 35[degrees] seat angle geometries having 0[degrees] cone angle. This is because of delayed flow separation from the seat face leading to a significant pressure recovery in the valve passage and higher flow performance. However, the increase in flow was followed by separation at high lifts L/D?0.14, which affected the performance significantly.
The 45[degrees] seat angle valve had a generally inferior performance in the low lift range. All the flow regimes occurred only in the 45[degrees] seat angle with 0[degrees] and 10[degrees] cone angle configurations. The transition from attached to detached flow from the seat face area was delayed in the 10[degrees] valve cone angle from L/D=0.14 for 0[degrees] cone angle to L/D=0.15 as a result of suppressed flow separation from the valve seat face caused by the larger cone angle. The separation at the seat from the valve occurred at L/D= 0.12 and from the seat face in the head occurred at L/D=0.14 and total separation occurred at L/D=0.18 for this valve geometry. The reattachment location on the valve seat face moved in downward direction as the seat angle was increased. Only for the 45[degrees] and 20[degrees] cone angle configuration, the separation and reattachment flow regimes occurred as shown in Fig. 16.
After analyzing various combinations of valve seat cone angles, the 35[degrees] seat angle with a flat valve shoulder i.e. 0[degrees] cone angle was found to exhibit a better flow condition with minimum separation and recirculation at intermediate lifts. Seat angle of 30[degrees] exhibited good flow characteristics in the low lift range.
The reattachment location on the valve seat face moved in the downstream position as the seat angle was increased at higher valve lifts. The variation in seat angle had the most influential effect on the flow of all the three parameters investigated.
The intake flow, on interacting with the cylinder walls and piston produces recirculation zones in the cylinder. These zones when moving close to the valve head also facilitated lesser separation area.
Back flow was found to occur for the engine configuration for all the models [Fig 17]. After analysis, it was found that the model SA 45, CA 20 with Fillet radius to diameter ratio of 0.2 had the maximum occurrence of backflow at 15[degrees] before the inlet valve closes [Fig 18].
[FIGURE 13 OMITTED]
[FIGURE 14 OMITTED]
[FIGURE 15 OMITTED]
[FIGURE 16 OMITTED]
[FIGURE 17 OMITTED]
[FIGURE 18 OMITTED]
The experimental setup is shown in the layout of Fig. 19. The engine selected is a Kirloskar make stationary four-stroke, compression ignition, single cylinder and water-cooled. As the air-fuel ratio is determined by the air and fuel flow measurements. Care has been taken to measure the airflow accurately. A calibrated orifice flow meter is used in combination with a U-Tube manometer. A plenum chamber having sufficient volume was fitted to suppress the air fluctuations, which was of significance. Air-cooled piezoelectric transducers are used for manifold pressure measurement. An optical Crank Angle Marker (CDM), fitted on engine crankshaft gives accurate crank angle position. Care has been taken to match piston top dead center position with the CDM signal for error free triggering. The CDM indicates both TDC position and the crank angle position to an accuracy of 0.05[degrees].
The TDC of the piston is identified by physically checking the movement of the piston with a dial gauge and verified by measuring the motored cylinder peak pressure position. After the engine is stabilized for a particular operating point, airflow is recorded.
The mass flow rate obtained from the experiment and the predicted mass flow rate are compared as shown in Fig. 20. Good agreement at the valve lift profiles was obtained and hence the model can be considered to be valid. The predicted values being higher than the experimental values may be due to heating up of inlet air by the manifold resulted in reduction of the flow rate.
[FIGURE 20 OMITTED]
From the parametric investigation of all the different configurations, we conclude that the
* Cone angle has influence on all the lift regimes
* The fillet radius was found to have the minimum influence for this configuration.
* The seat angle influenced the flow parameters most and proved to be very crucial in deciding the configuration.
* The range of effective operation of the 30 degree seat configuration was from L/D=0.01 to L/D=0.05.
* Maximum back flow occurred in the model with 45 degree seat angle and 20 cone angle with fillet radius to diameter ratio of 0.2
* A valve with seat angle of 35[degrees] and 0[degrees] cone angle improved the performance of the engine in the intermediate lift conditions minimizing separation with better flow conditions.
With geometrical modifications the transition points can be altered leading to improvement in valve flow characteristics and therefore the performance of the inlet port.
PISO--Semi-Implicit method for pressure linked equations. This algorithm was originally put forward by Patankar and Spalding (1972) for calculation of pressure on a staggered grid arrangement.
Nomenclature m - Mass flow rate at inlet B - Bore diameter of cylinder l - Connecting rod length a - Crank radius [D.sub.v] - Valve head diameter Ds - Valve stem diameter [D.sub.p] - Port diameter L - Valve lift [L.sub.t] - Valve lift at choked flow [L.sub.r] - Valve lift at end of ramp R - Valve Fillet Radius [beta] - Valve seat angle [alpha] - Valve cone angle w - Valve seat width [P.sub.l] - Piston location A - Piston stroke [[theta].sub.c] - Instantaneous angle [rho] - Density k - Kinetic energy [mu] - Viscosity
The authors acknowledge Dr. Nedunchezhian and his team, IC Engine Research Cell of Institute of Road Transport Technology, Erode for the experimental assistance rendered.
 Andreas Maier, Terry H. Sheldrake and Dennis Wilcock, "Geometric Parameters Influencing Flow in an Axisymmetric IC Inlet Port Assembly: Part 1--Valve Flow Characteristics", 2000, Transactions of ASME Vol. 122 pp 650-657.
 Andreas Maier, Terry H. Sheldrake and Dennis Wilcock, "Geometric Parameters Influencing Flow in an Axisymmetric IC Inlet Port Assembly : Part 2--Valve Flow Characteristics", 2000, Transactions of ASME Vol. 122 pp 658-665.
 John B. Heywood, Internal Combustion Engines, McGraw Hill International Edition, 1988.
 Franz J. Laimbock, Gerhard Meister and Simon Grilc, "CFD Application in Compact Engine Development", SAE paper 98016, 1998.
 Kastner, L. J., Williams, T.J., and White, J.B., "Poppet Inlet Valve Characteristics and their Influence on the Induction Process," Proceeding of Inst. Mech. Engg. 178, Part 1, 1963-64, No.36, p 955-975.
 Gordon P. Blair, " Design and Simulation of a Four Stroke Engines, SAE Publications, 1999.
 Fluent 6 Manuals, Fluent Incorporated, 2002.
 Z. Han and R.D. Reitz, Engine Research Center, University of Wisconsin-Madison, " Turbulence Modeling of Internal Combustion Engines using RNG k-[epsilon]Turbulence Modeling
 Pierre Godrie and Mark Zellat, "Simulation of Flow Field Generated by Intake Port-Valve-Cylinder configurations-Comparison with Measurements and Applications" SAE paper 940521, 1994.
 J.C. Dent and A.Chen, "An Investigation of Steady Flow through a Curved Inlet Port", SAE paper 940522, 1994.
(1) S. Thirumalini, (2) C. Lakshmikanthan and (3) S. Dhandapani
(1,2) Amrita School of Engineering
(3) Dr. N.G.P Institute of Technology
|Printer friendly Cite/link Email Feedback|
|Author:||Thirumalini, S.; Lakshmikanthan, C.; Dhandapani, S.|
|Publication:||International Journal of Applied Engineering Research|
|Date:||Jul 1, 2009|
|Previous Article:||Locating partially captured objects for eye-in-hand-robot systems.|
|Next Article:||Experimental studies in a single cylinder diesel engine using palm oil as alternate fuel.|