Exhaust Port Challenge

CFD analysis of exhaust port

Aim:-

To perform a CFD analysis on exhaust port to analysis the wall and surface heat transfer coefficient. Then evaluate velocity and temperature profile to predict the area of maximum velocity and heat transfer.

Introduction:-

The design of exhaust manifolds has been developed for many years. As engines have been improved so have exhaust port. Exhaust port is a part of IC engines, its role is to collect and carry the exhaust gases away from the cylinder head and send it to the exhaust system, with a minimum of back pressure. The exhaust manifold plays an important role in the performance of an engine system. Particularly, the efficiencies of emission and fuel consumption are closely related to the performance of exhaust manifold. Exhaust Manifolds are affected by thermal stresses and deformations due the temperature distribution, heat accumulation or dissipation and other related thermal characteristics.

The exhaust port is one of the most critical component in engine it able to influence the gas exchange process in several aspects, like the piston work during the exhaust stroke, the short-circuit of fresh charge from the intake into the exhaust and even the filling of the cylinder. In this sense, the most influential boundary condition imposed by the manifold is the pressure at the valve and especially the instantaneous pressure evolution. The mean backpressure is determined mainly by the singular elements, such as the turbine, the catalytic converter and the silencer.

Special interest must be given to the back pressure parameter. Back pressure is an undesired effect because as the back pressure increases so does the amount of residuals left in the head. The increase in weight of residuals will decrease the volume of the fresh charge, in turn increasing the temperature at the beginning of compression as well. Several experiments show how the increase in back pressure influences the thermal efficiency for different induction manifold pressures.

Theory:-

The functioning of exhaust manifold is complex and is dependent on many parameters viz. back pressure, exhaust velocity, scavenging etc. An exhaust manifold collects the exhaust gases from multiple cylinders into one pipe. It is attached downstream of the engine and is major relevance in multi‐ cylinder engines where there are multiple exhaust streams that have to be collected into a single pipe. When an engine starts its exhaust stroke, the piston moves up the cylinder bore, decreasing the total chamber volume. When the exhaust valve opens, the high pressure exhaust gas escapes into the exhaust manifold or header, creating an exhaust pulse comprising three main parts. The high pressure head is created by the large pressure difference between the exhaust in the combustion chamber and the atmospheric pressure outside of the exhaust system. As the exhaust gases equalize between the combustion chamber and the atmosphere, the difference in pressure decreases and the exhaust velocity decreases. This forms the medium‐pressure body component of exhaust pulse. The remaining exhaust gas forms the low pressure tail component. This tail component may initially match ambient atmospheric pressure, but the momentum of the high and medium pressure components reduces the pressure in the combustion chamber to a lower than atmospheric level . This relatively low pressure

helps to extract all the combustion products from the cylinder and induct the intake charge during the overlap period when both intake and exhaust valves are partially open. The effect is known as scavenging. Length, cross‐sectional area, and shaping of the exhaust ports and pipe works influences the degree of scavenging effect.

Back pressure usually refers to the pressure exerted on a moving fluid by obstructions against its direction of flow. Back pressure caused by the exhaust system of an automotive engine has a negative effect on engine’s performance as it will restrict the flow rate of the exhaust gasses. The result would be the engine not being able to expel the spent exhaust gasses fast enough to prevent spent exhaust gasses from contaminating the fresh air/fuel mixture that is drawn into the engine on the next intake stroke. Ultimately, this will result in reduced engine power.

The reciprocating engine causes the air-flow in the exhaust manifold to oscillate with a frequency that is a multiple of the engine speed, as a result of the oscillating air-flow the pressure in the exhaust manifold will also oscillate. The exhaust manifold pressure is a crucial variable for an IC engine, affecting the torque production and the emissions through variations in the EGR mass flow and in the residual mass fraction in the cylinder. Also it is a complex system subjected to thermo-mechanical loads. The analysis of such a system is critical due to the complexity of meeting the structural and flow requirements. The use of Computational Fluid Dynamics (CFD) and Finite element analysis (FEA) are inevitable tools to achieve this. In present case we use a Fluent software by ANSYS version 2019R3.

Conjugate heat transfer:-

The term conjugate heat transfer (CHT) is used to describe the processes which involve variations of temperature within solids and fluids due to thermal interaction between the solid and fluids. The exchange of thermal energy between the two physical bodies is called study of heat transfer, the rate of transferred heat is directly proportional to the temperature difference between the bodies. Conjugate heat transfer corresponds with the combination of heat transfer in solids and heat transfer in fluids. In solids, conduction often dominates. Efficiently combining heat transfer in fluid and solids is the key to designing effective coolers, heaters, or heat exchangers. Forced convection is the most common way to achieve high heat transfer rate. In some application the performance are further improved by combining convection with phase change.

Modelling Methodology:-

Exhaust port model is developed in Ansys Spaceclaim. External geometry file is imported in Spaceclaim and then we generate a fluid volume inside port as shows in Figure 1.To implement a interference between fluid and solid volume during meshing operation we have to form a new component in Spaceclaim then edit geometry to remove extra edges. After geometry clean up use share topology option to share the inference connection between sold and fluid volume as shows in Figure 2. In work bench drop down menu select Share to apply the interference.

Figure 1, Imported geometry Figure 2, Spaceclaim fluid volume extract

Then the geometry is updated to Fluent mesh as shows in Figure 3. In meshing we choose a tetrahedral mesh with sizing up to 100mm in global setting. To evaluate a Surface heat transfer coefficient we have to provide more than one cell along thickness of exhaust port. For this we choose a body sizing with 10 mm. To implement the near wall treatment we have to provide a Inflation layer at the fluid volume ,so we created a inflation layer with first cell height of 0.04 mm and growth rate of 1.2 and number of layer is set to 8 to smoothly trainsets to outer surface as shows in Figure 4 and 5. The Y + value is selected as on bases of initial guess then after completing simulation we can verify the value. Here we first assume its value to be 0.5 because we are using K- omega SST turbulence model and in this model Y+ value must be below 1. We can calculate first cell height by using any online Y+ value calculator. In our present case we get a value of 0.04 mm. Boundaries are named in meshing as shows in Figure 6 .

Figure 3, Meshed Geometry

Figure 4, Inflation layer on fluid volume Figure 5, 8 Inflation layer

Figure 6, Boundary name selection

Solver setting:-

In ANSYS Fluent we choose a pressure based solver with steady state condition. In model we turn on the energy equation to calculate temperature. For turbulence modelling we choose a K- omega SST model because it is good for adverse pressure gradient and separation flow , its more reliable model Air will be the working fluid considered to be operating at 700K. All property of fluid remains the same as for air . for solid we choose a aluminium from fluent database and its property remains the same as shown in Table 1..

Table-1: Properties of material

Property	Air	Aluminium
Density (kg/m3)	1.112	2917
Viscosity (KG/m-s)	1.7894e-05	-
Specific heat (J/kg-K)	1006.43	871
Thermal conductivity (W/m-K)	0.0242	202.4

The inlet boundary condition will be velocity inlet at velocity of 5 m/s , and inlet temperature will be 700 K. Turbulence intensity is 5% and turbulence viscosity ratio is 10. For outlet pressure outlet condition is chose at gauge pressure 0 pascal. From outlet wall of exhaust port the heat is carried out by convection mode of heat transfer for this we select outer wall thermal condition as convection with heat transfer coefficient (w/m2-k) equal to 20 and free stream temperature 300K. for inner solid wall it is stationary with no slip condition and thermal condition as couplet which means we need to calculate that region temperature. Scheme is Coupled with pressure and momentum be second order upwind. Solution will in initialized in Hybrid condition and simulation is conducted for 600 Iterations.

Dependency of solution on the grid size:-

The mesh size often has an impact on the accuracy of the solution. The size has to be small enough in order to properly resolve the fields that are solved for. To quantitatively compare the result with three different sizes.. The number of element used are tabulated in table 2

Table-2: Mesh dependency

S.NO	Mesh type	Number of element	Surface heat transfer coefficient (w/m2-k)	Wall adjacent heat transfer coefficient (w/m2-k)
1	Fine	945830	21.1368	1031.764
2	Medium	336369	21.1135	1034.429
3	Course	241829	21.1164	1035.750

From the above data its is clear that when we choose a base line mesh of element number 241829 we get surface heat transfer coefficient value of 21.1164 and its value change in minute size if we move up to element size of 336369 but value of wall adjacent heat transfer coefficient is change from 1035.750 to 1034.429 over a difference of 1.321 and this trend is continuous to show if refine our mesh size up to element size 945830 then we get a value of 1031.764 then we get a difference of 2.664 and its significant improvement so we choose a fine mesh size of number of element size 945830 for all calculation. By choosing a fine mesh size it takes nearly as double time than medium to complete the simulation but for accuracy we have to choose a fine size because it shows a significant difference in heat transfer coefficient value.

Results And Discussions :-

The results obtained by CFD simulations are displayed with the help of velocity and temperature contours. Convergence plot as shown in Figure 7, we can sure that solution is successfully converge and we can validate our result. all variables in convergence plot first start to decrease and then oscillate but after some time or when it cross 500 iteration its oscillation amplitude decrease and become more constant and then there be no drastic change in its value from that we can conclude that our simulation has reaches in steady state so we can stop calculation and go for validating result. From Figure 8, it shows the temperature profile on outer wall of exhaust port here we can see that at inlet a high temperature exhaust gas as enter in port, wall absorb heat from gas and wall begins to heat for end pipe the temperature is drop at bend or curvature and for mid pipes the temperature decrease from inlet to the region where the intersection comes. When all the gases from different inlet reach the intersection zone of exhaust pipe the temperature reaches to higher value because all hot gases combine here at exhaust pipe the temperature is very high hence the temperature of exhaust pipe wall intersect section is 553 K .as gas flow ,its continuous to heat exhaust port and wall temperature is highest at the end at 580K.same is also for inner surface of exhaust port as shown in Figure 9.

Figure 7, Convergence plot

Figure 8, Temperature on outer wall of port Figure 9, Temperature on inner wall of port

Streamline velocity profile is shown in Figure 10 . From the figure it is clear that velocity is continuous to increase from inlet to outlet and when it reaches at the outlet pie intersection its velocity increase from 9.96 m/s to 19.96 m/s. but if we look at the Figure 11, its shows the velocity is greatest at the curvature of the outlet pipe. We know the heat transfer occur more at region where the velocity is highest and from Figure 11,it shows that velocity is highest at the outlet section ,hence heat transfer is maximum at this region also. We can validate it by selecting the wall heat transfer coefficient at the outlet pipe mid plane as shown in Figure 12, it shows wall heat transfer coefficient value 1116.27 (w/m2-k^-1) and it will be maximum at region where the velocity is highest means at outlet pipe curvature region.

Figure 10, Velocity streamline Figure 11, Velocity profile on outlet pipe

Figure 12, Wall heat transfer coeffiicent on outlet pipe mid plane

We choose a K- omega SST model so we have to verify our first Y+ value for that we have to check for Y+ value calculated by fluent and compare its value what we have assumed as shows in Figure 13 and 14. So for this case we have chosen Y+ value of 0.5 and from figure its seems that our value lies in the limit so we can implement this turbulence model for present case.

Figure 13, Y+ value Plot

Figure 14, Y + value contour

Conclusion:-

The flow analysis of exhaust port was performed. As the hot flue gas entered in exhaust pipe with high temperature it is economical to reduce its temperature before it reaches at outlet , heat transfer through the wall is more suited for this purpose . from the above displayed result we can conclude that as the velocity increase the heat transfer tare is also increase and the region where there is maximum velocity heat transfer is also highest at that point. The region is at the curvature of outlet pipe. On inner surface of exhaust port value of Surface heat transfer coefficient is 21.1 (w/m2-k) and Wall adjacent heat transfer coefficient is 1031.76 (w/m2-k). The maximum velocity of flue gases is achieved near the outlet of exhaust port as the pressure at that position is low so the gases rush out of the exit of the duct .The temperature of flue gases in all the cases cools down as the gases proceed towards the outlet of the exhaust port. The parts where the temperature rises are the points of mixing of gases, where the temperature rises due to collision and rubbing among the gas molecules.

.