CONJUGATE HEAT TRANSFER ANALYSIS ON AN EXHAUST PORT OF AN I.C ENGINE USING k-epsilon TURBULENCE MODEL IN ANSYS FLUENT.
PROJECT TITLE: CONJUGATE HEAT TRANSFER ANALYSIS ON AN EXHAUST PORT OF AN I.C ENGINE USING k-epsilon TURBULENCE MODEL IN ANSYS FLUENT.
OBJECTIVE:
- Give a brief description of why and where a CHT analysis is used.
- Perform a CHT analysis on a model of an exhaust manifold. Compare the solutions for 2 sizes of meshes. The first one should be the baseline mesh and the second one should have a finer mesh on the solid zone and also with inflation layers. Show the velocity, temperature and heat transfer coefficient plots and explain if refining the mesh produced any changes to the results.
- How would one verify if the HTC predictions from the simulations are right? On what factors does the accuracy of the prediction depend on?
INTRODUCTION: The term conjugate heat transfer (CHT) is used to describe processes which involve variations of temperature within solids and fluids, due to thermal interaction between the solids 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. A typical example is the heating or cooling of a solid object by the flow of air in which it is immersed and some other example includes conduction through solids, free and forced convection in the gases/fluids and thermal radiation.
Fig. 1. Forced Convection CHT in Microprocessor
Fig. 2. CHT in Boiler
Conjugate heat transfer corresponds with the combination of heat transfer in solids and heat transfer in fluids. In solids, conduction often dominates whereas in fluids, convection usually dominates. Efficiently combining heat transfer in fluids 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 applications, the performances are further improved by combining convection with phase change (for example liquid water to vapor phase change).
Heat transfer in solids and heat transfer in fluids are combined in the majority of applications. This is because fluids flow around solids or between solid walls, and because solids are usually immersed in a fluid.
Fig. 3. CHT inside an Inverter
Modes of heat transfer
- Conduction: diffusion of heat due to temperature gradients. A measure of the amount of conduction for a given gradient is the heat conductivity.
- Convection: when heat is carried away by moving fluid. The flow can either be caused by external influences, forced convection; or by buoyancy forces, natural convection. Convective heat transfer is tightly coupled to the fluid flow solution.
- Radiation: transfer of energy by electromagnetic waves between surfaces with different temperatures, separated by a medium that is at least partially transparent to the (infrared) radiation. Radiation is especially important at high temperatures, e.g. during combustion processes, but can also have a measurable effect at room temperatures.
An accurate description of heat transfer modes, material properties, flow regimes, and geometrical configurations enables the analysis of temperature fields and heat transfer.
Typical design problems involve the determination of:
- Overall heat transfer coefficient, e.g. for a car radiator.
- Highest (or lowest) temperature in a system, e.g. in a gas turbine, chemical reaction vessels, food ovens.
- Temperature distribution (related to thermal stress), e.g. in the walls of a spacecraft.
- Temperature response in time dependent heating/cooling problems, e.g. engine cooling, or how fast does a car heat up in the sun and how is it affected by the shape of the windshield?
The fluid flow and heat transfer problems can be tightly coupled through the convection term in the energy equation and when physical properties are temperature dependent. While analytical solutions exist for some simple problems, we must rely on computational methods to solve most industrially relevant applications.
CHT can be performed to improve cooling performance of the water jacket and increase engine life. Advancements in cooling for applications such as gas turbines components require improved understanding of the complex heat transfer mechanisms and the interactions between those mechanisms, which our engineers can perform without hassle. Critical cooling applications often rely on multiple thermal protection techniques, including internal cooling, external film cooling, etc. which are efficiently used by our analysis to cool components and limit the use of coolant. We do extensive support for Motor and Battery CHT Analysis to get optimized design for High voltage systems. Conjugate Heat Transfer analysis provides the temperature distribution in solid and coolant of the engine and clear insight on velocity distribution and mechanism of heat transfer of coolant. Results of CHT analysis become input to structural simulations as thermal loads.
Fig. 4. CHT in an IC Engine
Engine CHT Analysis involves various type of engines like Bikes, Passenger Cars, Racing cars, Commercial Vehicles, Marine, Agricultural equipment and Earth-moving equipment etc. CHT analysis thus helps to visually see how fluids interact with solids and how energy is transferred from one state of matter to another. It also aids material selection as induced thermal stresses are a major problem in the scenarios stated above.
- Inlets - All the four faces from where the exhaust gases from each cylinder will come out.
- Outlet - Exhaust pipe which will be dumping the gases into the atmosphere.
- Outer wall convection - Heat transfer from the hot fluid inside to the manifold body.
Fig. 8. Flagged Boundary Conditions
Mesh is generated to get the Baseline Meshing and checked for quality. This configuration is used for getting the Baseline results while another meshing configuration(refined) is also used for obtaining the results and comparing it with the baseline mesh results.
Fig. 9. Non-Conformal Mesh
Fig. 10. Conformal Mesh
Fig. 11. Baseline Mesh
The second configuration involves refining the solid convective body and introducing inflation layers to the fluid volume. The solid volume is hidden and with the help of face selection all the faces are selected as shown below and named as 'inflation layer'.
Under Inflation option, 'All faces under chosen named selection' is opted for 'Use automatic inflation', for 'Named Selection' 'inflation layer' is selected. 'Total thickness' is given for 'Inflation option' with 6 layers and maximum thickness of 3mm.
A Face Sizing method is incorporated to refine the convective solid body. The solid body which was hidden during inflation layer creation is again made visisble. All the body parts are selected and given a size of 15.5mm with 'Capture Curvature' as ON. After all this, the mesh is generated and checked for mesh quality again. These data are then imported to ANSYS Fluent.
Fig. 12 Inflation Layers in Fluid Volume
Fig. 13. Refined Mesh and Mesh Quality
SETTING UP THE SIMULATION:
- ANSYS Fluent is opened with ‘Contact Precision’ option checked in at the starting. Firstly, a mesh check is being conducted to see for any mesh quality abnormality. Once it’s done, the physics which governs the CHT analysis for our problem is checked in.
- A Steady Flow Numerical Simulation is done with type as Pressure-Based since, the Mach No. is very small. Absolute Velocity formulation is selected and Energy equation is also solved to account for the Temperature variation around the manifold body.
- Standard k-epsilon model with Standard wall function for near wall treatment is used with Inlet velocity V = 10m/s with temperature of 800K and turbulence intensity is about 5% and turbulence viscosity ratio is 10 at inlet, turbulence intensity is about 5% and turbulence viscosity ratio is 10 with 0 gauge pressure at outlet.
- Boundary conditions are - uniform velocity at inlet, uniform pressure at outlet, convective outer solid wall with a heat transfer coefficient of 20`W/(m^2K)`, all the other bodies are automatically assigned as adiabatic wall condition.
- Solution method utilizes pressure-velocity coupling scheme as coupled with gradient: least square cell based method, turbulent kinetic energy and turbulent dissipation rate as first order upwind. Energy,pressure and momentum are evaluated by Second Order Upwind scheme.
- For material selection, ‘Cell Zones’ is selected, and the volume is edited. There we will get the option of assigning the fluid or add and then assign. For this analysis,fluid volume is assigned with air while the solid volume is assigned with aluminium.
- Density of air is 1.225 kg/m^3 and viscosity is 1.7894e-05 kg/m-s. Aluminium is used as solid with density of 2719 kg/m^3 and thermal conductivity of 202.4 W/m-K.
- At last, initialization is being done and the method used is Hybrid.
- One might also run into an error in Fluent after creating an inflation layer to the baseline mesh and then importing it to Fluent. The message will say that new zones are created and hence, the mesh will not get imported. One need to go to File > Recorded Mesh Operations > Match Zone Names and match the zones from the ANSYS Mesher and ANSYS Fluent. Then Reload to debug the error.
- In Post-processing, a temperature contour is created and locations selected are- inlets,outlets,convective heat transfer boundary and the other adiabatic boundary. An animation is also created to see how the conjugate heat transfer takes place as the exhaust air moves from the inlets to the outlet. In CFD-Post, cutplane is created to visualize the velocity contour and the wall heat transfer corfficient along the manifold duct. Velocity streamline is defined starting from the inlets to monitor the velocity streamlines emerging from the inlet and exiting to the outlet.
- Refined mesh is made to run for 300 iterations while the baseline mesh is made to run for 600 iterations.
RESULTS AND CONCLUSION:
Baseline Mesh -
Temperature contour
Velocity contour
Wall Heat Transfer Coefficient
Velocity Streamlines
Residual plot
Refined Mesh -
Temperature contour
Velocity contour
Wall Heat Transfer Coefficient
The circled area in the figure shown above is zoomed and attached below:
Velocity Streamlines
Residual plot
CONCLUSION: If we look at the temperature contour, we can see that, there is not much of a change in the temperature distribution when the mesh is refined. Therefore,the baseline mesh produced almost meaningful plot for the temperature.
But when we look at the velocity streamlines and the velocity contour we can see that the refined mesh produced smooth transitions of velocity whereas in baseline mesh, the velocity contour is dispersed due to lack of cells. This can be clearly observed near the bend where the maximum velocity is obtained. The red colour gets dispersed in the baseline mesh. The maximum value of velocity also changes from 75m/s to 83m/s as we refine the mesh. Therefore, further refining needs to be done in order to get the velocity.
When we move on to the wall heat transfer coefficient plot, there is a considerable amount of change. In the baseline mesh, the heat transfer coefficient, which can only be obtained on that layer of fluid volume which is in contact with the solid volume, is diffused resulting in poor values. The lack of cells near the interface resulted in interpolations because of which we ended up getting such kind of plot. In a refined mesh, where we introduced inflation or body fitted mesh near the interface, we got nice and smooth plots for heat transfer coefficient. This demarcation can be observed in the zoomed plot for refined mesh, where on the inflation side we can see a smooth transition while on the other side(solid side) the transition is vague/irregular due to interpolation. The maximum value for HTC is also changing by huge amount therefore, further refining must be done to get the best results. One interesting thing to note is that the HTC is maximum near the bend area.
One might wonder that why in the temperature contour the heat transfer and thus the temperature is maximum near the outlet. Intuitively it must be near the inlet where the exhaust air is at the highest temperature. The reason is, if we apply conservation of mass near the inlets and near the outlet, we will see that the mass flow rate from the 4 inlets is gushed into one single outlet and since, the simulation is steady state the velocity near the outlet must be maximum,which is validated from the velocity plot. Since, velocity is maximum over there hence, Reynolds Number must also be maximum near the bend. If Reynolds Number is maximum that means Nusselt Number is also maximum. (Nu directly proportional to Re)
We know Nu = hL/k, so, L and k remaining constant Nu maximum means h is maximum at that particular place which is exactly the case as inferred from the temperature contour. Near the bend, maximum velocity resulted in maximum heat transfer coefficient which resulted in maximum heat transfer from liquid to solid and hence, maximum solid temperature is observed over there.
The residual plot tells that the refined mesh configuration achieved a steady state pretty fast than the baseline mesh did.
In the concluding remarks, I want to mention the factors upon which the accuracy of the simulation result depends upon:
- Mesh refinement,body fitted mesh and mesh quality.
- Sharing the Topology for flow information from one zone to another.
- Conformal Meshing.
- Choosing correct Physical Models for the problem.
- Geometry cleanup.
- Residual convergence.
- Validation from experimental results.
Model link: https://drive.google.com/open?id=1_gK9Yxa5Iw4r7x-3oxRWjjVZ925mwpcR