Week 4 - CHT Analysis on Exhaust port
CHT Analysis
CHT stands for Conjugate Heat Transfer analysis. It is an approach of simultaneously analysing heat transfer between solid and fluid regions that share a boundary. It simulates heat transfer between solid and fluid domains by exchanging thermal energy at the interfaces between them. This type of analysis considers both conduction (between solids) and convection (between fluids) heat transfer.
CHT is important in many applications such as electronics cooling, heat exchangers, industrial machinery, space applications etc..
Aim & Introduction:
To perform CHT analysis on an exhaust port and calculate surface/wall heat transfer coefficient on the internal solid surface and to examine velocity/temperature profiles at various areas in the component.
An exhaust port for an inline 4 cylinder engine is given and the exhaust gases are assumed to flow into the exhaust port with a velocity and temperature of 5 m/s and 700k respectively. For simplicity, the exhaust gas is assumed to be air.
Geometry:
Given geometry is shown below
(Refer Pic 1)
As the exhaust gasses flow through inside of the port, inner volume is a computational domain along with outer solid volume. The inner fluid volume must be extracted first.
This is done by using "Volume extract" option in "Prepare" module. Select all the required inner volumes through which the exhaust gas flows.
(Refer Pic 2)
The fluid volume is extracted as below
(Refer Pic 3)
Final computational domain containing both solid and fluid volumes
(Refer Pic 4)
To generate conforming mesh, topology between solid and fluid volumes must be shared.
Without a conforming mesh, nodes between solid and fluid volumes are not connected properly and information transfer is not done resulting in inaccurate results.
For this, enable "share topology" option and click share in "workbench" module.
(Refer Pic 5)
The next step is to mesh the geometry.
Solving and Modelling approach:
As discussed in previous challenge, a boundary layer is formed whenever fluid moves over or comes in contact with solid object.
In this, exhaust gas is coming in contact with exhaust port walls. Due to this, a boundary layer is formed and this layer must be resolved properly to get accurate values of temperature, velocity and heat transfer coefficient.
To resolve this boundary layer, there are two approaches as mentioned in previous challenge - viscous sub layer resolving approach and wall functions approach.
For problems involving heat transfer, viscous sub layer resolving approach gives accurate results compared to wall functions approach.
In viscous sub layer approach, the first grid point should lie in viscous sub layer. For this, the y+ value should be 1.
Inflation layers should be added in the mesh to resolve the boundary layer. For this, distance from surface to first cell and no. of inflation layers to be added must be known.
For y+=1, distance from surface to first cell can be obtained from online y+ calculator given in the link below
https://volupe.com/support/all-y-calculator-when-meshing-a-geometry-for-cfd-analysis/
Free stream velocity, density, dynamic viscosity, characteristic length and desired y+ value are the inputs required to calculate first cell height from surface.
Free stream velocity = 5m/s
As the exhaust gas is taken as air,
density = 1.225 kg/m3.
dynamic viscosity = 1.7894e-5 Pa-sec.
characteristic length in circular pipe with internal flow will be the diameter of pipe which is 0.166m
(Refer Pic 6)
The first cell height from the surface should be 0.0001155m.
Boundary layer thickness is also obtained from above calculator.
(Refer Pic 7)
Boundary layer thickness is 0.00687m.
Next, no. of inflation layers must be known. The number of inflation layers should be selected in such a way that their total height should be more than the boundary layer thickness i.e., the total height of inflation layers should be minimum 0.0067m.
No. of inflation layers are calculated using below formula
(Refer Pic 8)
Therefore, 14 inflation layers must be added in the mesh with first cell height being 0.0001155 m.
By doing this, boundary layer is resolved properly and accurate values of various flow parameters can be obtained.
Pre-processor and Solver setting:
Before meshing is done, areas of geometry for which boundary conditions should be assigned must be given certain names using named selections.
(Refer Pic 9)
The mesh element size is taken as 10mm and mesh type is tetrahedrons.
Element order is taken as linear.
(Refer Pic 11, 12)
Next step is to add inflation layers. As said above, first layer thickness would be 0.1195 mm, growth ratio as 1.2 and no. of inflation layers as 14.
(Refer Pic 13)
Final meshed body
(Refer Pic 14, 15, 16, 17)
Total no. nodes and elements are
(Refer Pic 18)
Element metrics are below
(Refer Pic 19)
Next step is to solve the problem using CFD solver.
The first step after opening is to check the mesh quality.
Assign reference values.
(Refer Pic 20)
Next in "Setting up Physics" module, select steady state and pressure based solver.
As mach number for the flow is less than 0.3, pressure based solver can be used.
Select the "Energy" as we need temperature values.
(Refer Pic 21)
Next step is to select the CFD model. The k-w model gives good results for the viscous sub layer approach.
(Refer Pic 22)
Select air as working fluid.
(Refer Pic 23)
Next step is to assign boundary conditions.
Inlets are assigned with velocity boundary condition of 5 m/s and temperature of 700K.
(Refer Pic 24, 25)
Outlet is assigned with pressure boundary condition with gage pressure of 0 and temperature of 300K.
(Refer Pic 26)
Wall is assigned with a convective boundary condition with a heat transfer coefficient of 20 W/m2k and with a free stream temperature of 300K.
(Refer Pic 27)
Hybrid initialization is performed in next step and the problem is solved for 300 iterations.
(Refer Pic 28)
Various flow parameters such as velocity, temperature, wall heat transfer coefficient and area weighted average of heat transfer coefficient are calculated.
Results & Conclusions:
The problem is solved for 300 iterations and the results are as below
1. Convergence- The solution is converged from around 100th iteration.
(Refer Pic 29)
2. Area weighted average of heat transfer coefficient - The heat transfer coefficient is calculated and found out to be around 22.5 W/m2k.
(Refer Pic 30)
3. Velocity - Streamlines of velocity are created along the exhaust port and highest velocity of 42.44 m/s is found at the exit portion.
(Refer Pic 32, 33)
A mid section plane is taken on the exhaust port and various flow parameters are calculated on this plane.
(Refer Pic 31, 34)
It is observed that the velocity is high at the 90° bend area.
This is because of mass conservation. All the inlet flows are directed into one single area resulting in higher flow area. Since the flow area is same, velocity would be higher.
4. Temperature -
(Refer Pic 35)
As the velocity is high at the bend, heat transfer would be more resulting in higher wall temperatures.
5. Wall heat transfer coefficient -
(Refer Pic 36)
The analysis results are validated with analytical solution using below formulae
(Refer Pic 37)
From the above, it can be seen that heat transfer coefficient obtained by simulation and analytical method are 22.5 and 19.5 W/m2k respectively.
The variation is around 15% which is acceptable and is in compliance with industry standards.