CHT Analysis on Exhaust port

CHT Analysis on Exhaust port

 

AIM:

1.Description of why and where a CHT(conjugate heat transfer) analysis is used.

2. Maintain the y+ value according to the turbulence model and justify the results. 

3. Calculate the wall/surface heat transfer coefficient on the internal solid surface & show the velocity & temperature contours in appropriate areas.

4.How would you verify if the HTC predictions from the simulations are right? On what factors does the accuracy of the prediction depend on?

Explanation:

1.why and where a CHT(conjugate heat transfer) analysis is used.

 

Introduction: Conjugate heat transfer analysis is based on a mathematically structured problem, which describes the heat transfer between a body and a fluid flowing over or inside it as a result of interaction between two objects. At the matching interface, the details are provided for temperature distribution and heat flux along the interface eliminating the need of calculating the heat transfer coefficient. Moreover, the heat transfer coefficient can be calculated later.

One of the simplest ways to realize conjugation is through numerical methods. The boundary condition for the fluid and solid interface is set and solved through iteration methods. There are no right guesses for the values of the initial boundary condition for the convergence except through the hit and trial method.

Application: The conjugate heat transfer methods have become a more powerful tool for modeling and investigating nature phenomena and engineering systems in different areas ranging from aerospace and nuclear reactors to thermal goods treatment and food processing from the complex procedures in medicines to ocean thermal interaction in metrology.

CHT in recent years has significantly improved the cooling performance of electronic equipment such as the design of heat sinks and the design of heat exchangers for the waste treatment plant. One such application of CHT is the exhaust port system.

Solving and modeling approach

• The exhaust port was modeled into the Spaceclaim.
• The exhaust port is a three-dimensional model containing four inlets and one outlet. Despite having isothermal boundary conditions and a uniform flow rate at the four inlets, the model cannot be cut into two halves to save computational time because of its asymmetrical nature. Therefore the whole model is discretized and is considered for meshing. 
• CHT analysis requires both the solid and the liquid volume under consideration, Spaceclaim gives an option of volume extract for selecting edges for fluid volume.
• Both the solid volume and liquid volume are copied into one component.
• Share topology is created.
• Spaceclaim gives an option for share coincident topology, when share coincident topology is selected and executed, the mesh from the fluid volume and the solid volume are said to be conformal with each other which is a requirement for CHT analysis.
• The exhaust port is loaded into the meshing window and then simulated for baseline mesh and the refined mesh.
• The named selections are created ( inlet, outlet, outer wall convection)
• The necessary contour images and graphs are studied to understand the behavior of temperature, velocity, and surface heat transfer coefficient at the interface.

 

Pre prosessing and setting up Model:

First of all we open ansys and in Geometry portion just drag and drop the pre prossed model.

 

Geometry:

 

 

 

Then in geometry select Repair-extra edges and then select the edges and click on the green tic.Ansys will automatically remove all the extra edges.

Then in the prepare option select Volume extract -Edges and select the edges as sown .Here we are willing to capture the fluid volume.

 

Now rename the newly extracted volume as fluid volume by right click on it and rename.

Move the fluid volume and solid volume 1 to a new component named  as new- Geometry by selecting two volumes and then right click and click on new component and rename the new component.Then click on Design-1 right click and delete empty component.

 

After in the bottom left portion share topology-share (first select Design portion /FFF-1 then share topology will appear). Then in the workspace portion click on share as two geometry will be shared between a fixed portion and a pink circle will be appeared in the outer face of the pipe.

 

 

Then close Geometry and open the mesh.

Mesh:

Then in the mesh portion first name the portions of the body as inlet,outlet,boundary convection ,inflation_layer by clicking on the portion and nemed selection(by clicking 'n' key on keyboard).

 

 

select the outer body by double clik on it and name it as boundary- convection.Then select the outer body again -right click-hide body as we have to name the inner fluid volume as inflation_layer.

 

Then in the bottom left corner in the inflation portion(first select the mesh in the left upper then inflation portion will appear) select the things as below picture.

 

Then right click on mesh and generate mesh.

 How to choose First layer thickness and number of layers in inflation?

we are going to choose an Y+ value to calculate first layer thickness.

Since the value of the heat transfer coefficient takes the value of the first cell near the wall, so it can be inferred that the Y+ value will be in the viscous sub-layer which is taken to be 1.

Steps involved in calculating the first cell height.

Reynolds number=(ρ*v*L)/µ=(1.225*5*0.17)/(1.7894*10^-05) =58189.8960

The characteristics length L is taken as the inlet dia.

Skin friction coefficient,Cf=.058/(Re)^0.2 = 0.00646

                                           

Wall shear stress formula, Tw=0.5*ρ*Cf*v^2 =0.5*1.225*0.00646*5^2 =0.0989 pa

Frictional velocity formula, Ut=(Tw/ρ)^0.5 =0.2841

Now, Y+ =(△y*Ut*ρ)/µ

Since Y+ =1 (as its acting within laminar sub layer)

Therefore △y=µ/(Ut*ρ)=0.0000514162m=0.0514162mm

 WE can find number of inflation layer by the following formula

Where YH = height of first layer, G=growth rate,N=number of layers

Then close the mesh and open fluent set up.Here we are using default element size(i.e. 150mm)

Set-up:

Then in the set up 

set physics-

solver-pressure based coupled(as more than one inlet-outlet so pressure based coupled solver is used), steady state

Energy equation-enabled(as temperature is taken into account)

viscouse medium-k-omega,SST(As turbulence model is within laminar sub layer and renolds number is not so high )

material-fluid-air

             solid-Aluminium(Al)

 

Zones-Boundary condition

         . inlet- velocity-5m/s, temperature-700k

          . Outlet-pressure-0pa,temperature-300k

         . boundary-convection-  Thermal condition-convection,Heat transfer coefficient-20w/m^2 k,Free stream Temperature-300k

       . Other boundary conditions will be as per default

Then in  physics in the left portion solver-Reference values (choose reference values carefully as it will affect the solutions)

 

set solution-

In solution -Defination-new-solution Report-Area weighted average

Then choose surface-heat-transfer-coefficient of inner surface i.e. inflation_layer like below

 

Then t=0 initialize and no. of iteration- 150 and calculate

Results set up-

 In result portion go to insert-location-plane-choose plane1

Then in plane1 we can chage Geometry as plane-xy,z=0, in color we can use variable color as temperature,velocity,wall flux.

 

RESULTS:

 

surface heat transfer coefficient:

 Here surface heat transfer coefficient=22.4

Temperature contour:

 

 Velocity contour:

 

 

 

 

CASE-2:

Now we are going to refine the Element size of the mesh , at meshing take element size as 50mm.Preprossing , inflation layers are same.

Surface heat transfer coefficient:

 

 Here surface heat transfer coefficient=21.92

 

 Temperature contour:

 

 

Velocity contour:

 

CASE-3:

Now we are going to refine the Element size of the mesh , at meshing take element size as 16mm, inflanation layers 5.Preprossing  are same.

 

 

 surface Heat transfer coefficient=21.79

Temperature contour:

 

 

 

velocity contour:

 

 pathline for  Temperature of Exhaust port:

pathline of temperature of Exhaustport

 

 

DATA TABLE:

	surface Heat transfer coefficient(ANALYTICAL)	surface Heat transfer coefficient (Actual)	% Error	Element size(mm) & inflation layers	Number of Elements
case-1	22.4	20	12	150 & 7	304258
case-2	21.92	20	9.6	50 & 7	300584
case-3	21.79	20	8.95	16 & 5	450963

 

Conclusion:

• The CHT analysis on the exhaust port was simulated successfully on ANSYS-FLUENT.
• The pressure-based, coupled scheme solver is used to discretize the whole geometry.
• The deviation of numerical heat transfer coefficient values from the analytical solution was found to be within  5% to 10%  for the second and final mesh refinement are found to be in compliance with the industrial standards.
• The grid independence test was also observed during mesh refinement. The value of the heat transfer coefficient for the second and final mesh refinement are close to each other. It is important that we limit ourselves to the second refinement only to save the computational time and cost of the project.
  
• The value of the heat transfer coefficient is located in the cell adjacent to the wall which allows us to choose the value ofY+=1(viscous sublayer) and the turbulent model .
• The presence of the boundary layer is quite visible near the inlet of the pipe where the viscous force makes the velocity near the wall to be zero causing a no-slip condition to occur., but as the flow is turbulent in nature (Reynolds number ) the velocity profile goes from flat to the flutter and the boundary layer vanishes at the outlet. 
• The velocity at the outlet is higher than the velocity at the inlet can be attributed to the presence of four inlets and one outlet.
• The accuracy of the heat transfer coefficient depends on selecting the suitable value of Y+ and turbulence model  model. The heat transfer coefficient values predicted by CFD were validated against the numerical solution depicted the deviation in the range of  to which is in compliance with industrial standards. However, the accuracy of   model itself depends on the accuracy of the analytical solution, flow properties, and geometry. The values predicted by the baseline mesh and the refined mesh were close to each other this can be attributed to the fact that the boundary keeps on growing and declining from the inlet to the outlet owing to change in velocity, thus the value is predominant at the outlet section of the exhaust port.

 

 References:

https://www.youtube.com/watch?v=1gSHN99I7L4&t=2291s