Week 4 - CHT Analysis on Exhaust port

AIM - 

To learn where and why CHT analysis is used

To check for porpoer y+ value according to the turbulance model used  

To calculate the wall and surface heat transfer coefficient on the internal solid surface.

To create the Required plots of velocity and temperature contour

To check if the HTC value are right 

To show on what factor the accuracy of the CFD predictions depends

OBJECTIVE -

To do the CHT analysis of ann Exhaust port and refine the mesh to get a good quality results. 

CONJUGATE HEAT TRANSFER :

In certain cases it is possible that there is a temperature distribution for a solid body and a fluid is flowing over the solid which may be either used to cool or heat up the body. In such problems it is necessary to calculate the energy equation for the solid along with the fluid flow equations. This type of analysis is know as Conjugate Heat Transfer (CHT) analysis.

There are a lot of real life examples for which CHT analysis is necessary, for example the flow of high temperature gases through an exhaust port of a combustion engine , Flow of fluids in a heat exchanger, cooling of electronic devices, etc.   

 

BASELINE SIMULATION:

For this challenge we will be solving the Conjugate heat transfer analysis on an exhaust port where the inlet velocity of the hot gas at 700K is 5m/s and the convective heat transfer coefficient of the outer wall is taken as 20 W/(m^2_K) , this value of convective heat transfer coefficient is taken from the supportive video lecture or else we can also do another simulation just to find out the value this parameter. But for our case we will be going with the given value.

Geometry Prep-  

For the baseline simulation we will be first importing the exhaust port geometry into the spaceClaim as shown below

next we will go to the prepare tab and use the volume extract command to extract the fluid volume from the exhaust port geometry using the edge select option and then after selecting all the edges click on the green tick mark as shown below

our generated fluid volume is shown below while hiding the external exhaust port geometry

we will rename the imported exhaust geometry as solid volume and the extracted volume as fluid volume

next we will be moving both the parts to a new component and delete the empty components

now we will set the topology to share for our complete system that is by the name Design 1

next we will go to the workbench tab and select the share command to share the topology throught the fluid and solid volumes so that the elements will be aligned and can share all the properties for the calculations, last we will be selecting the green tick mark we get a conformal mesh.

Now our geometry is ready for meshing so will move to meshing to mesh this geometry.

Meshing

For the Baseline simulation we will be using the default mesh generated by meshing and add named selection to the inlets, oullet and the outer wall of the solid volume named as convection-wall.

first adding named seletions

meshing using default settings

the number of elements for this mesh are shown below

the minimum element quality is 0.17 that is good enough so we can using this mesh to do our baseline simulation.

 

Fluent Setup-

moving to fluent we will now set up the physics by turnig on the energy equation and selecting the k-epsilon viscous model.

now add the boundary conditions , for the inlets add the inlet velocity as 5 m/s and temperature as 700 K. 

also we will set the heat transfer coefficient for the convective wall as 20 W/(m^2_K)

after that we will initialize the solution and also add a temperature contour to create a solution animation and run the simulation.

residuals

Temp contour at steady state

animation of temperature contour

temperature contour - exhaust port

CFD post Results-

Now we will look for other results in CFD post

velocity streamlines through the exhaust port with temp contour on the convective wall

as we see that there are 4 inlets and just one outlet the velocity at the outlet will be higher than the velocity at the inlet so there will be more convection in the outlet part and that is why the temperature of the outlet art is higher than the inlet part.

velocity coontour at across the outlet port

Wall heat transfer coefficient:

here we can see that the inner bend has a higher value of heat treansfer because there the velocity is the highest. more clear image can be seen below

surface heat transfer for the inner surface of solid volume

wall y+ value of the interfering surface 

form here we can see that the range of y+ is very high it should be close to 30 as we are using k epsilon model.

 

Now we will be refining our MESH so that the y+ value is according to the turbulance model so here we will be adding inflation layer to our model so that the location near the wall is captured properly and the properties are calculated accurately.

REFINED MODEL : 

We will use the same geometry that was prepared for the earlier case and load it into ansys meshing.

Meshing

Here we will first give named selection as earlier for the inlet , outlet and the convective wall

also we will be adding one more named selection here on the wall of the fluid volume as shown below and we will be naming it as inflation-layer 

 

now for the meshing part we will add an inflation layer of height 1.7 mm on the named selection 'inflation-layer'  so that our y+ value is 30 . we will be adding 5 layer in total with growth rate of 1.2 

also we will be adding a body sizing to the solid volume so that there is proper heat conduction through it , here we will turn on the capture curvature option so that there is no deformation in the geometry

Now after generating the mesh it look like as shown below

the inflation layer is clearly visible in the above image

the number of element generated in this mesh are shown below

the element quality metrics for this mesh has the minimum element quality of 0.1 that is acceptable

So our refined mesh can now be used for the simulation in fluent . We will setup the condition for physics and the solution the same as we had set ealier and look for the results.

Results 

Residuals

our residuals are fluctuating but as we can see that our temperature contour has stablized we will consider our solution has converged

Temp contour at steady state

Animation of temperature contour during the simulation

CFD Post : 

Velocity streamline with temprature contour on the outer surface

 we can see the temperature of the region with higher velocity is high due to more convection.

 velocity contour across the outlet

wall heat transfer coefficient plot

 

 

Y+ contour

from here we can see that the y+ value of the simualtion are in the acceptable range of 30-300 for the k-epsilon model

the contour for the inner wall heat transfer coefficient is shown below

 

Surface heat transfer for the inner wall

 

 

 

Model	Elements	Inflation	Surface heat transfer (W/m^2_K)	Wall heat transfer (W/m^2_K)
Baseline model	137865	no	47.06	106.4
Refined Model	466451	yes	48.18	181.6

the rise in the wall heat transfer coefficient is due to the inflation.

VERIFICATION OF HEAT TRANSFER COEFFICIENT:

We can verify if the HTC from the simulation by the analagous calculations that can be done 

 We know that Nusselts number is given by

`Nu = (h.L)/k`

where h = heat transfer coefficient 

          L = characterstics length 

          k = thermal conductivity 

Nusselts number is also a function of Reynolds number , which is a function of flow velocity 

So, HTC is directly proportion to the flow velocity .

It is also clear from the above inmage of velocity contour and the temperatre contour

Theoratical calculations:

 reynolds number :

`Re = (rho *v *D)/mu = (1.225* 5 * 0.17)/1.7894*10^-5 = 58189.896`

nusselts number :

`Nu = 0.023 *(Re)^0.8 * (Pr)^0.4 = 0.023 *(58189.896)^0.8 * (0.684)^0.4 = 128.123`

for temp 700 K Pr = 0.684

heat transfer coefficient

`h = (Nu *k)/(D underset(h)()) = (128.123*0.0242)/0.17 = 18.23`

 

and if we take the maximum flow velocity for calculations and the outlet throat 

reynolds number:

`Re = (rho *v *D)/mu = (1.225* 40* 0.17)/1.7894*10^-5 =410752.207`

nusselts number :

`Nu = 0.023 *(Re)^0.8 * (Pr)^0.4 = 0.023 *(410752.207)^0.8 * (0.684)^0.4 = 611`

for temp 700 K Pr = 0.684

heat transfer coefficient

`h = (Nu *k)/(D underset(h)()) = (611*0.0242)/0.17 = 98.575`

 

this value are for a striaght pipe but for a complex geomtry like an exhaust port the values should be between this range .

 

FACTORS AFFECTING THE ACCURACY OF PRIDCITIONS:

The factors on which the accuracy of the simulation depends are

Mesh size - the size of mesh affect the results , if the meh size is too coarse the results will have high error

Element quality - the quality of elements in the mesh helps to reduce the approximations of the properties flowing through it so elements should have atleast the quality of 0.1 if the quality is less than this value we should refine our mesh.

Inflation - inflation help to capture the flow properties near the wall presisely 

y+  -  the value of y+ should be according to the turbulance model for the k-epsilon model the value should be between 30 to 300.