Conjugate heat transfer simulation
Aim:
1) To setup a flow simulation through a pipe with air as the flow fluid and post process the results such as pressure, temperature, velocity, cell count, y+ value.
2) Run a grid dependence test and show that the temperature of air at the outlet of the pipe converges to a particular value.
3) To show the effect of supercycle stage interval on the total simulation time.
INTRODUCTION AND THEORY:
Conjugate heat transfer:
Heat transfer refers to a branch of science which deals with the transfer of heat between two or more bodies, which may be solids or fluids or a combination of these. There are different ways in which heat is transferred. Namely, Conduction, convection and radiation. Conduction is transfer of heat between adjecent molecules of a body. The heat transfer takes place when the two adjecent molecules vibrate or oscillate with higher amplitudes hitting each other and transferring heat. This type of heat transfer is seen mostly in solids where the particles are more closely packed allowing for conduction to take place.
Convection, is a mode of heat transfer which takes place between two different bodies. This type of heat transfer is of two types. Natural convection and forced convection. In natural convection the heat transfer takes place due to density difference between the layers of molecules. For example, when we leave a cup of tea after making it for a while, the top most surface of tea starts cooling down as there is a temperature differnence between that layer of tea and the layer of atmospheric air in contact. As aresult of this the top layer becomes denser and then it goes below and the layer which is just below the top layer of the tea comes up and becomes the top layer and the process is continued. This is natural convection. Forced convection is where the heat transfer takes place due to an external force. For example, when we try to cool a cup of tea by keeping it under a fan. This results in transfer of heat due to the forced air by the fan. Convection is generally seen in fluids.
Conjugate heat transfer is the combination of heat transfer in solids and heat transfer in fluids. The governing equations of the two bodies is solved seperately in two sub domains.
Supercycling:
Supercycling is a technique which is used when there are more than one subjects under study and they have different converging rates over a particular phenomenon to adjust the converging rate and converge them at the same time. Here, in the conjugate heat transfer simulation, the solid pipe is heated constantly and the heat ois transferred from the solid pipe into the fluid which is flowing inside it. But, as the thermal conductivity of the solids is much larger when compared to that of fluids, solids take much longer time to change their temperature than fluids, in particularly gases. So, to converge the temperature of both solid and fluid, the solid temperature is averaged over certain fixed periods of time and the final temperature of the solid at the end of the simulation is brought up in a considerably short amount of time and while doing so the convergence of temperature of the fluid is stopped in periods to adjust the convergence at that time when the solid temperature will converge.
Y+ and it's significance:
Y+ is a non-dimensional quantity and a modified form of the distance of the fluid from the wall in the boundary layer. It is given by,
y+ = (y x ut)/v
where,
y= distance of the fluid from the wall in the boundary layer;
ut = frictional velocity,
v= kinematic viscosity.
When the flow is laminar then it is no-slip condition and we can solve the problem and simulate the flow.This means that we resolve the laminar region for whatever the grid size. But, when the flow is trbulent, there is a very thin laminar region near the wall and if we want to simulate the flow in that region with details of this thin laminar region then we have to select a very small grid size and this woud increase the time of simulation. Now, here we use y+ to select the appropriate grid size to optimize the time of simulation while capturing the details of the finnest gradients in the fluid.
It is found that, if y+ value is less than 10, then we are in the thin laminar region near the wall and if y+ is between 10 and 30, it means that we are in the transition region of the boundary layer. If the y+ value is more than 30 then we are in the turbulent region. So, by selecting the y+ value less than 10 or more than 30 we can achieve detailed simulation results by using wall functions.
Setting up the case of Conjugate heat transfer simulation in Converge studio. Let it be case set up 1.
GEOMETRY:
The geometry which we are considering is a hollow cylindrical pipe with a thickness of 5 mm and whose inner diameter is 0.03m. This geometry is not that complex and can be created in the Converge studio by using its CAD package.
Firstly, in the geometry section, select the create option, then click on shape. Select the option of cylinder. Select the radius of the cylinder as 0.015m and the start and end points of cylinder as (0,0,0) and (0,0,0.2) which means the length of the cylinder is 0.2m. See the image below for correspondance:
Now for creating the thickness of 5 mm, create another concentric cylinder with radius 0.02m and 0.2m length. See the image below:
Now, detete the two circles on each side of the cyclinder as they are overlapping circles which are not acceptable in Converge studio to run the case.
To delete the desired circles, in geometry section, select repair and then delete option, and select the triangle entity and also enable the angle type selection of triangles. Then click the desired circles and delete them.
See the picture below for correspondence:
Now, use the patch option to create the concentric regions at the two ends of the cylinder.
Now, we close the remaining cirular portion on both sides using to complete the geometry.
Now, we check for any normal orientation errors. We wnat the normals to face inside the cylinder as we want to simulate the flow inside the cylinder.
Flip the direction of normals by selecting transformation and then normal and then use one of the options mentioned to flip the direction of the normal to face inside the cylinder.
After this, we run a diagnosis test for the geometry to see if there are any errors to be fixed in it.
For this, go to diagnosis section and click on Find.
we can see in the below image the results of diagnonis.
We can observe in the above image that there are Non-manifold edges in the geometry and that is the only error in the geometry. Non manifold edge means an edge which is common for more than two edges. In the above image, the edges which appear in pink colour are the Non-manifold edges. But, these edges cannot be avoided in this type of simulation. So, we can continue with the above problem as Converge studio will understand that this is a conjugate heat transfer problem by the geometry and the way nonmanifold edges are present in it.
Next step is to set up the case. In this process we input all the necessary parameters for before processing the solution for the simulation.
CASE SETUP:
i) Application type: In the application type we select the time-based type as in our case the simulation is not for an IC engine. In the version prior to converge studio 3.0, the application type can be selected as General flow.
ii) Materials: We check Gas simulation. We select Air as the pre-defined mixture. We also check Solid simulation and species.
For gas simulation we use Redich_kwong method for equation of state and rest of the options are taken as follows:
In Solid simulation, we select the predefined solids option which is present at the bottom left of the solid simulation dialogue box as shown in the image below. After that we select Aluminium from the list.
The values for the global transport parameters are taken as follows:
1) Prandtl Number: 0.9
2) Schmidt Number: 0.78
In the species, in the gas tab, add the Oxygen and Nitrogen.
Under solid tab, click on Query available list and select Aluminium.
iii) Simulation parameters:
In simulation parameters we check run parameters, simulation time parameters and solver parameters.
Under run parameters set the simulation type to transient and run the simulation on full hydro mode.
Under the simulation time parameters the conditions are set as following:
1) start time = 0.0 s
2) End time = 0.5 s
3) Initial time step = 1e-7 s
4) Minimum time step = 1e-7 s
5) Maximum time step = 1 s
6) Maximum convetion cfl limit = 1.0
For Solver parameters, set Navier-stokes solver scheme to PISO.
iv) Regions and Initialization:
Under regions and initialization, add two regions, one as fluid region and the other as solid region.
For fluid region specify the following:
Stream ID: 0
Velocity: 0 m/s
Temperature: 300k
Pressure: 101325.0 Pa
Add Air as the species.
For solid region specify the following:
Stream ID: 1 and check the solid option beside it
Temperature: 300k
Select Aluminium as the species with mass fraction 1.0.
v) Boundary conditions:
Solid outer wall:
For solid outer wall set the following
Boundary type: WALL
Wall motion type: Stationary
Surface movement: Fixed
Select Slip from the drop down box.
Temperatuture boundary condition:
Select Heat flux from the drop down box and set it's value as -10,000 W/m2 for heat flow into the Aluminium cylinder.
Solid side:
For solid side boundary, set the following
Boundary type: WALL
Wall motion type: Stationary
Surface movement: Fixed
Select Slip from the drop down box.
Temperatuture boundary condition:
Select zero normal gradient (NE) from the drop down box.
Inlet:
For inlet boundary set the following
Boundary type: INFLOW
Pressure boundary conditions: Zero normal gradient (NE)
Velocity boundary conditions: Specified value (DI)
Calculating the velocity of air at inlet, using the following values
Reynolds number of 7000,
density of air at 300k is 1.16 kg/m3,
the characteristic length is inner diameter of cylinder= 0.03m
Dynamic viscosity of air at 300k is 1.846 x 10^-5 kg/m-s
Using the formula of reynolds number,
R= (density x Velocity x Characteristic length)/dynamic viscosity
we get velocity = 3.71 m/s.
So, take velocity of air at inlet = 3.71m/s.
Temperature boundary condition: specified Value (DI)
value of temperature= 300k
Species: Add air as species.
Outlet:
For outlet boundary set the following
Boundary type: OUTFLOW
Pressure boundary condition: Specified value (DI)
pressure value= 101325.0 Pa
Velocity boundary condition: Zero normal gradient (NE)
Temperature backflow: 300k
Add air as species.
Interface:
For interface boundary set the following
Boundary type: INTERFACE
Wall motion type: Stationary
For forward region select the following
Region: Fluid region
Wall treatment: Law of the wall
Temperature boundary condition: Law of the wall.
For reverse side select the following
Region: Solid region
Wall treatment: Slip
Temperature boundary condition: specified value (DI)
Vi) Physical models:
Under Physical models, check Turbulence modelling and Super-cycling modelling
For turbulence modelling select the following:
Turbulence model: RNG k-epsilon
Remaining parameters are set as default.
For super-cycling modelling set the following:
Begin storing gsuper-cycle data: 0.05 s
Solid side heat transfer solver: Steady-state solver
Time length of each cycle stage: 0.05 s
Total number of stages: 1
Conduction CFL number: 100
Sensible Internal Energy (SIE) tolerance: 1e-07
SIE relaxation factor for super-cycle: 1.4
vii) Grid control:
Base grid:
set base grid as dx=dy=dz=0.004m
viii) Output/Post processing:
Post variable selection:
Check y+ variable in combustion/turbulence tab.
Output files:
For output files, in the writing time intervals tab set the following
Time interval for writing 3D output data files: 0.01 s
Time interval for writing text output: 1e-06 s
Time interval for writing restarting output: 0.01 s
Now, the input files are exported to a folder and are processed in the software Cygwin terminal 64. Here the solver solves the Navier stokes equations and the results thus obtained are post processed in the Software called Paraview.
The above case setup is done again by changing the base grid size to dx=dy=dz=0.006m and then to dx=dy=dz=0.002m.
let us call these as case setup 2 and 3.
RESULTS AND DISCUSSION:
Mesh sizes for all the three cases are shown below:
The mesh size for case 1 which is dx=dy=dz= 0.004m:
The mesh size for case 2 which is dx=dy=dz= 0.006m:
The mesh size for case 3 which is dx=dy=dz= 0.002m:
It has been observed that the simulation time for the lowest mesh size was the most as it has more number of cells to compute.
Velocity Contours for all the three cases with different mesh sizes are shown below:
Velocity contour for the mesh size of case 1 which is dx=dy=dz=0.004m:
Velocity contour for mesh size of case 2 which is dx=dy=dz=0.006m:
Velocity contour for mesh size of case 3 which is dx=dy=dz=0.002m:
The part of the tube which has the least velocity of 0 m/s is the solid region and the velocity of air at the inlet being its lowest and as it flows further inside the pipe towards the outlet, the velocity of air increases because as the air moves forward towards outlet, the heat flowing through the cylinder thickness is transferred to the air and this increases the motion of each molecule of air and hence the velocity of air increases as it goes towards the outlet of the pipe. But when compared to the air which is in the centre of the cylinder, the velocity of the air near the walls of the cylindrical pipe is less because of the boundary layer effect, due to the sgearing friction between the walls of the pipe and the susequent layers of air.
On comparing the above three contour plots having three different mesh sizes, we can clearly observe that the contour plot with smaller mesh size has more vivid information for velocity than those with larger mesh size.
Pressure Contours for all the three cases with different mesh sizes are shown below:
Pressure contour for the mesh size of case 1 which is dx=dy=dz=0.004m:
Pressure contour for the mesh size of case 2 which is dx=dy=dz=0.006m:
Pressure contour for the mesh size of case 3 which is dx=dy=dz=0.002m:
The part of the tube which has the least pressure of 10^5 Pa is the solid region and the pressure of air at the inlet being its highest and as it flows further inside the pipe towards the outlet, the pressure of air decresses because as the air moves forward towards outlet, the heat flowing through the cylinder thickness is transferred to the air and this increases the distance between each molecule of air and hence the density of air decreases and as a result pressure of air also decreases as it goes towards the outlet of the pipe.
On comparing the above three contour plots having three different mesh sizes, we can clearly observe that the contour plot with smaller mesh size has more vivid information for pressure than those with larger mesh size.
Temperature Contours for all the three cases with different mesh sizes are shown below:
Temperature contour for the mesh size of case 1 which is dx=dy=dz=0.004m:
Temperature contour for the mesh size of case 2 which is dx=dy=dz=0.006m:
Temperature contour for the mesh size of case 3 which is dx=dy=dz=0.002m:
From the above contour plots of temperature, it can be observed that the temperature of the solid region of the pipe is maximum as the heat fux of 10,000w/m^2 is being supplied at the outer wall of the solid Aluminium pipe. The heat is being transferred from the inner most layer of the solid pipe to the layer of air which is in contact with it. Then it is transferred to the remaining air molecues layer by layer. It can be observed that the temperature of air decreases as we go towards the centre of pipe from its walls. Also, the amount of heat transferred to the air increases as the air near the inner wall of the pipe moves towards the outlet. As a result of this, the temperature of air also increases as it moves towards outlet. This is because the time for which the air is in contact with the inner wall of the pipe increases.
On comparing the above three contour plots having three different mesh sizes, we can clearly observe that the contour plot with smaller mesh size has more vivid information for temperature than those with larger mesh size.
Y+ Contours for all the three cases with different mesh sizes are shown below:
Y+ contour for the mesh size of case 1 which is dx=dy=dz=0.004m:
Y+ contour for the mesh size of case 2 which is dx=dy=dz=0.006m:
Y+ contour for the mesh size of case 3 which is dx=dy=dz=0.002m:
From the above contour plots of y+, we can observe that the range of y+ for case 1 is found to be between 0 and 16 and for case 2 it is between 0 and 31 and where as for case 3 it is between 0 and 7.3. So, for case 1 and case 2 at some parts of the region of air near the wall of the pipe it will be difficult to have detailed analysis where the values of y+ will be in between 10 and 30. But for case 3 we got all the values of y+ less than 10 and therefore we can go with an optimal grid size. Therefore, the grid size of 0.002m will give much accurate results near the wall of the pipe when compared with other two grid sizes.
Plots for average Velocity at inlet and outlet boundaries for all the three cases of different mesh sizes vs time taken are shown below:
Average velocity at inlet and outlet boundaries vs the time taken for case 1 with mesh size dx=dy=dz=0.004m:
Average velocity at inlet and outlet boundaries vs the time taken for case 2 with mesh size dx=dy=dz=0.006m:
Average velocity at inlet and outlet boundaries vs the time taken for case 3 with mesh size dx=dy=dz=0.002m:
On comparing the air velocity plots at outlets of the pipe, we have at the end of the simulation, the velocity of air of around 5.04 m/s for case 3 (grid size 0.002m), 4.8 m/s for case 1(grid size 0.004m) and 4.7 m/s for case 2(grid size 0.006m). So, the difference in the values of velocities oin thethree cases is due to the difference in accuracy of the three results obtained by using the corresponding mesh sizes. The accuracy depends upon the number of cells on which the computations are done and the corresponding y+ value.
Plots for Total pressure at inlet and outlet boundaries for all the three cases of different mesh sizes vs time taken are shown below:
Total pressure at inlet and outlet boundaries vs the time taken for case 1 with mesh size dx=dy=dz=0.004m:
Total pressure at inlet and outlet boundaries vs the time taken for case 2 with mesh size dx=dy=dz=0.006m:
Total pressure at inlet and outlet boundaries vs the time taken for case 3 with mesh size dx=dy=dz=0.002m:
The above plots show the variation of total pressure at inlet and outlet boundaries vs time taken. When we compare the plots for the three mesh sizes we can say that the accuracy of the total pressure has increased. But one can observe during solving the simulation that it takes more time to solve as the grid size is made smaller.
Plots for Static pressure at inlet and outlet boundaries for all the three cases of different mesh sizes vs time taken are shown below:
Static pressure at inlet and outlet boundaries vs the time taken for case 1 with mesh size dx=dy=dz=0.004m:
Static pressure at inlet and outlet boundaries vs the time taken for case 2 with mesh size dx=dy=dz=0.006m:
Static pressure at inlet and outlet boundaries vs the time taken for case 3 with mesh size dx=dy=dz=0.002m:
The above plots show the variation of static pressure at inlet and outlet boundaries vs time taken. One can observe that the static pressure is constant at the outlet boundary where as the total pressure is constant at the inlet boundary. When we compare the plots for the three mesh sizes we can say that the accuracy of the static pressure has increased. But one can observe during solving the simulation that it takes more time to solve as the grid size is made smaller.
Plots for average Temperature at inlet and outlet boundaries for all the three cases of different mesh sizes vs time taken are shown below:
Average Temperature at inlet and outlet boundaries vs the time taken for case 1 with mesh size dx=dy=dz=0.004m:
Average Temperature at inlet and outlet boundaries vs the time taken for case 2 with mesh size dx=dy=dz=0.006m:
Average Temperature at inlet and outlet boundaries vs the time taken for case 3 with mesh size dx=dy=dz=0.002m:
The temperature of the air at inlet is constant at a value of 300k and the temperature at the outlet is 300k initially and when the air reaches the outlet from inlet, the temperature of air increases to around 380k.
When we compare the plots for the three mesh sizes we can say that the accuracy of the average temperature has increased as there are more cells to compute the temperature at. But one can observe during solving the simulation that it takes more time to solve as the grid size is made smaller.
Plots for mass flow rate at inlet and outlet boundaries for all the three cases of different mesh sizes vs time taken are shown below:
Mass flow rate at inlet and outlet boundaries vs the time taken for case 1 with mesh size dx=dy=dz=0.004m:
Mass flow rate at inlet and outlet boundaries vs the time taken for case 2 with mesh size dx=dy=dz=0.006m:
Mass flow rate at inlet and outlet boundaries vs the time taken for case 3 with mesh size dx=dy=dz=0.002m:
For the above mass flow rate at the inlet and outlet boundaries vs time taken, the inflow mass flow rate is equal to the outflow mass flow rate which indicates that the convergence is reached.When we compare the plots for the three mesh sizes we can say that the accuracy of the mass flow rate has increased. But one can observe during solving the simulation that it takes more time to solve as the grid size is made smaller.
Plots for cell count vs time taken for all the three cases for different mesh sizes are shown below:
Cell count vs time taken for case 1 with mesh size dx=dy=dz=0.004m:
Cell count vs time taken for case 2 with mesh size dx=dy=dz=0.006m:
Cell count vs time taken for case 3 with mesh size dx=dy=dz=0.002m:
For the above plots of cell count vs time taken, in each plot, the total cells, the cells for which the calculation is performed by each processor is shown. As, the total cell count increases for a simulation, the total simulation time also increases and the accuracy of the results also invcreases as the solver solves equations for more number of cells and we will have more information at every smaller portion.
Plots for mean Temperature of Auminium outer wall for all the three cases of different mesh sizes vs time taken are shown below:
Mean Temperature of Aluminium outer wall vs the time taken for case 1 with mesh size dx=dy=dz=0.004m:
Mean Temperature of Aluminium outer wall vs the time taken for case 2 with mesh size dx=dy=dz=0.006m:
Mean Temperature of Aluminium outer wall vs the time taken for case 3 with mesh size dx=dy=dz=0.002m:
The mean temperature of aluminium outer wall is achieved by using super-cycle modelling. In this modelling, the temperature instead of running a transient simulation undergoes a steady state simulation at specified time intervals called super-cycle stage intervals. In all the three plots, the super cycling stage interval is 0.05 s. As the mesh size becomes smaller, we get more accurate results as there will be more number of cells at which the temperature values are obtained.
Grid dependence test:
From the above plot we can observe that, the value of temperature of air at outlet of the pipe has converged to values of 379.16k, 379.45k and 381.15k for cases with grid sizes of 0.002m, 0.004m and 0.006m.
The diference in the values of temperatures of air at the outlet of the pipe is due to the difference in accuracy while simulating using different grid sizes. Smaller the grid size, more is the accuracy of the result. Hence, the accurate value of average temperature would be 379.16k which is obtained with the smallest grid size of 0.002m.
Animations for all the three cases of different mesh sizes are shown below:
Velocity animations:
Link for velocity animation for case 1 with base grid size of dx=dy=dz=0.004m:
Link for velocity animation for case 2 with base grid size of dx=dy=dz=0.006m:
Link for velocity animation for case 3 with base grid size of dx=dy=dz=0.002m:
For the above velocity contour animations, we can observe that the development of velocity contour at each point of time is shown. The accuracy of this development increases as the grid size for simulation decreases. The velocity animation for the case 3 will be most accurate as it has the smallest mesh size. But the total simulation time for this case will be the longest.
Pressure animations:
Link for Pressure animation for case 1 with base grid size of dx=dy=dz=0.004m:
Link for Pressure animation for case 2 with base grid size of dx=dy=dz=0.006m:
Link for Pressure animation for case 3 with base grid size of dx=dy=dz=0.002m:
For the above velocity contour animations, we can observe that the development of pressure contour at each point of time is shown. The accuracy of this development increases as the grid size for simulation decreases. The pressure animation for the case 3 will be most accurate as it has the smallest mesh size. But the total simulation time for this case will be the longest.
Temperature animations:
Link for Temperature animation for case 1 with base grid size of dx=dy=dz=0.004m:
Link for Temperature animation for case 2 with base grid size of dx=dy=dz=0.006m:
Link for Temperature animation for case 3 with base grid size of dx=dy=dz=0.002m:
For the above temperature contour animations, we can observe that the development of temperature contour at each point of time is shown. The accuracy of this development increases as the grid size for simulation decreases. The temperature animation for the case 3 will be most accurate as it has the smallest mesh size. But the total simulation time for this case will be the longest.
Y+ animations:
Link for Y+ animation for case 1 with base grid size of dx=dy=dz=0.004m:
Link for Y+ animation for case 2 with base grid size of dx=dy=dz=0.006m:
Link for Y+ animation for case 3 with base grid size of dx=dy=dz=0.002m:
For the above y+ contour animations, we can observe that the development of y+ contour at each point of time is shown. The accuracy of this development increases as the grid size for simulation decreases. The y+ animation for the case 3 will be most accurate as it has the smallest mesh size. But the total simulation time for this case will be the longest.
Now, for case 3, we change the super-cycle stage interval from 0.05 to 0.03 and then to 0.02 and then to 0.01 and set up the case and run the simulations to study the effect of super-cycle stage interval on total simulation time.
Let us call these as case 4, case 5 and case 6.
Velocity Contour plots for the cases 4, 5 and 6 are shown below:
Velocity contour plot for case 4:
Velocity contour plot for case 5:
Velocity contour plot for case 6:
From the above three velocity contour plots we can observe that there is no change in the behavior of velocity of air at the end of the simulation with the change of super-cycle stage interval.
Pressure contour plots for cases 4, 5 and 6 are shown below:
Pressure contour plot for case 4:
Pressure contour plot for case 5:
Pressure contour plot for case 6:
From the above three pressure contour plots we can observe that there is no change in the behavior of pressure of air at the end of the simulation with the change of super-cycle stage interval.
Temperature contour plots for cases 4, 5 and 6 are shown below:
Temperature contour plot for case 4:
Temperature contour plot for case 5:
Temperature contour plot for case 6:
From the above three temperature contour plots we can observe that there is no change in the behavior of temperature of air at the end of the simulation with the change of super-cycle stage interval.
Y+ contour plots for cases 4, 5 and 6 are shown below:
Y+ contour plot for case 4:
Y+ contour plot for case 5:
Y+ contour plot for case 6:
From the above three y+ contour plots we can observe that there is no change in the behavior of Y+ value at the end of the simulation with the change of super-cycle stage interval.
Plot of mean temperature of Aluminium solid outer wall for cases 4, 5 and 6 is shown below:
From the above plot, we can observe that the intervals for which the temperature of air is averaged by doing the steady state simulations for three cases are 0.03s, 0.02s and 0.01s. We can also observe that there is no change in the temperature of aluminium outer wall at the end of simulation. The lower the super-cycle stage interval, more the number of points where the temperature of aluminium outer wall is averaged.
Plot of average temperature Air at outlet for cases 4, 5 and 6 is shown below:
As the solid outer wall has reached higher temperature values at less time in cases where the super-cycle stage interval is less, the temperature of air also becomes correspondingly higer due to the heat transfer from a higher temperature solid. Hence we see similar comparision between the temperatures of air at outlet for the cases corresponding to their solid outer wall temperatures. Here also, the average temperature of air at the outlet at the end time of simulation does not change with the change of super-cycle stage interval.
Animations for the cases 4, 5 and 6:
Velocity animations:
Link for velocity animation for case 4 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.03s:
Link for velocity animation for case 5 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.02s:
Link for velocity animation for case 6 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.01s:
For the above velocity contour animations, we can observe that the development of velocity contour at each point of time is shown. Also, the velocity contours at most of the points of time for the three cases are different as there is a different time period to time average the velocity using steady state simulation. But, we can observe that the velocity contour at the end time of simulation is same for all the three cases as we have run the simulation for same grid size.
Pressure animations:
Link for pressure animation for case 4 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.03s:
Link for pressure animation for case 5 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.02s:
Link for pressure animation for case 6 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.01s:
For the above pressure contour animations, we can observe that the development of pressure contour at each point of time is shown. Also, the velocity contours at most of the points of time for the three cases are different as there is a different time period to time average the pressure using steady state simulation. But, we can observe that the pressure contour at the end time of simulation is same for all the three cases as we have run the simulation for same grid size.
Temperature animations:
Link for Temperature animation for case 4 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.03s:
Link for Temperature animation for case 5 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.02s:
Link for Temperature animation for case 6 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.01s:
For the above temperature contour animations, we can observe that the development of temperature contour at each point of time is shown. Also, the temperature contours at most of the points of time for the three cases are different as there is a different time period to time average the temperature using steady state simulation. But, we can observe that the temperature contour at the end time of simulation is same for all the three cases as we have run the simulation for same grid size.
Y+ animations:
Link for Y+ animation for case 4 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.03s:
Link for Y+ animation for case 5 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.02s:
Link for Y+ animation for case 6 with base grid size of dx=dy=dz=0.002m and super-cycle stage interval of 0.01s:
For the above y+ contour animations, we can observe that the development of y+ contour at each point of time is shown. Also, the y+ contours at most of the points of time for the three cases are different as there is a different time period to time average the y+ using steady state simulation. But, we can observe that the y+ contour at the end time of simulation is same for all the three cases as we have run the simulation for same grid size.
Effect of super-cycle stage interval on total simulation time with respect to the base configuration:
For grid size of 0.002m and super-cycle stage interval of 0.05s the total simulation time is 2592 s.
For grid size of 0.002m and super-cycle stage interval of 0.03s the total simulation time is 2625 s.
For grid size of 0.002m and super-cycle stage interval of 0.02s the total simulation time is 2795 s.
For grid size of 0.002m and super-cycle stage interval of 0.01s the total simulation time is 2988 s.
As we can observe for the above 4 cases, when compared to the base configuration of case where grid size us 0.002m and super-cycle stage interval is 0.05 s, the total time taken to run the simulation increases as the super-cycle stage interval is decreased. Here, it is highest for the case where super-cycle stage interval is 0.01 s.
CONCLUSION:
We have successfully setup a flow simulation through a pipe with air as the flow fluid and post process the results such as pressure, temperature, velocity, cell count, y+ value.
Ran a grid dependence test and showed that the temperature of air at the outlet of the pipe converges to a particular value of around 380k.
We have observed the effect of super-cycle stage interval on the total simulation time. As the super-cycle stage interval increases the total simulation time decreases.
We have seen the importance of y+ in capturing the details of parameters such as velocity of the air, pressure of air, temperature of air near the solid inner wall while optimizing the grid size and total simulation time.