Conjugate Heat Transfer Simulation using Converge CFD   (Converge CFD, Skill Lync, Medium)
Aim:
To setup conjugate heat transfer simulation in Converge CFD and also observe the effect of super-cycle interval on computation time.
Introduction:
When there are multiple modes of heat transfer inside the simulation, the simulation is called a conjugate heat transfer (CHT) simulation. In this report, a CHT simulation of simple pipe flow inside hot pipe is performed. The solid pipe would recieve heat from outside and the pipe would heat the fluid inside it. The heat transfer from solid would take place using two modes, conduction and convection. The timescales of both the heat transfer modes are different, meaning that the conduction takes longer than convection. Hence, the simulation timestep would be restricted by conduction timestep. To fasten the simulation, the calculations on both the regions (solid and fluid) are done using different timesteps. This method is called super cycling.
The solver first solves the transport and energy equations for both regions and at a specified interval the fluid side solver stops. The solid region is solved using a steady state solver till convergence. Once convergence is reached in solid region, the flow solver resumes with new boundary values. The flow solver is stopped again after some interval and steady state solver runs for solid region. This continously happens till simulation time ends. This is the way a super cycling enabled transient CHT simulation works. The interval after which flow solver stops affects the computation time of simulation because the steady state solver is solve for more number of times. This effect is also studied in second part of report.
In this report, following geometry is used:
(The triangles in the image are not mesh elements but are triangles of surface in STL format.)
The pipe has internal diameter of 0.015 m, thickness of 0.005 m and length of 0.2 m. The pipe flow is axissymetric, so the simulations are performed using a 60 Deg sector of pipe. This reduces computation resources required. The fluid enters from inlet and a constant heat flux enters from top wall as shown. Following are the details of the setup:
Inlet:
Inlet velocity Reynolds number: 7000
According to properties of Air at 300K, the inlet velocity comes out to be as 3.64 m/s.
`V = (Remu)/(rhoD) = (7000 xx 1.849xx10^(-5))/(1.184xx0.03) = 3.64 m//s`
Pressure: zero normal gradient.
Temperature = 300 K
Outlet:
Pressure = 101325 Pa.
Side walls of fluid: Symmetry walls
Top wall of solid:
Temperature condition: constant heat flux of -10000 W/m^2
Side walls of solid: Symmetry walls
Front and back walls: Adiabatic walls
Interface:
Forward side: Fluid region with no slip wall condition.
Backward side: Solid region
Simulation time parameters:
Start time: 0 sec
End time: 0.5 sec
Initial timestep: 1e-7 sec
Minimum timestep: 1e-7 sec
Maximum timestep: 1 sec.
Max Conduction CFL number: 1
Max Diffusion CFL number: 2
Max Mach CFL number: 100
Region initialization:
Fluid region: pressure = Air at 101325 Pa and 300 K
Solid region: Aluminium at temperature of 300 K.
Mesh Settings:
Base mesh size (based on case number) (equal sizes in X, Y, Z directions) = 0.0020, 0.0015, 0.0010 m
Turbulence model: RNG k-e model with standard wall functions.
Supercycling settings:
Super cycling start time: 0.05 sec
Super cycling interval: 0.05 sec
Conduction CFL number: 100
Output files:
3D output saved at every 0.02 seconds (Gives 26 files)
Text output written at every 0.00001 seconds.
Results:
1) Mesh:
The image above shows the mesh generated for the three cases. The geometry is reflected along axis during post processing in paraview. This gives the cut section of a complete pipe at the centre plane. One peculiar thing to note in the right side cross sections is that the solid and fluid region seem to share the element, but its not so. The square cell is cut along the interface and it produces two cells out of a single square. Also, it might look that the cells at the axis have larger size, but its just a graphic issue. In the right side images we can see a small element near the axis.
2) Total cells:
The total cells in the mesh for a particular case remained same because there was no embedding or AMR function enabled.
3) Velocity:
The velocity profile of turbulent flow inside a pipe is seen in the images. The max velocity remains same for most of the cells along Y axis at the outlet. The max velocity can be seen changing depending on the mesh size. This tells that solution is not grid independent yet.
4) Y plus :
The values of y plus can be seen higher at the inlet side. In the case 2 mesh, the element size seems to be oddly less than other cases. Right now the only reason can be improper slicing, because even after checking the slicing coordinates the issue was not solved. Also, as the mesh became more fine the yplus must have reduced but the opposite can be seen here. This is also unexplained. Since the values are under 10, we can say the mesh is sufficiently fine.
5) Temperature plots and contours:
The figure above shows area averaged temperature of fluid(air) at the outlet. The steps in the graph lines indicate that supercycling took place at those points in time. The case 1 and 2 have nearly same temperature at outlets but case 3 has different values. This shows that solution is grid dependent.
The solid reaches a max temperature of 690 to 750 K. The temperature of fluid near wall is hot and at the centre is cold. This is expected because the flow did not mix till the pipe length ends.
The following video shows the development of temperature over time.
6) Supercycling temperature output:
The supercyling results in temperature changes in the solid. The plot shown below is the plot of temperature in solid at outlet region vs time. The steps in values indicate supercycling intervals.
7) Effect of super cycling intervals on computation time:
The super cycling intervals tell the time after which fluid solver will stop and solid region solver will solve till steady state. For judging the effect, super cycling intervals of 0.01, 0.02, 0.03 sec were compared with interval of 0.05 sec. All of these were done on base mesh having element size of 0.002 m.
As the super cycling interval reduces we require more computation time because the solid steady state solver solves multiple time. The temperature profile vs time gets more smoooth as we reduce the interval times. The final temperature is same for all intervals except 0.05 sec interval. This shows that end time of simulation must be increased for last case.
Conclusion:
The CHT simulation is performed using Converge CFD and effect of supercycling time interval was also observed.