Week 6: Conjugate Heat Transfer Simulation

The fluid flow and heat transfer problems can be tightly coupled through the convection term in the energy equation and when physical properties are temperature dependent. While analytical solutions exist for some simple problems, we must rely on computational methods to solve most industrially relevant applications.

CHT can be performed to improve cooling performance of the water jacket and increase engine life. Advancements in cooling for applications such as gas turbines components require improved understanding of the complex heat transfer mechanisms and the interactions between those mechanisms, which our engineers can perform without hassle. Critical cooling applications often rely on multiple thermal protection techniques, including internal cooling, external film cooling, etc. which are efficiently used by our analysis to cool components and limit the use of coolant. We do extensive support for Motor and Battery CHT Analysis to get optimized design for High voltage systems. Conjugate Heat Transfer analysis provides the temperature distribution in solid and coolant of the engine and clear insight on velocity distribution and mechanism of heat transfer of coolant. Results of CHT analysis become input to structural simulations as thermal loads.

We have a wide experience in Engine CHT Analysis for various type of engines like Bikes, Passenger Cars, Racing cars, Commercial Vehicles, Marine, Agricultural equipment and Earth-moving equipment etc.

Mathematical Modeling

The flow of thermal energy from matter occupying one region in space to matter occupying a different region in space is known as heat transfer. Heat transfer can occur by three main methods:

• Conduction
• Convection
• Radiation

Physical models involving conduction and/or convection only are the simplest while buoyancy-driven flow or natural convection and radiation models are more complex.

Super Cycling Concept

Super cycling is a technique which is used in Converge studio in the case of conjugate heat transfer problems with a solid and liquid regions. Main poblem is that both solvers cannot run at the same speed since solving in fluid domain is much faster owing to the time scale difference for heat transfer in liquids as compared to the solids. This causes problems during the solution given that the solid side solver would not have reached a steady state/convergene in the time the liquid solver does. This is where the concept of super cycling is based.

The basic idea of super cycling is that the solver for the fluid domain is paused until the solver for the solid domain converges. The following steps are involved in performing the super cycling

1. Solve the fluid and the solid together with the transient solver. store the instantaneous Heat transfer coefficients and temperature on the interface during process.
2. Freeze the fluid solver. Time-averages the Heat transfer coefficients and temperatures and applies them as boundary conditions at the interface.
3. Solves the solid temperature until it reaches steady-state.
4. Update the solid temp field and unfreezes the fluid solver.
5. Repets until the solid temp converges.

Calculate velocity at inlet based on Reynold numbers:

Given:

Re.No = 7000

Inner diameter (Fluid region diameter) = 0.03D

At 300K, properties of air at 1atm pressure

Density(`rho`) = 1.161 `frac{kg}{m^3}`

dynamic viscosity (`mu`) = 0.00001846 `frac{kg}{ms}`

Velocity calculation based on Reynold numbers

`V = frac{R_e mu}{rho D}`= `frac{(7000)(0.00001846)}{(1.161)(0.03)}=3.71 m/s`

Skin friction drag co-efficient = `C_f` = 0.058`Re^(-1/5)` (For external flows)

C_f = (0.058)(`7000^(-1/5)`) = 0.0098720736

Wall shear stress = `tau_w` = 1/2(`C_f`)(`rho`)(`U^2`) = 1/2(0.0098720736)(1.161)(`3.71^2`)

`tau_w` = 0.0788784611 `frac{N}{M^2}`

Frictional velocity = `u_t` = `sqrtfrac{tau_w}{rho}` = `sqrtfrac{0.0788784611}{1.161} = sqrt(0.0679401043) = 0.2606532261`

Assume the desired `Y^(+) =`32

The first cell center to boundary distance = `Y^(+). frac{nu}{u_t}` = `32 * frac{0.000015859}{0.2606532261} = 0.0019469853 m`

Geometry dimensions:

Inner diameter = 0.03 m

Thickness diameter = 0.01 m

Length of pipe = 0.2 m

• A diagnosis check is performed to check for errors.
• Diagnosis check1- After geometry setup

The non-manifold problems occur due to the presence of three surfaces of a triangular element in contact with each other which are not recommended in ordinary simulations but are unavoidable in CHT analysis. This error will automatically disappear after the case setup procedure as Converge identifies this simulation to be a CHT analysis.

Diagnosis Check-2 After Case Setup

Case-setup

• In order to begin the case-setup, click on the case-setup and click begin case-setup and click Time based.
• Then click on Materials and select Air to be predefined mixtures. Also enable the solid simulation and species.

• Then open the Gas simulation and Global transport parameters and retain the default setting. Then open the species tab, in the Query available list choose the Aluminum as a solid species. Then goto gas and in the Query available list, choose N2 and O2 as a gas species.
• Then click on the Run Parameter under the Simulation Parameter and choose the transient solver under the solver tab and then choose the Full Hydrodynmic under the simulation mode. And then choose the Compressible under the Gas flow solver.
• In the simulation time parameter do the following changes.

• In the solver time parameter, we only choose the pressure based solver and retain the remaining setting.

• Add the boundaries by clicking create multiple boubdaries to create all boundaries at a once and name them like Outer_solid_wall, Solid_wall, inlet, outlet and interface by selecting the respective triangles.

• In the outer solid wall, we select the boundary type as a wall. And we are choosing the -10000 as a Heat flux in the temperature boundary condition. And also select the region as a solid region.

• In the solid wall, we are choosing the Wall type boundary condition. We are choosing the velocity boundary condition as a slip. And temperature boundary condition as a zero normal gradient. And also select the region as a solid region.

• We are choosing the boundary type as a inflow. And also select the region as a Fluid region. Choose the zero normal gradient in the pressure boundary condition. In the velocity boundary condition choose 3.71 m/s in the z-positive direction. And we are selecting the 300K in the temperature boundary condition. Ans select the air as a species.

• Choose outflow as the boundary type and select the region as the fluid region. Pressure boundary are specified as a 101325Pa. And we are choosing the velocity boundary condition as a zero normal gradient. Choose 300K temperature as a backflow boundary condition. And for species backflow, we are choosing the air.

• In interface, it has forward and reverse direction.
• If you have hide the inlet boundary, we can see that normals are pointing towards the fluid domain that direction is called the forward direction for an interface boundary.
• If the normals pointing towards the solid, then the foward direction indicates the solid region.
• Internally we are going to say that we have two boundaries forward and reverse boundary. Internally when converge runs, its going to create the copy of the interface boundary, one belonging to the fluid side and other belonging to the other side.
• So far the Forward boundary that is toward the fluid region. And for the fluid region the boundary need the law of wall boundary condition.
• And for the reverse region pointing toward the solid region.

Forward side boundary condition

Reverse side boundary condition

• In Regions and Initializations, click Add as Region-0 and Region-1

• In the fluid region set the stream-id as 0 and velocity condition as (0,0,0). Temperature initial condition as 300K and pressure condition as 101325 pa.

• In the solid region set the stream-id as 1. Set the temperature boundary condition as 300K . Specify the boundary condition as Aluminum with a mass fraction of 1.00.
• Then goto physical modelling and enable the turbulence and super cycling modelling .

• The first option is to set the initial time at which the super-cycle begins storing data. This can be set from 0 to any value less than or equal to the total simulation time.
• The solvers used for the solid region can be a steady or transient solver that is independent of the solver set in the run parameters window and can be steady or transient.
• The time length fo each cycle determines the intervals at which the fluid domain is paused and the solid domain solved for. This inteval is taken into account after the initial pause of the fluid solver at 1.
• The CFL number, SIE tolerance and relaxation factors are solver parameters that are given for the purpose of accuracy and speed of the solver.
• An output point must be defined in the solid region to let the solver know at which the temperature data must be calculated. This point must be given in the solid domain as the solver runs for the solid domain and once this value converges, the fluid domain solver is continued.
• We are running the simulation using three base grid which is 0.001, 0.002, 0.003 and 0.004.

• Now we are select the post variables. Then goto post variable selection `rightarrow` Combustion/Turbulence `rightarrow` and enabled the `y^(+)`. And retain the remaining setting.
• Then open the output files and do the following settings.

• At the end all the inputs files have to be exported:

File -->Export-->Export input files

Mesh representation at 0.001 Mesh

Mesh representation at 0.002 Mesh

Mesh representation at 0.003 Mesh

Mesh representation at 0.004 Mesh

Pessure contours at 0.001 Mesh

Pessure contours at 0.002 Mesh

Pessure contours at 0.003 Mesh

Pessure contours at 0.004 Mesh

Velocity contours at 0.001 Mesh

Velocity contours at 0.002 Mesh

Velocity contours at 0.003 Mesh

Velocity contours at 0.004 Mesh

Y-Plus contours at 0.001 Mesh

Y-Plus contours at 0.002 Mesh

Y-Plus contours at 0.003 Mesh

Y-Plus contours at 0.004 Mesh

Near wall modelling it is well-known that the mesh size should be small enough because near wall regions have large gradients in the solution variables.The wall `y^+`is a non-dimensionalize distance similar to local Reynolds. When you are solving your cfd simulations, you need to provide boundary condition. And for your turbulence equations perform correctly, you need to make sure that your first cell height in the right loction. Inside the boundary layer that y-plus is useful here is a simple example. If you take k-epsilon equation that is called high reynold number equation. It is not applicable in the scenrio where flow is laminar and flow is laminar inside the viscous sublayer. And the value of y-plus is between 1 and 10. k-epsilon model only used in the outer region, where y-plus is between 30 and 100. And y-plus of 30 means that you are 30 times this characteristics length away from the wall.

In the above y-plus contours we can easily observe that the for the different sizes of mesh the values the y-plus are given in the following table.

Mesh size	Y-plus
0.001m	7.7
0.002m	7.3
0.003m	17
0.004m	16

At the finer mesh we got the low value of mesh and at the coarser mesh we got the high value of mesh.

Temperature contours at 0.001 Mesh

Temperature contours at 0.002 Mesh

Temperature contours at 0.003 Mesh

Temperature contours at 0.004 Mesh

SC_AVG_HTC at Mesh 0.001

SC_AVG_HTC at Mesh 0.002

SC_AVG_HTC at Mesh 0.003

SC_AVG_HTC at Mesh 0.004

SC_AVG_Temp at Mesh 0.001

SC_AVG_Temp at Mesh 0.002

SC_AVG_Temp at Mesh 0.003

SC_AVG_Temp at Mesh 0.004

SC_Wall_Temp at Mesh 0.001

SC_Wall_Temp at Mesh 0.002

SC_Wall_Temp at Mesh 0.003

SC_Wall_Temp at Mesh 0.004

Results

Fluid side temperature

Table:

Mesh Size	Temperature Value
0.001 mesh	353.285
0.002 mesh	351.738
0.003 mesh	345.402
0.004 mesh	344.572

Solid side temperature

Table:

Mesh Size	Temperature Value
0.001 mesh	665.76
0.002 mesh	745.452
0.003 mesh	823.746
0.004 mesh	858.071

Supercycle at the monitor point (-0.0078, 0.015665, 0.18):

Table:

Mesh Size	Temperature Value
0.001 mesh	676.006
0.002 mesh	754.873
0.003 mesh	829.274
0.004 mesh	863.189

In this part we performed the grid independency test with 0.001m, 0.002m, 0.003m and 0.004m mesh size. By oberving the above plots we can easily say that at the finer mesh we got the more accurate values of temperature. But at the finer mesh computational effort has been increased.

Effect of supercycle stage interval

Fluid Side Mean temperature

Table:

Supercycle stage interval	Temperature Value
0.01	358.622
0.02	358.129
0.03	356.986

Solid Side Mean Temperature

Table:

Supercycle stage interval	Temperature Value
0.01	704.614
0.02	701.658
0.03	692.928

Supercycle at the monitor point

Table:

Supercycle stage interval	Temperature Value
0.01	717.875
0.02	714.077
0.03	704.367

In the above reults, we set the different values of supercycle stage interval. The time length for each cycle stage from supercycling modelling to 0.01, 0.02 and 0.03. In the supercycling mode converge continue to solve both the fluid and solid equations and stores the heat transfer coefficient and near-wall fluid cell temperatures for a time equal to the supercycle stage interval. In the start converge solves both fluid and solid equations together using the transient solver (but does not store the solid heat transfer data ) from the start of the simulation until the supercycle start time in order to develop the fluid flow field. At supercycle start time converge begins storing values for a heat transfer coefficient and near wall temperature fpr each cell at the solid/fluid interface, one value for each time-step.

In the above plots, we can easily observe that setting the lower value of supercycle stage interval converges to the exact values of temperatures. Basically we increase the value of supercycle stage interval from 0.01 to 0.03. we got the more exact values at 0.03 supercycle stage interval.

Time at mesh 0.001

Time at mesh 0.002

Time at mesh 0.003

Time at mesh 0.004

Table:

Mesh Size	Time (S)
0.001 mesh	21389.769258
0.002 mesh	1287.318420
0.003 mesh	346.041404
0.004 mesh	127.080322

Pressure animation at mesh 0.001

Pressure animation at mesh 0.002

Pressure animation at mesh 0.003

Pressure animation at mesh 0.004

Velocity animation at mesh 0.001

Velocity animation at mesh 0.002

Velocity animation at mesh 0.003

Velocity animation at mesh 0.004

Y-Plus animation at mesh 0.001

Y-Plus animation at mesh 0.002

Y-Plus animation at mesh 0.003

Y-Plus animation at mesh 0.004

SC_AVG_HTC at Mesh 0.001

SC_AVG_HTC at Mesh 0.002

SC_AVG_HTC at Mesh 0.003

SC_AVG_HTC at Mesh 0.004

SC_AVG_Temp at Mesh 0.001

SC_AVG_Temp at Mesh 0.002

SC_AVG_Temp at Mesh 0.003

SC_AVG_Temp at Mesh 0.004

SC_Wall_Temp at Mesh 0.001

SC_Wall_Temp at Mesh 0.002

SC_Wall_Temp at Mesh 0.003

SC_Wall_Temp at Mesh 0.004

Conclusion:

Results discussion of mesh independency:

• In this challenge we have performed the conjugate heat transfer analysis in a solid pipe.
• We have performed the grid independency test with 0.001m, 0.002m, 0.003m and 0.004m. From the above plots, we can clearly say that the as the mesh finer, the accuracy in the results increases. But when the mesh goes more finer and finer the computational cost has been increased.

Mesh size	0.001	0.002	0.003	0.004
Fluid mean temperature(K)	353.285	351.738	345.402	344.572
Solid mean temperature(K)	665.76	745.452	823.746	858.071
Computational time used by program(S)	21389.769258	1287.318420	346.041404	127.080322

As i summarized in the above table, as the mesh becomes finer we got the values which is near to the exact solution. At the 0.001 mesh we can observe that it takes too much time as compared to the other ones.

Results discussion of the effect of supercycle stage:

We set the supercycle stage interval, i.e time length for each cycle stage from supercycle modelling is used 0.01, 0.02 and 0.03. And for smallar value of supercycle stage interval the convergence is achieved faster. A monitor point is also create in the solid thickness boundary to observe the effects of super cycling. The plot shows that the steady state solver is employed in the solid region at fixed intervals of time (i.e. the super-cycle stage interval) and the results are compared while the transient solver computing the fluid flow is temporarily paused. Super-cycling is done as the heat flow in the solids when depicted by a transient solver, is time consuming. Hence it is better to apply steady-state analysis for the heat transfer through the solid while studying the behaviour of fluid flow through the pipe.

Temperature profile in the solid region

As we mentioned above, the steady state solver is employed in the solid region resulting in the sudden increase in temperature at various time intervals. This does not represent the actual temperature flow in the solid and only the steady-state temperature. Note that the increase in the temperature in the solid regions is due to the heat flux added to the solid outer wall.

Temperature profile in the fluid region

The transient solver is used to simulate the flow in the fluid region and hence the actual increase in the temperature is observed in this case. The increase in temperature is due to the transfer of heat from the solid to the fluid.