Simulation of thermal mixing in a mixing tee using Ansys fluent

I. Aim: To determine the effectiveness of thermal mixing of a fluid at different temperatures in a mixing Tee.

II Introduction:

Mixing Tees are pipe connectors used for mixing fluids at different temperatures, velocities, composition, etc. to attain a desired temperature, velocity, and composition. These are used in many industries such as for mixing different chemicals in chemical industries to produce a new chemical, fluids at different temperatures in nuclear reactors, and in HVAC applications. It is important that the geometry of the mixing Tee, inlet velocities, and temperatures of the fluids are optimized to get the desired mixture at the required velocity and temperature.  CFD analysis can be employed in optimizing the mixing effectiveness of mixing tee by parametric analysis of the flow phenomenon. 

The objective of this project is to simulate the effectiveness of thermal mixing of air at different temperatures and velocities in a mixing tee by evaluating the temperature at the cross-section of the tee,s exit.

III: Solving & Modelling approach:

Two 90 degree Mixing Tees of different lengths are considered to evaluate the effect of geometry on the effectiveness of the mixing. Steady-state simulations are conducted to compare the mixing effectiveness when hot inlet temperature is 36^oC & the Cold inlet is at 19^oC. Also, the effect of inlet fluid velocities on the mixing effectiveness is compared for different cold-hot fluid inlet velocity ratio's. The different cases considered are:

1. Case 1 
   • Short mixing tee with a hot inlet velocity of 3m/s.
   • Momentum ratio(MR) of 2, 4. 
2. Case 2 
   • Long mixing tee with a hot inlet velocity of 3m/s.
   • Momentum ratio(MR) of 2, 4.

where,

Momentum ratio = velocity at cold inlet / velocity at hot inlet.

The mixing effectiveness is evaluated by examining the temperature profile and the average temperature at the cross-section of the exit of the mixing Tee. A more uniform profile indicates more effective mixing.

3D steady-state CFD analysis of thermal mixing in the mixing tee is carried in the Ansys workbench Fluent component. The workflow of Fluent in Ansys workbench is shown below:

 

IV: Pre-processing and solver setting:

The first step in a CFD analysis is preprocessing. This includes preparing the geometry/ computational domain, discretization of the domain (meshing), assigning material properties, boundary conditions, solver setup.

1. Geometry/Domain:

The computational domain is prepared using Ansys space-claim design modeler. The domain is generated from the mixing tee geometries using the 'volume extract' option in the prepare tab of Space-claim. The details about geometry and extracted fluid domain are given in the below figures:

Case 1 - Short mixing tee
Geometry	Front view of the extracted fluid domain
Case 2 - Long mixing tee
Geometry	Front view of the extracted fluid domain

 

 2. Domain discretization /Meshing:

The extracted fluid volume is discretized into a finite number of control volumes using the Ansys meshing component. A 3D Tetrahedral mesh, with a global element size of 4 mm is used for the analysis, with the cells near to the walls of the pipe are inflated using the inflation option to create boundary layer cells. A total of 5 boundary layer cells are created with a growth rate of 1.2. The generated mesh for both short and long mixing tees are shown below:

Short mixing tee	Long mixing tee
Global element size = 4 mm, Cells = 32830 Average Element quality = 0.543	Global element size = 4 mm, Cells = 43208 Average Element quality = 0.510

 

 Although, the element size used is the same for both the tees, the longer tee has more cells due increase in length of the tee. The boundaries of the domain are also defined in the Ansys mesher using the named selection option. The boundaries are defined as follows:

Boundary	Boundary name
hot fluid inlet	hot_in
cold fluid inlet	cold_in
mixing tee outlet	outlet
tee pipe  walls	walls

 

3. Solver setup:

The analysis is performed on the discretized domain(meshed model) in Ansys Fluent CFD software. A double-precision parallel solver with 4 cores is used. The double-precision solver uses 64-bit precision, which reduces the round-off error in the results.

3D steady-state analysis is performed, because the objective is to check the effectiveness of mixing by observing the temperature at the outlet reaches steady-state and not tracking the time-dependent variations.

The above settings are defined at the fluent launcher setup as shown below:

 

Once the mesh is opened in fluent, mesh quality is checked using the check mesh, quality -report quality options in the domain tab. 

The fluid considered for the analysis is air at atmospheric conditions. The properties of the air are given in the below table:

Fluid properties
Fluid	Density (kg/m^3)	Dynamic viscosity (Pa.s)	Thermal conductivity (W/mK)
Air at atmospheric conditions	1.225	0.000017894	0.042

The inlet velocities,  Reynolds number (`Re = (rhoVD)/mu`) for both hot and cold fluids cases considered are given below:

Short Tee	Hot fluid inlet velocity (m/s)	cold fluid inlet velocity  (m/s)	Hot fluid inlet Reynolds number	cold fluid inlet Reynolds number
MR = 2	3	6	6958.14	6966.36
MR = 4	3	12	6958.14	13932.71
Long Tee
MR = 2	3	6	6958.14	6966.36
MR = 4	3	12	6958.14	13932.71

 

From the above table, it can be inferred that the inlet Re for both cold and hot fluid is in the turbulent regime(Re>2300). Hence turbulence has to be modeled for accurately capturing the physics. For this purpose, turbulence modeling is carried using the `k-epsilon` and `k-omega` SST  RANS models. Also, the pressure-based solver, which is suitable for incompressible flows is selected as the velocities in the current problem are in the incompressible flow region (Mach Number <0.3).

The type of solver, operating conditions, turbulence model, material properties, zones, and boundary conditions are defined in the respective section of the physics tab as in the below figures.  The operating conditions define the atmosphere in which the analysis is caried out. This sets the reference pressure. In this analysis, a reference pressure of 1 Bar(101325 Pa) is considered to simulte atmospheric conditions. By default, Fluent solves only continuity and momentum equations. In order to see the termperature variation in the mixing tee we have to check on the energy option in the models section of the physics tab. Turbulence model is selected in the viscous option of models section. The properties of the air are defined in the materials section. Cell zones are defined to apply the materials to the domains. In the current problem, we have only one zone ie. fluid zone with material as 'air'.

 

Since the flow is in the incompressible regime, velocity inlet and pressure outlet are suitable for the analysis. The inlet velocities are defined as values corresponding to the fluid velocities. The outlet BC is pressure type with gauze pressure equal to zero, as it is open to the operating condition(atmosphere). These along with wall boundary conditions of no-slip are assigned in the boundaries option of the zones section. The turbulent quanties are defined interms of turbulent viscosity ratio and turbulent intensity at the inlet and outlet with default values provided by Fluent. The thermal conditions are also defined at the inlet as temperature BC with values given for the hot and cold fluid temperatures respectively. The walls of the mixing tee are assumed to be adiabatic and a heatflux BC with value 0 is assigned. The below images represent the BC assignment in Fluent.

 

Momemtum BC:

 

Thermal BC:

 

Solution setup:

After setting up the operating conditions, turbulence model, material properties, zones, and boundary conditions, the solution method,controls , type of reports required, initialization type , and number of iterations to solve are defined in the solution tab.

The default coupled pressure-based solver is used with the pseudo transient option. The coupled pressure-based solver solves the momentum and continuity equation simultaneously to compute velocity and pressure in the flow field. It is recommended for steady-state incompressible flows simulations. A pseudo transient is a form of implicit under-relaxation for steady-state cases. It helps in stabilizing the case and at the same time gives faster convergence. The default relaxation factors for the pseudo transient approach provided by fluent are used. The discretization schemes chosen for flow variables and gradients are as shown below. Second-order upwind schemes are used for flow variables to improve the solution accuracy.

 

Reports:

The convergence criteria for the governing equations can be setup using residual monitors in the report section. Also, the outlet temperature is monitored by using surface report as shown below:

 

 

The residual convergence is set to 1e-6 for all the flow equations to have tighter convergence. The residuals indicate the difference between the values in two successive iterations. The reports can be viewed while solution progresses by plotting them.

Initialization:

After setting all the above setup conditions, initialization of the domain has to be done necessary, because the solution is an iterative process that can only be executed if there is an initial guess of the solution variables. Hybrid initialization is employed in the current project, which solves the potential flow field equations in the domain to to setup the initial values for the solution. 

V. Solution Run/ Solving:

After initialization, the iterative solution process is executed using the run calculation section of the solution tab. We have to provide the number of iterations to be performed and click calculate to start the iterative solution process.

VI. Postprocessing/ Results extraction:

After the solution process is completed, post-processing has to be done to extract and analyze the results. Post-processing can be done in Fluent as well as Ansys dedicated postprocessor CFD-Post.

VII. Results :

1. Comparison of Turbulence model:

To check the efficiency of the turbulence models `k-epsilon` and `k-omega`, an initial case with the following parameters is carried.

Case 1A:

• Short mixing tee with a hot inlet velocity of 3m/s.
• Momentum ratio of 2 (ie. cold inlet velocity of 6 m/s)

BC:

	Inlet	Outlet	Walls
Momentum	Hot = velocity 3 m/s cold = velocity 6 m/s	Gauge pressure = 0	No-slip
Energy	Hot = 36 deg C cold = 19 deg C	-	Heat flux = 0

 

The realizable `k-epsilon` model with standard wall functions is compared with `k-omega` SST model in this analysis.

Convergence plot:

Realizable `k-epsilon`	`k-omega` SST

 

The above table compares the residual convergence and outlet temperature variation for both realizable `k-epsilon` and `k-omega` SST models. The convergence is said to be attained if the residual value decreases below a certain predefined criteria value and becomes constant in successive iterations or the pattern repeats after successive iterations. From the above plots it can be seen that in both the models the residuals fall below the convergence criteria. In the case of realizable `k-epsilon` the residuals attain a constant value after 400 iterations, hence the convergence is attained at around 400 iterations.  But in the case of the `k-omega` SST model the residuals are still decreasing even after 500 iterations. Hence this model requires more number of iterations to attain convergence. 

Also, monitoring the solution variables of interest can give information about convergence. The average temperature at the outlet is plotted to see if the temperature has attained a steady-state value. It can be seen that the average temperature value attains a steady-state value after around 200 iterations in both the cases. 

The results post-processed in CFD-Post are given below:

1. Velocity contour

Realizable `k-epsilon` model	`k-omega` SST model
On a central cut plane along the length of the mixing Tee
Across the cross-section along the length of the mixing tee

 

The velocity profile is almost identical in both the models. But towards the exit of the mixing tee, more uniform velocity contours are observed in `k-epsilon` model when compared to `k-omega` SST model.

2. Temperature  contour:

Realizable `k-epsilon` model	`k-omega` SST model
On a central cut plane along the length of the mixing Tee
Across the cross-section along the length of the mixing tee

 

The above temperature contours along and across the mixing tee length indicate that the temperature distribution is similar in both the cases at the mixing junction, but varies towards the outlet section. A more uniform temperature profile is observed in the `k-epsilon` model when compared to `k-omega` SST model.

1. Velocity plots:

Realizable `k-epsilon` model	`k-omega` SST model
Centreline velocity variation along the length of the mixing Tee
Across the cross-section along the length of the mixing tee

1. Temperature plots:

Realizable `k-epsilon` model	`k-omega` SST model
Centreline temperature variation along the length of the mixing Tee
Across the cross-section along the length of the mixing tee

 

The temperature profile is more uniform at the outlet in case of `k-epsilon` model , when compared `k-omega` SST model.

A converged solution doesn't mean it is accurate. The CFD results should be compared with analytical or experimental results to validate the numerical scheme. Since the main purpose of mixing tee is to give effective mixing temperature at the outlet , the average  outlet temperature value is selected for validation of CFD result. It is compared with the analytical result calculated from below formula found in literature.

`T_(mixture) = (m_(hot)*T_(hot)+m_(cold)*T_(cold))/(m_(hot)+m_(cold))`

`m = rhoAV`, is the mass flowrate.

	`k-epsilon` model	`k-omega` model	Analytical result	Error `%` `k-epsilon` model	Error `%` `k-omega` model
Avg_Outlet Temperature,  `T_(mixture)`, deg C	30.521	30.635	30.325	0.646	1.022

The numerical results are in good agreement with that of analytical value with the `k-epsilon` model having the least amount of error in computing the outlet temperature.

The above convergence, contour, and line plots as well as comparison of outlet temperature with analytical value indicate that the `k-epsilon` model predicts the mixing more efficiently than the `k-omega` SST model in less number of iterations. Hence, in further cases `k-epsilon` model is the turbulence model used.

Grid independence study:

The accuracy of numerical results also depends on the mesh size. The numerical results should not vary drastically when the mesh size is reduced. This is called grid independence. In order to check the effect of mesh size on the numerical result, grid independence is carried using 3 mesh sizes. The results are tabulated below:

Case 1A:

• Short mixing tee with a hot inlet velocity of 3m/s.
• Momentum ratio of 2 (ie. cold inlet velocity of 6 m/s)
• `k-epsilon` turbulence model

Mesh Element Size (m)	No of cells	Average outlet-temperature (deg C)
0.004	32830	30.521
0.0035	42444	30.540
0.003	56415	30.561

 

The outlet temperature value doesn't change very much when reducing the mesh size. Hence, the solution is grid-independent  at mesh size of 0.004 m. For the current problem increase in the number of cells only increases the computational cost with very little variation in results. In further cases the mesh size of 0.004 m is used along with `k-epsilon` turbulence model.

Case 1B:

• Short mixing tee with a hot inlet velocity of 3m/s.
• Momentum ratio of 4 (ie. cold inlet velocity of 6 m/s)

BC:

	Inlet	Outlet	Walls
Momentum	Hot = velocity 3 m/s cold = velocity 12 m/s	Gauge pressure = 0	No-slip
Energy	Hot = 36 deg C cold = 19 deg C	-	Heat flux = 0

 

Convergence plot:

Residuals	Outlet temperature

 

The residuals decrease to a value and show a repeated fluctuation after around 200 iterations. Also, the outlet temperature reaches a steady value after 200 iterations. Hene the solution is converged in 200 iterations.

1. Velocity contour

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

2. Temperature contour

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

3. Velocity plot

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

4. Temperature plot

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

 

It can be seen that the velocity and temperature profiles are more uniform at the outlet in this case(MR =2) when compared to MR=1 case, because the increase in the cold inlet velocity led to the enhanced mixing in the tee.

Case 2A:

• Long mixing tee with a hot inlet velocity of 3m/s.
• Momentum ratio of 2 (ie. cold inlet velocity of 6 m/s)

BC:

	Inlet	Outlet	Walls
Momentum	Hot = velocity 3 m/s cold = velocity 6 m/s	Gauge pressure = 0	No-slip
Energy	Hot = 36 deg C cold = 19 deg C	-	Heat flux = 0

Convergence plot:

Residuals	Outlet temperature

 

The residuals decrease to a value and become after around 450 iterations. Also, the outlet temperature reaches a steady value after 200 iterations. Hene the solution is converged in 450 iterations.

1. Velocity contour

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

2. Temperature contour

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

3. Velocity plot

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

4. Temperature plot

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

 

 

It can be seen that the velocity and temperature profiles are slightly more uniform at the outlet in this case(long pipe,MR =1) when compared to the short pipe(MR=1) case because the increase in the tee length at the exit section led to the little increase in mixing in the tee.

Case 2B:

• Long mixing tee with a hot inlet velocity of 3m/s.
• Momentum ratio of 4 (ie. cold inlet velocity of 12 m/s)

BC:

	Inlet	Outlet	Walls
Momentum	Hot = velocity 3 m/s cold = velocity 12 m/s	Gauge pressure = 0	No-slip
Energy	Hot = 36 deg C cold = 19 deg C	-	Heat flux = 0

Convergence plot:

Residuals	Outlet temperature

The residuals decrease to a value and show constantly repeated pattern after around 250 iterations. Also, the outlet temperature reaches a steady value after 200 iterations. Hene the solution is converged in 250 iterations.

1. Velocity contour

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

2. Temperature contour

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

 

3. Velocity plot

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

4. Temperature plot

On a central cut plane along the length of the mixing Tee	Across the cross-section along the length of the mixing tee

 

It can be seen that the velocity and temperature profiles are more uniform at the outlet in this case(long pipe,MR =2) when compared to the long pipe(MR=1) case because the increase in the cold inlet velocity led to the enhanced mixing in the tee.

 

 Results Comparison:

	Case 1: short pipe		Case 2: long pipe
	MR = 2	MR = 4	MR = 2	MR = 4
Cell count	32830	32830	43208	43208
Avg Outlet temperature  `T_(mixture)` in deg C	30.521	27.704	30.435	27.000
Analytical  `T_(mixture)` in deg C	30.325	27.500	30.325	27.500
No. of Iterations to convergence	400	250	450	250

 

 

 

 

 

 

 

 

 

 

The numerical outlet temperature values are in good agreement with that of analytical results. The outlet temperature in case of (MR =2) has values around 27 deg C for both the short and long tee, which is almost equal to the average of the inlet hot and cold fluid temperatures. An effective mixing should lead to a temperature that is average of the inlet temperatures at the outlet. This indicates that the case(MR=2) has better thermal mixing effectiveness.

 

Conclusion:

The aim of this project is to simulate the thermal mixing of air at different temperatures and velocities in a mixing tee of two different configurations. 3D steady-state CFD analysis is performed in Ansys Fluent. A comparison is made for two different turbulence models `k-epsilon` model and the `k-omega` SST model. The numerical results are validated using analytical results. The conclusions from the analysis are as follows:

1. Realizable `k-epsilon` model predicted the thermal mixing effectively when compared to the and  `k-omega` SST model.

2.  Increase in inlet velocity of the cross-flow fluid (MR =2) enhances mixing greatly due to more turbulent mixing of the fluids at the mixing junction as well as the cold fluid penetrating more into the hot fluid resulting in more uniform temperature at the outlet when compared to the low-velocity case (MR=1). The outlet temperature in case of (MR =2) has values around 27 deg C for both the short and long tee, which is almost equal to the average of the inlet hot and cold fluid temperatures.  This indicates effective thermal mixing of the fluids.

3. Increase in length of the mixing tee has shown a little improvement in the uniformity outlet temperature when compared to the short tee.

4. Although, increase in length of the mixing tee increased the effectiveness of mixing, this is very marginal when compared to the mixing enhancement by increasing the momentum ratio(velocity of cold fluid). Hence, thermal mixing effectiveness can be optimized greatly by considering the inlet fluid velocities rather than increasing the tee exit section length.

In this project, Air is used as the test fluid. The flow phenomenon and mixing may change for fluids with different densities and viscosities. Further, investigation can be done for different fluids to check the effect of fluid properties on the mixing effectiveness of the tees.