COMSOL 6.4 - Turbulent Flow Through a Shell-and-Tube Heat Exchanger Cross Section

Turbulent Flow Through a Shell-and-Tube Heat Exchanger Cross Section

This example describes a part of a shell-and-tube heat exchanger (see Figure 1), where hot water enters from above. The cooling medium, commonly water, flows through the pipes and enters from the side. The tubes are assumed to be made of stainless steel.

Figure 1: A tube bundle from a shell-and-tube heat exchanger. The arrows indicate the flow directions.

Assuming that the cooling water is in abundant supply, the flow through the pipes has a constant temperature. Under that assumption, you can model this heat exchanger by a 2D model as shown in Figure 2, and the corresponding 2D domain appears in Figure 3. Note that the pipe interiors are not part of the domain because the model assumes the temperature to be constant there.

Figure 2: The dashed line marks the model region, which is shown in Figure 3.

Figure 3: The modeled 2D region.

The Need for a Turbulence Model

An important characteristic of the flow is the Reynolds number, Re, defined as

where U is a velocity scale, L is a length scale, and η is a kinematic viscosity. If the Reynolds number is low, no turbulence model is needed. If, on the other hand, the Reynolds number is high, then the flow is dominated by convection, and a turbulence model is necessary.

In this case, a suitable velocity scale is the mean inlet velocity, which is 1.5 m/s, and L is set to the pipe radius. Then, using standard values for water for the density and viscosity, the equation gives an approximate Reynolds number of 75,000, which is high enough to warrant the use of a turbulence model (see Ref. 1 for more information on flow regimes for different Reynolds numbers).

The following example demonstrates how to model a coupled fluid-thermal interaction problem with COMSOL Multiphysics, using the Nonisothermal Flow multiphysics coupling.

Model Definition

Solid and Fluid Heat Transfer — Including the Fluid Dynamics

The governing equations in this model are (Ref. 2–Ref. 4)

•

The Reynolds-Averaged Navier–Stokes (RANS) equations and a k-ε turbulence model.

•

Heat transport equations in the water and the solid (steel) tube walls.

The Nonisothermal Flow multiphysics coupling sets up both sets of equations together with the applicable couplings, making it easy to model the fluid-thermal interaction.

The model uses temperature-dependent properties for water and steel from the built-in material library. It incorporates the influence of the turbulent fluctuations on the temperature field by using the Kays–Crawford model for the turbulent Prandtl number (for details, see the section Turbulent Nonisothermal Flow Theory in the Heat Transfer Module User’s Guide). Furthermore, to account for the effect of mixing due to eddies, it is necessary to correct the fluid’s thermal conductivity. The turbulence results in an effective thermal conductivity, keff, according to the equation

where k is the fluid’s physical thermal conductivity and κT is the turbulent thermal conductivity. Furthermore, μT denotes the turbulent dynamic viscosity, Cp is the heat capacity, and PrT refers to the turbulent Prandtl number. Be careful not to confuse k in the meaning of thermal conductivity with k in the meaning of turbulent kinetic energy.

The boundary conditions for the problem are:

•

k-ε equations in the fluid domain:

Specified initial velocity

Symmetry at the region borders

Wall function at the pipe/water interfaces

Fixed outlet pressure

•

Heat transport equations:

Fixed temperature at the inlet

Convection-dominated transport at the outlet

Symmetry (thermal insulation) at the region borders

Thermal wall function at the pipe/water interfaces

Fixed temperature at the inner pipe surfaces

Results for the Flow/Heat Model

Figure 4 shows the velocity in the inlet of several segments in the middle of the computational domain. The flow field is periodic in the y direction with the constant pressure drop of about 1350 Pa. (Figure 5).

Figure 4: Velocity at y = 400, 500, 600, and 700 mm.

Figure 5: Pressure at y = 400, 500, 600, and 700 mm.

Figure 6 depicts the temperature distribution and velocity streamlines in the segment. The heat transfer is strongly influenced by the details of the velocity field. Observe the low-temperature zones behind the pipes created by the recirculation zones.

Figure 7 shows the temperature profiles at y = 400, 500, 600, and 700 mm.

Figure 6: Temperature distribution in the segment.

Figure 7: Temperature distribution at y = 400, 500, 600, and 700 mm.

Notes About the COMSOL Implementation

You start by performing an initial calculation for the single segment of the computational domain (Figure 8). Proceed by creating a linear array of the segments. The appropriate physical interface settings are automatically extended to all elements of the array.

Figure 8: Modeled segment of the heat exchanger with boundary conditions.

References

1. J.R. Welty, C.E. Wicks, and R.E. Wilson, Fundamentals of Momentum, Heat and Mass Transfer, 3rd ed, John Wiley & Sons, 1984.

2. B.E. Launder and D.B. Spalding, “The Numerical Computation of Turbulent Flows,” Computer Methods in Applied Mechanics, vol. 3, pp. 269–289, 1974.

3. D.C. Wilcox, Turbulence Modeling for CFD, 2nd ed, DCW Industries, 2000.

4. H.K. Versteeg and W. Malalasekera, An Introduction to Computational Fluid Dynamics, Prentice Hall, 1995.

Heat_Transfer_Module/Heat_Exchangers/turbulent_heat_exchanger

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select > > > ε.

Click .

Click

In this model, the flow will be considered nearly incompressible and independent of temperature variations. Under these assumptions, the study performs best.

In the tree, select > .

Click

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Value	Description
T_in	323[K]	323 K	Inflow temperature
T_pipe	278[K]	278 K	Pipe temperature
v_in	-1.5[m/s]	-1.5 m/s	Inflow velocity

Geometry 1

In the window, under click .

In the window for , locate the section.

From the list, choose .

Now draw the segment of the heat exchanger that forms the model geometry for the first simulation.

Rectangle 1 (r1)

In the toolbar, click

In the window for , locate the section.

In the text field, type 50.

In the text field, type 100.

Click

Circle 1 (c1)

In the toolbar, click

In the window for , locate the section.

In the text field, type 27.5.

Click

Circle 2 (c2)

In the toolbar, click

In the window for , locate the section.

In the text field, type 25.

Click

Difference 1 (dif1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

Click to select the

toggle button for .

Select the object only.

Click

Copy 1 (copy1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

In the text field, type 0 50.

In the text field, type 100 50.

Click

Union 1 (uni1)

In the toolbar, click

and choose .

Click in the window and then press Ctrl+A to select all objects.

In the window for , click

Delete Entities 1 (del1)

In the window, right-click and choose .

In the window for , locate the section.

From the list, choose .

On the object , select Domains 1, 2, 5, 7, 8, and 10 only.

It might be easier to select the domains by using the window. To open this window, in the toolbar click and choose . (If you are running the cross-platform desktop, you find in the main menu.)

In the toolbar, click

You should now see the following geometry.

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select > .

Click the button in the window toolbar.

In the tree, select > .

Click the button in the window toolbar.

In the toolbar, click

to close the window.

Materials

Steel AISI 4340 (mat1)

Select Domains 1, 3, and 4 only.

Water, liquid (mat2)

In the window, click .

Select Domain 2 only.

In the window for , locate the section.

Click

In the dialog, type Water in the text field.

Click .

Heat Transfer in Fluids (ht)

Set the reference temperature to an estimated value of T_in where the flow operates.

In the window, under click .

In the window for , locate the section.

In the Tref text field, type T_in.

Solid 1

In the toolbar, click

and choose .

Select Domains 1, 3, and 4 only.

Turbulent Flow, k-ε (spf)

The density variations are small enough to consider the fluid as incompressible. Change the compressibility option accordingly in the physics interface. The reference temperature is set in the Heat Transfer interface.

In the window, under click ε.

In the window for ε, locate the section.

From the list, choose .

Locate the section. From the list, choose .

Inlet 1

In the toolbar, click

and choose .

Select Boundary 7 only.

In the window for , locate the section.

Click the button.

Specify the u0 vector as


0	x
v_in	y

Symmetry 1

In the toolbar, click

and choose .

Select Boundaries 2, 8, and 11 only.

Outlet 1

In the toolbar, click

and choose .

Select Boundary 6 only.

Heat Transfer in Fluids (ht)

In the window, under click .

Inflow 1

In the toolbar, click

and choose .

Select Boundary 7 only.

In the window for , locate the section.

In the Tustr text field, type T_in.

Outflow 1

In the toolbar, click

and choose .

Select Boundary 6 only.

Temperature 1

In the toolbar, click

and choose .

Select Boundaries 12, 15, 18, and 19 only.

In the window for , locate the section.

In the T0 text field, type T_pipe.

Mesh 1

In the window, under click .

In the window for , locate the section.

From the list, choose .

Right-click > and choose .

Size 2

In the window, under > click .

In the window for , locate the section.

Click the button.

Locate the section.

Select the checkbox. In the associated text field, type 0.5.

Click

Study 1

Solve the problem for a single heat exchanger segment.

In the toolbar, click

Results

Velocity (spf)

The default plots show the velocity, the wall resolution, and the temperature distribution in the segment.

Geometry 1

Continue with creating the array of the elements.

Array 1 (arr1)

In the toolbar, click

and choose .

Select the object only.

In the window for , locate the section.

From the list, choose .

In the text field, type 10.

Locate the section. In the text field, type -100.

In the toolbar, click

Click the

button in the toolbar.

You should now see the following geometry:

COMSOL Multiphysics automatically extends the material properties, meshes, and physical interface settings to all segments of the exchanger.

Study 1

In the toolbar, click

Results

Default Plot Groups

Default plots are generated for the velocity magnitude, pressure, boundary wall resolution, and temperature.

Proceed as follows to plot the y-velocity component for a few segments in the middle of the computational domain (Figure 4).

Velocity Along Arc Length

In the toolbar, click

In the window for , type Velocity Along Arc Length in the text field.

Click to expand the section. From the list, choose .

In the text area, type Velocity field, y-component (m/s).

Line Graph 1

In the toolbar, click

Click the

button in the toolbar.

Select Boundary 44 only.

In the window for , click in the upper-right corner of the section. From the menu, choose > ε > > > .

Click to expand the section. Select the checkbox.

From the list, choose .

In the table, enter the following settings:


Legends
At y=700 mm

In the toolbar, click

Line Graph 2

Right-click and choose .

In the window for , locate the section.

Click

Select Boundary 45 only.

Locate the section. In the table, enter the following settings:


Legends
At y=600 mm

In the toolbar, click

Line Graph 3 and Line Graph 4

Create two more line graphs by repeating the steps for , except select boundaries 46 and 47, respectively.

Velocity Along Arc Length

From Figure 4 it is evident that the flow field is periodic in the y direction. The pressure drop on the segment is about 1500 Pa. To plot the pressure distribution (Figure 5), proceed as follows.

Pressure Along Arc Length

In the window, right-click and choose .