PDF
Cross-Flow Heat Exchanger
Introduction
This application simulates the fluid flow and heat transfer in a micro heat exchanger of cross-flow type made of stainless steel. Heat exchangers of this type are found in lab-on-chip devices in biotechnology and microreactors, for example for micro fuel cells. The application takes into account heat transferred through both convection and conduction. The geometry and material properties are taken from Ref. 1.
Model Definition
Figure 1 shows the heat exchanger’s geometry. Notice that the fluid channels have a square cross section rather than the circular cross section more commonly used in micro heat exchangers. A cross-flow heat exchanger can typically consist of about 20 unit cells. However, because the unit cells are identical except for edge effects in the outer cells, you can restrict the model to a single unit cell.
Figure 1: Depiction of the modeled part of the micro-heat exchanger.
Because heat is transferred by convection and conduction, the model uses a Conjugate Heat Transfer interface in the laminar flow regime.
The boundary conditions are insulating for all outer surfaces except for the inlet and outlet boundaries. At the inlets for both cold and hot streams, the temperatures are constant and a laminar inflow profile with an average velocity of 50 mm/s is defined.
At the outlet, the heat transport is dominated by convection, which makes the outflow boundary condition suitable. For the flow field, the model applies the outlet boundary condition with a constant pressure.
As shown in Figure 1, you can take advantage of the model’s symmetries to model only half of the channel height. Therefore, the symmetry boundary condition applies to the channels.
Results and Discussion
Figure 2 shows the temperature at the channel walls as well as temperature isosurfaces in the device, which clearly reveal the influence of the convective term.
Figure 2: Channel wall temperature and isotherms through the cell geometry.
As can be seen in Figure 3, the temperature differs significantly between the different outlets in both hot and cold streams. This implies that the hot stream is not cooled uniformly.
Figure 3: Temperature field at the outlet boundaries.
The flow field in the channels is a typical laminar velocity profile; see Figure 4.
Figure 4: Velocity profile in the channels.
There are several quantities that describe the characteristics and effectiveness of a heat exchanger. The mixing-cup temperature of the fluid leaving the heat exchanger is calculated according to (1.4 in Ref. 2).
(1)
COMSOL Multiphysics provides built-in variables to easily calculate 〈T〉. At the upper channels, the outlet mixing-cup temperature is about 40.5°C. At the lower channels, a higher value of 43°C is found for the outlet mixing-cup temperature. The maximum pressure drop in the heat exchanger is about 92 Pa.
The overall heat transfer coefficient is another interesting quantity. It is a measure of the performance of a heat exchanger design defined as
(2)
where P is the total exchanged power and A is the surface area through which P flows. In this model, the value of heq is about 3150 W/(m2·K).
References
1. W. Ehrfeld, V. Hessel, and H. Löwe, Microreactors, John Wiley & Sons, 2000.
2. P.K. Nag, Heat and Mass Transfer, 2nd ed., Tata McGraw Hill, 2007.
Application Library path: Heat_Transfer_Module/Heat_Exchangers/crossflow_heat_exchanger
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Heat Transfer > Conjugate Heat Transfer > Laminar Flow.
3
Click Add.
4
Click  Study.
In this model, the flow will be considered nearly incompressible and independent of temperature variations. Under these assumptions, the Stationary study performs best.
5
In the Select Study tree, select Preset Studies for Selected Multiphysics > Stationary, One-Way NITF.
6
Click  Done.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
T_cold
300[K]
300 K
Temperature, cold stream
T_hot
330[K]
330 K
Temperature, hot stream
u_avg
50[mm/s]
0.05 m/s
Average inlet velocity
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose µm.
First, create the cross section of one unit cell and extrude it.
Block 1 (blk1)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 800.
4
In the Depth text field, type 800.
5
In the Height text field, type 60.
6
Click  Build Selected.
Block 2 (blk2)
1
In the Geometry toolbar, click  Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 800.
4
In the Depth text field, type 100.
5
In the Height text field, type 40.
6
Locate the Position section. In the y text field, type 200.
7
Click  Build Selected.
Array 1 (arr1)
1
In the Geometry toolbar, click  Transforms and choose Array.
2
Select the object blk2 only.
3
In the Settings window for Array, locate the Size section.
4
From the Array type list, choose Linear.
5
In the Size text field, type 5.
6
Locate the Displacement section. In the y text field, type 120.
7
Locate the Selections of Resulting Entities section. Find the Cumulative selection subsection. Click New.
8
In the New Cumulative Selection dialog, type Channels in the Name text field.
9
Click OK.
Rotate 1 (rot1)
1
In the Geometry toolbar, click  Transforms and choose Rotate.
2
Click in the Graphics window and then press Ctrl+A to select all objects.
3
In the Settings window for Rotate, locate the Rotation section.
4
In the Angle text field, type 180.
5
Locate the Point on Axis of Rotation section. In the z text field, type 60.
6
Locate the Rotation section. From the Axis type list, choose Cartesian.
7
In the x text field, type 1.
8
In the y text field, type 1.
9
In the z text field, type 0.
Keep the existing unit cell by the following step.
10
Locate the Input section. Select the Keep input objects checkbox.
11
Click  Build All Objects.
12
Click the  Zoom Extents button in the Graphics toolbar.
Define several selections that will help throughout the model setup.
Definitions
Upper Inlets
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Upper Inlets in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 41, 48, 55, 62, and 69 only.
Lower Inlets
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Lower Inlets in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 8, 14, 20, 26, and 32 only.
Upper Outlets
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Upper Outlets in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 44, 51, 58, 65, and 72 only.
Lower Outlets
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Lower Outlets in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 77–81 only.
Symmetry
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Symmetry in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select the Group by continuous tangent checkbox.
Select one of the uppermost and lowermost boundaries, which now automatically will select all uppermost and lowermost boundaries thanks to the continuous tangency.
The next selections are needed to evaluate the equivalent heat transfer coefficient.
Outlets
1
In the Definitions toolbar, click  Union.
2
In the Settings window for Union, type Outlets in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Boundary.
4
Locate the Input Entities section. Under Selections to add, click  Add.
5
In the Add dialog, in the Selections to add list, choose Upper Outlets and Lower Outlets.
6
Click OK.
Materials
Define the material properties.
Stainless Steel
1
In the Materials toolbar, click  Blank Material.
2
In the Settings window for Material, type Stainless Steel in the Label text field.
3
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Thermal conductivity
k_iso ; kii = k_iso, kij = 0
15[W/(m*K)]
W/(m·K)
Basic
Density
rho
7800[J/(kg*K)]
kg/m³
Basic
Heat capacity at constant pressure
Cp
420[kg/m^3]
J/(kg·K)
Basic
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in > Water, liquid.
4
Click the Add to Component button in the window toolbar.
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Materials
Water, liquid (mat2)
1
In the Settings window for Material, locate the Geometric Entity Selection section.
2
From the Selection list, choose Channels.
Heat Transfer in Solids and Fluids (ht)
Set the reference temperature to an estimated value of (T_cold+T_hot)/2 where the flow operates.
1
In the Model Builder window, under Component 1 (comp1) click Heat Transfer in Solids and Fluids (ht).
2
In the Settings window for Heat Transfer in Solids and Fluids, locate the Physical Model section.
3
In the Tref text field, type (T_cold+T_hot)/2.
Fluid 1
1
In the Model Builder window, under Component 1 (comp1) > Heat Transfer in Solids and Fluids (ht) click Fluid 1.
2
In the Settings window for Fluid, locate the Domain Selection section.
3
From the Selection list, choose Channels.
Inflow 1
1
In the Physics toolbar, click  Boundaries and choose Inflow.
2
In the Settings window for Inflow, locate the Boundary Selection section.
3
From the Selection list, choose Upper Inlets.
4
Locate the Upstream Properties section. In the Tustr text field, type T_hot.
Inflow 2
1
In the Physics toolbar, click  Boundaries and choose Inflow.
2
In the Settings window for Inflow, locate the Boundary Selection section.
3
From the Selection list, choose Lower Inlets.
4
Locate the Upstream Properties section. In the Tustr text field, type T_cold.
Outflow 1
1
In the Physics toolbar, click  Boundaries and choose Outflow.
2
In the Settings window for Outflow, locate the Boundary Selection section.
3
From the Selection list, choose Upper Outlets.
Outflow 2
1
In the Physics toolbar, click  Boundaries and choose Outflow.
2
In the Settings window for Outflow, locate the Boundary Selection section.
3
From the Selection list, choose Lower Outlets.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
In the Settings window for Symmetry, locate the Boundary Selection section.
3
From the Selection list, choose Symmetry.
So far, the boundary conditions for heat transfer have been specified. Continue with the setup of the flow equation.
Laminar Flow (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.
1
In the Model Builder window, under Component 1 (comp1) click Laminar Flow (spf).
2
In the Settings window for Laminar Flow, locate the Physical Model section.
3
From the Compressibility list, choose Incompressible flow.
4
Locate the Domain Selection section. From the Selection list, choose Channels.
Because of the different inlet temperatures, the densities for the hot and cold stream vary and produce different velocities when the laminar inflow boundary condition is used. In order to have the same velocity profile on each inlet, define the laminar inflow boundary condition for the hot and cold inlet boundaries separately.
Inlet 1
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
In the Settings window for Inlet, locate the Boundary Selection section.
3
From the Selection list, choose Upper Inlets.
4
Locate the Boundary Condition section. From the list, choose Fully developed flow.
5
Locate the Fully Developed Flow section. In the Uav text field, type u_avg.
Inlet 2
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
In the Settings window for Inlet, locate the Boundary Selection section.
3
From the Selection list, choose Lower Inlets.
4
Locate the Boundary Condition section. From the list, choose Fully developed flow.
5
Locate the Fully Developed Flow section. In the Uav text field, type u_avg.
Outlet 1
1
In the Physics toolbar, click  Boundaries and choose Outlet.
2
In the Settings window for Outlet, locate the Boundary Selection section.
3
From the Selection list, choose Upper Outlets.
Outlet 2
1
In the Physics toolbar, click  Boundaries and choose Outlet.
2
In the Settings window for Outlet, locate the Boundary Selection section.
3
From the Selection list, choose Lower Outlets.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
In the Settings window for Symmetry, locate the Boundary Selection section.
3
From the Selection list, choose Symmetry.
After solving the model, the equivalent heat transfer coefficient is evaluated according to Equation 2. To do so, define the following nonlocal coupling.
Multiphysics
Nonisothermal Flow 1 (nitf1)
1
In the Model Builder window, under Component 1 (comp1) > Multiphysics click Nonisothermal Flow 1 (nitf1).
2
In the Settings window for Nonisothermal Flow, locate the Material Properties section.
3
Select the Boussinesq approximation checkbox.
Definitions
Average on Upper Channel Walls
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
In the Settings window for Average, type Average on Upper Channel Walls in the Label text field.
3
Locate the Source Selection section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 40, 42, 45, 47, 49, 52, 54, 56, 59, 61, 63, 66, 68, 70, and 73 only.
To select more easily these boundaries, use the Paste button and insert the list of numbers above in the Paste Selection dialog.
Study 1
In the Study toolbar, click  Compute.
Results
Change the unit of the temperature results to degrees Celsius.
Preferred Units 1
1
In the Results toolbar, click  Configurations and choose Preferred Units.
2
In the Settings window for Preferred Units, locate the Units section.
3
Click  Add Physical Quantity.
4
In the Physical Quantity dialog, select General > Temperature (K) in the tree.
5
Click OK.
6
In the Settings window for Preferred Units, locate the Units section.
7
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Temperature
K
°C
8
Click  Apply.
Temperature (ht)
COMSOL Multiphysics automatically creates four default plots: a temperature plot, a slice plot for the velocity field, a surface plot for the pressure field, and a plot showing both the temperature of solids and walls, and the velocity in the fluid. Additional plots, such as the isothermal contours are available in the Result Templates. The latter will be used to create the plot shown in Figure 2.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Heat Transfer in Solids and Fluids > Isothermal Contours (ht).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Surface 1
1
In the Model Builder window, expand the Isothermal Contours (ht) node.
2
Right-click Isothermal Contours (ht) and choose Surface.
3
In the Settings window for Surface, locate the Data section.
4
From the Dataset list, choose Exterior Walls.
5
Click to expand the Inherit Style section. From the Plot list, choose Isosurface 1.
6
In the Isothermal Contours (ht) toolbar, click  Plot.
To visualize the velocity field as in Figure 4, follow the steps below:
Slice
1
In the Model Builder window, expand the Velocity (spf) node.
2
Right-click Slice and choose Delete.
Surface 1
1
In the Velocity (spf) toolbar, click  Surface.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Laminar Flow > Velocity and pressure > spf.U - Velocity magnitude - m/s.
3
Locate the Expression section. From the Unit list, choose mm/s.
4
In the Velocity (spf) toolbar, click  Plot.
To show the temperature on the outlet boundaries only, as in Figure 3, first produce a new dataset for the selection built before. Then use this dataset for a surface plot of the temperature.
Outlets
1
In the Results toolbar, click  More Datasets and choose Surface.
2
In the Settings window for Surface, type Outlets in the Label text field.
3
Locate the Selection section. From the Selection list, choose Outlets.
Outlet Temperature
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Outlet Temperature in the Label text field.
Surface 1
1
In the Outlet Temperature toolbar, click  Surface.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Outlets.
4
Locate the Coloring and Style section. From the Color table list, choose HeatCameraLight.
5
In the Outlet Temperature toolbar, click  Plot.
Mixing-Cup Temperatures
1
In the Results toolbar, click  Global Evaluation.
2
In the Settings window for Global Evaluation, type Mixing-Cup Temperatures in the Label text field.
3
Click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component 1 (comp1) > Heat Transfer in Solids and Fluids > Temperature > Weighted average temperature > ht.ofl1.Tave - Weighted average temperature - K.
4
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
ht.ofl1.Tave
°C
Weighted average temperature (Upper Outlets)
ht.ofl2.Tave
°C
Weighted average temperature (Lower Outlets)
5
Click  Evaluate.
Table 1
1
Go to the Table 1 window.
The mixing-cup temperature at upper outlets is about 40.5°C and at the lower outlets about 43°C.
Results
To calculate the maximum pressure drop proceed as follows:
Maximum Pressure Drop
1
In the Results toolbar, click  More Derived Values and choose Maximum > Surface Maximum.
2
In the Settings window for Surface Maximum, locate the Selection section.
3
From the Selection list, choose All boundaries.
4
Click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component 1 (comp1) > Laminar Flow > Velocity and pressure > p - Pressure - Pa.
5
In the Label text field, type Maximum Pressure Drop.
6
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
p
Pa
Maximum pressure drop
7
Click  Evaluate.
Table 2
1
Go to the Table 2 window.
The maximum pressure is about 92 Pa. The minimum pressure is defined by the outlet boundary conditions and is zero. Thus, the maximum pressure drop is also 92 Pa.
Now, evaluate the equivalent heat transfer coefficient as defined in Equation 2. You can use the integration operators defined previously in Component 1 > Definitions.
Results
Heat Transfer Coefficient
1
In the Results toolbar, click  Global Evaluation.
2
In the Settings window for Global Evaluation, locate the Expressions section.
3
In the table, enter the following settings:
Expression
Unit
Description
aveop1(ht.ntflux)/(T_hot-T_cold)
W/(m^2*K)
Heat transfer coefficient
4
In the Label text field, type Heat Transfer Coefficient.
5
Click  Evaluate.
Table 3
1
Go to the Table 3 window.
The equivalent heat transfer coefficient is about 3143 W/(m2·K).