Convection Heat Transfer in Offset-Strip Fins

By: Kuan-Ting Lin

1.1 Learning Outcome

The convection heat transfer in an offset-strip fin is simulated in this example. Students would be able to build a three-dimensional flow domain and conjugate heat transfer simulation after finishing this example.

1.2 Introduction

Offset-strip fin is one of the most popular enhanced fin cores in the application of compact heat exchanger. The geometrical features are shown in the following figure. Compared to plain plate-fin, the improvement in heat transfer is mainly due to periodic disruption of boundary layers and downstream fluid mixing.

In this simulation, fin spacing s = 0.002 m, fin thickness t = 0.00015 m, fin height hf = 0.01 m, and offset length l = 0.0032 m. Since only the fully developed condition is considered, the calculation domain consists of two periods of the offset length (2l) within a single channel (s + t), and the periodic boundary condition is applied at the inlet and outlet boundaries. The boundaries in the transverse direction will be considered as symmetry planes. The top and bottom surfaces are considered as no-slip walls with uniform and constant temperature. The flow condition is considered as constant-property, laminar, and steady airflow. The thermophysical properties of air are dynamic viscosity μ =1.87e-5 Pa-s, density ρ = 1.166 kg/m3, specific heat cp = 1005 J/kgK, and thermal conductivity k = 0.0264 W/mK.

Schematic view of an offset-strip fin and the boundary conditions of the simulation
Reynolds number equation

The Reynolds number of the offset-strip fin is defined as:

Hydraulic diameter equation

Where the hydraulic diameter dh can be expressed as:

In this simulation, the Reynolds number is set as 600, and from the calculation the corresponding mass flow rate is 6.732e-5 kg/s. Moreover, the material of the fin is aluminum, which has a thermal conductivity of 237 W/mK.

1.3 Steps

  • Building Geometry / Step 1
  • Topology / Step 2
  • Meshing / Step 3
  • Physics Models and Boundary Conditions / Step 4
  • Preparing Simulation / Step 5
  • Post Processing / Step 6

1.3.1 Building Geometry / Step 1

Diagram to Create a new geometry

To begin with, the geometry of the fluid domain needs to be created. Right-click on the 3D-CAD Models and select “New” to start building a CAD model.

Program showing how to create a new sketch

Create a sketch by right-clicking on the XY plane and select Create Sketch.

Diagram showing Grid spacing adjustment of the sketch

For our convenience, we will set the grid spacing of the sketch to 0.001 m.

Draw a rectangle that starts from the origin. Right-click at the point at the origin to apply the fixation constraint so that the location of the bottom left corner of the rectangle will be fixed.

Diagram of Draw a rectangle in the sketch

Right-click on the lines to apply dimensions and set the length and width as in the figure. Click OK to exit the sketch.

Diagram of how to Apply length dimension

Right-click on Sketch1 and extrude for 0.01 m.

Diagram of Extrusion of the sketch

Right-click on the top surface and create a sketch on the +z face.

Diagram of Create a new sketch on face

Use the icon in the display option to view the x-y plane in the sketch if the scene has been rotated.

View normal to sketch plane

Right-click on the line and project the line to the sketch. Right-click on the line again to set it as a construction line.

Project the line and set it as a construction line

Draw a rectangle from the construction line and set the dimensions as in the figure.

Draw a rectangle and set the dimensions

Select the bottom-left point and set the y-coordinate. Then click OK to exit the sketch.

Set the coordinate of one point

Right-click on Sketch2 and extrude the body into the first block.

Extrusion of the sketch without body interaction

Expand Bodies in the tree. Right-click on Body2 and use the linear pattern tool.

Create a linear pattern for a feature

Set the distance in the x-direction to 0.0048 m and the number of instances to 2.

Set the parameters of a linear pattern (x-direction)

Right-click on the top surface again and create another sketch on the +z face.

Create a new sketch on face

Project the bottom line on the sketch and set it as construction. Draw a rectangle from the construction line and set the dimensions as in the figure. Set the x-coordinate of the bottom-left point.

Draw a new rectangle and set the coordinate of one point

Right-click on Sketch3 and extrude.

Extrusion of the sketch without body interaction

Right-click on Body4 and use the linear pattern tool. Set the instances of x and y to 1 and 2, respectively. Change the distance in the y-direction to 0.002075 m.

Set the parameters of a linear pattern (y-direction)

Right-click on Body1 and rename it to Fluid. Rename the other bodies from Fin1 to Fin4 in sequence.

Rename bodies

Use Shift to select all the bodies, then right-click and use the subtract in Boolean operation.

Boolean operation

Fluid is the target body and the other fins are tool bodies. If the bodies are not in the correct boxes, right-click and remove all the components.

Remove all components in target and tool bodies

Click the Target Bodies box and select Fluid. Click the Tool Bodies box and use Ctrl to select from Fin1 to Fin4. If the fins are blocked by the Fluid, right-click on the top surface and hide it.

Hide the surface on the top

After finish selecting the bodies, activate the option to keep the tool bodies after the operation. Click Close 3D-CAD to exit the CAD mode.

Set the target and tool bodies

1.3.2 Topology / Step 2

In the topology, the flow domain and the boundary faces would be determined in this step. The naming of each boundary face is shown in the figure and would follow the rules as follows:

-x: Inlet

+x: Outlet

-z:  Bottom

+z: Top

-y and +y: Symmetry

Boundary conditions of the simulation

Right-click on the 3D-CAD Model 1 and select “New Geometry part”. Use default settings and click OK.

Create a new geometry part

Create a geometry scene from the toolbar.

Create a geometry scene

Expand Fluid, right-click on Default and select Split by Patch. Be sure you have created the geometry scene before you execute this command.

Use split by patch to separate the surface

Use Ctrl to select the two faces at the -x. The selected faces would also be highlighted in the box. Name them as Inlet and click create, and these two faces would disappear. Repeat the process and name the other faces as well.

Split and rename the surfaces accordingly

The final surfaces of each part would be as in the figure.

The list of the named surfaces in each part

Collapse all the parts. Right-click on Fluid and select Assigned Parts to Regions and make changes to the boundary options. A “Region” would be created under the “Region” folder. Rename the “Region” to “Fluid”.

Create the fluid region

Use Shift to select all the fins. Right-click and select Assigned Parts to Regions and make changes to the boundary options. Another “Region” would be created under the “Region” folder. Rename the new “Region” to “Fins”.

Create the solid region

Change the type of Fins in the Region to a solid region.

Change the type of the region

1.3.3 Meshing / Step 3

A structured directed mesh is used for this simulation. To build the directed mesh, Right-click on Operations and select the directed mesh option. Select all the bodies in the pop-up window.

Create the directed mesh

A new directed mesh is created under operation. Right-click on it and select edit.

Edit the directed mesh

The surfaces for the source mesh and target mesh need to be specified.

The tree list of the directed mesh

For the source mesh, assign all the bottom surfaces in the bodies to it.

Set the source surfaces for the directed mesh

Similarly, assign all the top surfaces to the target mesh.

Set the target surfaces for the directed mesh

Right-click on Source Meshes and select Patch Mesh.

Create the patch mesh

To have a better view on the xy-plane, use the view from +z direction.

Set the view of the window

The lines need to be populated with dots before further editing. Under the Patch Topology mode, use the first icon to auto-populate the edges with dots.

Populate the lines with dots

Use the scissor tool to add four additional dots on the lines. Then use ESC to dismiss the scissor function.

Create dots in the patch topology

The coordinate of the dot will be shown in the left column after selecting it. To form a structured mesh, the added dots in the lower half will be specified with y = 7.5e-5 m, and the added dots in the upper half will be specified with y = 0.002075 m.

Set the coordinates of the newly created dots

Use the second icon and select two dots to form a straight line in between. Press ESC to dismiss the function and select the icon to form another line between the other two dots.

Form straight lines between dots

After connecting all the dots, the color of the lines will turn to green.

Completion of the patch topology

Change the mode from Patch Topology to Patch Mesh. Selecting the line in the figure will highlight all the lines that will be using the same number of divisions. The number of divisions in each set of lines is shown in the figure.

Set the number of divisions in each line

The final surface mesh will be constructed after finishing the settings. Then click Close.

Final surface mesh

Right-click on Mesh Distribution and select New Volume Distribution. Set the number of layers to 100. Select Close Directed Mesh

Set the number of divisions in the extrusion mesh
Generate the volume mesh

Use the icon to generate volume mesh.

Create a mesh scene to check on the mesh in the window.

Create a mesh scene

The final mesh can be visualized in the mesh scene.

Visualization of the volume mesh

In this section, physics models for the simulation and the boundary conditions would be determined. Right-click on Continua and create another Physics Continuum. One of the physics continuums is created for Fluid and the other for Fins. Therefore, rename Physics 1 and Physics 2 to Fluid and Fins, respectively.

Create physics models for “Fluid” and “Fins”

To enable the required physics models for Fluid, expand Fluid and double-click on “Models” and select the following models in the order of:

  1. Three dimensional
  2. Steady
  3. Gas
  4. Segregated flow
  5. Constant density
  6. Laminar
  7. Segregated fluid temperature
Set the physics models for “Fluid”

The thermophysical properties of air can be set in the models, which dynamic viscosity μ =1.87e-5 Pa-s, density ρ = 1.166 kg/m3, specific heat cp = 1005 Jkg/K, and thermal conductivity k = 0.0264 W/mK.

Set the air properties

To enable the required physics models for Fins, expand Fins and double-click on “Models” and select the following models in the order of:

  1. Three dimensional
  2. Steady
  3. Solid
  4. Segregated flow
  5. Constant density
  6. Segregated solid energy
Set the physics models for “Fins”

Assign the Fluid and Fins physics continuums to Fluid and Fins regions, respectively.

Assign each region with the appropriate physics

The developing flow behavior in the offset-strip fin is neglected and simulated by using the periodic boundary condition. To create the boundary condition, the interface between the inlet and outlet at the fluid region needs to be set up first. Use Ctrl to select both Inlet and Outlet and right-click to create an interface.

Create interface between the inlet and outlet

A new interface is created under the Interfaces folder. Set the topology of the interface to Periodic and the type of the interface to Fully-Developed Interface. 

Set the periodic boundary condition

Since the wall temperature at the top and bottom plates are considered as constant temperature boundary conditions, change the Fully Developed Energy Option to Constant Temperature Walls. Assigned Fluid.Top and Fluid.Bottom as the reference temperature. Also, a certain mass flow rate is specified in the simulation, and thus the Fully Developed Flow option needs to be changed to Mass Flow Rate. Set the mass flow rate under Physics Values. The default bulk inflow temperature is used, which is set as 300K.

Set the parameters for periodic boundary condition

Set the thermal boundary conditions at the top and bottom plates. First, expand Fluid and set thermal specification to temperature and set the temperature to 400K.

Set the constant temperature boundary condition

Repeat the process to the top plate in Fluid, and the top and bottom plates in Fins.

The surfaces that are assigned to constant temperature boundary condition

Change the type of the boundary of Symmetry in Fluid and Fins to Symmetry Plane.

Set the symmetry boundary condition

In this step, we will set up the scenes and monitors. This will allow us to check the results while running and after the simulation is finished. To visualize the temperature contour, create a scalar scene from the toolbar.

Create a scalar scene

Change the view of the scalar scene.

Change the view of the scalar scene

In the scalar scene, right-click on the legend and select the temperature function.

Select the scalar function for scalar scene

Expand Scalar Scene 1 under Scenes, assign the whole regions to the Parts so that it will show in the window.

Assign the parts to show in the scalar scene

Before running the simulation, the stopping criteria needs to be reset. To make sure the results are dependable, the residuals of continuity, momentum, and energy should converge below a certain limit. Right-click on “Stopping Criteria” and create new criteria from the monitor. Choose energy on the list.

Create a new converging criterion from monitor

An energy criterion will be created. After that, set the “Logical Rule” to “And” and set the minimum limit for “Energy Criterion” to 1E-8.

Set the minimum converging limit for energy

Repeat the previous steps and create the other three monitors for “Continuity”, “X-momentum”, and “Y-momentum”. Set the “Logical Rule” to “And”. Set the minimum limit for these criteria to 1E-6.

Create new converging criteria from monitor

The maximum steps would be set at a relatively large number, which is 10000 in this case, so that a sufficient number of iterations are allowed for the convergence of parameters.

Set the maximum number of iterations

Select the green icon in toolbar and initialize the solution. Click run to start the calculation.

Initialize the solution and run

Post processing is rather important because we need to examine the result and further analyze it. After finishing the simulation, check the residual plot and see if all the converging criteria are satisfied. The temperature contour would be shown in the scalar scene.

Temperature contour of the offset-strip fin

To have a better view of the flow temperature distribution, a cross-section at the middle of the fin height can be created. Right-click on Derived Parts and create a section plane.

Create a section plane at the middle of the fin height

Set the coordinate and the normal vector of the plain. Select No Displayer. After finishing the settings, click Create.

Set the coordinate and the normal vector of the plane

Create a new scalar scene from the tool bar.

Create a new scalar scene

Change the contour style to Smooth Filled to have a continuous distribution. Also, assign the part and the field function you would like to present in the scalar scene.

Set the part and scalar field for the scalar scene to show

The scalar scene will show the temperature distribution at the selected plane section.

The temperature distribution at the plane

Similarly, by assigning the velocity magnitude to Scalar Field, the velocity contour will be shown in the scalar scene.

The velocity distribution at the plane

The pressure at the inlet and outlet of the fluid can be shown from the report. Right-click on Reports and select Surface Average. A new Surface Average 1 is created.

Create a surface average report

Set the pressure as the field function. Assign two surfaces, the inlet and outlet of the fluid, to Parts.

Set the scalar function and location for the surface average report

Double-click on Surface Average 1, the average pressure at these two faces will show in the Output window.

Average pressure at the inlet and outlet

Similarly, the inlet and outlet mean temperature of the fluid can also be obtained. Right-click on Reports and select Mass Flow Averaged. A new Mass Flow Averaged 1 is created.

Create a mass flow averaged report

Set the temperature as the field function. Again, assign the inlet and outlet faces of the fluid to Parts. Double-click on Mass Flow Averaged 1, the mean temperature of the fluid at these two faces will show in the Output window.

The mean temperature at the inlet and outlet