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.
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.
The Reynolds number of the offset-strip fin is defined as:
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.
- 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
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.
Create a sketch by right-clicking on the XY plane and select Create 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.
Right-click on the lines to apply dimensions and set the length and width as in the figure. Click OK to exit the sketch.
Right-click on Sketch1 and extrude for 0.01 m.
Right-click on the top surface and create a sketch on the +z face.
Use the icon in the display option to view the x-y plane in the sketch if the scene has been rotated.
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.
Draw a rectangle from the construction line and set the dimensions as in the figure.
Select the bottom-left point and set the y-coordinate. Then click OK to exit the sketch.
Right-click on Sketch2 and extrude the body into the first block.
Expand Bodies in the tree. Right-click on Body2 and use the linear pattern tool.
Set the distance in the x-direction to 0.0048 m and the number of instances to 2.
Right-click on the top surface again and create another sketch on the +z 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.
Right-click on Sketch3 and extrude.
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.
Right-click on Body1 and rename it to Fluid. Rename the other bodies from Fin1 to Fin4 in sequence.
Use Shift to select all the bodies, then right-click and use the subtract in 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.
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.
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.
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:
-y and +y: Symmetry
Right-click on the 3D-CAD Model 1 and select “New Geometry part”. Use default settings and click OK.
Create a geometry scene from the toolbar.
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 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.
The final surfaces of each part would be as in the figure.
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”.
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”.
Change the type of Fins in the Region to a solid 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.
A new directed mesh is created under operation. Right-click on it and select edit.
The surfaces for the source mesh and target mesh need to be specified.
For the source mesh, assign all the bottom surfaces in the bodies to it.
Similarly, assign all the top surfaces to the target mesh.
Right-click on Source Meshes and select Patch Mesh.
To have a better view on the xy-plane, use the view from +z direction.
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.
Use the scissor tool to add four additional dots on the lines. Then use ESC to dismiss the scissor function.
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.
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.
After connecting all the dots, the color of the lines will turn to green.
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.
The final surface mesh will be constructed after finishing the settings. Then click Close.
Right-click on Mesh Distribution and select New Volume Distribution. Set the number of layers to 100. Select Close Directed Mesh
Use the icon to generate volume mesh.
Create a mesh scene to check on the mesh in the window.
The final mesh can be visualized in the mesh scene.
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.
To enable the required physics models for Fluid, expand Fluid and double-click on “Models” and select the following models in the order of:
- Three dimensional
- Segregated flow
- Constant density
- Segregated fluid temperature
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.
To enable the required physics models for Fins, expand Fins and double-click on “Models” and select the following models in the order of:
- Three dimensional
- Segregated flow
- Constant density
- Segregated solid energy
Assign the Fluid and Fins physics continuums to Fluid and Fins regions, respectively.
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.
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.
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 thermal boundary conditions at the top and bottom plates. First, expand Fluid and set thermal specification to temperature and set the temperature to 400K.
Repeat the process to the top plate in Fluid, and the top and bottom plates in Fins.
Change the type of the boundary of Symmetry in Fluid and Fins to Symmetry Plane.
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.
Change the view of the scalar scene.
In the scalar scene, right-click on the legend and select the temperature function.
Expand Scalar Scene 1 under Scenes, assign the whole regions to the Parts so that it will show in the window.
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.
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.
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.
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.
Select the green icon in toolbar and initialize the solution. Click run to start the calculation.
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.
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.
Set the coordinate and the normal vector of the plain. Select No Displayer. After finishing the settings, click Create.
Create a new scalar scene from the tool bar.
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.
The scalar scene will show the temperature distribution at the selected plane section.
Similarly, by assigning the velocity magnitude to Scalar Field, the velocity contour will be shown in the scalar scene.
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.
Set the pressure as the field function. Assign two surfaces, the inlet and outlet of the fluid, to Parts.
Double-click on Surface Average 1, the average pressure at these two faces will show in the Output window.
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.
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.