Flow in Heated Plain Fins Example

Learning Outcome

Students would be able to build a flow domain and do basic convection heat transfer simulation after finishing this example.

Introduction to the problem

Plain fin is widely used in the industry to extend the heat exchange surface. In this example, we simulate the flow between heated plain fins. The model consists of an inlet section, plain fin section, and an outlet section. Pressure and temperature are specified at the inlet boundary, and on the other hand, the outlet is set as atmospheric pressure. Temperature of the heated plates is maintained at 350 K.

Figure 1 Schematic view of the model

Figure 1 Schematic view of the model

Steps

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

1. Building Geometry

To begin with, we will need to create the geometry of the flow domain. Right-click on the 3D-CAD Models and select “New” to start building a CAD model.

Figure 2 Create a new geometry

Figure 2 Create a new geometry

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

Figure 3 Create a new sketch

Figure 3 Create a new sketch

For our convenience, we will set the grid spacing of the sketch to 10 mm.

Figure 4 Grid spacing adjustment of the sketch

Figure 4 Grid spacing adjustment of the sketch

Draw a rectangle that starts from the origin and right-click to apply the fixation constraint at the sketch origin so that the bottom left corner of the rectangle will be fixed when we give the dimensions later.

Figure 5 Draw a rectangle in sketch

Figure 5 Draw a rectangle in sketch

Similarly, draw the other 2 rectangles in the right and specify the lengths as shown. Then, Delete the lines in the middle. 

Figure 6 The complete sketch for CAD

Figure 6 The complete sketch for CAD

Click “ok” to exit the sketch and extrude the sketch with the thickness of 10 mm.

Figure 7 Extrusion of the sketch

Figure 7 Extrusion of the sketch

Since we are not simulating the solid parts, we can now cut them out. Create sketch on the +z face.

Figure 8 Create another sketch on face

Figure 8 Create another sketch on face

Right click and project the line to sketch and set it as a construction line. A construction line is only a reference.

Figure 9 Line projection and construction line

Figure 9 Line projection and construction line

Draw a rectangle on the construction line with the length of 90 mm and the width of 2 mm.

Figure 10 Draw a rectangle on the new sketch

Figure 10 Draw a rectangle on the new sketch

Extrude the sketch towards the geometry with the distance of 10 mm and set the body interaction to none.

Figure 11 Extrusion of the new sketch

Figure 11 Extrusion of the new sketch

Right click on “Body 2” and select “Linear Pattern Cut.”

Figure 12 Linear pattern cut

Figure 12 Linear pattern cut

Set the parameters as in the following figures, then the solid parts would be cut out.

Direction: (0,1,0)

Distance: 18 mm

Number of instances: 6

Figure 13 Parameters of linear pattern cut

Figure 13 Parameters of linear pattern cut

Close 3D-CAD and go back to the main panel.

Figure 14 Exit the 3D-CAD mode

Figure 14 Exit the 3D-CAD mode

Rename the body that was created in the 3D-CAD to “Fluid”. 

2. Topology

We will need to prepare a topology for simulation. The flow domain and the boundary faces would be determined in this step. Right-click on the Fluid and select “New Geometry part” and click ok by agreeing to use the default settings.

Figure 16 Creating a new geometry part

Figure 16 Creating a new geometry part

Create a geometry scene from the toolbar.

Figure 17 Create a geometry scene

Figure 17 Create a geometry scene

Rename “Body1” to “Fluid” and expand the “Surfaces” under the fluid. Right-click on “Default” and select “Split by Patch”. Be sure you have created the geometry scene before you execute this command.

Figure 18 Split the default surface

Figure 18 Split the default surface

Name each boundary by selecting the surface from the numbers or from the geometry. Set the surface that lies on the xy-plane as “Domain”.

Figure 19 Setting up the boundary surfaces

Figure 19 Setting up the boundary surfaces

Right-click on “Fluid” in “Parts” and select “Badge for 2D Meshing” and click ok. 

Figure 20 Badge for 2D meshing

Figure 20 Badge for 2D meshing

Right-click on “Badge for 2D Meshing” and select “Execute”. The flow domain will now be converted to 2D. The solid icon under the “Surfaces” represents the flow domain and the empty icon represents the boundary. The “Default” surface will not be used in the future simulation.

Figure 21 Execution of badge for 2D meshing

Figure 21 Execution of badge for 2D meshing

Assigned parts to regions and make a change on the boundary option. A “Region” would be created under “Region” folder. Rename the “Region” under to “Fluid”. 

Figure 22 Creating simulation region

Figure 22 Creating simulation region

3. Meshing

Before simulation, we have to discretize the calculation domain, which also called meshing. We can do it by creating the mesh from “Fluid” under “Parts”. Use “Automated mesh” instead of “Automated mesh (2D)”.

Figure 23 Creating mesh operation

Figure 23 Creating mesh operation

Select “Surface Remesher” and “Trimmed Cell Mesher” as the meshing models.

Figure 24 Mesh model selection

Figure 24 Mesh model selection

“Automated Mesh” will be created under “Operations”. Change the base size to 1 mm.

Figure 25 Change the case size of the mesh

Figure 25 Change the case size of the mesh

Click on the icon in the toolbar to generate the mesh.

Figure 26 Generating mesh

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

Figure 27 Create a mesh scene

Figure 27 Create a mesh scene

The final mesh will show in the mesh scene.

Figure 28 Final mesh

Figure 28 Final mesh

4. Physics Models and Boundary Conditions

Now we have to decide the physics models for the simulation and set the boundary conditions as well. To enable the required physics models, double click on “Models” under “Continua” and select the following models in the order of:

  • Two dimensional
  • Steady
  • Gas
  • Segregated flow
  • Constant density
  • Laminar
  • Segregated fluid temperature
Figure 29 Physics model selection

Figure 29 Physics model selection

After finishing the selection of physics models, we will set the boundary conditions face by face. The default settings of all the boundaries would be wall, so we have to change them accordingly. The boundary condition of the heated plain fins is wall with constant temperature. Since the boundary of “Fluid.Fins” is already wall, we will expand the “physics conditions” and change the thermal specification to “Temperature”.

Figure 30 Thermal specification at the wall

Figure 30 Thermal specification at the wall

Set the static temperature under “Physics Values” to 350 K. Now, the boundary condition of the plain fins has been specified.

Figure 31 Wall temperature setting

Figure 31 Wall temperature setting

We will then set the inlet boundary condition. Go to “Fluid.Inlet” and change the type of the boundary to pressure outlet and set the value of pressure to 0.2 Pa.

Figure 32 Inlet boundary settings

Figure 32 Inlet boundary settings

Set the backflow specification to “static” to keep the inlet pressure as we set earlier.

Figure 33 Backflow specification at inlet

Figure 33 Backflow specification at inlet

Go to “Fluid.Outlet” to set the boundary condition of outlet. Change the type of the boundary to pressure outlet, and leave the pressure as default, which is 0 Pa. It is noteworthy that the pressure is the gauge pressure.

Figure 34 Outlet boundary setting

Figure 34 Outlet boundary setting

We consider the walls of inlet and outlet section as adiabatic walls so that there will be no heat exchange at these surfaces. To achieve this, go to “Fluid.Wall” and make sure the type of boundary is wall.

Figure 35 Adiabatic wall at the inlet and outlet sections

Figure 35 Adiabatic wall at the inlet and outlet sections

5. Preparing Simulation

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

Figure 36 Create a scalar scene

Figure 36 Create a scalar scene

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

Figure 37 select the function of scalar scene

Figure 37 select the function of scalar scene

In order to show the mean temperature at the outlet, use “mass flow averaged” in “Reports”. Choose the temperature for the field function and the outlet for parts.

Figure 38 Report for mean temperature

Figure 38 Report for mean temperature

Right-click on “Mass Flow Averaged 1” and select “Create Monitor and Plot from Report” to monitor the temperature while calculating.

Figure 39 Create monitor and plot from report

Figure 39 Create monitor and plot from report

Next, we will have to provide the stopping criteria for the simulation. Set the maximum steps of iterations to 10000 under “Stopping Criteria”.

Figure 40 Maximum iteration steps

Figure 40 Maximum iteration steps

We can also set the stopping criteria by checking the residuals instead of giving a fixed iteration step alone. Right-click on “Stopping Criteria” and create new criterion from monitor.

Figure 41 Create new converging criterion from monitor

Figure 41 Create new converging criterion from monitor

Choose energy in the list. After that, set the “Logical Rule” to “And” and set the minimum limit for “Energy Criterion” to 1E-7. 

Figure 42 The minimum converging limit for energy

Figure 42 The minimum converging limit for energy

Repeat the previous steps and create 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. 

Figure 43 Create new converging criteria from monitor

Figure 43 Create new converging criteria from monitor

From the settings in the stopping criteria, the simulation will stop when the maximum iteration steps is reached or all of the converging criteria has been satisfied. Select the icon in tool bar and initialize the solution.

Figure 44 Solution initialization

Figure 44 Solution initialization

Click run to start the calculation.

Figure 45 Run the solution

Figure 45 Run the solution

6. Post Processing

Post processing is rather important because we need to examine the result and further analyze it. After finishing the simulation, the temperature contour will be shown in the scalar scene.

Figure 46 Temperature contour

Figure 46 Temperature contour

Double click on “Mass Flow Averaged 1” from “Report” then you can get the mean outlet temperature.

Figure 47 Mean temperature at the outlet

Figure 47 Mean temperature at the outlet

Create a new report for mass flow and assigned fluid outlet to “Parts” at the properties window.

Figure 48 Create a report for mass flow rate

Figure 48 Create a report for mass flow rate

Double click on “Mass Flow 1” than you can get the mass flow rate at the outlet.

Figure 49 Mass flow rate at the outlet

Figure 49 Mass flow rate at the outlet

The total heat transfer rate Q can be determined by the change of enthalpy

Change in enthalpy formula

where m is the mass flow rate, Cp is the specific heat, Tout is the outlet temperature, and Tin is the inlet temperature. Nusselt number can then be obtained from the total heat transfer rate Q and the log-mean temperature difference Delta Tlm

Nusselt number formula

where

mean temperature formula

For further examination, we can create a line probe and see how the flow temperature varies along the line. The line probe will locate at the vicinity of one of the fin walls. Right-click on “Derived Parts” and create a line from the menu. Set the coordinate of point 1 and point 2 to (0 mm, 54 mm, 0 mm) and (290 mm, 54 mm, 0 mm), respectively. Change the resolution to 50. Select “No Displayer”.

Figure 50 Create a line probe

Figure 50 Create a line probe

Right-click on “Plot” and create a XY plot.

Figure 51 Plot for the values on the line probe

Figure 51 Plot for the values on the line probe

Left-click on “XY Plot 1” and click on “Parts” in the properties. Select “XY Plot 1” under “Derived Parts”. Expand “XY Plot 1” and assign temperature to the scalar function under “Y Types”.

Figure 52 Parts and scalar function selection for the plot

Figure 52 Parts and scalar function selection for the plot

Change the maximum and the minimum values of y-axis to 350 K and 300K.

Figure 53 Set the scale for y-axis

Figure 53 Set the scale for y-axis

Figure 54 Temperature plot along the probe

Figure 54 Temperature plot along the probe

Similarly, we can create line probes in between fins.Right-click on “Derived Parts” and create a line from the menu for 3 times.

Line 1: (60 mm, 38 mm, 0 mm) and (60 mm, 54 mm, 0 mm)

Line 2: (95 mm, 38 mm, 0 mm) and (95 mm, 54 mm, 0 mm)

Line 3: (130 mm, 38 mm, 0 mm) and (130 mm, 54 mm, 0 mm)

Change the resolution to 15.

Figure 55 Create 3 line probes in between fins

Figure 55 Create 3 line probes in between fins

Rename the 3 lines to 10 mm, 45 mm and 80 mm at the corresponding location.

Figure 56 Rename the line probes

Figure 56 Rename the line probes

Create a new XY Plot and assign the line 10 mm, 45 mm and 80 mm to the parts in the plot properties.

Figure 57 Select the parts for plot

Figure 57 Select the parts for plot

Change the “Vector Quantity” of x-axis and assign x-axis to left axis. Likewise, assign y-axis to bottom axis.

Figure 58 Switch the x-axis and y-axis

Figure 58 Switch the x-axis and y-axis

Expand “Y Types” and select velocity magnitude in the scalar function for velocity profile. Similarly, Select temperature in the scalar function for temperature profile.

Figure 59 Scalar function selection for the plot

Figure 59 Scalar function selection for the plot

Expand the line probes and select the line style in the properties to connect all of the data points.

Figure 60 Line style of the plot

Figure 60 Line style of the plot

The final velocity profile will show in the plot if the velocity magnitude is selected as the scalar function.

Figure 61 Velocity profiles

Figure 61 Velocity profiles

The final temperature profile will show in the plot if the temperature is selected as the scalar function.

Figure 62 Temperature profiles

Figure 62 Temperature profiles

Example By: Kuan-Ting Lin