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


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

1. Building Geometry

Figure 2 Create a new 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 3 Create a new sketch

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

Grid spacing adjustment of the sketch

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

Draw a rectangle in 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.

Sketch with three rectangles

Similarly, draw the other 2 rectangles in the right.

Apply length dimension

Apply length dimension to the first rectangle.

Apply coincident constraint

Use Ctrl to select the points shown in Figure, and right click to apply coincidence constraint so the width of the second rectangle would be the same as the first one. Apply the same constraint to the third rectangle. 

The dimensions of rectangles

Apply the length dimension as shown in Figure.

The complete sketch for CAD

Delete the lines in the middle.

Exit sketch mode

Click "ok" to exit sketch mode.

FiExtrusion of the sketch

Extrude the sketch with the thickness of 10 mm.

Extrusion of the sketch

The thickness can be arbitrary since the simulation is only two-dimensional.

Create another sketch on face

Only the fluid part would be simulated in this example so the solid part can be cut off. To do this, create sketch on the +z face of the extruded body.

Line projection and construction line

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

Set construction line

A construction line is only a reference.

Draw a rectangle on the new sketch

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

Extrusion of the new sketch

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

Linear pattern cut

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

Parameters of 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

Exit the 3D-CAD mode

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

Rename the 3D-CAD

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

2. Topology

Creating a new geometry part

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.

Create a geometry scene

Create a geometry scene from the toolbar.

Split the default surface

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.

Setting up the boundary surfaces

Name each boundary by selecting the surface from the numbers or from the geometry. 

Setting up the boundary surfaces second step

Set the surface that lies on the xy-plane as “Domain”.

Badge for 2D meshing

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

Execution of badge for 2D meshing

Right-click on “Badge for 2D Meshing” and select “Execute”. The flow domain will now be converted to 2D.

Execution of badge for 2D meshing, step 2

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.

Creating simulation region

Assigned parts to regions and make a change on the boundary option. 

Creating a boundary
Creating simulation region, step 2

A “Region” would be created under “Region” folder. Rename the “Region” under to “Fluid”. 

3. Meshing

Creating mesh operation

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)”.

Mesh model selection

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

Change the case size of the mesh

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

Generating mesh

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

Create a mesh scene

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

Final mesh

The final mesh will show in the mesh scene.

4. Physics Models and Boundary Conditions

Physics model selection

Now we have to decide the physics models for the simulation and set the boundary conditions as well. 

Physics model selection

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
Thermal specification at the wall

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”.

Wall temperature setting

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

Inlet boundary settings

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.

Backflow specification at inlet

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

Fluid wall selection

The walls of inlet and outlet section are considered 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.

Outlet boundary setting

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

5. Preparing Simulation

Figure 36 Create a scalar scene

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 37 select the function of scalar scene

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

Report for mean temperature

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 39 Create monitor and plot from report

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

Figure 40 Maximum iteration steps

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

Figure 41 Create new converging criterion from monitor

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 42 The minimum converging limit for energy

Choose energy in the list. After that, set the “Logical Rule” to “And” and set the minimum limit for “Energy Criterion” to 1E-8. 

Figure 43 Create new converging criteria from monitor

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 44 Solution initialization

From the settings in the stopping criteria, the simulation will stop when all of the converging criteria has been satisfied. Before running the simulation, initial values should be given. Check the initial static temperature and make sure it is 300 K. Then select the icon in tool bar and initialize the solution.

Figure 45 Run the solution

Click run to start the calculation.

6. Post Processing

Figure 46 Temperature contour

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.

Residual plot graph

The temperature contour would be shown in the scalar scene.

Temperature countour diagram

To include the boundary temperature in the contour, change the contour style to “Smooth Filled”. The range of the legend would become 300 K to 350 K.

Figure 47 Mean temperature at the outlet

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

Figure 48 Create a report for mass flow rate

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

Figure 49 Mass flow rate at the outlet

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

Change in enthalpy formula

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

Nusselt number 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

mean temperature formula


Figure 50 Create a line probe

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 51 Plot for the values on the line probe

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

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”.

Set the scale for y-axis

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

Figure 54 Temperature plot along the probe

The temperature profile along the wall can be shown in the plot. It should be noted that the values at the fin section are the temperatures in the cells next to the wall.

Figure 55 Create 3 line probes in between fins

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 56 Rename the line probes

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

Figure 57 Select the parts for plot

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

Switch the x-axis and y-axis

Change the “Vector Quantity” of x-axis to (0, 1, 0) and assign x-axis to left axis. Likewise, assign y-axis to bottom axis. Also click on “Smooth Values”.

Figure 59 Scalar function selection for the plot

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

Line style of the plot

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

Figure 61 Velocity profiles

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

Figure 62 Temperature profiles

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

Example By: Kuan-Ting Lin