Flow in Heated Plain Fins Example

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.

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 10 mm.

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.

Similarly, draw the other 2 rectangles in the right.

Apply length dimension to the first rectangle.

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. 

Apply the length dimension as shown in Figure.

Delete the lines in the middle.

Click "ok" to exit sketch mode.

Extrude the sketch with the thickness of 10 mm.

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

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.

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

A construction line is only a reference.

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

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

Right click on “Body 2” and select “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

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

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

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 from the toolbar.

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.

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”.

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

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.

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”. 

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)”.

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

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

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

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

The final mesh will show in the mesh scene.

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

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”.

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

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.

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

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.

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.

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.

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

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.

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

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

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.

Choose energy in the list. 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 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. 

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.

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 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.

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

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

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

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

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

Where

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”.

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”.

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

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.

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

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

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”.

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

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

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

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