FLUENT - Flat Plate Boundary Layer - Mesh

Step 3: Mesh

In this section the geometry will be meshed with 3000 elements. That is, the field will be divided into 50 elements in the x direction and 60 elements in the y direction.

Launch Mesher

In order to begin the meshing process, go to the Workbench Project Page, then (Double Click) Mesh.

Default Mesh

In this section the default mesh will be generated. In order to generate the default mesh first click on Mesh, then click on Update as shown in the image below.



You should then obtain the following mesh.

Mapped Face Meshing

For this particular problem, we are interested in creating a grid style of mesh that can be mapped to a rectangular domain. This meshing style is called Mapped Face Meshing. In order to incorporate this meshing style (Click) Mesh Control > Mapped Face Meshing as can be seen below.

Now, the Mapped Face Meshing still must be applied to the air field geometry. In order to do so, first click on the surface body(filled rectangle), which should then highlight green. Next, (Click) Apply in the Details of Mapped Face Meshing table, as shown below.




This process is shown in the link below.


Now, generate the mesh by clicking Mapped Face Meshing.

Edge Sizing

The desired mesh has specific number of divisions in the x direction and a specific number of divisions in the y direction. In order to obtain the specified number of divisions Edge Sizing must be used. The divisions in the x direction will be specified first. Now, an Edge Sizing needs to be inserted. First, (Click) Mesh Control > Sizing as shown below.

Now, the geometry and the number of divisions need to be specified. First (Click) Edge Selection Filter, . Then hold down the "Control" button and then click the bottom and top edge of the rectangle. Both sides should highlight green. Next, hit Apply under the Details of Sizing table as shown below.




Now, change Type to Number of Divisions as shown in the image below.




Then, set Number of Divisions to 50 as shown below.



Next, set the Behavior to Hard as shown in the image below. This step will disable the ANSYS Mesher from overwriting any of our edge sizing specifications.



At this point, the edge sizing in the the y direction will be specified. Follow the same procedure as for the edge sizing in the x direction, except select the left and right side instead of the top and bottom and set the number of division to 60. Remember to set the Behavior to Hard. Then, click Update to generate the mesh with the new specifications. You should obtain the following mesh.




Your mesh should now have 3,000 elements (50x60). In order to check how many elements your mesh has, expand Statistics under "Details of Mesh" as shown below.



Make sure that you also have 3,00 elements.

Meshing Method

We would also like to create a structured mesh where the opposite edges correspond with each other. Let's insert a Mapped Face mesh.  Under Outline, right click on Mesh, move cursor to Insert, and select Mapped Face Meshing. Alternatively, you can click on Mesh Control on the third menu and select Mapped Face Meshing. Finally select the flat plate surface body in the Graphics window and click Apply next to Geometry.

This is what you should end up with;

 

Edge Sizing

Now let us move on to specify the element sizing along the pipe radial direction.
Outline > Mesh > Insert > Sizing
In the Graphics window, select both the top and bottom edges of the geometry (click on the Edge tab on the Fluid flow Fluent - Mesh window and then press Ctrl + mouse click to multiple select). Under Details of "Edge Sizing", click Apply next to Geometry. Change the edge sizing definition Type to Number of Divisions. Enter 50 for Number of Divisions. Next to Behaviour, change Soft to Hard

You should have something that looks like this;

 
Now continue with the sizing in the y-axis direction.

Outline > Mesh > Insert > Sizing
In the Graphics window, select the left side edge of the geometry (press Ctrl + mouse click to multiple select). Under Details of "Edge Sizing", click Apply next to Geometry. Change the edge sizing definition Type to Number of Divisions. Enter 60 for Number of Divisions. Next to Behaviour, change Soft to Hard (This is to overwrite the sizing function employed by ANSYS Mesher). Then under Bias Type enter 100.

 

 You should get this;

 
Now follow the same steps for the right side edge sizing as delineated for the left side above.

Now you should get something like this:

We have specified all the meshing conditions. Click Update on the third menu to see the mesh.

It should look like this;

Click on Mesh and look under Details of "Mesh", next to Statistics, you should see that we have 6120 Elements for our mesh.

Create Named Selection

Next, we will name the edges accordingly so that we can specify the appropriate boundary conditions in the later step. We know the bottom edge of the geometry is the center line of the flat plate, the left edge is the inlet of the flat plate, the right edge is the outlet, top side edge is the far field. Remember to click on the Edge tab on the Fluid flow Fluent - Mesh window and then press Ctrl + mouse click to multiple select the 3 line sections that make up the center line before naming it.

Select the left edge and right click and select Create Named Selection. Enter Inlet and click OK. Under Outline, you will see the name Inlet under Named Selections. Note that the flat plat surface is designated as the center line.

Finish naming rest of the edges. 

Finally, click Update.

Go to Step 4: Setup (Physics)