FLUENT - Forced Convection - Step 3

Step 3: Mesh

In the Workbench window, right click on Mesh, and click Edit. A new ANSYS Mesher window will open. We will create a mesh with 200x30 elements along the pipe. This means that we will divide the pipe with 200 elements in axial direction and 30 elements along the radial direction.

First make sure that the unit we are working on is meter Metric unit. On the top menu, click on Units and make sure that Metric (m, kg, N, s, V, A) is selected.

Since we are going to manually specify meshing type and element size, we should turn off ANSYS build-in advanced sizing function. Under Details of "Mesh", expand Sizing, select Off next to Use Advanced Size Function.
 
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 pipe surface body in the Graphics window and click Apply next to Geometry.
 
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 left and right 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 30 for Number of Divisions.

 

 
Now continue with the sizing in the axial direction.

Outline > Mesh > Insert > Sizing
In the Graphics window, select all the top and bottom edge of the geometry (press Ctrl + mouse click to multiple select). Under Details of "Edge Sizing", click Apply next to Geometry. Enter 0.03 for Element Size (this will give us roughly 200 divisions). Next to Behaviour, change Soft to Hard (This is to overwrite the sizing function employed by ANSYS Mesher. Try meshing with soft behavior and see what you get).

We have specified all the meshing conditions. Click Update on the third menu to see the mesh (Note: disregard the inch unit appear next to the element size. This is recording error. The unit should be in meter).
 
Click on Mesh and look under Details of "Mesh", next to Statistics, you should see that we have 6120 Elements for our mesh.