For this tutorial we are going to be using a 2D rectangular geometry. Please download the files here. The Workbench file has geometry and a coarse mesh. We will refine this mesh for solving turbulence.
Open up the project provided above in the Geometry section and then you can follow the next steps.
Right click on Mesh . Then click on Duplicate, which will duplicate the mesh from the previous tutorial. Enter "Turbulent Flow" in the highlighted field to rename it. At this point your project schematic window should appear as below:
Next, double click on the Mesh cell so we can edit the mesh.
We need to change the edge sizing, as we did in the previous tutorial, to 100 by 30 (instead of 100 by 5). We are also going to need to bias it. This is because we want smaller divisions the closer you get to the wall. First, right click on Edge Sizing 2 in the Project tree on the left, and click Delete to remove the existing edge sizing on the inlet and outlet.
Next, we'll apply an edge sizing with bias to the inlet, the left end of the pipe. Click Mesh Control > Sizing. Using the edge selection tool, highlight the inlet (left end) of the pipe and click Apply next to Geometry. As in the Laminar Pipe Flow tutorial, change Type to Number of Divisions, and enter 30. Change Behavior to Hard. Now, let's apply a bias to the edge sizing. Under Bias Type, select the second option, - – — ----. Enter a Bias Factor of 10. Your Details of "Edge Sizing 2" should now appear like the image below.
Now we would like to apply an edge sizing to the outlet, the right end of the pipe. Once again, we'll use 30 divisions, with a bias factor of 10 and with the smaller divisions at the top, near the wall. This time, when selecting Bias Type, choose the first option, ---- — – -. This will put the smallest divisions at the top. Other than this, the procedure is the same as for the inlet. When complete, your Details of "Edge Sizing 3" should look like this:
Right click on Mesh and select "Generate Mesh." The bias factor generates a finer mesh near the pipe wall. This is done to compute the small fluctuation in fluid property near the wall.
Next, close the meshing window to return to the main project view.
The Workbench file already now has the following boundary types created.