Sign-up for free online course on ANSYS simulations!...
Your current Workbench Project Page should look comparable to the following image. Regardless of whether you downloaded the mesh and geometry files or if you created them yourself, you should have checkmarks to the right of Geometry and Mesh.
Next, the mesh and geometry data need to be read into FLUENT. To read in the data (Right Click) Setup > Refresh in the Workbench Project Page as shown in the image below.
After you click Update, a question mark should appear to the right of the Setup cell. This indicates that the Setup process has not yet been completed.
...
First, the mesh will be checked to verify that it has been properly imported from Workbench. In order to obtain the statistics about the mesh (Click) Mesh > Info > Size, as shown in the image below.
Then, you should obtain the following output in the Command pane.
The mesh that was created earlier has 22000 elements. Note that in FLUENT elements are called cells. The output states that there are 22000 cells, which is a good sign. Next, FLUENT will be asked to check the mesh for errors. In order to carry out the mesh checking procedure (Click) Mesh > Check as shown in the image below.
You should see no errors in the Command Pane. Now, that the mesh has been verified, the mesh display options will be discussed. In order to bring up the display options (Click) General > Mesh > Display as shown in the image below.
The previous step should cause the Mesh Display window to open, as shown below. Note that the Named Selections created in the meshing steps now appear.
...
You should have all the surfaces shown in the above snapshot. Clicking on a surface name in the Mesh Display menu will toggle between select and unselect. Clicking Display will show all the currently selected surface entities in the graphics pane. Unselect all surfaces and then select each one in turn to see which part of the domain or boundary the particular surface entity corresponds to (you will need to zoom in/out and translate the model as you do this). For instance, if you select wall, outlet, and centerline and then click Display you should then obtain the following output in the graphics window.
Now, make sure all 5 items under Surfaces are selected. The 
button next to Surfaces selects all of the boundaries while the 
button deselects all of the boundaries at once. Once all the 5 boundaries have been selected click Display, then close the Mesh Display window. The region displayed in the graphics window corresponds to our solution domain.
...
In this section the various solver properties will be specified in order to obtain the proper solution for the laminar pipe flow. First, the axisymmetric nature of the geometry must be specified. Under General > Solver > 2D Space select Axisymmetric as shown in the image below.
Next, the Viscous Model parameters will be specified. In order to open the Viscous Model Options Models > Viscous - Laminar > Edit.... By default, the Viscous Model options are set to laminar, so no changes are needed. Click Cancel to exit the menu.
Now, the Energy Model parameters will be specified. In order to open the Energy Model Options Models > Energy-Off > Edit.... For incompressible flow, the energy equation is decoupled from the continuity and momentum equations. We need to solve the energy equation only if we are interested in determining the temperature distribution. We will not deal with temperature in this example. So leave the Energy Equation set to off and click Cancel to exit the menu.
...
Now, the properties of the fluid that is being modeled will be specified. The properties of the fluid were specified in the Problem Specification section. In order to create a new fluid (Click) Materials > Fluid > Create/Edit... as shown in the image below.
In the Create/Edit Materials menu set the Density to 1kg/m^3 (constant) and set the Viscosity to 3.61e-2 kg/(ms) (constant) as shown in the image below.
Click Change/Create. Close the window.
...
In order to start the process (Click) Boundary Conditions > inlet > Edit... as shown in the following image.
Note that the Boundary Condition Type should have been automatically set to velocity-inlet. Now, the velocity at the inlet will be specified. In the Velocity Inlet menu set the Velocity Specification Method to Magnitude, Normal to Boundary, and set the Velocity Magnitude (m/s) to 0.277 m/s, as shown below.
...
First, select Wall in the Boundary Conditions menu, as shown below.
As can be seen in the image above the Type should have been automatically set to wall. If the Type is not set to wall, then set it to wall. Now, no further changes are needed for the wall boundary condition.
...
In order to save your work (Click)File > Save Project as shown in the image below.
Go to Step 5: Numerical Solution
...