Sign-up for free online course on ANSYS simulations!Unable to render {include} The included page could not be found.
Step 4: Setup (Physics)
In the Workbench window, this is what you should see currently in the Project Schematic space.
Double click on Setup which will bring up the FLUENT Launcher. Click OK to select the default options in the FLUENT Launcher. Twiddle your thumbs a bit while the FLUENT interface comes up. This is where we'll specify the governing equations and boundary conditions for our boundary-value problem. On the left-hand side of the FLUENT interface, we see various items listed under Problem Setup. We will work from top to bottom of the Problem Setup items to setup the physics of our boundary-value problem. On the right hand side, we have the Graphics pane and, below that, the Command pane.
Display Mesh
Let's first display the mesh that was created in the previous step.
Problem Setup > General > Mesh > Display...
The long, skinny rectangle displayed in the graphics window corresponds to our solution domain. Some of the operations available in the graphics window to interrogate the geometry and mesh are:
Translation: The model can be translated in any direction by holding down the Left Mouse Button and then moving the mouse in the desired direction.
Zoom In: Hold down the Middle Mouse Button and drag a box from the Upper Left Hand Corner to the Lower Right Hand Corner over the area you want to zoom in on.
Zoom Out: Hold down the Middle Mouse Button and drag a box anywhere from the Lower Right Hand Corner to the Upper Left Hand Corner.
Use these operations to zoom in and interrogate our mesh.
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, the surface labeled heated_section should correspond to the part of the wall where heating occurs.
Next, we specify that we want FLUENT to solve the axisymmetric form of the governing equations.
General > Solver > 2D Space > Axisymmetric
The energy equation is turned off by default. Turn on the energy equation.
Models > Energy - Off > Edit...
Turn on the Energy Equation and click OK.
By default, FLUENT will assume the flow is laminar. Let's tell it that our flow is turbulent rather than laminar and that we want to use the k-epsilon turbulence model to simulate our turbulent flow. This means FLUENT will solve for mean (i.e. Reynolds-averaged) quantities at every point in the domain. It will add the k and epsilon equations to the governing equations to calculate the effect of the turbulent fluctuations on the mean, as discussed in the powerpoint presentation.
Models > Viscous - Laminar > Edit...
Under Model, select k-epsilon (2 eqn). Since we'll use the default settings for the k-epsilon turbulence model, click OK.
This is what you should currently see under Models.
Now let's move on to setting up the materials properties.
Materials > Fluid air > Create/Edit...
We will use the properties of heated air. Change the Density (kg/m3) from constant to incompressible-ideal-gas.
Enter for following properties for air.
Cp (Specific Heat) (j/kg-k): 1005
Thermal Conductivity (w/m-k): 0.0266
Viscosity (kg/m-s): 1.787e-5
Molecular Weight (kg/kgmol): 28.97
Click Change/Create and Close the Create/Edit Materials window.
Let's set up the boundary conditions now. We will first specify our operating conditions.
Boundary Conditions > Operating Conditions...
Enter 98338.2 under Operating Pressure and click OK.
Next we will specify boundary for centerline.
Boundary Conditions > centerline
Change the Type to axis and click OK.
Now let's set up the heated wall section.
Boundary Conditions > heated_section > Edit...
A new Wall window will open. Click on Thermal tab and enter 3473.9 next to Heat Flux (w/m2) and click OK.
Now let's set the inlet boundary condition.
Boundary Conditions > inlet
Note that the boundary Type is automatically set to velocity-inlet. FLUENT has automatic mechanism to set the boundary condition according to the name you give. So let's click Edit... to set up the correct inlet parameters. A Velocity Inlet window pop out. Enter 25.05 next to Velocity Magnitude (m/s). For Turbulent Kinetic Energy (m2/s2), enter value 0.09. For Turbulent Dissipation Rate (m2/s3), enter value 16. Note that k and epsilon are not measured and are rough guess values. Click OK to close the window.
Now click on Thermal tab and enter 298.15K for Temperature. Click OK to close the window.
Finally, set up the outlet boundary condition.
Boundary Conditions > Outlet
Again, proper pressure-outlet boundary Type is set. Click Edit... to set up appropriate pressure outlet condition. Enter -1112.3 for Gauge Pressure (From experiment, measured outlet pressure is 97225.9 Pa. Corresponding gauge pressure = 97225.9 Pa - reference pressure = -1112.3 Pa)
We are done setting up the boundary conditions.