Physics Setup

Launch Fluent

...

Check the option "Double Precision". This will make the simulation more accurate, since Fluent will use twice more as many bits in the calculations.

...

It is always a good practice to check the mesh, specially especially if you are importing a mesh that wasn't was not created by you. It is not rare to get matching errors, ; particularly when with meshes with that have multiple Cell-Zones like our casemesh.

In order to do thatcheck the mesh, you can click on Mesh > Check under the , which is located under the upper tab with options, next to File.

You can also note that , when Fluent is first launched, an option to check the mesh was is available , under "General". You can see this highlighted in the above figure.

...

Create mesh interfaces

As briefly discussed before, we need to start by creating the interfaces between the different zones of the mesh.

To account for the rotation of the mesh, we couldn't simply have created cannot simply create one single mesh. Instead, we had to create sub regions , or Zones of meshing.

The mesh created is "non-conformal", i.e. the nodes does do not match across the interface), so we need to tell Fluent that the adjacent cell across that interface share information.

To make the "Interfaces" option appear, first go to "Boundary Conditions". Select the first Zone on the list, "blade_bot_in," and change the type to "Interface". Click OK in the popped window to keep the default name.

Note that the "Mesh Interfaces" option appear appears on the main menu to the left.

Go ahead and set the other interfaces Boundary Conditions. There is no quick way to do that , as Fluent does not allow you to Copy Interfaces Boundary Conditions. So, proceed as before and assign the following Zones to Interface:

...

In our case, each pair of Interface Boundary Condition will be an Interface Zone. So, there will be 4 zones in total.

...

In the first box, "Mesh Interface", write "blade_bot". That's the name of the interface. Select as Under Interface Zone 1 the , select blade_bot_in. For Interface Zone 2, select blade_bot_outer. Click "Create". The window will not close by it self, itself so go ahead and close it.

Repeat this and create the remaining 3 interface zones.

Be careful to select the correct in-outer pairs!!

Note: you don't do not have to close the Mesh Interface window all the time. After clicking "Create" you can go ahead and give the name for the new Interface and create it.

...

Here we can change key information about the solver, like whether it's steady or transient, planar or axisymmetric, etc.

For our problem, you can leave the default options , i.e., Pressure-Based, Steady and Planar.

Lastly, click in "Units" and change the "angular-velocity" unit to rpm.

...

Here is where we tell FLUENT all the simplifications for the model it can assume. For instance, here you specify if the model is Inviscid, Laminar or Turbulent, if you should consider the Energy Equation (for supersonic flows), and other options.

For us, we are will be considering turbulence, and we will use the k-epsilon Realizable model.

Highlight "ModelModels" and double click the third item in the list, "Viscous - Laminar". Select "k-epsilon (2 eqn)". Change "k-epsilon Model" to Realizable. Retain the rest as default. Click Ok.

...

Here we specify to fluent the material of each meshed zone (usually correct by default, unless we create a new material).

Also, we set this if we 're are solving a moving mesh problem or moving frame of reference problem (our case!). We can also set here the centroid of each zone and the angular velocity of that zone here.

Highlight "Cell Zone Conditions". Note that our problem is made out of 5 zones:

• blade_bot: corresponds to the mesh around the bottom blade
• blade_right: similar as above, but for the right blade
• blade_top: againsimilar as above, but for the top blade
• fluid-surface_body: corresponds to the big circular mesh around the main geometry of the turbine.
• inner: corresponds to the zone between the blades , inside the hub.

These are the same zones described previously , when creating the mesh interfaces. We will have to edit parameters for each of them.

...

From the geometry, the centroid is at the global origin (0,0). Verify that that 's is inputted.

From the problem statement, the turbine is spinning at 40rpm, so go ahead and input 40 to "Rotational Velocity". This is the absolute velocity. Note that "absolute" is selected under "Relative Specification". 

...

Under "Turbulence", change the "Specification Method" to "Intensity and Length Scale". Set the "Turbulence Intensity (%)" to 5 and the "Turbulent Length Scale (m)" to 1.

Pressure at the outlet

Locate and highlight "farfield2". Change its Type to "pressure-outlet".

...

Go to Step 5: Numerical Solution

Go to all (ANSYS or FLUENT ) Learning Modules