# Geometry - Region - Physics Continuum

**Geometry**

As in the simulation with virtual disks, the wind turbine studied is the Repower MM70 :

As it is difficult to create a turbine geometry from scratch in StarCCM+, a possible solution is to import an *.stl file created with a CAD software. It is easy to find one on the internet. The one used here is taken from the website GrabCAD.

Firstly, the *.stl geometry file is imported :** Geometry **$\rightarrow$ right click on **3D-CAD models** $\rightarrow$ **New** $\rightarrow$ right click on **3D-CAD model 1 **$\rightarrow$ **import **$\rightarrow$ **CAD models**.

Next, the idea is to modify the bodies to be as close as possible to the geometry of the MM70.

Here, mainly Scaling is used. Finally :

After this step being done, parts need to be created : here, to simplify, only blades and the nacelle will be represented.

**Geometry **$\rightarrow$ **3D-CAD models** $\rightarrow$ **3D-CAD model 1 **$\rightarrow$ **bodies **$\rightarrow$ right click on the body $\rightarrow$ **New geometry part**.

Now, let us create the domain : right click on** Part** $\rightarrow$ **New Shape Part **$\rightarrow$ **Block**. Be careful to create a domain big enough to avoid problems of limit conditions having an impact on the solution. Split the domain's surface** Domaine** $\rightarrow$** Surfaces **$\rightarrow$ right click on **Surface** $\rightarrow$** Split by angles**. Rename the surfaces created (inlet, outlet, side, floor...).

The next step is to create the moving part : it is defined as

To do that, create a cylinder which include the geometry (**Part** $\rightarrow$ **New Shape Part **$\rightarrow$ **Cylinder**). Then, select both part (the geometry part and the cylinder) $\rightarrow$ **Boolean** $\rightarrow$ **Substract parts**. Do the same as before to split the surfaces.

**The region**

Select both the domain and Substract $\rightarrow$ **Assign Parts to region** :

Rename the regions : domain and moving_region.

Now, create an interface : select both region $\rightarrow$ right click $\rightarrow$ **Create interface $\rightarrow$ Overset Mesh**. Check that the interface node created has the moving region as region-0 and the domain as region-1.

Set the boundary conditions : for the moving_region, everything has a type "wall" excepted the cylinder surface whose type is "Overset mesh". For the domain :

**The Physics Continuum**

To create a physics continuum** **right click on** Continua $\rightarrow$ New $\rightarrow$** **Physics Continuum**. Now select the models : right click on **models $\rightarrow$ Select Models**. Select :

It is now generally necessary to add a source term : "This source term is required for such cases because the overset mesh method is not conservative and comes with an interpolation error that prevents residuals from converging. STAR-CCM+ automatically calculates the source term." (starCCM+ documentation).

To activate it : right click on **Models** $\rightarrow$** Edit **$\rightarrow$ **Segregated Solver**

It is now possible to put initial conditions for the velocity (10 m/s here) and turbulence intensity (0.12) :

It is the good moment to set up the boundary conditions (0.12 as turbulence intensity and 10m/s as entering velocity):

The next step is the creation of the mesh