Domain - Region - Physics Continuum

 


The Domain

 

First, it is important to create the domain. Its characteristics are gathered here :

In order to do that, first create a new simulation. Then the idea is to create the block:

geometry  $\rightarrow$ parts. Right click New Shape Part $\rightarrow$ Block

 

The domain can be visualized by right clicking on Scene $\rightarrow$ Geometry.

Right click Block $\rightarrow$ rename "Domain"

It is important to split the surface. Indeed, at this point, the surface gather all the boundaries of the domain which would make it impossible to define different limit conditions.

To do that, Parts $\rightarrow$ domain $\rightarrow$ Surfaces. Right click on split by angle. Ok.

Rename every boundaries by right clicking on the surface $\rightarrow$ rename.


The region

Then we have to create the region :

Parts right click on Domain, $\rightarrow$ Assign part to regions.

(be careful to select Create a Boundary for Each Part Surface).

 


Physics continuum

It is now important to create a physics continuum : right  click on Continua $\rightarrow$ New $\rightarrow$ Physics Continuum.

Select the physic required by the simulation. Here :

It is now necessary to enter the characteristics of the wind turbine : StarCCM+ requires the power and thrust curves. So, a file *.csv is created with the wind velocity in the first column, the power in the second and the thrust coefficient in the third.

In StarCCM+ : Tools $\rightarrow$ Table. Right click New $\rightarrow$ File Table.  Choose the *.csv you previously created.

 

Now, one can create the virtual disk in the physics continuum :

right click $\rightarrow$ New right click on virtual disk $\rightarrow$ edit. Method $\rightarrow$ 1D momentum.

The configuration chosen for the first disk is the following :

It is now easier to copy and paste this virtual disk and translate the copy of $2.85 D_{blades}$ by right clicking on Virtual Disk 1 $\rightarrow$ copy $\rightarrow$ paste.

 


Boundary Conditions and Initialization

Now, let us define the boundary conditions (right click on the Boundary $\rightarrow$ Edit) :

One can define a field function as velocity inlet and initialization to represent accurately the atmospheric boundary layer :

Tools $\rightarrow$ right click on field function $\rightarrow$ New $\rightarrow$ Vector. Here, a class 2 wind is used :

Now, this function "in_velocity" can be used as initialized velocity and inlet velocity :

Regions $\rightarrow$ Region $\rightarrow$ Boundaries $\rightarrow$ Domain.inlet $\rightarrow$ Physics values $\rightarrow$ Velocity magnitude (right click $\rightarrow$ edit $\rightarrow$ field function ) and then choose "in_velocity".

The turbulence intensity needs to be 12% on the inlet as well. Physics values $\rightarrow$ turbulence intensity $\rightarrow$ 0.12.

 

The next step is to create the mesh.