Physics Setup

Material, Coordinate System, and Thickness

In this section, we will assign the material that we created to our blade, we will create a new coordinate system and we will define the thickness for both parts. 

<iframe width="640" height="360" src="//www.youtube.com/embed/yxAzjxWLCkg" frameborder="0" allowfullscreen></iframe>

Summary of steps in the above video:

1. Material assignment
   1. In Mechanical, under geometry -> assign the composite material. 
2. Define coord. System for the blade elements
   1. Create a new coordinate system, defined by global coordinates, don’t change anything else.
   2. Under where you specified the material, select the coordinate system just created.
3. Thickness
   1. Select all surface bodies in the tree and change the thickness to 0.001m.
   2. Blade variable thickness
      1. Right click Geomery -> Insert thickness
      2. Change scoping method to named selections and choose the blade surface.
      3. Click the small arrow next to the yellow box and select tabular.
      4. Put -1m and -44.2 for x. Next to -1, input 0.1 for thickness and next to -44.2, put in 0.005m. Be careful as the order of the points might change on you. 
   3. Root variable thickness
      1. Do the same thing but for the spar this time.
      2. The tabular data for the spar is -3, 0.1 and -44.2, 0.03.

Remote Point, Remote Displacement, Connections, Large Deflection, Rotational Velocity

We proceed by specifying many other important physics settings like the fixed support and the angular velocity. 

<iframe width="640" height="360" src="//www.youtube.com/embed/krVsJiXlfwQ" frameborder="0" allowfullscreen></iframe>

Summary of steps in the above video:

1. Remote Point
   1. Right-click Model, insert remote point
   2. Select the 4 root edges for the geometry
   3. The point is located at the origin so input 0,0,0 for the coordinates
   4. Change the behavior to rigid
2. Remote Displacement
   1. Right-click Static Structural, insert remote displacement
   2. Change to scoping method to Remote Point
   3. Select the remote point in the yellow box
   4. Put in zeros for all remaining required entries
3. Connections
   1. Delete the automatic contacts that was generated. 
4. Rotational Velocity
   1. Right-click Model, insert remote velocity
   2. Define by components
   3. Magnitude is -2.22 rad/s in the z-component
5. Large deflection
   1. Turn on large deflection in analysis settings
6. Save your project

Importing the Pressure Load

This is the exciting part! We are now at the point where we utilize the pressure results generated from the CFD portion of the tutorial and transfer it to the FEA. 

<iframe width="640" height="360" src="//www.youtube.com/embed/jH7mqKKn9-Q" frameborder="0" allowfullscreen></iframe>

Summary of steps in the above video:

1. Transfer the loads from CFD to FEA in Workbench
   1. Close Mechanical 
   2. Drag the solution cell from the CFD project to the Setup cell of the FEA project
   3. Double-click on physics setup to go back in mechanical and update the upstream data when prompted.
2. Import the pressure in Mechanical
   1. The imported load solution folder will appear in the tree outline. Right-click it and select insert pressure.
      1. For the top field, select the blade surface from FEA the wetted surface. 
      2. For the bottom field, select the blade surface from CFD.
   2. Open the report and check how the forces match and if 100% of the nodes have been mapped. 

Go to Step 5: Numerical Solution

Go to all ANSYS Learning Modules