Modeling Fan or Propeller Blades

Fan or propeller blades are aerodynamic shapes. To have a functional fan or propeller blades you will need to do some calculations or you might already have the data configured for your projects. In this tutorial I will only create a shape from my imagination without a proper dimension. Here's where I'll start:

Start your CATIA program and go to the Part Design workbench (Start > Mechanical Design > Part Design). I will start by creating the hub for the blades to be connected to. Select the zx-plane and start the Sketcher workbench. Draw something like I draw in the 1st picture.

After finishing creating the Sketch.1, exit the Sketcher workbench and you will notice the Sketch.1 link in the design tree. Select the Sketch.1 and click the create Shaft icon or Insert > Sketch-based features > Shaft. Then select the x-axis as the rotation axis. Press OK and the hub will be created.

Now I want to create a drill hole at the center of the hub. Select the front flat surface and click on the Hole icon on the toolbars or Insert > Sketch-based Features > Hole. In the Hole Definition box, select Up to Last for the hole extension type, set the diameter to be 20mm and maybe Countersunk for the hole type. Press OK when you satisfied with the hole.

Then go to the Generative Shape Design Workbench (Start > Shape > Generative Shape Design). Create a new plane using the xy-plane as reference. Set the offset to be around 40mm. After done creating the new plane. Select the plane and click on the Sketcher tool. We are going to make a new sketch on this plane. In the Sketcher workbench, create the starting shape for your propeller blade using the Spline tool. If you want to create a real propeller blade you might need to create points based on your propeller dimension and then connect the points. I just made up the shapes as shown in the next picture.

When you exit the Sketcher workbench it will look like this:

Repeat the steps (creating planes and profiles) with different profile shapes to look like a propeller blade. Mine look like shown in the next picture:

Now in the Surfaces toolbar, select the Multi-Sections Surface tool. (Insert > Surfaces > Multi-Sections Surface). Then when the Multi-Section Surface box appeared. Select all the profiles you have just created. Press the preview button and it will look a bit weird. Don't worry about that. Create the profiles properly next time. In the Coupling tab in the definition box select Tangency for the Sections Coupling. Press OK when done.

Then select the last profile/sketch you've created (mine is Sketch.10). Click the Fill tool on the Surfaces toolbar. When the Fill Definition box appeared. Sketch.10 will appear for the curves. Click on the Multi-Section surface we created before and it will then become the support for the Fill. Set the Fill Continuity as Tangent. Press OK when done and the fill will be a continuation of the Multi-section surface.

Then use the Join tool on the Operations toolbar (Insert > Operations > Join) for the Fill and Multi-Section Surface to make them become 1 entity.

To make things easier, hide everything except those we created in the Part Design Workbench and the Join.1. The go back to the Part Design Workbench. Click on the Close Surface tool, Insert > Surface-based Features > Closed Surface. Then select the Join.1 entity as the object to close. Then press OK.

The Close Surface and Join.1 is now at the same location. Next hide the Join.1 and let only the CloseSurface.1 to be visible. A blade is now created. Next use the Circular Pattern (Insert > Transformation Features > Circular Pattern) to multiply the blade. The Circular Pattern definition box will appear. In the Axial Reference tab, select Complete Crown for the Parameters, select any circular or cylindrical surface for the Reference Direction > Reference Element, and Instance(s) to be 4, 5 or any amount you like. Done. You blades have been created.

A video for this will be uploaded when I have access to faster internet connection.