2 Replies Latest reply on Aug 15, 2013 8:44 AM by John Burrill

    Propeller modelling

    Gaurav Yadav

      Hello everyone.I am trying to create a propeller geometry in Solid works.I have to arrange different airfoil sections at different radial positions from the center.I have created the profiles as planner sections as given in the dataset,now

      I want to bend them at different radius.Is there any option available in Solidworks for this.

      Thank You

        • Re: Propeller modelling
          Chris Michalski

          Research the "wrap" function.  This will wrap a flat sketch around a curved surface. 

          • Re: Propeller modelling
            John Burrill

            Gaurav, I may be oversimplifying the process of propeller design, but what you'll probably need to do is create a guide curve to describe the path of of your cross sections as the propeller surfaces transition.  You may also want to create an alignment curve that controls the orentation of each section. 

            Create reference points (reference goemetry toolbar) along the guide curve using stationing or equal spacing or percentage along curve and then create a sketch plane  perpendicular to the guide curve at each point. 

            Now mount your sections to your planes.  It's not clear how you're

            getting your sections into SolidWorks, so I'll assume you've got them in DXF and you're going to import them one at a time onto your planes.  Use the DWG import wizard if that's the case.

            In each section sketch you'll need to create or identify a point where that helical path intersects the section plane.  If you made an alignment curve you will want to establish a point in each section that intersects that curve. 

            At this point, you're going to construct boundary surfaces to connect your sections and fill surfaces to create the rounded end. 

            You model a single propeller blade and then pattern it about an axis.

            Couple of recommendations:

            First, you want to simplify your blade cross sections so that they have as few sketch segments as possible.  You're probably starting from CMM collected data and that probably means you've got hundreds of points per sections which is way to many.  Irregularities turn into surface defects, tangency becomes difficult to control and rebuild times escalate.  If your metrology software hasn't done it for you, you'll need to normalize the number of points and generalize the segments into less than a dozen sketch segments.  Ideally, all of your sections should have the same number of sketch segments.

            Second when you create your boundary, turn off 'merge result' so that you don't get hung up on blending the blade into the hub.  It's a lot easier to add a transition between the blade and the hub after you have the solid bodies than it is to set up the boundary and sections so that the feature lands on the hub .  When I model fan blades, I make the geometry pass well inside the hub so that I can blend the interface with a fillet.

            To align the section geometry, draw a line between your first and second guide curve points and create a block from all of the sketch goemetry.  Then make a point that intersects the alignment curve (pierce sketch relation) You can then add a coincident relation between the first point and the path guide and a coincident relation between the line that you drew and that point that's coincident to the alignment guide.  Using a line to create the coincident relation instead of a another point gives you some flexiblity for the inaccuracies in splines and physical measurements.  It's easier to hit a pitch with a bat than it is to hit it with another baseball.