Helix

"Gadget Man" wrote in news:T2v_b.3714$253.479767 @news20.bellglobal.com:

there can be a lot of details involved in this, but the basics are to create a helix, and to make a swept cut (Insert, Cut, Sweep). Check out the help on sweeps to see how to make the profile for the sweep. The helix will be either the Path or the Guide Curve depending on how involved you get with it.

matt

The simplest I can think of is create the proper helix and then sweep cut the profile along it.

WT

1) If it is on a shaft, start a sketch on the end of the shaft. Convert entities, which makes a circle. Exit sketch. 2) Go to view, turn on "curves" 3) Insert > Curves > helix/spiral 4) Set the "starting angle" to "0", this is important. 5) Set the other boxes to suit, OK. 5) Hopefully your shaft is centered on the starting planes, pick the plane that goes thru the "starting point" of the helix/spiral and start a sketch. Draw your profile for the groove and it is helpful (but not absolute) if you make your groove related to the starting point of the helix/spiral. After you define the groove/profile, exit sketch. 6) Insert > cut > sweep [ for threads ]

or

Insert > boss > sweep [ for springs ]

And select the groove for the profile and the helix for the path, hit ok and you are done.

This works great for threads and springs.

I hope this helps.

Dan B.

6

One detail that sometimes people ignore at their peril (and Matt knows this well, but just didn't mention it) . . . make sure your profile extends OUTSIDE the part being cut. If you make the outside of your profile coincident with the outside edge of the solid you may find the the Sweep-Cut will fail. The reason (as I understand it) is that a helix is an approximate function . . . not an entirely accurate function as would be an equation like a binomial expression. Since it is an approximation a coincident relationship may result in a "zero thickness" solid, and a zero thickness solid is an invalid entity.

Mark 'Sporky' Stapleton WaterMark Design, LLC Charlotte, NC