Copying a helix in SW04

[ourious78]

How do you copy a helix spiral in SW?? I an trying to draw a helical tooth (Citroen) Gear but I cant figure out how to copy, pattern or mirror the single tooth I have drawn? Also how do you trim and helix/spiral? There's no set pitch, addendum, dedendum, or working depth set for tooth profile just trying to figure out how to do it.

TIA

 

[thermoD]

Look at the picture attached..if it is similar to what you are trying to do, it is actually so easy..after you create your first tooth (I used a loft feature) then create an axis (select the gear body and then create the axis) then use a circular pattern (equal spacing) enter the number of teeth and IT'S DONE..
Good luck

 

[ourious78]

But how did you draw the First tooth? With a helix/spiral? If so How do you terminate the spiral at the end of the extrusion. The trim entities feature is turned off when you select the drawn helix and there isn't a "up to next" available with the spiral draw dialog? Sorry, I haven't really ever used this feature before. What I am trying to draw is almost exactly that picture but mirrored on the midplane of the extrusion. "V" tooth.

TIA

 

[TheTick]

You can not copy a helix or other curve feature. You can copy and pattern features (i.e. a sweep). I think what you want is to copy a pattern of your tooth ("Insert --> Pattern/Mirrot --> Circular Pattern".

sample model:
<

http://www.esoxrepublic.com/models/>

Gear-A-out.zip

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[CorBlimeyLimey]

The helix is used to create the path for a Sweep. Another sketch has to be created at the end of the Helix which is then used to create either a Swept Boss or Swept Cut feature.

Take a look at the Types of Threads example at

http://www.scottjbaugh.com/Design_Portfolio/Design.htm

 

[thermoD]

ourious78,
maybe I am missing something but I didn't use spiral/helix feature..here's what I did:

Extruded the gear body (from a circle), then I made a sketch on the front face of the gear to outline the tooth, then made identical sketch on the back face of the gear, it was shifted 20 deg angle (neither the shape of the tooth nor the angle is related to any of gear standards, I use approx. values to come up with a similar shape)
then you use the LOFT feature to come up with 1st tooth (you have to exit the 2 sketches first) and then continue with circular pattern as I mentioned on my previous post..

I'll add a pic to see these sketch
Good luck

Note: to do you design V-shape, you can have 3 identical sketches one on the front face, one in the back and one in the middle, then use a loft command..if it didn't give you good results, you can draw a center line or use a guide curve to get what you want.

or simply you can use the existing shape and mirror the whole thing

 

[TheTick]

Loft won't give you proper control over the tooth section from one end to another.

The best way to create the tooth would be a sweep with the sweep section held normal to the gear axis (not normal to helix).