Solidworks helix

Is there a way create a helix whose sketch isn't based on a circle? For
instance, could I use a sketch of a triangle with round edges and
create a helicle shape based on that geometry?

 

I have a helical torsion spring model in my models dump,
<http://www.esoxrepublic.com/models/>. This may give you some ideas.

 

1-Use a surface sweep with the twist option to create a surface whose
outside edge is a circle-based helix.
2-Use a second surface sweep (without twist) whose profile is the shape you
want for the helix.
3-Use a surface trim to trim the twisted surface using the profile surface
as the trim tool.
4-The resulting surface should have an egde with the path curve you need.

A similar method might be to use an intersection curve instead of steps 3
and 4.

 

Ben Eadie has a fantastic video tutorial on the most simple way of
making a Helix that I have seen. Visit his mountain-wave site at
http://mountain-wave.blogspot.com/
and download his video labeled "Springs Drawings and Weldments". You
won't find a better tutorial anywhere.

Good luck,
G. De Angelis

De Angelis Tool
Valhalla Grafix
www.deangelistool.com

 

Ben Eadie at: www.mountain-wave.ca has a super simple tutorial on
the creation of a Helix. Go there and download the tutorial labeled
"springs Drawings and Welments". You can search the net, and never find
a better tutorial than that one.
Good luck,
G. De Angelis
Valhalla Grafix
www.deangelistool.com

 

Well what i used to is create a surface sweep on a helix which is
created using circle as a base. then a surface extrude of the shape.
Now open a new 3d sketch and use the option intersection curve
(tools>skecth tools), which will generate a helix with the combination
of both the surfaces.


I wish it helps.

Regards

Deepak Gupta

 

I can't believe I never tried to do that Sweep with a Turn to create a
spring. I've used the Turn option in so many other places, but never
tried a spring. Good find Ben!!

Steve O

 

I was able to create the ideal helical shape, but when I tried sweeping
the threading shape around that helix, the resulting sweep became more
and more distorted throughout its path. Is this a guide lines issue?
Because I tried creating different guide lines, but they didn't seem to
help. And the same distortion occurs if I use a sweeping extrusion or a
sweeping cut.

 

Use a "pierce" constraint to relate the section sketch to the guide
curve.