Connecting spiral and sketches to path

Hello,

I need to make a spring in SW. Essentially it consists of a
curved piece on plane1, then a spiral that goes up to plane2,
and then another curved piece on that plane. I can do the pieces
separately but I don't know how to connect them to form a single
curve along which I could extrued the cross-sectional feature.

Of course I don't really need to design that damn spring in SW;
it's going to be bent by hand until it fits, but for a
presentation I'm doing it would be nice to have it in the assy.

Any tips?

--Daniel

 

Look in help under Composite Curve.

HTH,
Muggs

 

I usually don't do entire springs as a single path. Many reasons for
this.

Usually I sketch the ends' positions in a master sketch that controls
the helix. I make the helix sweep, then the ends as separate features.
I use spherical revolves to fill the gaps between ends and helix.

I have always modelled torsion spring arms on planes normal to spring
body axis. I have tinkered with modelling springs with ends that ome
off tangent to the coil direction (not normal to main body axis). This
falls apart after the first bend if there are bends in the end arms.

I have some torsion spring samples at
<http://www.esoxrepublic.com/models/>
TorsionSpringByTheTick.zip
Hinge.zip (includes barrel-shaped torsion spring with multiple
positions)

 

There are several spring models on 3DCC under User Library/Hardware/Springs.
I have used several of them. I would think you would find one that at least
gets you most of the way there.

WT

 

Draw all the elements you just mentioned, the two flat ends and the helix.

open a 3D sketch and use Convert Entities to bring them into the 3D sketch

use Split Entities (Tools, Sketch Tools, Split Entities) to "trim" both
the planar ends and the helical sketch entity back so you can transition
smoothly between them

turn the unwanted sections of the sketch entities into reference geometry

draw a two point spline between the trimmed back ends of the helix and
the flat, and assign tangency or equal curvature to the ends.

exit the 3d sketch and make it the path for a sweep.

here's an example:

www.dezignstuff.com/swparts/spring.zip

 

Not quite your problem - but it should give you an idea on general
solutions.
http://home.pct.edu/~jmather/content/DSG322/SolidWorks Tutorials/SolidWorks Tutorial 7.pdf

 

I did, but it didn't work. It wouldn't let me join the 2D sketches of the
end pieces to the spiral.

I've now found out why: I can only join 3D sketches to the spiral. So I
made a couple of 3D "glue" sketches, each with a spline between the
straight end pieces and the spiral.

Speaking of 3D sketches: Boy, do I hate them. All I wanted to do was, in
straight Top view, to draw a spline, merge its end points to existing
curves (both in the Top plane), make the spline tangential to those and
be done with it. Fiddle, fiddle, fiddle. Red curves all over the place.
Then I rotate the model a bit to see what's going on, and I see that there
is a mile-long loop of spline jutting into outer space along Y. Why is
that?

--Daniel