Helical cut on a shaft

I am attempting to model a helical cut on a shaft.

That is, a cut like the spiral that you see on a barbershop pole. But
rather than just a painted red stripe, I want a groove that's the width
of the stripe, and cuts into the cylinder. An example would be a 1/2"
diameter cylinder, with a 1/16" endmill helical cut going around it,
just like the barbershop stripe.

I am coming to the conclusion that it is not an easy thing to do at
all.

Has anyone accurately modeled a helical cut on a shaft?

I now believe it's not as simple as sweeping a rectangular cross
section. This seems right, until I try to model the entry and exit
points of the endmill. These entry and exit points clearly show
there's a problem.

I've tried making the sweeping cross section be tangent to the path of
the helix, and all seems well until modeling the "start" and "end"
positions of the endmill. If they walk off the ends of the barbershop
pole, the error isn't noticable. But if you try to start and end while
still on the barbershop pole, the error is obvious.

Pretty interesting stuff, and frustrating!!!

I read some old posts on a mechanical desktop or something or other
forum, and people were claiming it's not quite possible to do. I'm
beginning to agree with them.

 

Here are some pictures of the endmill exit point I was refering to:

http://www.precisionmechanicaldesign.com/images/helicalcutexit1.jpg

http://www.precisionmechanicaldesign.com/images/helicalcutexit2.jpg

 

Has anyone accurately modeled a helical cut on a shaft?

I think you are correct. Planar sections won't work and the reason is seen if
you consider the "pitch angle" (cutter tangent) for a given pitch helix at
different radii. At the work piece axis (zero rad) the angle is zero, relative
the axis, and moves toward 90 with increasing radius.

The best deal I've found is to model a "ribbon" surface (by what ever means is
available to you) that would represent the trace of the cutter axis. If, for
instance, you use the work piece axis as a sweep trajectory, the helix as the
section X vector control, and section (profile) plane defined as normal to work
piece axis; you can than sweep a line connecting the axis and helix to produce
the desired surface. (You'd actually want to sweep a portion of the line or
trim the surface at groove diameter.) Some "loft" or "blend" functions appear
to work as well, I believe. Depends on how they map the input curves (axis and
helix). Wrapping a curve on cylinder and then surface normal "pulling" it to
groove dia can also give you a good set of curves for a loft type function or
maybe sweep. Doing a symmetric, surface normal thicken of that surface should
produce an accurate groove. Groove walls should be, I can't remember if it
looked like a good rep of groove bottom as cut by an end mill or not. Ball end
would make things just a little more complicated, but I think combining a swept
circle cut and the thicken might work.

(Ya know, I've never actually heard this from a machinist but think what they
will really be interested in is a curve that describes the intersection of the
cutter axis with a cylindrical surface of some (any arbitrary) diameter. I'm
guessing they'd be happier having that curve than trying to reverse engineer it
from model surfaces. More important if the curve isn't something as simple as a
helix (?).)

 

Dr J.D Mather Has some very good tutorials that may be of use checkout 5b.

http://home.pct.edu/~jmather/content/DSG322/solidworks_surface_tutorials.htm

John Layne
www.solidengineering.co.nz

 

James,

Try performing two extruded cuts simulating the plunging of a slot
drill (you can't plunge end mills in the real world) into the start and
end of the helix. This may be difficult to set up, but you should be
able to work it out. Then perfom a sweep along the helix with a
rectangle normal to the helix like you were before. These "plunge
cuts" are good machining practice, and should provide the runout you
need at the end of the helix to overcome this problem. It is something
that you don't notice in the real world and most machinist would not
know about it, as it cannot be distinguished from normal tool chatter
in smaller sizes.

Dominic V.

 

James,

What you are trying to do is actually more complex than one would think.

There are multiple ways to create the slot with actual machine tools. The
most common misconception is that you can just plunge the tool in and then
rotate the part about Y for instance while traversing in X. This will
create a slot with the requested width, pitch and max depth, however the
slot will
be shallower at the side walls due to the undercut created by the diameter
of the tool. The correct way to create such a slot is to use a small tool
(roughly 25% of the slot diameter) and perform a pocketing routine using the
slot outline as your boundary. The easiest way I have found to create this
is to model the slot in 2D then wrap the profile using Y axis substitution
to control the Y rotation. (in mastercam not SolidWorks)

That said, the second method of creating the slot on an actual machine takes
longer than the first to program (not too much though) so we calculate the
undercut for a given tool diameter and pitch then select the appropriate
depth to compensate for that undercut. Then we create the helical blind
slot the easy way as is modeled in the SolidWorks Part below.

You can also make sure your CAM that follows the slot has a generous enough
radius that the undercut doesn't matter.

I have inserted a link below to the part for you to look at in SW2006 SP0

Cadguru

http://home.comcast.net/~productcreationstudio/Simple_Machined_Spiral_Slot.SLDPRT

 

Thanks for the tips guys.

Cadguru, thanks for posting the part. However, my SW2006 is still
sitting in its pretty little box on the shelf. None of my clients have
upgraded yet. I'd love to, but until at least one of my clients do, I
probably won't.

I agree with Jeff Howard - what the machinist probably really wants is
the centerline of the endmill cutting the helix. The rest is sort of
for looks.

For the function of the part, I need to have a pin follow the helical
path. I know if a 1/16" end mill could do it, that a slightly
undersized pin will follow the groove. So really, the rest is just for
looks in my case.

 

You don't have to upgrade to 2006 - just load it as a new installation.
That way you can have both. I install each version in its own folder
such as C:\Program Files\SolidWorks2006 and the same thing with the
common files. However, I don't have toolbox, so there may be an issue
there. Someone that does, please chime in here.

WT

 

Yeah, I'm sure I'll end up using both simultaneously, but I'm not
looking forward to it.

"Ooops, I opened the SW2005 client's files in SW2006...". I'm dreading
the day I do that. The longer I postopone installing 2006 as a second
installation, the longer I'm safe from that happening.

It's frustrating though, because I'd really like to start playing with
it!

 

Here is a link to the part you can open in 2005. It is featureless, but
shows the actual geometry created by the tool in this type of cut path.

Cadguru

http://home.comcast.net/~productcreationstudio/Simple_Machined_Spiral_Slot.x_t

r-click save target as. Then open with SolidWorks 2000-2006