NE1 know a better way -- cylindrical cam

I'm struggling with something that should be easier, and so I wonder
whether someone can tell me what I'm doing wrong. I'm actually
achieving what I want to achieve, but in a VERY roundabout method. 'S
got to be a better way. One can look at what I've achieved at the
following link, and the panels are numbered 1 thru 4 as I roll down the
History bar in the Feature Tree.

http://www.h2omarkdesign.com/img/cylindrical_cam.jpg

Obviously I'm trying to make a cylindrical cam with a cut that is radial
to the axis of the cam. In order to do it I created a Spline on Surface
(outer surface of the half-cylinder) and used it for a SplitLine
separating the outer surface into two. Then I offset the upper one of
those two surfaces to the inside, and I created a loft surface between
the bottom edge of both the original (SplitLine) surface and the surface
offset from it. That makes a surface which is radial to the center of
the half-cylinder. I used THAT radial loft surface to Cut the original
solid and then I inserted a Body-Delete to obscure all of the remaining
surfaces. That CAN'T be the best way to do it. Somebody perform a
reality check for me, willya?

Thanks,
'Sporky'

 

BTW, if you get a 403 Forbidden error when trying to access that JPEG on
my Web host just try again . . . it seems to come and go for some
reason.

 

zero offset , cut thicken

 

Mark,

I lay the cam out as a flat pattern, and use sheetmetal to roll it up. I
usually program cams as flat patterns, and use "A" axis mapping fpr the 4th
axis. This is much more accurate than programming splines.

Most cylindrical cams have a cross section that's perpindicular to, and
coincident with the axis.

Regards

Mark

 

You can do it with a sweep I think you will get a better profile. I sent
you an example. This was discussed here in October of 2003 I don't remember
the name of the thread.

Corey

 

Yeh, thanks Amigo. I did do that in another incarnation of the cam, and
I agree that's probably a better way in general, since one can use a
function and/or a spreadsheet to drive the cut profile.

Best regards,
'Sporky'

 

Thanks to you and also Kenneth Barrentine who ALSO sent me an example of
a different way to achieve something similar. I learn something new
every day thanks to people like you.

'Sporky'

 

I'll try it. Thanks.

 

Well I'd be happy to put the files up on my Web host, but they're not my
files. I'd need permission. The methods are self-evident by the files,
and not something that was spelled out. But in regards to the sheet
metal method, that can be used to create something that could be molded
if you simply add some draft AFTER the cylindrical cut is create, and
that's what this would be. In that case, the K-factor (or "neutral
axis") is kind of irrelevant. If you use .5 it means no stretch or
compression added (or subtracted) and so the profile used for the cut
would be exactly as if it were "wrapped" around whatever radius
specified. In other words, just because you use the sheet metal
functionality to create the geometry doesn't mean the part has to be
made of sheet metal.

'Sporky'

 

You can post mine.

Corey

 

post it if you like.

 

I have been searching for a better way of creating cylindrical cams for
two years.
As near as I can determine a method is needed to sweep one solid
(representing and endmill) along a path on a part removing intersecting
body. The loft of rectangle sections does not produce the same
geometry as the manufacturing process because the tangent of the side
of the endmill is continuously variable.

Anyone interested experimenting with a technique try Tutorial 5b at:
http://home.pct.edu/~jmather/content/DSG322/SolidWorks_surface_tutorials.htm

If you find a problem with this technique or can demonstrate a better
technique please let me know.

J.D.