SUCCESS!! A toolpath cut normal to a cylinder (cylindrical cam)

Anyone else besides me think that the Offset Surface oughta work

Mark, when you say "radial surface" do you mean something like what's in
the screenshot_cam.jpg? If it is, the easiest way to see why that won't
work well is to simply create a planar sketch of an arc of, say, 320
degrees rotation and offset that. Offset it to the inside and outside by
some distance. If you draw rays thru the arc end points they should
intersect at the arcs' center. The same thing happens when offsetting
surfaces. (Also applies to emboss type features which work by creating
surface offsets.)

If, on the other hand you when you say "radial surface" you mean something
like J.D.'s example; it should work for groove sides when "mid" offset or
thickened (I have a theory that using a "thicken" function will also give
you a good groove bottom surface). If you think it's not working can you
explain?

 

Hello All,
I sent this to spork, but you all might have a look:

http://home.comcast.net/~muggs828/solidworks/3-inch_Dia-3.SLDPRT

It avoids the offset surface problem, but still doesn't seem to be right.

Muggs
Change "home" to"comcast" to reply

 

I would have thought that sweeping along a path created by the Wrap
feature

Hi, John. Sorry 'bout my email goof up. Guess "---" isn't going to get it
anywhere.

I have to occasionally "re-learn" why sweeping a 2D section doesn't work
well. Visualizing the reason is pretty simple though (unless I'm confusing
myself again). Simply wrap an inclined line around a cylinder (a helix).
Offset the wrapped curve to a smaller diameter cylinder. These two curves
could represent sweep paths for the groove ID and OD but they have
different normal angles. The difference changes with offset distance; if
you offset to 0 diameter the curve is equivalent to the cylinder axis. A
planar section is only good for pure annular (revolving about cylinder
axis) or axial (parallel to cylinder axis) cuts (or so I believe).

 

What a wonderful discussion, thanks folks this is very entertaining and
educational.

A DUMB QUESTION, though...

I can't claim to be a SW guru, so perhaps I'm just missing something and
somebody here can *_edumacate_* a goofy Southern boy with wa-a-ayy too much
*_edumacation_*. I read, and re-read, the posts, and didn't see anything
addressing my question.

Consider this:

Since the cam follower path is explicitly defined by a function of (x,
theta) where 'x' is the distance of the path in the direction of
longitudinal axis of the cylinder and 'theta' is the rotational component of
the path on the cylinder

Then why is it not possible to:
(a) program a Visual Basic macro of API calls that creates 3D points around
the cylinder (on surface or at a depth...no matter)
(b) create a 3D spline through the 3D points
(c) put a plane normal to the endpoint of the spline
(d) put a cutting profile sketch on the normal plane
(e) sweep-cut a path along the spline?

I played around with this concept briefly, manually creating abitrary 3D
points through a solid object, 3D spline, planes, sketches, 3D sweep. I
couldn't figure out how to sweep-cut, though, even though the Help says I
can do this (getting too old & lazy, need more coffee). Once upon a time I
had
done something very similar with Alibre Design and THAT's where I got the
idea.

It seems like this would be straightforward to do this. I can't say if the
geometry would be accurate, tho.

The original idea that I had was to program a VB macro to create a kazillion
3D points around the surface of the cylinder, create a sketch plane at each
point, then extrude-cut the cutter shape all the way around the cylinder as
if it was an actual machining process. But I figure that method would have
created a
monster part file, so I dropped that idea.

Comments?

Kev

 

"I think what we really need is a way to sweep one solid (endmill) along a
path on
another solid resulting in the intersecting body being removed - just
like the actual machining operation."

This is the method I like to use.

Best Regards,
Devon T. Sowell
www.3-ddesignsolutions.com

 

This is the method I like to use.

Show me an example. I was not aware that it was possible to sweep one
solid along a path on another solid with the resulting intersection
removed. Please try this problem before replying and provide example
files. You can post files at the SolidWorks forum at mcadforums.

 

: Stepping through the tutorial, it doesn't appear to model what and endmill
: would cut. The cam path generated is the shape left by a flat rectangle
: swept around the path. Since the endmill has width, there will be parts of
: the profile that do not appear to form a smooth surface.If you made an SLI
: cam from this model, a cylindrical cam follower would bind in it.

You're right. The tool profile or cross section needs to be always normal to the
cut C/L for the model geometry of the cut to be realistic.

David Janes

 

You're right. The tool profile or cross section needs to be always normal
to the

David, I believe the problem (with a swept planar section) is that there is
not a constant normal direction. To cut an accurate groove the plane of
the section must warp to match differences in what can essentially be
thought of as "pitch angle" at different radii. Or, I might just be
confusing myself. Anyhow, I've posted a STEP from a WF2 model at

http://www.mcadforums.com/forums/viewtopic.php?t=2201

If you've got the time and inclination examine it and let me know if you
spot any inaccuracies. I can also email you a swept groove (WF2 also) and
proof that it's not accurate (simple check-fit pin surfaces and
intersection curves) to the tune of about .025" on a radius (if I remember
correctly).

 

Here is the method I'm referring to:

1. Create a "solid" of the path the cutter creates. This solid can follow a
linear or curved path, as needed.

2. In an assembly, mate the two parts correctly.

3. Using the cavity feature, subtract the "solid" cut from the part.

Best Regards,
Devon T. Sowell
www.3-ddesignsolutions.com

 

Dr. Mather and All,

I've posted an example of what Devon is talking about in the Solidworks
portion of the mCADForum.
But it still seems to be not quite right.

Muggs

 

FYI here is the post to which Muggs is referring

http://www.mcadforums.com/forums/viewtopic.php?t=2211

 

Hi, Devon.
I think it can be said that whenever you do a "solid" cut operation you are
just doing a boolean addition of a solid lump and a "void" lump. It's just
a transparent way of doing what you describe. The problem of defining the
shape of the void lump will be the same either way.

 

(d) put a cutting profile sketch on the normal plane

I think the problem will be understood if you compare the angles of normal
planes for helix (what's the plural of that?) of given pitch and different
radii. The angle out of the (normal to cylinder axis) XY plane decreases
with radius, becoming zero at zero rad. So, if I'm thinking correctly, any
helical sweep of a planar 2D section is, at best, an approximation when
describing the volume removed by the end mill though valid for a 2D
operation like thread cutting. Dunno, I'm confused.

 

..... the one (?) exception being a spherical cutter?

 

Devon T. Sowell wrote

Devon,
I think you sent me the wrong file. The file you sent me has nothing
to do with the problem in question. Also it is not a sweep of one solid
along a path of another resulting in the intersection removed. It is
one swept solid subtracted from another solid. This is does not
address the problem of creating a cylindrical cam as manufactured.
There is good reason this problem has tried some of the best modeling
minds I am aware of. Try again.
J.D.

 

Mark,

I am trying to catch up on this thread and I am having a hard time
determining wether you got your profile to work correctly yet or not. What
is the nature of your cam follow? How many revolutions do you want to make?
Does the movement have to be constant (helical)? Have you gotten an
adequate solution? I might like to try a few off the wall techniques
depending on your answers.

Thanks,

Corey

 

.... helices.

Ahh! Thank you, Dale.
Guess that show how much * I * know about geometry. 8~)

 

I have run into this problem in attempting to make a caming fixture
with a helical slot in a cylinder 4 years back.

I got acceptable results by doing a helical cut with a rectangle
representing the cutter, with a little extra effort, though.

I set up my sketch on a sketch plane to start the cut so it matched the
helix angle of the cam surface on the outside of the cylindrical part.

I do NOT know how accurate the geometry is, but I know the roller cam
operated in the slot with minimal clearance just fine.

Maybe the "Prof" can analyze just how close this technique gets to
being "dead on".

Bo <use my short name @ my domain>

 

Muggs,
I posted the file Devon sent me at -
http://www.mcadforums.com/forums/viewtopic.php?t=2211

Bo,
Could you post your solution at the same site. I am using SWX 2004, so
please post as STEP if you are using 2005.
Thanks,
J.D.

 

Hi, Bo.
Yeah, I think this goes back to the question of how the part is actually
made and what it takes to define it so it can be made to meet the "design
intent". I don't know anything about this stuff but if I go with the
assumption that the groove is cut with an end mill (diameter equal to
groove dimension, to keep it simple) and there is a relative motion that
equates to the cylinder translating and rotating under a stationary cutter
I'd say that the solid geometry in a model isn't worth much. All I'd need
to know is that the cutter axis should intersect the cylinder axis, the
curve described by the cutter axis and cylinder surface intersection,
groove width and depth. If those things can be extracted from the model
....?