To all you math whizzes,
I am making parts now which require an .844 dia hole canted at 40
degrees to go through the .125 thick wall of the parts. Each part gets
6 holes spaced over 28 inches. Currently I am machining a straight
hole through on the CNC mill and then finish boring the hole at the 40
degree angle on the Bridgeport. It occurred to me that I can program
the CNC to machine an ellipse and then move X and Z axes
simultaneously to get the 40 degree angle. I made up a tool which has
enough radial clearance to clear the material when machining the part
of the hole that is on the underside of the part. This tool has a
point on it with a small radius, about .010. I would like to use a
woodruff key cutter with a full radius to bore the holes because I
could feed it faster than the single point tool I ground up. But after
thinking about it I realized that the tool would contact the work at a
different radius as it contoured the ellipse. This is because the
tangent point on the radius on the periphery of the woodruff cutter
will change as the cutter moves around the ellipse contour. So I'm
thinking that if I calculate the tangent point along the long axis of
the ellipse I can program an ellipse different than the one I want
that will result in the proper ellipse being cut. Im thinking that I
will need to program the ellipse to be less elliptical to get the
ellipse I want. Am I correct? If not, how should I change the program?
I am going on vacation for a week and so I will not be able to read
anybody's reply until I get back.
Thanks,
Eric

On Mon, 13 Aug 2012 10:58:58 -0700, etpm wrote:

To all you math whizzes,
I am making parts now which require an .844 dia hole canted at 40
degrees to go through the .125 thick wall of the parts. Each part gets
6 holes spaced over 28 inches. [big snip]
I am going on vacation for a week and so I will not be able to read
anybody's reply until I get back.

It would be better to clarify the problem before running off and
letting mayhem ensue as people guess what you are talking about.
Is the overall shape of the part a long cylinder? What's the
diameter and the material? Do the holes go in one side of cylinder
and out the other, or just into one side? Is the cant angle relative
to long axis of part? (Ie, is long axis of the ellipse aligned with
long axis of part, or across the part?) Is the Bridgeport head
tilted to 40 degrees?

--
jiw

On Mon, 13 Aug 2012 18:24:19 +0000 (UTC), James Waldby
wrote:

On Mon, 13 Aug 2012 10:58:58 -0700, etpm wrote:

To all you math whizzes,
I am making parts now which require an .844 dia hole canted at 40
degrees to go through the .125 thick wall of the parts. Each part gets
6 holes spaced over 28 inches. [big snip]
I am going on vacation for a week and so I will not be able to read
anybody's reply until I get back.

It would be better to clarify the problem before running off and
letting mayhem ensue as people guess what you are talking about.
Is the overall shape of the part a long cylinder? What's the
diameter and the material? Do the holes go in one side of cylinder
and out the other, or just into one side? Is the cant angle relative
to long axis of part? (Ie, is long axis of the ellipse aligned with
long axis of part, or across the part?) Is the Bridgeport head
tilted to 40 degrees?
The hole is going through one side of a 2 inch square tube. The wall
thickness is .125. The holes are to accept an .834 dia tube canted
over at 40 degrees relative to the long axis. I just need to know if I
need to make the ellipse longer or shorter along the long axis. The
short axis will of course stay the same if my thinking is correct.
Eric

fired this volley in
:

I just need to know if I
need to make the ellipse longer or shorter along the long axis

Longer.

Your problem was clear from the beginning, despite the last poster's
comments. It wouldn't matter through what (flat) surface you were making
them.

FWIW, a single-point tool simplifies the math. Otherwise, you have to
make the "effective" radius of the tool when canted at 40 degrees less
than or equal to the minor axis of the ellipse, or it will cut over-
sized.

I know you're not canting the tool, but viewing it as if it were will be
useful to you.

Lloyd

On Mon, 13 Aug 2012 12:35:56 -0700, wrote:

On Mon, 13 Aug 2012 18:24:19 +0000 (UTC), James Waldby
wrote:

On Mon, 13 Aug 2012 10:58:58 -0700, etpm wrote:

To all you math whizzes,
I am making parts now which require an .844 dia hole canted at 40
degrees to go through the .125 thick wall of the parts. Each part gets
6 holes spaced over 28 inches. [big snip]
I am going on vacation for a week and so I will not be able to read
anybody's reply until I get back.

It would be better to clarify the problem before running off and
letting mayhem ensue as people guess what you are talking about.
Is the overall shape of the part a long cylinder? What's the
diameter and the material? Do the holes go in one side of cylinder
and out the other, or just into one side? Is the cant angle relative
to long axis of part? (Ie, is long axis of the ellipse aligned with
long axis of part, or across the part?) Is the Bridgeport head
tilted to 40 degrees?
The hole is going through one side of a 2 inch square tube. The wall
thickness is .125. The holes are to accept an .834 dia tube canted
over at 40 degrees relative to the long axis. I just need to know if I
need to make the ellipse longer or shorter along the long axis. The
short axis will of course stay the same if my thinking is correct.
Eric

This is what CAD programs are for. spend the time to get a good
drawing, then only cut once.

karl

On Mon, 13 Aug 2012 15:00:58 -0500, Karl Townsend
wrote:

On Mon, 13 Aug 2012 12:35:56 -0700, wrote:

On Mon, 13 Aug 2012 18:24:19 +0000 (UTC), James Waldby
wrote:

On Mon, 13 Aug 2012 10:58:58 -0700, etpm wrote:

To all you math whizzes,
I am making parts now which require an .844 dia hole canted at 40
degrees to go through the .125 thick wall of the parts. Each part gets
6 holes spaced over 28 inches. [big snip]
I am going on vacation for a week and so I will not be able to read
anybody's reply until I get back.

It would be better to clarify the problem before running off and
letting mayhem ensue as people guess what you are talking about.
Is the overall shape of the part a long cylinder? What's the
diameter and the material? Do the holes go in one side of cylinder
and out the other, or just into one side? Is the cant angle relative
to long axis of part? (Ie, is long axis of the ellipse aligned with
long axis of part, or across the part?) Is the Bridgeport head
tilted to 40 degrees?
The hole is going through one side of a 2 inch square tube. The wall
thickness is .125. The holes are to accept an .834 dia tube canted
over at 40 degrees relative to the long axis. I just need to know if I
need to make the ellipse longer or shorter along the long axis. The
short axis will of course stay the same if my thinking is correct.
Eric

This is what CAD programs are for. spend the time to get a good
drawing, then only cut once.

karl
Greetings Lloyd and Karl,
I do have a good CAD program. That's how I drew the first ellips and
generated the toolpath. I know my cutter needs to be smaller than the
small dimension of the ellipse.
Eric

fired this volley in
:

I do have a good CAD program. That's how I drew the first ellips and
generated the toolpath. I know my cutter needs to be smaller than the
small dimension of the ellipse.

You should not have had to draw elipses. You should be able to spiral-
drill a round hole on any angle, using XY interpolation; that is, presuming
the material is thin enough such that the vertical tool shank doesn't
impinge on the top end of the hole.

Perhaps that's the missing piece for you.

Lloyd

On Mon, 13 Aug 2012 15:31:01 -0500, "Lloyd E. Sponenburgh"
lloydspinsidemindspring.com wrote:

fired this volley in
:

I do have a good CAD program. That's how I drew the first ellips and
generated the toolpath. I know my cutter needs to be smaller than the
small dimension of the ellipse.

You should not have had to draw elipses. You should be able to spiral-
drill a round hole on any angle, using XY interpolation; that is, presuming
the material is thin enough such that the vertical tool shank doesn't
impinge on the top end of the hole.

Perhaps that's the missing piece for you.

Lloyd
Well, first I thought that I could just feed at the 40 degree angle
with a tool that had the proper relief. That didn't work. What I got
was an oval. Sort of. That's when I realized that of course that
wouldn't work. Another way to look at what I did was to divide the
hole into steps. So there was a round hole on top of another and so on
with the holes displaced in one axis. But a hole penetrating a plane
surface at an angle makes an ellipse. So that's when I realized that I
needed to program an ellipse and feed that in a helical fashion at the
40 degree angle. Can an ellipse be fed helically? Certainly not
spirally because the diameter isn't constantly increasing or
decreasing. And isn't a circle an ellipse with both the long and short
axes the the same?
Eric

fired this volley in
:

Well, first I thought that I could just feed at the 40 degree angle
with a tool that had the proper relief. That didn't work. What I got
was an oval. Sort of.

What I meant was to draw a circle on a plane 40-degrees off the
horizontal, and drill it perpendicular to the plane using XY
interpolation rather than a tilt axis.

Another way to get the elipse you need would be to draw a cylinder of
exactly the size hole you need, then slice that cylinder with a plane 40-
degrees off horizontal. Then erect the shape resulting.

From the web, here's the formula for the elipse formed such:

The intersection will be a ellipse with semi-major axis r/Cos[a] and
semi-minor axis r

where r is the radius of the right-circular cylinder and a is the
slice angle.

On Mon, 13 Aug 2012 18:12:15 -0500, Lloyd E. Sponenburgh wrote:

fired this volley in
:

Well, first I thought that I could just feed at the 40 degree angle
with a tool that had the proper relief. That didn't work. What I got
was an oval. Sort of.

What I meant was to draw a circle on a plane 40-degrees off the
horizontal, and drill it perpendicular to the plane using XY
interpolation rather than a tilt axis.

Another way to get the elipse you need would be to draw a cylinder of
exactly the size hole you need, then slice that cylinder with a plane 40-
degrees off horizontal. Then erect the shape resulting.

From the web, here's the formula for the elipse formed such:

The intersection will be a ellipse with semi-major axis r/Cos[a] and
semi-minor axis r

where r is the radius of the right-circular cylinder and a is the
slice angle.

That formula is correct, from the geometry, but if a Woodruff cutter
of thickness t is used and descends through the part, it will overcut
the major axis length by a distance of t*tan(a). If you shorten the
ellipse by that amount it will have the wrong shape, so some other
method (like cutting half the ellipse from above and the other half
from below) might be needed if tolerances are tight.

--
jiw

James Waldby fired this volley in news:k0c6qg$n77$1
@dont-email.me:

That formula is correct, from the geometry, but if a Woodruff cutter
of thickness t is used and descends through the part, it will overcut
the major axis length by a distance of t*tan(a). If you shorten the
ellipse by that amount it will have the wrong shape, so some other
method (like cutting half the ellipse from above and the other half
from below) might be needed if tolerances are tight.

Use a double-angle cutter instead. It will behave like a single-point
tool, but with more teeth, and a smoother cut. Using it will not require
that you adjust for the thickness of the tool, since the cutting edge is
still a "single point".

LLoyd

42.

That's the answer to life, the universe, and..... EVERYTHING!!!!

Christopher A. Young
Learn more about Jesus
www.lds.org
..

wrote in message
...
To all you math whizzes,
I am making parts now which require an .844 dia hole canted at 40
degrees to go through the .125 thick wall of the parts. Each part gets
6 holes spaced over 28 inches. Currently I am machining a straight
hole through on the CNC mill and then finish boring the hole at the 40
degree angle on the Bridgeport. It occurred to me that I can program
the CNC to machine an ellipse and then move X and Z axes
simultaneously to get the 40 degree angle. I made up a tool which has
enough radial clearance to clear the material when machining the part
of the hole that is on the underside of the part. This tool has a
point on it with a small radius, about .010. I would like to use a
woodruff key cutter with a full radius to bore the holes because I
could feed it faster than the single point tool I ground up. But after
thinking about it I realized that the tool would contact the work at a
different radius as it contoured the ellipse. This is because the
tangent point on the radius on the periphery of the woodruff cutter
will change as the cutter moves around the ellipse contour. So I'm
thinking that if I calculate the tangent point along the long axis of
the ellipse I can program an ellipse different than the one I want
that will result in the proper ellipse being cut. Im thinking that I
will need to program the ellipse to be less elliptical to get the
ellipse I want. Am I correct? If not, how should I change the program?
I am going on vacation for a week and so I will not be able to read
anybody's reply until I get back.
Thanks,
Eric

"Lloyd E. Sponenburgh" lloydspinsidemindspring.com fired this volley in
. 3.70:

Use a double-angle cutter instead.

I should have said "... or a dovetail cutter of 40 degrees."

Lloyd

"Lloyd E. Sponenburgh" lloydspinsidemindspring.com fired this volley in
. 3.70:

I should have said

And then I should have said... either will require making a starting hole
at least as large as the tooth gullet diameter of the tool...

(duh!)

On Mon, 13 Aug 2012 21:07:09 -0400, Stormin Mormon wrote:

42.

That's the answer to life, the universe, and..... EVERYTHING!!!!

I think that's OT and isn't specific enough to answer Eric's question.
Here's a very slightly more relevant "42" link (still OT) that has some
great advice:
http://institute.lds.org/content/images/manuals/chft/42-02.gif

wrote ...
To all you math whizzes,
I am making parts now which require an .844 dia hole canted at 40
degrees to go through the .125 thick wall of the parts. Each part gets
....

--
jiw

Thanks, that's a good link. You have acted well, thy part.

Christopher A. Young
Learn more about Jesus
www.lds.org
..

"James Waldby" wrote in message
...
On Mon, 13 Aug 2012 21:07:09 -0400, Stormin Mormon wrote:

42.

That's the answer to life, the universe, and..... EVERYTHING!!!!

I think that's OT and isn't specific enough to answer Eric's question.
Here's a very slightly more relevant "42" link (still OT) that has some
great advice:
http://institute.lds.org/content/images/manuals/chft/42-02.gif