I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

I am sure that something simple and stupid is wrong. I am not really
sure how to approach this.

I will, first, get a known best quality endmill, they are still
somewhat affordable in 1/8". I am thinking, get a 2 flute, 1/8"
endmill, 1/2" DOC. I am thinking TiN coating?

In addition I will get a known 1018 block, I only need a small piece.

I do not want to up the RPM beyond 2,000: at 2k RPM, the spindle is
nice and barely warm to the touch, and at higher RPMs it gets
warmer. Since this is a job that takes forever to complete, I would
prefer to keep the sipndle cool.

Any ideas?

I know that I could make the program run faster with tool changes and
a larger end mill doing boring and such. But I wanted to learn more
about small work.

i

On 2011-02-21, Ignoramus17758 wrote:
I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

Forgot to say, I always limit the depth of cut to 1/3 of the end mill
diameter.

i

I am sure that something simple and stupid is wrong. I am not really
sure how to approach this.

I will, first, get a known best quality endmill, they are still
somewhat affordable in 1/8". I am thinking, get a 2 flute, 1/8"
endmill, 1/2" DOC. I am thinking TiN coating?

In addition I will get a known 1018 block, I only need a small piece.

I do not want to up the RPM beyond 2,000: at 2k RPM, the spindle is
nice and barely warm to the touch, and at higher RPMs it gets
warmer. Since this is a job that takes forever to complete, I would
prefer to keep the sipndle cool.

Any ideas?

I know that I could make the program run faster with tool changes and
a larger end mill doing boring and such. But I wanted to learn more
about small work.

i

On 2/20/2011 9:40 PM, Ignoramus17758 wrote:
On 2011-02-21, wrote:
I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

Forgot to say, I always limit the depth of cut to 1/3 of the end mill
diameter.

i

I am sure that something simple and stupid is wrong. I am not really
sure how to approach this.

I will, first, get a known best quality endmill, they are still
somewhat affordable in 1/8". I am thinking, get a 2 flute, 1/8"
endmill, 1/2" DOC. I am thinking TiN coating?

In addition I will get a known 1018 block, I only need a small piece.

I do not want to up the RPM beyond 2,000: at 2k RPM, the spindle is
nice and barely warm to the touch, and at higher RPMs it gets
warmer. Since this is a job that takes forever to complete, I would
prefer to keep the sipndle cool.

Any ideas?

I know that I could make the program run faster with tool changes and
a larger end mill doing boring and such. But I wanted to learn more
about small work.

i

if it breaks after 1/2 hour, that means either that you are doing
something different 1/2 hour into the program, or that it is getting a
little dull - maybe less depth of cut would help it

--
www.wbnoble.com

Ignoramus17758 wrote:

(...)

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

(...)

Sounds like too narrow an end mill for the depth of cut, Iggy.

http://www.endmill.com/pages/training/spdfeed.html

"Excessive depth of cut will result in tool deflection.
As required, the depth of cut increases use the largest
diameter cutter available to maintain a depth to diameter
ratio of 1 : 1."

Advise use a 5 mm endmill.

--Winston

Ignoramus17758 fired this volley in
:

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

Ig, you can probably hear what the problem is.

When the bit's tip starts to deflect and "orbit" about center, rather
than cutting true, you'll hear those little bits start to "sing" as they
make a cut. When you hear that "zzzziiiiiiinnnnnnnnnggg" sound, they're
chattering at enough amplitude to rapidly fatigue the metal.

I know you want to get familiar with small detail work... well... small
detail work involves hogging out all the excess stock you can with drills
and larger bits, then using lighter cuts for the finishing.

Tiny bits were never intended to remove large volumes of stock.

LLoyd

Ignoramus17758 wrote in
rec.crafts.metalworking on Sun, 20 Feb 2011 23:28:01 -0600:

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM

So your chip load (per rev) is 1"/2000rpm = .0005"per rev.
/4(flutes)=0.000125.

I think that is too small of a chip load. Increase your feed, or
decrease your RPM. I would aim for .002 per tooth.

..002load * 4flutes = .008/rev. * 2000rpm = 16ipm

I would also slow down(feed) on inside corners, where extra load is
encountered.

BTW, I once saw what you are making in a catalog some ware. It was to
use in a 1/2" drill to crank the knee up and down.
--

Dan H.
northshore MA.

On 2011-02-21, dan wrote:
Ignoramus17758 wrote in
rec.crafts.metalworking on Sun, 20 Feb 2011 23:28:01 -0600:

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM

So your chip load (per rev) is 1"/2000rpm = .0005"per rev.
/4(flutes)=0.000125.

I think that is too small of a chip load. Increase your feed, or
decrease your RPM. I would aim for .002 per tooth.

.002load * 4flutes = .008/rev. * 2000rpm = 16ipm

I would also slow down(feed) on inside corners, where extra load is
encountered.

BTW, I once saw what you are making in a catalog some ware. It was to
use in a 1/2" drill to crank the knee up and down.

Seems pretty high for a puny 1/8" end mill.

I now also suspect that the unknown steel bar was not 1018.

i

On Sun, 20 Feb 2011 23:28:01 -0600, Ignoramus17758
wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

I am sure that something simple and stupid is wrong. I am not really
sure how to approach this.

I will, first, get a known best quality endmill, they are still
somewhat affordable in 1/8". I am thinking, get a 2 flute, 1/8"
endmill, 1/2" DOC. I am thinking TiN coating?

In addition I will get a known 1018 block, I only need a small piece.

I do not want to up the RPM beyond 2,000: at 2k RPM, the spindle is
nice and barely warm to the touch, and at higher RPMs it gets
warmer. Since this is a job that takes forever to complete, I would
prefer to keep the sipndle cool.

Any ideas?

I know that I could make the program run faster with tool changes and
a larger end mill doing boring and such. But I wanted to learn more
about small work.

i

First thing that strikes me is that the feed rate is extremely low. It
sounds like you're dulling the tool with a way too conservative DOC.

--
Ned Simmons

"Ignoramus17758" wrote in message
...
I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

I am sure that something simple and stupid is wrong. I am not really
sure how to approach this.

I will, first, get a known best quality endmill, they are still
somewhat affordable in 1/8". I am thinking, get a 2 flute, 1/8"
endmill, 1/2" DOC. I am thinking TiN coating?

In addition I will get a known 1018 block, I only need a small piece.

I do not want to up the RPM beyond 2,000: at 2k RPM, the spindle is
nice and barely warm to the touch, and at higher RPMs it gets
warmer. Since this is a job that takes forever to complete, I would
prefer to keep the sipndle cool.

Any ideas?

I know that I could make the program run faster with tool changes and
a larger end mill doing boring and such. But I wanted to learn more
about small work.


Carbide or HSS end mill?

Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

What depth of cut are you using? What is your chip load per tooth? What
is your cutter SFM?

You should never use an end mill smaller than you need, and from memory,
the knee crank "crown" could be milled with at least a 1/4" end mill
which will be stronger, have a higher SFM at your spindle speed and have
more chip clearance.

Ignoramus562 wrote:

On 2011-02-21, dan wrote:
Ignoramus17758 wrote in
rec.crafts.metalworking on Sun, 20 Feb 2011 23:28:01 -0600:

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM

So your chip load (per rev) is 1"/2000rpm = .0005"per rev.
/4(flutes)=0.000125.

I think that is too small of a chip load. Increase your feed, or
decrease your RPM. I would aim for .002 per tooth.

.002load * 4flutes = .008/rev. * 2000rpm = 16ipm

I would also slow down(feed) on inside corners, where extra load is
encountered.

BTW, I once saw what you are making in a catalog some ware. It was to
use in a 1/2" drill to crank the knee up and down.

Seems pretty high for a puny 1/8" end mill.

I now also suspect that the unknown steel bar was not 1018.

i

Remember, too low a chip load = rubbing and dulling = eventual breakage.

Ned Simmons wrote:

On Sun, 20 Feb 2011 23:28:01 -0600, Ignoramus17758
wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

I am sure that something simple and stupid is wrong. I am not really
sure how to approach this.

I will, first, get a known best quality endmill, they are still
somewhat affordable in 1/8". I am thinking, get a 2 flute, 1/8"
endmill, 1/2" DOC. I am thinking TiN coating?

In addition I will get a known 1018 block, I only need a small piece.

I do not want to up the RPM beyond 2,000: at 2k RPM, the spindle is
nice and barely warm to the touch, and at higher RPMs it gets
warmer. Since this is a job that takes forever to complete, I would
prefer to keep the sipndle cool.

Any ideas?

I know that I could make the program run faster with tool changes and
a larger end mill doing boring and such. But I wanted to learn more
about small work.

i

First thing that strikes me is that the feed rate is extremely low. It
sounds like you're dulling the tool with a way too conservative DOC.

Chip load, not DOC. Agree, the tool is rubbing more than cutting and as
a result is rapidly dulling, deflecting more and more as it dulls and
eventually snaps.

Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

BTW Iggy, that "dog clutch" will introduce tremendous backlash if you
are thinking of running your servo drive through it. For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.

"Pete C." fired this volley in news:4d62907a$0$1855
:

For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.


So long as you mean "tight", not "hard" I agree.

A lot of stepper-drive machines use a Lovejoy coupling between motor and
ball screw, with a very tight (even very tightly compressed) spider.

LLoyd

"Lloyd E. Sponenburgh" wrote:

"Pete C." fired this volley in news:4d62907a$0$1855
:

For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.


So long as you mean "tight", not "hard" I agree.

A lot of stepper-drive machines use a Lovejoy coupling between motor and
ball screw, with a very tight (even very tightly compressed) spider.

LLoyd

By "hard" I mean any connection that does not introduce appreciable
backlash. This could be a low-backlash version of the Lovejoy type
connector, a helicle coupler, flex plate coupler or a rigid coupling as
used in most commercial CNC machines where the motor has a precision
mount.

On 2011-02-21, Pete C. wrote:

"Lloyd E. Sponenburgh" wrote:

"Pete C." fired this volley in news:4d62907a$0$1855
:

For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.


So long as you mean "tight", not "hard" I agree.

A lot of stepper-drive machines use a Lovejoy coupling between motor and
ball screw, with a very tight (even very tightly compressed) spider.

LLoyd

By "hard" I mean any connection that does not introduce appreciable
backlash. This could be a low-backlash version of the Lovejoy type
connector, a helicle coupler, flex plate coupler or a rigid coupling as
used in most commercial CNC machines where the motor has a precision
mount.

If I make it precisely, there will not be much backlash.

i

On Mon, 21 Feb 2011 10:19:00 -0600, "Pete C."
wrote:


Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

BTW Iggy, that "dog clutch" will introduce tremendous backlash if you
are thinking of running your servo drive through it. For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.

So something like this would be better?
http://tinyurl.com/5uqt5ne

--
The more passions and desires one has,
the more ways one has of being happy.
-- Charlotte-Catherine

Ignoramus562 wrote:

On 2011-02-21, Pete C. wrote:

"Lloyd E. Sponenburgh" wrote:

"Pete C." fired this volley in news:4d62907a$0$1855
:

For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.


So long as you mean "tight", not "hard" I agree.

A lot of stepper-drive machines use a Lovejoy coupling between motor and
ball screw, with a very tight (even very tightly compressed) spider.

LLoyd

By "hard" I mean any connection that does not introduce appreciable
backlash. This could be a low-backlash version of the Lovejoy type
connector, a helicle coupler, flex plate coupler or a rigid coupling as
used in most commercial CNC machines where the motor has a precision
mount.

If I make it precisely, there will not be much backlash.

You already have inherent backlash in the right angle gear drive from
the hand crank shaft to the Acme screw, as well as backlash in the screw
itself, though the screw backlash should not be an issue if the table
isn't over counterbalanced. You don't want to introduce any more
backlash if you can avoid it.

On 2011-02-21, Pete C. wrote:

Ignoramus562 wrote:

On 2011-02-21, Pete C. wrote:

"Lloyd E. Sponenburgh" wrote:

"Pete C." fired this volley in news:4d62907a$0$1855
:

For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.


So long as you mean "tight", not "hard" I agree.

A lot of stepper-drive machines use a Lovejoy coupling between motor and
ball screw, with a very tight (even very tightly compressed) spider.

LLoyd

By "hard" I mean any connection that does not introduce appreciable
backlash. This could be a low-backlash version of the Lovejoy type
connector, a helicle coupler, flex plate coupler or a rigid coupling as
used in most commercial CNC machines where the motor has a precision
mount.

If I make it precisely, there will not be much backlash.

You already have inherent backlash in the right angle gear drive from
the hand crank shaft to the Acme screw, as well as backlash in the screw
itself, though the screw backlash should not be an issue if the table
isn't over counterbalanced. You don't want to introduce any more
backlash if you can avoid it.

I agree with you.

i

My first suggestion would be to use a 2-flute. The 4-flute is getting
dull and then loading up and breaking.

Can you rough it out with a larger diameter 2-flute?

Dave

Larry Jaques wrote:

On Mon, 21 Feb 2011 10:19:00 -0600, "Pete C."
wrote:


Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

BTW Iggy, that "dog clutch" will introduce tremendous backlash if you
are thinking of running your servo drive through it. For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.

So something like this would be better?
http://tinyurl.com/5uqt5ne

Yep, that's a helical coupler which has little or no backlash. There are
other types of low/no backlash flex couplers as well.

"Ignoramus17758" wrote in message
...
I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

That's what wax is for. To show the product (and to make lost wax molds).


In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

I don't do much with steel, but end mills definitely have a fixed life. I
use a lot of those smaller ones in aluminum and the life has become pretty
measurable. Since I do aluminum I use the solid carbide. I've tried a
number of different brands and types, and I've found the Kyocera ones work
good for me. I don't have any HSS or Cobalt so I have no personal
experience to draw on there.


1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

Plug that into ME Consultant and see what kind of numbers you get back.
Also, depth of cut could be an issue. With that small stuff I have to
compromise depth of cut to about half what they tell me is possible,
Sometimes a lot less. Steel is nice in that it doesn't build up on the
cutter like aluminum does, but it also takes a lot more force to cut.

I am sure that something simple and stupid is wrong. I am not really
sure how to approach this.

Nah, you are probably pretty close. Just may have to tweak things a bit.

I will, first, get a known best quality endmill, they are still
somewhat affordable in 1/8". I am thinking, get a 2 flute, 1/8"
endmill, 1/2" DOC. I am thinking TiN coating?

1/2" DOC? Wow, that is aggressive unless you are taking a very small
stepover. I was thinking a LOT less. Then I just go seat of the pants.
Most of my 1/8 end mills are not even fluted that deep. I like 2 flute in
aluminum, but doesn't more flutes usually mean a better cut and faster feed
rate possible in steel?

I AM SO CONFUSED.

In addition I will get a known 1018 block, I only need a small piece.

I do not want to up the RPM beyond 2,000: at 2k RPM, the spindle is
nice and barely warm to the touch, and at higher RPMs it gets
warmer. Since this is a job that takes forever to complete, I would
prefer to keep the sipndle cool.

Any ideas?


Like I said. Plug your numbers into ME Consultant and then adjust from
there.

I know that I could make the program run faster with tool changes and
a larger end mill doing boring and such. But I wanted to learn more
about small work.

The first thing I learned about small work is remove as much as possible
with a larger cutter first and then ONLY use the smaller cutter when
necessary to finish. I am a lot happier with that. When I talk about jobs
taking 6-30 hours Its usually detail work that I just can't do with a bigger
cutter. Also, remember that even if your cutter can handle the depth of cut
you get friction from the next pass if the sides of a pocket or feature are
above the flutes.

Lets us know how it works.

..020" DOC, 2500RPM, 30IPM. Use carbide endmill, .125" stepover.
Run like this until you get to .005" above your desired depth. I do it
all the time, every day.

Have fun.

On Mon, 21 Feb 2011 09:37:05 -0800, Larry Jaques
wrote:

On Mon, 21 Feb 2011 10:19:00 -0600, "Pete C."
wrote:


Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

BTW Iggy, that "dog clutch" will introduce tremendous backlash if you
are thinking of running your servo drive through it. For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.

So something like this would be better?
http://tinyurl.com/5uqt5ne

that's the coupling you normally see between the servo and ball screw.
0 backlash.

On Mon, 21 Feb 2011 09:52:32 -0600, "Pete C."
wrote:


Ned Simmons wrote:


First thing that strikes me is that the feed rate is extremely low. It
sounds like you're dulling the tool with a way too conservative DOC.

Chip load, not DOC. Agree, the tool is rubbing more than cutting and as
a result is rapidly dulling, deflecting more and more as it dulls and
eventually snaps.

Oops, I meant feed per tooth...

--
Ned Simmons

On Mon, 21 Feb 2011 10:23:58 -0600, "Lloyd E. Sponenburgh"
lloydspinsidemindspring.com wrote:

"Pete C." fired this volley in news:4d62907a$0$1855
:

For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.


So long as you mean "tight", not "hard" I agree.

A lot of stepper-drive machines use a Lovejoy coupling between motor and
ball screw, with a very tight (even very tightly compressed) spider.

Unlike steppers, servo tuning is compromised by lack of angular
stiifness in the loop. Lovejoy couplings are quite soft in that
regard, and I think that's the sense Pete was using when recommending
a "hard" coupling. Oldham couplings are often a good compromise when
highest performance is not required.

--
Ned Simmons

Ned Simmons wrote:

On Mon, 21 Feb 2011 09:52:32 -0600, "Pete C."
wrote:


Ned Simmons wrote:


First thing that strikes me is that the feed rate is extremely low. It
sounds like you're dulling the tool with a way too conservative DOC.

Chip load, not DOC. Agree, the tool is rubbing more than cutting and as
a result is rapidly dulling, deflecting more and more as it dulls and
eventually snaps.

Oops, I meant feed per tooth...

Yep.

The key thing we need to get across to Iggy is that in machining the
feed rate is not a case where you can go from zero up to the maximum
permissible feed before having problems, rather there are both maximum
and minimum feed rates and exceeding the limits in either direction will
cause problems. A minimum feed rate is required to ensure that there is
cutting action vs. rubbing action, and allowing rubbing from too low a
feed rate will cause a failure just as surely as too high a feed rate
will.

Karl Townsend wrote:
On Mon, 21 Feb 2011 09:37:05 -0800, Larry Jaques
wrote:

On Mon, 21 Feb 2011 10:19:00 -0600, "Pete C."
wrote:


Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

BTW Iggy, that "dog clutch" will introduce tremendous backlash if you
are thinking of running your servo drive through it. For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.

So something like this would be better?
http://tinyurl.com/5uqt5ne

that's the coupling you normally see between the servo and ball screw.
0 backlash.


this type of coupling can still act rather springy, even though there
isn't really and backlash.

Ignoramus17758 wrote:

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

Why not use carbide? If you push it too hard it will break quickly. If HSS is breaking
after 30 minutes on a cnc, I suspect you got the life time out of it.

Wes
--
"Additionally as a security officer, I carry a gun to protect
government officials but my life isn't worth protecting at home
in their eyes." Dick Anthony Heller

Wes wrote:

Ignoramus17758 wrote:

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

Why not use carbide? If you push it too hard it will break quickly. If HSS is breaking
after 30 minutes on a cnc, I suspect you got the life time out of it.

Look at his cut parameters, as Dan noted, his chip load is 0.000125 per
tooth. His feed is too low and the end mill is rubbing and dulling.

Pete C. wrote:
Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

What depth of cut are you using? What is your chip load per tooth? What
is your cutter SFM?

You should never use an end mill smaller than you need, and from memory,
the knee crank "crown" could be milled with at least a 1/4" end mill
which will be stronger, have a higher SFM at your spindle speed and have
more chip clearance.

So, say I'm making a rectangular hole. Would I cut it with, say, a 1/4"
side mill, and finish up with a broach?

Thanks,
Rich

Rich Grise wrote:

Pete C. wrote:
Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

http://igor.chudov.com/projects/Brid...-8057.jpg.html

I wrote a G code program that makes such a clutch from a flat block of
metal, with a 1/8" end mill.

In machinable wax, it does a great job, zips through it, and makes a
surface that mates with the crank handle perfectly, I was very
impressed.

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

1/8" end mill
4 flute
1 IPM feedrate
2,000 RPM
plenty of coolant
unknown steel, but feels like 1018.

What depth of cut are you using? What is your chip load per tooth? What
is your cutter SFM?

You should never use an end mill smaller than you need, and from memory,
the knee crank "crown" could be milled with at least a 1/4" end mill
which will be stronger, have a higher SFM at your spindle speed and have
more chip clearance.

So, say I'm making a rectangular hole. Would I cut it with, say, a 1/4"
side mill, and finish up with a broach?

You would certainly need to finish with a broach if you need square
inside corners. If you can live with rounded inside corners of a small
diameter end mill you can certainly do a finish pass with a small end
mill, but it would be insane to try to mill say a 2"x3" pocket with an
1/8" end mill just because you need 1/8" for the finish pass.

At any rate, that is not relevant to Iggy's machining issue, since his
part does not have any inside corners. For his part he should be using a
3/16" end mill or slightly larger, milling the outside diameter, the
inside circular pocket, the radial bulk material removal cuts between
each section of the "crown", and then finishing by milling the exterior
of each "crown" island wedge. The limitation on the end mill diameter is
the spacing between the inner points of the "crown" islands which is
around .2".

On 2011-02-21, Pete C. wrote:

Wes wrote:

Ignoramus17758 wrote:

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

Why not use carbide? If you push it too hard it will break quickly. If HSS is breaking
after 30 minutes on a cnc, I suspect you got the life time out of it.

Look at his cut parameters, as Dan noted, his chip load is 0.000125 per
tooth. His feed is too low and the end mill is rubbing and dulling.

I think that you have an extra zero in your calculation.

A little update: I am now using a 12L14 bar that is exactly the right
diameter. I drilled a hole in the middle with a drill bit and am
machining the teeth right now. I found a couple of bugs in the code,
that I fixed, and so far, it is running OK.

If the teeth do not exactly mate, I can file them down with a regular
file. I will see how it goes, I have a little extra of this 12L14 bar
stock.

i

On 2011-02-21, Cydrome Leader wrote:
Karl Townsend wrote:
On Mon, 21 Feb 2011 09:37:05 -0800, Larry Jaques
wrote:

On Mon, 21 Feb 2011 10:19:00 -0600, "Pete C."
wrote:


Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

BTW Iggy, that "dog clutch" will introduce tremendous backlash if you
are thinking of running your servo drive through it. For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.

So something like this would be better?
http://tinyurl.com/5uqt5ne

that's the coupling you normally see between the servo and ball screw.
0 backlash.


this type of coupling can still act rather springy, even though there
isn't really and backlash.

I am not totally sure, but I think that I can handle that sort of
thing with proper choice of servo loop parameters P, I and D.

i

On 2011-02-21, Lloyd E. Sponenburgh lloydspinsidemindspring.com wrote:
"Pete C." fired this volley in news:4d62907a$0$1855
:

For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.


So long as you mean "tight", not "hard" I agree.

A lot of stepper-drive machines use a Lovejoy coupling between motor and
ball screw, with a very tight (even very tightly compressed) spider.

My servo motor driven rotary table (4th axis) is based on this kind of
coupling.

As for the knee, if, say, I have one degree of "slop", which is a lot,
this amounts to roughly 1/5"*1/360 = 0.0006" of accuracy. Remember
that 360 degree turn is only 1/5 of an inch or something like that.

I am not building a space station here, so 0.0006" extra inaccuracy, I
can live with. (and deal with programmatically)

i

Ignoramus562 wrote:
On 2011-02-21, Cydrome Leader wrote:
Karl Townsend wrote:
On Mon, 21 Feb 2011 09:37:05 -0800, Larry Jaques
wrote:

On Mon, 21 Feb 2011 10:19:00 -0600, "Pete C."
wrote:


Ignoramus17758 wrote:

I am trying to make a dog clutch that mates with the knee crank and
replaces the crank handle:

BTW Iggy, that "dog clutch" will introduce tremendous backlash if you
are thinking of running your servo drive through it. For a servo
connection you need to use a "hard" connection. Note that in a manual
mill, the feedback from the dial or from a scale is after the handle
clutch and thus the handle clutch backlash is not a factor.

So something like this would be better?
http://tinyurl.com/5uqt5ne

that's the coupling you normally see between the servo and ball screw.
0 backlash.


this type of coupling can still act rather springy, even though there
isn't really and backlash.

I am not totally sure, but I think that I can handle that sort of
thing with proper choice of servo loop parameters P, I and D.

i

maybe, I don't know- but I was surprised as how much those things can bend
and twist. Keep them as short as possible to minimize this.

Pete C. wrote:
Rich Grise wrote:
Pete C. wrote:

So, say I'm making a rectangular hole. Would I cut it with, say, a 1/4"
side mill, and finish up with a broach?

You would certainly need to finish with a broach if you need square
inside corners. If you can live with rounded inside corners of a small
diameter end mill you can certainly do a finish pass with a small end
mill, but it would be insane to try to mill say a 2"x3" pocket with an
1/8" end mill just because you need 1/8" for the finish pass.

At any rate, that is not relevant to Iggy's machining issue, since his
part does not have any inside corners. For his part he should be using a
3/16" end mill or slightly larger, milling the outside diameter, the
inside circular pocket, the radial bulk material removal cuts between
each section of the "crown", and then finishing by milling the exterior
of each "crown" island wedge. The limitation on the end mill diameter is
the spacing between the inner points of the "crown" islands which is
around .2".

Thanks! :-)
Rich

Ignoramus562 wrote:

On 2011-02-21, Pete C. wrote:

Wes wrote:

Ignoramus17758 wrote:

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

Why not use carbide? If you push it too hard it will break quickly. If HSS is breaking
after 30 minutes on a cnc, I suspect you got the life time out of it.

Look at his cut parameters, as Dan noted, his chip load is 0.000125 per
tooth. His feed is too low and the end mill is rubbing and dulling.

I think that you have an extra zero in your calculation.

No, the calculation Dan posted is correct:

"So your chip load (per rev) is 1"/2000rpm = .0005"per rev.
/4(flutes)=0.000125."

1 IPM / 2000 RPM = 0.0005" of feed per revolution of the end mill,
divided by the 4 flutes = 0.000125" chip load per tooth, which is too
low by a factor of probably 10X.


A little update: I am now using a 12L14 bar that is exactly the right
diameter. I drilled a hole in the middle with a drill bit and am
machining the teeth right now. I found a couple of bugs in the code,
that I fixed, and so far, it is running OK.

Bugs in the code can certainly get you, and they can be subtle enough to
no be noticed on more forgiving material like wax. Have you got any CAD
/ CAM software yet, or are you still hand coding with your modular
routines?


If the teeth do not exactly mate, I can file them down with a regular
file.

Only if they're too tight. If they are too loose filing won't help.

On 2011-02-22, Pete C. wrote:

Ignoramus562 wrote:

On 2011-02-21, Pete C. wrote:

Wes wrote:

Ignoramus17758 wrote:

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

Why not use carbide? If you push it too hard it will break quickly. If HSS is breaking
after 30 minutes on a cnc, I suspect you got the life time out of it.

Look at his cut parameters, as Dan noted, his chip load is 0.000125 per
tooth. His feed is too low and the end mill is rubbing and dulling.

I think that you have an extra zero in your calculation.

No, the calculation Dan posted is correct:

"So your chip load (per rev) is 1"/2000rpm = .0005"per rev.
/4(flutes)=0.000125."

1 IPM / 2000 RPM = 0.0005" of feed per revolution of the end mill,
divided by the 4 flutes = 0.000125" chip load per tooth, which is too
low by a factor of probably 10X.

OK, great, sorry.


A little update: I am now using a 12L14 bar that is exactly the right
diameter. I drilled a hole in the middle with a drill bit and am
machining the teeth right now. I found a couple of bugs in the code,
that I fixed, and so far, it is running OK.

Bugs in the code can certainly get you, and they can be subtle enough to
no be noticed on more forgiving material like wax. Have you got any CAD
/ CAM software yet, or are you still hand coding with your modular
routines?

I am hand coding with modular routines.

I have not even looked at CAD/CAM.

I have to admit that I kind of like that, I am in my natural
programming mode of thinking.


If the teeth do not exactly mate, I can file them down with a regular
file.

Only if they're too tight. If they are too loose filing won't help.

Yep.

So, in the end, they were just a bit too large to mate, I filed them
down slightly with a file, and now they seem to mate, though tightly
-- which is great.

i

Ignoramus19981 wrote:

On 2011-02-22, Pete C. wrote:

Ignoramus562 wrote:

On 2011-02-21, Pete C. wrote:

Wes wrote:

Ignoramus17758 wrote:

In steel, however, this little 1/8" endmill works for a while, then
breaks after 1/2 hour.

Why not use carbide? If you push it too hard it will break quickly. If HSS is breaking
after 30 minutes on a cnc, I suspect you got the life time out of it.

Look at his cut parameters, as Dan noted, his chip load is 0.000125 per
tooth. His feed is too low and the end mill is rubbing and dulling.

I think that you have an extra zero in your calculation.

No, the calculation Dan posted is correct:

"So your chip load (per rev) is 1"/2000rpm = .0005"per rev.
/4(flutes)=0.000125."

1 IPM / 2000 RPM = 0.0005" of feed per revolution of the end mill,
divided by the 4 flutes = 0.000125" chip load per tooth, which is too
low by a factor of probably 10X.

OK, great, sorry.


A little update: I am now using a 12L14 bar that is exactly the right
diameter. I drilled a hole in the middle with a drill bit and am
machining the teeth right now. I found a couple of bugs in the code,
that I fixed, and so far, it is running OK.

Bugs in the code can certainly get you, and they can be subtle enough to
no be noticed on more forgiving material like wax. Have you got any CAD
/ CAM software yet, or are you still hand coding with your modular
routines?

I am hand coding with modular routines.

I have not even looked at CAD/CAM.

I have to admit that I kind of like that, I am in my natural
programming mode of thinking.

CAD/CAM has some advantages in visualizing the part, cutter clearances
and the like, and of course a huge advantage in dealing with machining
operations on complex contours.



If the teeth do not exactly mate, I can file them down with a regular
file.

Only if they're too tight. If they are too loose filing won't help.

Yep.

So, in the end, they were just a bit too large to mate, I filed them
down slightly with a file, and now they seem to mate, though tightly
-- which is great.

The end result is what matters, at least for one off parts.