End Mills -- 2-Flute vs. 4-Flute?
 

This is a dumb question, but what are the relative advantages of
4-Flute vs. 2-Flute end mills, and on what applications should one type
be chosen over the other?

Harry C.

Wow, those responses were fast! :-)

Thanks both Jack and Pete. This is exactly the type of information that
I needed.


Harry C.

"Pete Snell" wrote in message
...
wrote:

This is a dumb question, but what are the relative advantages of
4-Flute vs. 2-Flute end mills, and on what applications should one type
be chosen over the other?

Harry C.


2 flute can plunge cut, 4 flute cannot.

Pete,
Not quite correct.
4-flutes come in "center cutting" and non-center-cutting varieties.
Center-cutting 4 flutes plunge readily. May not have quite the chip
ejection as 2 flutes, but they still plunge very well--may have to peck
more.
Altho I never thought of it, I realize now I've never seen a
non-center-cutting 2-flute!
FWIC, I don't think there is that great a price diff between 4 fl center
cut/non-center cut.

You can also get better finishes w/ a 4 flute, as you are getting more cuts
per rotation.

They also have 3-flute cutters, center/non-center also, I believe. Think
I've also seen 6 flute.
----------------------------
Mr. P.V.'d
formerly Droll Troll

--
__
Pete Snell
Royal Military College
Kingston Ontario


The reasonable man adapts himself to the world;
the unreasonable one persists in trying to adapt the world to himself.
Therefore all progress depends on the unreasonable man.
- George Bernard Shaw

Pete Snell wrote:
wrote:

This is a dumb question, but what are the relative advantages of
4-Flute vs. 2-Flute end mills, and on what applications should one type
be chosen over the other?

Harry C.


2 flute can plunge cut, 4 flute cannot.


Today, a sizable fraction of 4-flute cutters CAN plunge cut (they have
one long tooth extending to the center). Not really well, I'll grant
(not much chip clearance). Drills are far better for making holes than
milling cutters.

2-flute cutters are also better for slotting to size (especially in thin
materials) in one pass. Side deflection of the cutter still occurs, but
it doesn't widen the cut as it does with 4-flute cutters ... think about
it).

Dan Mitchell
============

The previous responses were general, but not absolute. You can use 2 flute
on steel and there are 4 flute end mills that plunge. It is all about chip
clearance really.
Steve

wrote in message
oups.com...
Wow, those responses were fast! :-)

Thanks both Jack and Pete. This is exactly the type of information that
I needed.


Harry C.

On Tue, 01 Mar 2005 15:16:34 -0500, Pete Snell wrote:

wrote:
===
=== This is a dumb question, but what are the relative advantages of
=== 4-Flute vs. 2-Flute end mills, and on what applications should one type
=== be chosen over the other?
===
=== Harry C.
===
===
=== 2 flute can plunge cut, 4 flute cannot.


So far so good with the info given, but I have 4 flute that I plunge
cut with all the time. If they are center cut they will plunge cut..

2 flute so I am told and from my own experieince makes a slot closer
to the dimension of the endmill than a 4 flute does as well.......

==============================================
Put some color in your cheeks...garden naked!

"Grant Erwin" wrote in message
...
wrote:

2-flute for slots, 4 flute for when you want higher feed rates (keeping
the advance/tooth constant, the only way you can up your feed is by
adding teeth).

I don't buy the steel/aluminum answer, sorry.

I agree that just saying 2 flute is for aluminum and 4 flute is for steel is
not a correct answer. But I think it is correct in a way.

Because aluminum is (typically) quite a bit softer than steel, one can take
very aggressive cuts which leads to larger chips. These larger chips need
more clearance which is a characteristic of 2 flute endmills.

Just to put my own "me too" in, I use 2 flute cutters when removing a lot of
material, or making a feature which does not allow for (easy) chip removal -
slots and pockets. I use a 4 flute for finishing because of the doubled
feedrate and light depth of cut.

Also, I find 4 fluted cutters to be more stable (less deflection). I think
this is because they have more meat, but that's certainly just a guess.

As far as really practical advice, I'd want a good selection of 2 fluted
cutters in my box, while having an odd 4 flute for times when I'm doing a
lot of finishing.

Regards,

Robin

Sure you do. In that 2 flute gives more chip clearance, and in
aluminum you can take a thicker chip and a higher sfm than you can in
steel.

Dan


Grant Erwin wrote:

I don't buy the steel/aluminum answer, sorry.

GWE

Grant Erwin wrote:
wrote:

This is a dumb question, but what are the relative advantages of
4-Flute vs. 2-Flute end mills, and on what applications should one type
be chosen over the other?

Harry C.


2-flute for slots, 4 flute for when you want higher feed rates (keeping
the advance/tooth constant, the only way you can up your feed is by
adding teeth).

I don't buy the steel/aluminum answer, sorry.

GWE
That's ok Grant, alot of people will understand what i was talking about.
yes you can cut alum with a 4-flute and you can cut steel with a 2-flute.
alum. roughing I like 3-flute cutters and 2-flute for finishing.
(4-flute tend to wad up the alum to easily)
2-flutes on steel are not my favorite due to slower sfm which results in
slower feed rates. I'd use 4 or more flutes on steel.

On Tue, 01 Mar 2005 17:29:30 -0600, jackK
wrote:

Grant Erwin wrote:
wrote:

This is a dumb question, but what are the relative advantages of
4-Flute vs. 2-Flute end mills, and on what applications should one type
be chosen over the other?

Harry C.


2-flute for slots, 4 flute for when you want higher feed rates (keeping
the advance/tooth constant, the only way you can up your feed is by
adding teeth).

I don't buy the steel/aluminum answer, sorry.

GWE
That's ok Grant, alot of people will understand what i was talking about.
yes you can cut alum with a 4-flute and you can cut steel with a 2-flute.
alum. roughing I like 3-flute cutters and 2-flute for finishing.
(4-flute tend to wad up the alum to easily)
2-flutes on steel are not my favorite due to slower sfm which results in
slower feed rates. I'd use 4 or more flutes on steel.
I generally use two flutes on aluminum because the cutter can be run
faster with a heavier chip load without clogging. Steel gets 4 flutes
because the usual limiting factor is rpm, not depth of cut. And
because they neeed to be run slower four flutes gets to be run at
twice the feed of two flutes. Even with the cutter buried in steel as
far as it can the speed is usually slow enough to allow chips to get
out of the endmill with four flutes. But hey, that's just me. YMMV
Eric R Snow,
E T Precision Machine

jackK wrote:
wrote:

This is a dumb question, but what are the relative advantages of
4-Flute vs. 2-Flute end mills, and on what applications should one type
be chosen over the other?

Harry C.

4-flute = steel
2-flute = aluminum

Yeah, it sounds so simple. But, the real problem is the primary and
secondary relief angles cut into the back of the cutting flutes.
You really want more relief for aluminum, but a 2-flute EM does NOT
guarantee that, at all. There are special aluminum end mills that have
less metal backing up the cutting edge, so you can increase the feed
like crazy without the back of the flutes rubbing on the advancing work.
I accidentally made one of these when resharpening some end mills, and
they were awesome! You want just a tiny bit of primary relief behind
the cutting edge, and then a 15 degree secondary relief right behind
the edge. You can tell if the back of your flutes are rubbing if they
have aluminum rubbed onto them after heavy stock removal passes.

Without having to buy $60 Ski-Carb end mills, I generally use small
4-flute end mills in aluminum, as you get twice as many cutting edges
per revolution.

Today, practically all 4-flute cutters are center-cutting, too. Also,
don't forget the 3-flute cutters. They are a nice compromise. You can
even get 1-flute cutters!

Jon

"Jon Elson" wrote in message
rvers.com...
snip---

Without having to buy $60 Ski-Carb end mills, I generally use small
4-flute end mills in aluminum, as you get twice as many cutting edges
per revolution.

But at the cost of less chip clearance. You generally can't run the table
feed fast enough to load the cutter well with two flutes, so 4 really serve
no purpose, and the minimal clearance you spoke of make using them a real
PITA. Lots of flute loading if you run at respectable speeds, and smearing
at the cutting edge. Avoid using 4 flute end mills in aluminum when
possible.

Today, practically all 4-flute cutters are center-cutting, too. Also,
don't forget the 3-flute cutters. They are a nice compromise. You can
even get 1-flute cutters!

Jon

But if you're serious about machining aluminum specify aluminum cutters, as
Jon already advised. The clearances are way different so they perform heads
and shoulders better. Aluminum cutting end mills are often so marked on
the shank. Don't use them for steel. They'll cut, but the slender edges
can't cool very fast and quickly burn.

Harold

"Pete Snell" wrote in message
...
wrote:

This is a dumb question, but what are the relative advantages of
4-Flute vs. 2-Flute end mills, and on what applications should one type
be chosen over the other?

Harry C.


2 flute can plunge cut, 4 flute cannot.


Not true. Center cutting 4 flute end mills are available. See above
comments on clearances for aluminum versus steel cutters. That, and chip
clearance, are the real issues.

Harold

"Steve Lusardi" wrote in message
...
The previous responses were general, but not absolute. You can use 2 flute
on steel and there are 4 flute end mills that plunge. It is all about chip
clearance really.
Steve

Nope. It's about relief angles, which are the real limiting factors if you
expect good tool life and good cutting performance. Chip clearance is not to
be ignored, however. Properly ground 4 flute end mills applied to aluminum
would likely suffer from chip clearance problems with considerable loading
of the flutes, often leading to broken end mills.

Harold

"Proctologically Violated©®" wrote in message
...
snip---
You can also get better finishes w/ a 4 flute, as you are getting more
cuts
per rotation.

Depends on the job at hand. Often you are better off with fewer flutes so
you can eject the chips----nothing is cut and dried when machining with end
mills----each job may have a different requirement. That's why there's such
a large variety of configurations.

Harold

"Daniel A. Mitchell" wrote in message
...
snip-

2-flute cutters are also better for slotting to size (especially in thin
materials) in one pass. Side deflection of the cutter still occurs, but
it doesn't widen the cut as it does with 4-flute cutters ... think about
it).

Yep! Special short 2 flute end mills are made expressly for cutting
keyways.

Harold

"Grant Erwin" wrote in message
...
snip-----

You will when you're faced with a serious application. Don't think so?
Try using a 4 flute half inch end mill taking a serious cut (full width and
half inch depth) on some ½" 6061-T6 aluminum plate, high spindle speed
(4,000 RPM) and fast feed. Then lets talk.

Harold

Proctologically Violated©® wrote:


2 flute can plunge cut, 4 flute cannot.


Pete,
Not quite correct.
4-flutes come in "center cutting" and non-center-cutting varieties.
Center-cutting 4 flutes plunge readily. May not have quite the chip
ejection as 2 flutes, but they still plunge very well--may have to peck
more.

Yes, I realized I was being pretty general, but most of the general
purpose 4 flutes don't center cut. (or at least they didn't used to. I'm
getting kinda old and haven't had to buy a 4 flute end mill in a while.....)

Pete

--
__
Pete Snell
Royal Military College
Kingston Ontario


The reasonable man adapts himself to the world;
the unreasonable one persists in trying to adapt the world to himself.
Therefore all progress depends on the unreasonable man.
- George Bernard Shaw

"Pete Snell" wrote in message
...
Proctologically Violated©® wrote:


2 flute can plunge cut, 4 flute cannot.


Pete,
Not quite correct.
4-flutes come in "center cutting" and non-center-cutting varieties.
Center-cutting 4 flutes plunge readily. May not have quite the chip
ejection as 2 flutes, but they still plunge very well--may have to peck
more.

Yes, I realized I was being pretty general, but most of the general
purpose 4 flutes don't center cut. (or at least they didn't used to. I'm
getting kinda old and haven't had to buy a 4 flute end mill in a
while.....)

Pete

Your comments were quite on target for older end mills, Pete. I recall
when the vast majority of 4 flute end mills not only were not center
cutting, but the center area was totally relieved. When rebuilding such
end mills, the gashing process to restore the rake angle on the ends
eliminates the center area as well. Center cutting 4 flute end mills are
far more difficult to grind than when using the gashing process.

Harold

Harold and Susan Vordos wrote:

"Grant Erwin" wrote in message
...
snip-----

You will when you're faced with a serious application. Don't think so?
Try using a 4 flute half inch end mill taking a serious cut (full width and
half inch depth) on some ½" 6061-T6 aluminum plate, high spindle speed
(4,000 RPM) and fast feed. Then lets talk.


Well, I NEVER run an end mill with a plunge depth equal to the diameter.
My general rule is that the plunge depth should never be more than 1/2 the
tool diameter, ESPECIALLY when cutting at full width. Maybe some
end mills can take this, but to my mind, that is really pushing things.
Of course, on a finish pass, I might use the full length of cut of the
cutter,
but the width of cut is real light.

Are you talking about solid carbide cutters, here?

Jon

"Jon Elson" wrote in message
...
Well, I NEVER run an end mill with a plunge depth equal to the diameter.
My general rule is that the plunge depth should never be more than 1/2 the
tool diameter, ESPECIALLY when cutting at full width. Maybe some
end mills can take this, but to my mind, that is really pushing things.

You should try taking heavier cuts. Roughing endmills can easily meet this
ratio in tool steel, and exceed it in aluminum.

Just buy two of the same endmill - run the first progressively harder until
it breaks (_if_ it breaks, perhaps), and then back off the feeds for the
second one - only half kidding.

It has been my limited experience that feeds and speeds in aluminium are
usually dicated by the spindle horse power.

Of course, on a finish pass, I might use the full length of cut of the
cutter,
but the width of cut is real light.

Are you talking about solid carbide cutters, here?

HSS. Coolant (lots) is important at this surface speed (300-500 FPM) to
prevent chips from welding to the cutter.

As an aside, it's interesting to see the feeds and speeds for aluminum that
the guys over in AMC are using. 5,000 FPM with diamond cutters.

Regards,

Robin

"Jon Elson" wrote in message
...


Harold and Susan Vordos wrote:

"Grant Erwin" wrote in message
...
snip-----

You will when you're faced with a serious application. Don't think so?
Try using a 4 flute half inch end mill taking a serious cut (full width
and
half inch depth) on some ½" 6061-T6 aluminum plate, high spindle speed
(4,000 RPM) and fast feed. Then lets talk.


Well, I NEVER run an end mill with a plunge depth equal to the diameter.
My general rule is that the plunge depth should never be more than 1/2 the
tool diameter, ESPECIALLY when cutting at full width. Maybe some
end mills can take this, but to my mind, that is really pushing things.
Of course, on a finish pass, I might use the full length of cut of the
cutter,
but the width of cut is real light.

Are you talking about solid carbide cutters, here?

Jon


No, HSS, which can deal with a cut of that nature with no problems as long
as you don't subscribe to the theory that how an end mill is ground makes no
difference as to performance. The amount of relief for four flute end
mills is such that they don't respond well to rapid feeds, so when you crowd
them, they tend to drag on the bottom of the primary relief, plus the chips
tend to overwhelm the flutes.

Have you ever operated a hydraulic duplicating (tracer) mill profiling
aluminum? You can generally plunge diameter depth and run like hell so
long as you lubricate well and use 2 flute end mills. Makes all the
difference in the world.

Harold

Harold and Susan Vordos wrote:
"Jon Elson" wrote in message
...


Harold and Susan Vordos wrote:


"Grant Erwin" wrote in message
...
snip-----

You will when you're faced with a serious application. Don't think so?
Try using a 4 flute half inch end mill taking a serious cut (full width

and

half inch depth) on some ½" 6061-T6 aluminum plate, high spindle speed
(4,000 RPM) and fast feed. Then lets talk.



Well, I NEVER run an end mill with a plunge depth equal to the diameter.
My general rule is that the plunge depth should never be more than 1/2 the
tool diameter, ESPECIALLY when cutting at full width. Maybe some
end mills can take this, but to my mind, that is really pushing things.
Of course, on a finish pass, I might use the full length of cut of the
cutter,
but the width of cut is real light.

Are you talking about solid carbide cutters, here?

Jon



No, HSS, which can deal with a cut of that nature with no problems as long
as you don't subscribe to the theory that how an end mill is ground makes no
difference as to performance. The amount of relief for four flute end
mills is such that they don't respond well to rapid feeds, so when you crowd
them, they tend to drag on the bottom of the primary relief, plus the chips
tend to overwhelm the flutes.

Have you ever operated a hydraulic duplicating (tracer) mill profiling
aluminum? You can generally plunge diameter depth and run like hell so
long as you lubricate well and use 2 flute end mills. Makes all the
difference in the world.

Harold


That reminds me of the good old days.... 2 spindle bridgeports... 4
spindle cincinati hydrotails.... 6 spindle wilsons.... tracer lathes...

back when sheep were scared, Jack

"jackK" wrote in message
news:0iwVd.2186$ju.517@okepread07...
Harold and Susan Vordos wrote:
"Jon Elson" wrote in message
...


Harold and Susan Vordos wrote:


"Grant Erwin" wrote in message
...
snip-----

You will when you're faced with a serious application. Don't think
so?
Try using a 4 flute half inch end mill taking a serious cut (full width

and

half inch depth) on some ½" 6061-T6 aluminum plate, high spindle speed
(4,000 RPM) and fast feed. Then lets talk.



Well, I NEVER run an end mill with a plunge depth equal to the diameter.
My general rule is that the plunge depth should never be more than 1/2
the
tool diameter, ESPECIALLY when cutting at full width. Maybe some
end mills can take this, but to my mind, that is really pushing things.
Of course, on a finish pass, I might use the full length of cut of the
cutter,
but the width of cut is real light.

Are you talking about solid carbide cutters, here?

Jon



No, HSS, which can deal with a cut of that nature with no problems as
long
as you don't subscribe to the theory that how an end mill is ground
makes no
difference as to performance. The amount of relief for four flute end
mills is such that they don't respond well to rapid feeds, so when you
crowd
them, they tend to drag on the bottom of the primary relief, plus the
chips
tend to overwhelm the flutes.

Have you ever operated a hydraulic duplicating (tracer) mill profiling
aluminum? You can generally plunge diameter depth and run like hell
so
long as you lubricate well and use 2 flute end mills. Makes all the
difference in the world.

Harold


That reminds me of the good old days.... 2 spindle bridgeports... 4
spindle cincinati hydrotails.... 6 spindle wilsons.... tracer lathes...

back when sheep were scared, Jack

Chuckle! Apparently you have!

Harold

"Harold and Susan Vordos" wrote in message
...

"Pete Snell" wrote in message
...
Proctologically Violated©® wrote:


2 flute can plunge cut, 4 flute cannot.


Pete,
Not quite correct.
4-flutes come in "center cutting" and non-center-cutting varieties.
Center-cutting 4 flutes plunge readily. May not have quite the chip
ejection as 2 flutes, but they still plunge very well--may have to
peck
more.

Yes, I realized I was being pretty general, but most of the general
purpose 4 flutes don't center cut. (or at least they didn't used to. I'm
getting kinda old and haven't had to buy a 4 flute end mill in a
while.....)

Pete

Your comments were quite on target for older end mills, Pete. I recall
when the vast majority of 4 flute end mills not only were not center
cutting, but the center area was totally relieved. When rebuilding such
end mills, the gashing process to restore the rake angle on the ends
eliminates the center area as well. Center cutting 4 flute end mills are
far more difficult to grind than when using the gashing process.


Probly easiest just to take one flute clear past center while its chucked in
the T&C grinder, then let there be a 'gash' in the other three flutes--kinda
similar to the typical three flute centercutting end grind......

We keep a ~5 in dia x 1/2 thick white wheel on one of our bench grinders at
all times just for the detailing of endmill ends....

It's dressed out something like this :

| |
| |
| |
| |
\ |
\ |
|_|

| |------.040in appx.

--

SVL

"Harold and Susan Vordos" wrote in message
...

"jackK" wrote in message
news:0iwVd.2186$ju.517@okepread07...
Harold and Susan Vordos wrote:
"Jon Elson" wrote in message
...


Harold and Susan Vordos wrote:


"Grant Erwin" wrote in message
...
snip-----

You will when you're faced with a serious application. Don't think
so?
Try using a 4 flute half inch end mill taking a serious cut (full
width

and

half inch depth) on some ½" 6061-T6 aluminum plate, high spindle
speed
(4,000 RPM) and fast feed. Then lets talk.



Well, I NEVER run an end mill with a plunge depth equal to the
diameter.
My general rule is that the plunge depth should never be more than 1/2
the
tool diameter, ESPECIALLY when cutting at full width. Maybe some
end mills can take this, but to my mind, that is really pushing
things.
Of course, on a finish pass, I might use the full length of cut of the
cutter,
but the width of cut is real light.

Are you talking about solid carbide cutters, here?

Jon



No, HSS, which can deal with a cut of that nature with no problems as
long
as you don't subscribe to the theory that how an end mill is ground
makes no
difference as to performance. The amount of relief for four flute
end
mills is such that they don't respond well to rapid feeds, so when you
crowd
them, they tend to drag on the bottom of the primary relief, plus the
chips
tend to overwhelm the flutes.

Have you ever operated a hydraulic duplicating (tracer) mill profiling
aluminum? You can generally plunge diameter depth and run like hell
so
long as you lubricate well and use 2 flute end mills. Makes all the
difference in the world.

Harold


That reminds me of the good old days.... 2 spindle bridgeports... 4
spindle cincinati hydrotails.... 6 spindle wilsons.... tracer lathes...

back when sheep were scared, Jack

Chuckle! Apparently you have!


Hmmm....my stepfather knew Henry Wilson personally....

Lessee....at Certified, we did have at least one 12 spindle hydrotel.....we
had to run 1/2 the cutters as L/H and conventional cut--wasnt worth a damned
for finishing, but for 17-4 and 6al4v it sure shaved off a bunch of time in
the ruffing stages.......

There was also a couple of Wilson's converted planers there that were setup
with ~ 15 ft long tilt tables.....along with the std 3d tracer valve, the
pattern and table would both tilt upon -x- axis travel, via a separate
template attached to the bed....

Wilson's valves would sometimes inexplicably stick and scrap parts, and were
particularilarly subject to problems with fluid temperature...so much that
in the latter days Boing dis-allowed Wilson's valves in their quality
program... no biggee...(LOL) Certified just made up a bunch of data plates
that said "rosebrook" on em and attached em to all the Wilson valves....

Yup, those were the days, all right....

--

SVL

"PrecisionMachinisT" wrote in message
...

"Harold and Susan Vordos" wrote in message
...

"Pete Snell" wrote in message
...
Proctologically Violated©® wrote:


2 flute can plunge cut, 4 flute cannot.


Pete,
Not quite correct.
4-flutes come in "center cutting" and non-center-cutting varieties.
Center-cutting 4 flutes plunge readily. May not have quite the chip
ejection as 2 flutes, but they still plunge very well--may have to
peck
more.

Yes, I realized I was being pretty general, but most of the general
purpose 4 flutes don't center cut. (or at least they didn't used to.
I'm
getting kinda old and haven't had to buy a 4 flute end mill in a
while.....)

Pete

Your comments were quite on target for older end mills, Pete. I
recall
when the vast majority of 4 flute end mills not only were not center
cutting, but the center area was totally relieved. When rebuilding
such
end mills, the gashing process to restore the rake angle on the ends
eliminates the center area as well. Center cutting 4 flute end mills
are
far more difficult to grind than when using the gashing process.


Probly easiest just to take one flute clear past center while its chucked
in
the T&C grinder, then let there be a 'gash' in the other three
flutes--kinda
similar to the typical three flute centercutting end grind......

We keep a ~5 in dia x 1/2 thick white wheel on one of our bench grinders
at
all times just for the detailing of endmill ends....

It's dressed out something like this :

| |
| |
| |
| |
\ |
\ |
|_|

| |------.040in appx.

--

SVL


Pretty cool setup! Where I was trained we used a parting wheel and did
the gashing with the cutter grinder and an index head, so the rake angle and
chip relief was already established and ready to sharpen. Parting wheels cut
fast and cool and saves hand dressing time, but that's no big deal.

Sadly, we were not taught to make them center cutting. I especially like
your comments on the one long tooth. Would work great and be easier to
generate. Thanks for the tip! When that magic day comes that I have my
shop in full swing, I'll certainly put it to good use.

Harold

"PrecisionMachinisT" wrote in message
...
snip-----

There was also a couple of Wilson's converted planers there that were
setup
with ~ 15 ft long tilt tables.....along with the std 3d tracer valve, the
pattern and table would both tilt upon -x- axis travel, via a separate
template attached to the bed....

Interesting! Converting old planers must have been fairly common. Not
long after I started my shop ('67) I landed the first serious contract that
got me on my feet, making templates for components for the Boeing 747
superstructure. The job had been handed down through several shops
before it got to me, but prints came from LTV. At any rate, the shop for
which I made the templates (McGee & Hogan, now defunct) used a planer that
had been converted to tracer application by adding two milling heads to it.
I never saw it in operation, but with it they produced four different
components, each of which required four templates, one for each face of the
required parts.

Harold

"Harold and Susan Vordos" wrote in message
...

Sadly, we were not taught to make them center cutting. I especially like
your comments on the one long tooth. Would work great and be easier to
generate. Thanks for the tip! When that magic day comes that I have my
shop in full swing, I'll certainly put it to good use.


Well.....

Not sure if it's true or not, but I've heard some rumours--something about
some "great machine shop in the sky"....where the cutting tools are always
freshly sharpened, and the machines all brand sparkling new, and deadly
accurate....

The blueprints are all carefully dimensioned--and if even a hint of any
problem crops up, there's a whole staff of engineers that are just *dying*
to help us out.

Man, I tell ya....that's where *I* wanna go when *I* die.....

--

SVL

"Harold and Susan Vordos" wrote in message
...

"PrecisionMachinisT" wrote in message
...
snip-----

There was also a couple of Wilson's converted planers there that were
setup
with ~ 15 ft long tilt tables.....along with the std 3d tracer valve,
the
pattern and table would both tilt upon -x- axis travel, via a separate
template attached to the bed....

Interesting! Converting old planers must have been fairly common. Not
long after I started my shop ('67) I landed the first serious contract
that
got me on my feet, making templates for components for the Boeing 747
superstructure. The job had been handed down through several shops
before it got to me, but prints came from LTV. At any rate, the shop for
which I made the templates (McGee & Hogan, now defunct) used a planer that
had been converted to tracer application by adding two milling heads to
it.
I never saw it in operation, but with it they produced four different
components, each of which required four templates, one for each face of
the
required parts.


The tilt tables used a "180 valve"--these were typically used for tool
height control when operating in 2d mode...push up on the probe and the head
rises.....let loose of it and the head travels slowly downward until it hits
something--kind of a "floating" sort of arrangement, and really handy if you
were using preset tool lengths....what you would do is put a small turret
with adjusting screws underneath the probe...similar to the end stops on
your typical turret lathe....

But in the case of this particular machine, an additional 180 valve was
attached to the tilt tables and another pattern was afffixed to the machine
bed--I recall some sort of linkage or maybe it was the other way around,
with the probe affixed to the bed--its been quite some time now and for the
life of me I can't remember all of the details anymore...

--

SVL

"Robin S." wrote in message
. ..

As an aside, it's interesting to see the feeds and speeds for aluminum
that
the guys over in AMC are using. 5,000 FPM with diamond cutters.


Robin,

I routinely run cobalt hss tools in 6061 aluminum at appx that
speed.....2-1/2in dia shell mills....at 7500rpms to be exact....

The material removal rates are kinda awesome what with having 15 hp
available at the spindle and feeding it fast enough to peg the meter...

--

SVL

"PrecisionMachinisT" wrote in message
...

"Robin S." wrote in message
. ..

As an aside, it's interesting to see the feeds and speeds for aluminum
that
the guys over in AMC are using. 5,000 FPM with diamond cutters.


Robin,

I routinely run cobalt hss tools in 6061 aluminum at appx that
speed.....2-1/2in dia shell mills....at 7500rpms to be exact....

The material removal rates are kinda awesome what with having 15 hp
available at the spindle and feeding it fast enough to peg the meter...

--

SVL


***WOW!***

Very impressive, Sam. The marvels of high speed spindles!

Harold

q
"PrecisionMachinisT" wrote in message
...
snip-----

--I recall some sort of linkage or maybe it was the other way around,
with the probe affixed to the bed--its been quite some time now and for
the
life of me I can't remember all of the details anymore...

Don't think for even one moment you have a corner on that market! This
getting old thing really sucks.

Harold

"Harold and Susan Vordos" wrote in message
...

I routinely run cobalt hss tools in 6061 aluminum at appx that
speed.....2-1/2in dia shell mills....at 7500rpms to be exact....

The material removal rates are kinda awesome what with having 15 hp
available at the spindle and feeding it fast enough to peg the meter...

--

SVL


***WOW!***

Very impressive, Sam. The marvels of high speed spindles!


One thing that I forgot to mention is these are roughers--you know, the
'hogger' style shell mills....

--

SVL