Hi, I'm currently making a thick flange on a CNC mill. The material is
a 1/2" thick plate of 321 stainless. Previously, we made a prototype
out of 3/8" mild steel. That piece cut relatively easy, as was
expected. We knew that the thicker stainless piece was going to be
much tougher to cut, so we made sure that we used lower speeds and
plenty of coolant.

Here's the problem: Starting with a new Sossner 4 flute high speed
steel endmill, the same kind that we used to cut the prototype, we
began cutting the 321 stainless. The first 1/8 inch or so it was slow
but steady, we expected it to be tough. But after that it began to
chatter and the cutting slowed down. By about 1 inch of cutting, the
endmill was worn out.

Something's not right here. I knew it would be tough but not THAT
tough. How come the endmill wore out so quickly? I know that people
who work with stainless don't go through 30 endmills to make a
relatively small piece.

Does anyone have any recommendations of what kind of endmill to use to
cut thick 321 stainless? Is the material that our endmill is composed
of simply too soft a metal? Replacing cutters every couple of inches
isn't an option.

I'm sure that someone can lead me in the right direction.


Thanks,

Marshall

In article , Marshall Johnson
says...

Something's not right here. I knew it would be tough but not THAT
tough. How come the endmill wore out so quickly?

Post up the sfpm you were running on the tool,
and the feed rate. Either your idea of 'slow'
for the rpm is incorrect, or you were running
the feed rate so slow as to allow the material
to work harden under the tool.

Just a guess, there will be others here that
will be more accurate.

Jim

==================================================
please reply to:
JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com
==================================================

jim rozen wrote:

In article , Marshall Johnson
says...


Something's not right here. I knew it would be tough but not THAT
tough. How come the endmill wore out so quickly?


Post up the sfpm you were running on the tool,
and the feed rate. Either your idea of 'slow'
for the rpm is incorrect, or you were running
the feed rate so slow as to allow the material
to work harden under the tool.

Just a guess, there will be others here that
will be more accurate.

Jim

Besides rpm, endmill diameter, depth of cut, and conventional or climb
milling should be considered.
I like big roughers.

wws

jim rozen wrote in message ...

Post up the sfpm you were running on the tool,
and the feed rate. Either your idea of 'slow'
for the rpm is incorrect, or you were running
the feed rate so slow as to allow the material
to work harden under the tool.


Sorry for the late reply.

The spindle speed was 200 rpm. Originally the feed rate was 1.5" per
minute, but that was when we wrote the program for the mild steel. By
the time we were taking a good cut into the metal, we had the feed
rate slowed down to about 1/10" an inch per minute.

Keep in mind that we were trying to cut through this 1/2" piece in one
pass. It looks like we're going to have to bump up the feed rate and
only go half way through the piece on each pass, or maybe even less.

In article , Marshall Johnson
says...

The spindle speed was 200 rpm.

Ok, that's only *part* of the number you need.
How large is the end mill diameter? From that
you can calculate the *surface* feet per minute
that the cutting tool is running at. That's
what counts.

Jim

==================================================
please reply to:
JRR(zero) at yktvmv (dot) vnet (dot) ibm (dot) com
==================================================

On 8 Dec 2003 18:18:56 -0800, the renowned
(Marshall Johnson) wrote:

jim rozen wrote in message ...

Post up the sfpm you were running on the tool,
and the feed rate. Either your idea of 'slow'
for the rpm is incorrect, or you were running
the feed rate so slow as to allow the material
to work harden under the tool.


Sorry for the late reply.

The spindle speed was 200 rpm. Originally the feed rate was 1.5" per
minute, but that was when we wrote the program for the mild steel. By
the time we were taking a good cut into the metal, we had the feed
rate slowed down to about 1/10" an inch per minute.

The feed rate, if it was right originally, should not be that much
different. The spindle RPM ought to be much less. But, as Jim said,
what's the cutter diameter of your 4-flute end mill?

RPM ~= SFM * 4/(cutter diameter)
Feedrate = RPM * feed per tooth * 4 for a 4-flute end-mill

(the recommended feed per tooth also depends on the cutter diameter)

Best regards,
Spehro Pefhany
--
"it's the network..." "The Journey is the reward"
Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog Info for designers: http://www.speff.com

Marshall Johnson wrote:

jim rozen wrote in message ...



Post up the sfpm you were running on the tool,
and the feed rate. Either your idea of 'slow'
for the rpm is incorrect, or you were running
the feed rate so slow as to allow the material
to work harden under the tool.




Sorry for the late reply.

The spindle speed was 200 rpm. Originally the feed rate was 1.5" per
minute, but that was when we wrote the program for the mild steel. By
the time we were taking a good cut into the metal, we had the feed
rate slowed down to about 1/10" an inch per minute.


Well, there's your problem! With any material that work hardens (SS is
notorious for this, but many other harder materials also do it) you reduce
the depth of cut, and may need to INCREASE the feedrate!
There's no way you can make this cut in a single pass except with monster
machines and very large diameter cutters.

(A horizontal mill could do it in one pass if rigid enough, but due to
the nature
of the cutting action, a vertical mill ends up producing very thin chips
at the
sides when plowing at full width, and this is where the work hardening
begins to develop.)

Jon

Keep in mind that we were trying to cut through this 1/2" piece in one
pass. It looks like we're going to have to bump up the feed rate and
only go half way through the piece on each pass, or maybe even less.

I have been milling a lot of 316 lately and have found that the main
thing you need is a lot of intestinal fortitude to crank up the feed
rate. Especially on a middle weight mill like I have. You have to be
pretty agressive to get under the surface that was work hardened on the
previous rotation.

Marshall Johnson wrote:

Hi, I'm currently making a thick flange on a CNC mill. The material is
a 1/2" thick plate of 321 stainless. Previously, we made a prototype
out of 3/8" mild steel. That piece cut relatively easy, as was
expected. We knew that the thicker stainless piece was going to be
much tougher to cut, so we made sure that we used lower speeds and
plenty of coolant.

Here's the problem: Starting with a new Sossner 4 flute high speed
steel endmill, the same kind that we used to cut the prototype, we
began cutting the 321 stainless. The first 1/8 inch or so it was slow
but steady, we expected it to be tough. But after that it began to
chatter and the cutting slowed down. By about 1 inch of cutting, the
endmill was worn out.

Something's not right here. I knew it would be tough but not THAT
tough. How come the endmill wore out so quickly? I know that people
who work with stainless don't go through 30 endmills to make a
relatively small piece.

Does anyone have any recommendations of what kind of endmill to use to
cut thick 321 stainless? Is the material that our endmill is composed
of simply too soft a metal? Replacing cutters every couple of inches
isn't an option.

I'm sure that someone can lead me in the right direction.


Thanks,

Marshall

--
Glenn Ashmore

I'm building a 45' cutter in strip/composite. Watch my progress (or lack
there of) at: http://www.rutuonline.com
Shameless Commercial Division: http://www.spade-anchor-us.com

(Marshall Johnson) wrote in message . com...

Something's not right here. I knew it would be tough but not THAT
tough. How come the endmill wore out so quickly? I know that people
who work with stainless don't go through 30 endmills to make a
relatively small piece.

321 is a horse of a different color. When you think you're slow
enough, cut the speed in half, and don't even think of letting that
cutter idle for even one turn. We made a lot of stuff for aircraft
exhaust systems, and 321 is the material of choice. Doesn't make you
like it, but does make you slow down. Try different coolants/cutting
compounds, sometimes that helps. Carbide cutter may help, just as
likely to be more of the same. Might try a cobalt alloy cutter.
Rotsa ruck.

Marshall,
I'm not familiar with 321, but with 316 the best cutter I have used is from
M42. This is an chrome vanadium ISO alloy and it is high in cobalt (5%). Use
a very slow speed, a high feed rate, lotsa coolant and small cuts. Take your
time. Do not use a dull tool. As soon as the edge starts to fail, change
immediately to prevent excessive work hardening.
Steve

"Marshall Johnson" wrote in message
om...
Hi, I'm currently making a thick flange on a CNC mill. The material is
a 1/2" thick plate of 321 stainless. Previously, we made a prototype
out of 3/8" mild steel. That piece cut relatively easy, as was
expected. We knew that the thicker stainless piece was going to be
much tougher to cut, so we made sure that we used lower speeds and
plenty of coolant.

Here's the problem: Starting with a new Sossner 4 flute high speed
steel endmill, the same kind that we used to cut the prototype, we
began cutting the 321 stainless. The first 1/8 inch or so it was slow
but steady, we expected it to be tough. But after that it began to
chatter and the cutting slowed down. By about 1 inch of cutting, the
endmill was worn out.

Something's not right here. I knew it would be tough but not THAT
tough. How come the endmill wore out so quickly? I know that people
who work with stainless don't go through 30 endmills to make a
relatively small piece.

Does anyone have any recommendations of what kind of endmill to use to
cut thick 321 stainless? Is the material that our endmill is composed
of simply too soft a metal? Replacing cutters every couple of inches
isn't an option.

I'm sure that someone can lead me in the right direction.


Thanks,

Marshall

replying to Marshall Johnson, WTF STEEL wrote:
Marshallj25 wrote:

Hi, I'm currently making a thick flange on a CNC mill. The material is
a 1/2" thick plate of 321 stainless. Previously, we made a prototype
out of 3/8" mild steel. That piece cut relatively easy, as was
expected. We knew that the thicker stainless piece was going to be
much tougher to cut, so we made sure that we used lower speeds and
plenty of coolant.
Here's the problem: Starting with a new Sossner 4 flute high speed
steel endmill, the same kind that we used to cut the prototype, we
began cutting the 321 stainless. The first 1/8 inch or so it was slow
but steady, we expected it to be tough. But after that it began to
chatter and the cutting slowed down. By about 1 inch of cutting, the
endmill was worn out.
Something's not right here. I knew it would be tough but not THAT
tough. How come the endmill wore out so quickly? I know that people
who work with stainless don't go through 30 endmills to make a
relatively small piece.
Does anyone have any recommendations of what kind of endmill to use to
cut thick 321 stainless? Is the material that our endmill is composed
of simply too soft a metal? Replacing cutters every couple of inches
isn't an option.
I'm sure that someone can lead me in the right direction.
Thanks,
Marshall


sadly you will have to cut a few inches and replace cutter because the 321
stainless is to tough for it to work

--
posted from
http://www.polytechforum.com/metalwo...te-298349-.htm
using PolytechForum's Web, RSS and Social Media Interface to
rec.crafts.metalworking and other engineering groups

WTF STEEL wrote:
replying to Marshall Johnson, WTF STEEL wrote:
Marshallj25 wrote:

Hi, I'm currently making a thick flange on a CNC mill. The material
is a 1/2" thick plate of 321 stainless. Previously, we made a
prototype out of 3/8" mild steel. That piece cut relatively easy, as
was expected. We knew that the thicker stainless piece was going to
be much tougher to cut, so we made sure that we used lower speeds and
plenty of coolant.
Here's the problem: Starting with a new Sossner 4 flute high speed
steel endmill, the same kind that we used to cut the prototype, we
began cutting the 321 stainless. The first 1/8 inch or so it was slow
but steady, we expected it to be tough. But after that it began to
chatter and the cutting slowed down. By about 1 inch of cutting, the
endmill was worn out.
Something's not right here. I knew it would be tough but not THAT
tough. How come the endmill wore out so quickly? I know that people
who work with stainless don't go through 30 endmills to make a
relatively small piece.
Does anyone have any recommendations of what kind of endmill to use
to cut thick 321 stainless? Is the material that our endmill is
composed of simply too soft a metal? Replacing cutters every couple
of inches isn't an option.
I'm sure that someone can lead me in the right direction.
Thanks,
Marshall


sadly you will have to cut a few inches and replace cutter because
the 321 stainless is to tough for it to work


Bull**** . They make solid carbide end mills just for such tough materials
.. Cobalt EM's too might do the job , I haven't tried mine on that particular
alloy but it worked well on some 4140 I cut recently - I'd go with at least
3/8 or 1/2 inch , low rotation speed and fairly heavy feed with plenty of
coolant .
--
Snag



---
This email is free from viruses and malware because avast! Antivirus protection is active.
http://www.avast.com

In article ,
"Snag" wrote:

They make solid carbide end mills just for such tough materials
. Cobalt EM's too might do the job , I haven't tried mine on that particular
alloy but it worked well on some 4140 I cut recently - I'd go with at least
3/8 or 1/2 inch , low rotation speed and fairly heavy feed with plenty of
coolant .

Aaaand the fundamental difference (which leads to Snag correctly
recommending slow rotation and heavy feed) is that unlike mild steel,
stainless work hardens very significantly. If you "take it easy" and cut
fine shavings you will fail 10 times out of 10. You have to cut serious
chips or not at all. It can be hard to wrap your head around, since the
instinctive response is to back off and go easy since it cuts hard -
that just happens to be exactly wrong for stainless.

Each new cut needs to get "beneath/beyond" the work-hardened "crust" of
the previous cut.

Lubrication was not mentioned - use some.

--
Cats, coffee, chocolate...vices to live by
Please don't feed the trolls. Killfile and ignore them so they will go away.

Just out of curiosity, now that the OP has work hardened the part, how does
he get going again? Will the solid carbide cutter do it?

Pete Stanaitis
----------------

Pete S wrote:
Just out of curiosity, now that the OP has work hardened the part,
how does he get going again? Will the solid carbide cutter do it?

Pete Stanaitis
----------------


If it does like 4140 that hard area will only be a skin a few thou thick .
If he can get under that skin it should be OK - and yes , carbide will cut
it . So will diamond ... I have a handful of diamond router bits , they were
too dull to cut particle board/MDF at 35,000 RPM but they do a swell job for
light cuts at lower speeds in very hard materials . They don't like
interrupted cuts ...
--
Snag



---
This email is free from viruses and malware because avast! Antivirus protection is active.
http://www.avast.com