What's a good endmill for cutting stainless plate? (encountering problems)
Marshall Johnson
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
jim rozen
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
==================================================
Glenn Ashmore
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:
--
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
wws
> In article <63e2da16.03120...@posting.google.com>, 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
Lennie the Lurker
>
> 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.
>
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.
Steve Lusardi
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" <Marsh...@hotmail.com> wrote in message
news:63e2da16.03120...@posting.google.com...
Marshall Johnson
> 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.
jim rozen
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.
Spehro Pefhany
(Marshall Johnson) wrote:
>jim rozen <jim_m...@newsguy.com> wrote in message news:<bqtp5...@drn.newsguy.com>...
>
>> 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"
sp...@interlog.com Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog Info for designers: http://www.speff.com
Jon Elson
Marshall Johnson wrote:
>jim rozen <jim_m...@newsguy.com> wrote in message news:<bqtp5...@drn.newsguy.com>...
>
>
>
>>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
WTF STEEL
stainless is to tough for it to work
--
posted from
http://www.polytechforum.com/metalworking/what-s-a-good-endmill-for-cutting-stainless-plate-encounte-298349-.htm
using PolytechForum's Web, RSS and Social Media Interface to
rec.crafts.metalworking and other engineering groups
Snag
. 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
Ecnerwal
> 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 .
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.
Pete S
he get going again? Will the solid carbide cutter do it?
Pete Stanaitis
----------------
Gunner Asch
rate, with the proper coolant.
Doesnt anybody read materials data sheets anymore????
http://cartech.ides.com/datasheet.aspx?i=103&e=218
Workability
Hot Working
Carpenter Stainless Type 321 can be readily forged, hot headed,
riveted and upset. Because of its high red-hardness, more power for a
given reduction is required than with mild steel.
Forging
Heat uniformly to 2100/2300�F (1149/1260�C). Do not forge below 1700�F
(927�C). Forgings can be air-cooled. For full corrosion resistance,
forgings must be water quenched or annealed.
Cold Working
Carpenter Stainless Type 321 is readily fabricated by cold working.
Being extremely tough and ductile, it responds to deep drawing,
bending, forming and upsetting. After cold working, it is slightly
magnetic. The tensile strength and hardness of Carpenter Stainless
Type 321 can be significantly increased by cold working.
Machinability
Like all the austenitic steels, this alloy machines with a tough and
stringy chip. Rigidly supported tools, with as heavy a cut as
possible, should be used to prevent glazing. Moderate cold working can
improve machined surface finish.
Following are typical feeds and speeds for Carpenter Stainless Type
321.
Machinability Tables
***See link below .....
Additional Machinability Notes
When using carbide tools, surface speed feet/minute (sfpm) can be
increased between 2 and 3 times over the high speed suggestions. Feeds
can be increased between 50 and 100%.
Figures used for all metal removal operations covered are average. On
certain work, the nature of the part may require adjustment of speeds
and feeds. Each job has to be developed for best production results
with optimum tool life. Speeds or feeds should be increased or
decreased in small steps.
Weldability
Carpenter Stainless Type 321 can be satisfactorily welded by the
shielded fusion and resistance welding processes. Oxyacetylene welding
is not recommended, since carbon pickup in the weld may occur. Since
austenitic welds do not harden on air cooling, the welds should have
good toughness. When a filler metal is required, AWS E/ER347 welding
consumables should be considered. To decrease the susceptibility to
hot cracking, keep heat inputs, base metal dilution, and joint
restraint to a minimum. The alloy can be used in the as-welded
condition; however, for elevated temperature service, a postweld
stabilizing heat treatment should be considered."
http://cartech.ides.com/ImageDisplay.aspx?E=218&IMGURL=%2fCarpenterImages%2fB-StainlessSteel%2f49-SS49-Type321%2f01_SS49_TypicalMachining.gif&IMGTITLE=Machinability+Tables
Geeze guys..its not fucking rocket science.....
Gunner
__
"Anyone who things Obama is doing a good job
is either stupid or a perpetual societal leech"
Snag
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 ...
Gunner Asch
<sp...@baldwin-telecom.net> 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
and fast and dig into it. With fresh inserts....!!
__
"Anyone who things Obama is doing a good job
is either stupid or a perpetual societal leech"