speeds for .5mm end mill in 316ss

[Joel Schreiner]

I have to cut a slot using .5mm x 12mm osg fx endmill in 316ss . I only have 8000 rpm spindle.

I was hoping someone could help me with some speeds, feeds and doc. I have to be able to plug.

Thank you for all your help today and in the past.

Joel

[TREV]

good day,

you have your hands full with only 8000 rpm's.

id use it all and only take .0005 step down max and with that rpm youd be looking at only maybe 10 ipm (aprox .ooo5 chip load assuming its a 2 flute)

best of luck to you, hth

trevor

[Quickmike]

I went to the OSG website and found no feed or speed recomendations. Usually manufacturers have some litature available. I look up a similar tool, with the same coating in a competators catalog or website. It won't be exact but a good start. I haven't used OSG other than for taps but they are good cutters from what I've heard of them here on the forum.

[Fig sign]

S8000 f80 take-off 0.05 mm each cut .

if proportion height/diameter less than 3 add feed,more -feed slowly.

BTW I have 3 fluted 0.5 mm tools very heavily built ,so you can move faster.

But never move less than 0.05 -0.03 mm ,you`ll kill your tool ,this is not high speed machining ,the tool must cut !!!!!!!1

[TREV]

quote:

__________________________________________________

S8000 f80

__________________________________________________

 

wow thats a .oo5 chip load on a .0196 cutter.

call me a sissy but that seems reaaaal aggresive to me

trevor

[Philcott]

Trev,

 

I believe the wise Owl was talking 80mm per min not 80inches per min. 80mm works out to about .0002 feed per tooth.

 

Phil

[Fig sign]

You alwais have a dilemma :

what `s better to cut or to lick ?

If you have far less speed than you need to cut is better .

If you will lick with low speed you`ll ruin tool very fast ,so you will not succeed anyway.

I have 8000 rpm and my 0.3 end mill works on copper days and my 0.5 mill life on steel is also good .

Once I worked on machine with only 4000 rpm and took this principle from that days - low speed big take off and reasonable feed and good results !

If you afraid make your feed f240 and take off 0.01 mm and see what`s better

[Joel Schreiner]

Thank you for your advise . I agree that does seem a real agresive for a cutter that is .0196 in dia

and .5" long but the doc recommended is only .001.

I only have one cutter and a new one is weeks away. I have to do it right the first time.

I was thinking .001 chip load. Is that not enough?

joel

[Fig sign]

The question was about metric tool ,so was an answer .

0.05 mm take off stands for 0.002 step doun and I call it cutting

_________

0005 step down max

____________

 

I call this licking

 

HTH

[mold100]

when in doubt burn it out.You got an edm there?

 

I am all for milling but one cutter .02 x .5 reileved, nah I cut down to .012 ribs but no where near that depth.

 

Try it thats the only way to find out,8000 rpms I

havent been faced with that dilema - but I would try about 1.5 to 2 ipms .0005/.0007 d.o.c you gotta consider the length my air preesure if pointed dirctly at that would snap it off.

 

in the words of Crazy Mill man -

Dont be afriad to try something new.

[mold100]

Corey teh me and TREV are sissys Iskander da man

 

I would like to see footage of milling a .02 wide slot .5 deep with only 8000 rpms and a .002 step down at 3.2 inches per minute, I do alot of tedious **** with 42,000 rpms and I wouldnt take that on with one endmill.

 

8000*.0002*2=3.2

[Fig sign]

Joel ?

Do You have a lot of work to do with a tool ?

If no go with steps 0.03 mm but no less .

[Fig sign]

_______

I have to cut a slot using .5mm x 12mm osg fx endmill in 316ss

----------

Sorry ,guys ,i have not saw it is 12 mm long ( you really mean flute 12 mm long )?,

if so :

 

So drop the speed ,

s5500 f20 take off 0.01 all in mm

[Joel Schreiner]

I only have one slot 20mm ramped from full depth to nothing. I'm sorry I thought you meant 80 ipm just didn't think. I think I will try .002"doc with .0002 ipt. Thank you for all your help.

It will be a couple of hours before I cut it so If you think of anything else please let me know.

One other thing should I use coolant or air?

joel

[Fig sign]

Let`s say this is a tool 5 mm 120 mm long 2 flutes (10 times bigger ) and you must do the same .

How many times you`ll drop the tool speed to get rid of the chatter while slotting 0.1 mm on steel ?(5 times ,10 times ?)S3800 for short tool looks frightful ,right ?

 

and I think this is not strait analogy ,0.05*12 mm less rigid .

Sorry for misunderstanding and fooling of everyone !

[Fig sign]

Joel !

 

It wouldn`t stand 0.002 step down ,it is not enough rigid .

Also feed is too much .

I talk metric I mealn f20 max.

You will not hear any chatter ,you`ll hear a click and that`s all if any

[Fig sign]

________--

Corey teh me and TREV are sissys Iskander da man

 

____-----------

 

Iskander teh stupid fool

[Joel Schreiner]

I think I may have been typing when your post came up I didn't see it till after I sent mine. I do not know what to do? I will think about it over lunch.I will let you know what I come up with.

joel

[Fig sign]

Standart mill has a fute length 3*d.

it means for 0.5 -1.5 max .

Now a rigid cyllinder is a proportion dia/height 1/5 .

Your tool is completly not rigid ,you can broke it with a metal touch .

So don`t run it fast and you have enough speed for such a tool ,you will not run it faster anyway .

And coolant -water ,I think .

 

Good luck .

[mold100]

Joel,

 

sounds kinda like you may want to start off with or close to my numbers,Iskander thinks you should drop the rpms Normally I garee to reduce chatter at lenghths over 3*dia but I rarely back off rpms at tools under 1/32 - also what kind of flute legnth you have, you actually want little flute length and solid body through the reach.

[Joel Schreiner]

Thank you for all the help.

Went with .0007 doc 1. ipm 8000 rpm.

Worked great once again thank you for your help.

Joel

[mold100]

Glad we could be of assistance.Thanks for the update on how it went.

[Fig sign]

Joel !

 

Nice to know that your work is OK .

 

Next time I`ll try to read better from the start .

 

At youe service

[TREV]

glad it went well

trevor