Machining 304 Stainless Steel: Feeds & Speeds WW167

Sharing buttons:

hi folks 304 stainless it's a material

that has a notorious reputation for

being difficult to machine or rather

easy to destroy end mills with let's

walk through some speeds and feeds for

both external features as well as some

internal pockets and drilling welcome to

our Wednesday widget


in Wednesday widget 164 we covered

speeds and feeds for aluminum and

regular or mild steel both of those

materials they're relatively forgiving

they're relatively free machining

there's a wider range of speeds and

feeds that will work and they're not too

particular about what type of end Miller

tool that you use 304 stainless or many

of the same a series are the exact

opposite you've got a more narrow range

of speeds and fees the materials less

forgiving or it can work harden on you

and you've got to be much more conscious

of the tools that you use we're using in

fact a completely different end mill

when we're doing outside features versus

the tool that we use when we've got to

interpolate in to an inside pocket and a

shout-out to Tyson lamb Tyson's got a

great Instagram page where he makes a

lot of golf related accessories as well

as lamb crafted comm where he makes some

incredible putters and ball markers and

golf doughnuts and divot tool repairs

really cool stuff and Tyson has become

really good at machined stainless so he

was really helpful in some of the tips

and tricks and I want to show you guys

it's not that hard we can totally do

this we're using this five flute end

mill from lakeshore let's show the

speeds and feeds and the cuts and then

we'll come back afterwards and we'll

talk about the tools that we're using

why we're using them in some of the

additional details


first we'll start with the outside

profile we'll do a 2d adaptive first 200

service feet per minute mm of an inch

feed per tooth that's about point zero

five millimeters 0.05 inch that spent

1.3 millimeters or 20% of the tools and

our optimal load we're leaving 20

thousands of an inch or about half a

millimeter as well one of the big

differences with this 2d adaptive plus

2d con to a recipe is in the 2d adaptive

I normally don't leave as much radial

stock to leave but I want to leave

enough here that the tool can dig

underneath the 304 skin which can often

work harden and is something where

you're just not going to be able to take

just like we talked about in Wednesday

widget 164 you can't take little one

foul on stainless it will devastate your

tools quite quickly and finally a 2d

contour same recipe on the cleanup 200

surface feet 2001 foul of the floor just

to avoid rubbing along that floor

switching over to internal pockets so

totally different strategy what's

interesting to me is we're going

actually against the recommendation of

even lakeshore here and I say that only

because that's one of the things when

you get into these materials is you have

to figure out what simply works for you

so I wanted to do two things I want to

give you guys a starting recipe just to

run with but also the kind of confidence

to start thinking about this on your own

so we're using a for flute regular

variable food EndNote so that's not

their stainless style and it's for

flutes instead of five boots again we'll

come back to more about that in a minute

225 Service feet only one thousandth of

an inch per tooth a reduced optimal load

in this case is only 10% of the tool

diameter or point zero to five max

roughing step down of 0.15 inches 15

valve radial stock to leave and max to

degree helix





let's take a look under a microscope at

these chips we've got an aluminum chip a

mild steel chip and then the 304

stainless chip you take a look at the

aluminum chip you can see how the

material appears to be almost like it's

slightly torn it doesn't have that

really crisp it cut we look at the mild

steel it does have pretty clean shear

lines and then if we go to the stainless

chip it appears to have similarities

back to that aluminum where it's

slightly gummy there's a slight amount

of it just doesn't want to shear as

cleanly as that mild steel now let's

drill 304 stainless first off we need to

spot drill it 75 or so surface

feet-per-minute we're going 3,000 and

we're going down negative 30,000 this is

really important because this is going

to be what sort of breaks through that

hardened skin of the stainless steel and

presents a better non-work hardened

surface for our drill to do its job then

we're drilling 3/16 drill

it's cobalt we'll come back to that in a

second 45 surface feets per minute 3000

we're taking pretty big Peck depths

bigger than I would normally go in this

case just shy of 1 times diameter so

it's a point 1 875 drill about four

point seven millimeters and we're

pecking about that same amount worked

great which gets me really really

excited and I really can appreciate

Tyson he was spot-on and here was his

advice cobalt is the way to go for

drilling 304 it's great because it's

actually pretty darn inexpensive the

drill bit we just use is from McMaster

for 3 dollars and 67 cents that's a very

inexpensive for it for what the task is

at hand

45 service feet per minute 3000 we just

mentioned that full or big peck depth

that's what's really important here if

you take small pecks what you're

possibly doing is exposing the drill to

more of a work hardened surface here's

the other funny thing to walter COBOL

type drills from Lowe's or Home Depot

can work as well for example this guy

off Amazon 20 bucks but for a pack of 12

135-degree tip is what you want stay

away from the drills that have this sort

of branded thing they think they call it

pilot point you don't want to use those

so that's the good news you can probably

even find these drills locally we've

never bought a drill for another reason

I in this for the CNC shop at a home

depot or lowes however you are going to

need a spot drill to Center drill it

that has equal or bigger angle and I

actually didn't have one of those laying

around the shop so we went on to

McMaster and purchased this link in the

video description 140 degree carbide

spotting drill should last a pretty

darned a long time another important tip

is make sure your first Peck isn't a

shallow Peck what do I mean by that

take a look at a wireframe view we're

coming in and we're spot drilling down

to that depth and then we are doing our

Peck 0.16 inch deep but if you look at

my height stab the top height is a hole

top in the feed height I mean where do

we start drilling we don't start

drilling at the top of the hole we have

to start drilling or transitioning from

this yellow rapid move to a green drill

move in this case I set it at 20,000 the

top hole if we watch a simulation peck

peck peck peck peck back up so see that

first Peck was deep a bad example would

be if in our Heights tab we had done

something like change the top height to

have a point one inch offset we're gonna

Peck in point one six depths but we're

raising the top of our hole this way so

what can happen is that first Peck

doesn't go very deep or deep at all and

that can instantly fry a drill couple

final tips if you're going smaller than

1/8 of an inch

don't use cobalt but rather use carbide

the good news is the car by drills are

less expensive in those smaller

diameters and then just be careful with

really thin sheet stainless or sheet

because you've got a skin on both the

top and the bottom then stuff is more

skin relative to the overall thickness

so it's actually more difficult to drill

and so you may be better off

interpolating it quick recap we've got

two different quarter-inch end mills the

five flute four stainless we recommend

for outside profiling or cleaning up

don't ramp in with it here's the link

and here are the basic speeds and feeds

and we have the four flute quarter-inch

this even though it's not technically

meant for stainless we've had great luck

with it as has Tyson use it for internal

pockets or when you've got a ramp into

something and here are your starting

fees and speeds so let's talk a little

bit more about these two tools and

what's interesting so when I go to

lakeshore comm and I click on carbide

end mills

I've got variable for flute for tool


I've got variable v flute for stainless

and mild so what's the difference

between these two well the most obvious

difference is this is for flutes and

this is five flutes but these tools are

actually very different and that the

biggest difference is this four flute

has a more of a honed edge so it has a

more blunt edge what that means it is a

stronger edge because it's actually

honed over but what that also means is

you generally need to increase your chip

load per tooth remember again back to

the speeds and feeds in widget 164 this

inch per tooth because it's a honed edge

or has less sharpness we need to

increase that inch per tooth so as it

engages that material that more honed

edge is still able to dig underneath and

not rub the variable v flute for

stainless has a much sharper edge which

is really good for stainless steel

because believe it or not stainless

steel is kind of like aluminum it's

actually a gummy material it doesn't

really like to be cut so you need to use

a sharper edge to shear it so we use

that v flute for these external features

we found this to be really reliable and

really great the problem with the v

flute is it doesn't like to ramp that's

the red helical lead into a blind pocket

and the biggest reason that doesn't like

to do that is only

one of those five flutes actually goes

all the way to the center of the face so

in some respects you're only cutting

with one flute as you're doing an

interpolation and there's very little

gash clearance which is ability on the

face of that tool to evacuate or cut the

chip so you could adjust the helical

ramp diameter to try to work around that

but the better answer and again shout

out to Tyson for the help years just use

the four flutes

yes it's technically in the title not

meant for stainless in the description

includes stainless steels and I'll admit

as a layman this sometimes is

frustrating but as you get into these

more exotic materials you've got to use

recipes that your tooling supplier or

people who have done this before work

and if it works awesome some other tips

and tricks when you do a helical ramp in

never use more than two degree Rankine

again we recommend and Tyson recommended

using the four flute instead of the five

flute don't go greater than up 3/16 inch

or about four point seven millimeter

depth of cut I reduced this one to 0.15

because it's a point three deep pocket

so just taking it half at a time you

absolutely need an air-blast to help

evacuate the chip the number one cause

of end mill failure and stainless is

recutting your chips

you also need coolant for the lubricity

to help avoid the chips sticking to the

end mill so that's why I like the fog

Buster here with the air pressure and

some of the quality chem mixed into it

flood coolant it would work as long as

it's high enough pressure to really

evacuate those chips start off with a

reduced optimal load here we're doing

10% you can increase that but start with

something that works and then start

increasing your way up and experimenting

again ramp with a four flute once you're

ramped in you can go ahead and finish

with a five flute because again once

you've done that helical interpolation

the fact that it's an inside pocket is

no different really than the outside

pocket tools that have a small corner

radius in this case it may only be ten

fifteen twenty thousand seven-inch can

really help increase your tool life

because the very tip of that flute is

the weakest part so by getting rid of

that weakest

by adding a radius you're really helping

extend your tool life and avoid shallow

pockets because stainless steel has a

work-hardened scale when you purchase it

if you try to take say a ten or fifteen

thousand in all work-hardened some

material so if you have to do that

you're better off decking it off first

and so long as you have good feeds and

speeds when you do that you shouldn't

rework harden that service at least

that's my understanding we're gonna do

some more experimenting because quite

frankly this is pretty fun and it's good

to push myself

we tried machining three or four years

back and we failed so quickly that I

gave up you know it's intimidating I

think it's something where I'm hoping

giving you guys the right recipe the

right speeds and feeds the right tooling

we can all be cut in three or four folks

hope you learn something hope you

enjoyed take care see you next Wednesday