How to cut hard metals (stainless,mild steel etc...)

[tef9]

Hi There,

I have a BF30 mill (cnc) and would like to cut mainly stainless steel but perhaps some mild steel or free machining steel as well. I have a stepper motor system, so not servo based.

I have carbide tools (solid carbide not inserts) ... do I need coolant/Air blast? I take it I have to put the machine into low gear mode, I have also been told that spindle speed and feed rate should be much lower than Aluminum. I have some scrap stainless to test out cuts with however I dont want to destroy expensive tools without being armed by all the facts.

Any help appriciated.

Thanks,

Andy

[dugpits]

I hear ya...carbide is expensive!

Well, in general, the RPM is set by:

RPM = (12 * SFM)/(Pi * Diameter of tool).

I usually use [12 * SFM / 3 * Diameter] as a quick simplification.

I'm doing these calcs in our dang "American" units...but you get the idea.

There are guidelines for different materials being cut with HSS or Carbide.

There are many of these type charts out there...here is one:

Solid Carbide Speed & Feed

Carbide actually likes heat (to a point). Sometimes using liquid coolant on carbide actually shortens the tool life because if the coolant does not completely flood the flutes then the heat cycles (if that makes sense...hot outside the coolant flow, then cooled...hot...etc) - and the heat shock can lead to premature failure.

For a quick example...cutting 303 stainless. For a hobby machine a conservative feedrate might be a good place to start. Say as low as even 100 SFM.

Assuming 1/2" cutter.

RPM = 100*12/3*.5 = 800 RPM. Assuming 4 flutes at .0015"/flute = .006/rev = 4.8 IPM (~120 mm/min).

That is pretty conservative. A typical SFM for aluminum would be 10x that (1000 SFM) which would equate to 8,000 RPM and 48 IPM - most of us don't have that ability on these small mills. At work we run a 1/2 carbide with only 2 flutes in aluminum at about 10k and over 100IPM and it lasts forever....but we'll run a 4 flute 1/2 inch around 1600 RPM around 10-15 IPM in steel and it will be warn out in an hour or less.



The problem you may have with carbide on a hobby mill is that carbide is very hard - but very brittle whereas HSS isn't as hard but is more flexible.

Carbide can break surprisingly easy with a shock load, and hobby size machines aren't as rigid so they may vibrate more...generate more shock...break more carbide.

I wouldn't recommend it for interrupted cuts because of this fact either - as much as you can avoid it at least.

SO for the coolant part...I don't think it is NECESSARY...but chip evacuation is needed so a few air blasts would be nice.

The RPM restriction and rigidity of machines (and expense) is why a lot of people here on the zone will recommend against carbide...you just don't get the added benefit over HSS most of the time. I would at recommend at least getting some "cheap" HSS roughers and just finish with your carbide to make them last a bit longer.

Good luck with that steel!

-Doug

PS - also be aware that a lot of the commercial cutter recommendations are based on an expected tool life of as low as 30 minutes...so take them with a grain of salt. They market to production shops and want people to buy more cutters of course!

[El Ventu]

Take care on stainless, it hardens if you don't cool it during working.
303 contains sulfur than is more simple to work, 304 and 316 aren't so lovely...

[tef9]

Sorry for the late reply, work is a nightmare atm however its holidays now! Thanks so much for the info on stainless as its something I will have to machine at some point, however yesterday I had a bit of a blow as my mill is still having massive vibration problems. If this continues I think I will either have to buy a comercial machine or take up knitting

Still gives me an excusse to ogle kool machine tools. perhaps i will buy a Wabeco after all!

A

[UUU]

Hardening of the stainless is what you need to avoid. So your tools need to cut, not rub.

Try to avoid the tool pausing during a cut - you can feel this effect by hand if you drill some stainless. If you let up on the cutting process for an instant, you get a hard layer in the bottom of the hole. If you're lucky, you can break through it: if not, you break the drill. It will be the same when milling, so keep the right feed rate going - climb mill if you can so the cutter starts with a bite, not a rubbing motion.

[El Ventu]

I have a small benchtop mill (about the same thing of the XJ25, if I'm right) and I work stainless steel without problems.

I worked for seven years as turner and miller in a factory that made a lot of stainless parts (for operating tables for hospitals) and I learned to work the stainless steel to perfection.


On AISI304-316 I use a cutting speed of about 15meters per minute, (for example, for a 8mm drill/mill I use about 600rpm), with a lot of coolant (the cooler are the tool and the material, the little is the hardening of the surface) and I try to use the right feed rate, I try because I have only manual feed.
However, more feed is better than less... :P

There are a lot of kind of stainless steel, the ferritic ones are mor similar to carbon steel to work, and the austenitic-ferritic (duplex) are pratically impossible to work on our little milling machines...

On small machines, and on the austenitic S.S., a sharp tool is more important than a coated or a harder tool.

I have only a few of "special" tools I bought from sellers on eBay selling tools from companies failed or unused tools that they changed for other reasons.

The rest are tools made ​​of HSS-Co, good tools, not cheap Chinese junk which operate for 2 minutes, but not specific tools for steel, light alloys and so on.
I quietly use it on every material, from plastic to aluminum, from carbon steel to stainless steel...

[fragger6662000]

a lot of cutter now recommend not using coolant when cutting steels with carbide as they are using the heat generated to soften the metal and make cutting easier. chips should come off as a straw yellow colour. BF30 is more than capable, but if you are ust to cutting ally you need to check the gibs and settings. multi flute tools are better with high helix angle as more flutes will be in the cut.

[El Ventu]

Benchtop machines can't work with tools that mill stainless without coolant at high speed and feed...

I start from this idea, simply you can't work with that tools, becouse that tools need a lot more stability from the machine.

Then you must use sharp HSS tools, coolant, low cutting speed and the right feed...

[fragger6662000]

i have done this and it does work you need to turn down the depth of cut i have taken 1.5mm DOC in 303 at 200mm/min with no coolant with a 10mm 2 flute carbide cutter on a bf20.

coolant i would avoid lubrication is required.

[El Ventu]

For me milling is an operation like "http://www.youtube.com/watch?v=mS9gSIuHzRI"]this.

You can do the same work divided by 10 times, I prefeer the "old style" with my little mill...

[lcvette]

Those are some nice chips... is that aluminum your milling?

[El Ventu]

Those are some nice chips... is that aluminum your milling?

I've found that video on the web, I haven't machines like that...
In the video they mill AISI316 with the best set up (professional stable machinery and tool).

I worked in a factory that have three Bridgeport CN, I remember that we mill steels like 39NiCrMo3 with Z4 solid carbide mills for high productivity.
I can't remember the brand, but I clearly remember that for an error in the positioning one of those mills started the work in the vice.

The operation was stopped after more than 30mm of milling with a 10mm mill for a depth of about 15mm in the milling vise (hard steel, tempered, the vice comes from Gerardi, 60HRC...), and the tool did not have any problem.

I think if I try to do a similar thing on my benchtop mill I broke the tool in about 0.1 second...