milling 4140

[Miksak]

Hey guys, I need to mill a small part (about 4"X4"X2") out of 4140... The problem is i cant remove material at any speed without disastrous results...

Here is what I am running
A 1995 HAAS VF-4 (15 Horsepower, High Torque, Max Spindle RPM 7500)
BobCAD/CAM V24
1/2" Dia. Z-CARB Endmill (solid carbide, variable rake, variable helix, AiTin coating)
4140 steel (I think its in annealed condition)

Currently I have my settings at:
.030" DOC
1300 RPM
6 IPM
and it sounds horrible...

I have a lot of material to remove and at this rate I think its going to take over 6 hrs per part, and I think I am rapidly killing my tooling...

Any Suggestions? any help is greatly appreciated.

Thanks,
Mike

[fizzissist]

1/8 DOC, 2300rpm, 16IPM (based on 4fl, .002/tooth), no more than 3/4dia's engagement, and climb cutting.

I think this is being conservative.

[BobWarfield]

Some thoughts:

4140 will work harden to a degree, and you've got real low chipload on that cut. fizzissist is right to kick up the feedrate, and you probably want a little more depth of cut too for same reason. I like his 1/8" number.

While you suspect it is annealed, it gets quite a bit harder if it isn't. For example, annealed is 187 Brinell but hot rolled is 280.

1/8" DOC, full slot, annealed and G-Wizard recommends 1700 rpm and 18 IPM feedrate to rough it.

1/8" DOC, full slot, hot rolled and it changes to 1600 rpm @ 17 IPM.

Assuming we don't have to full slot, let's cut back the width of cut to minimize engagement and let those flutes cool for more of a revolution--0.165 stepover is 1/3 of a diameter engagement. We'll get a little benefit from radial chip thinning too. Meanwhile, let's bump up the depth of cut.

Now for the hot rolled, G-Wizard suggests 2000 rpm and 16 IPM. Not a lot different, but the material removal rate is 1.297 instead of the 0.2557 from 0.030" DOC and full slot. At that stepover, you can run a ton of depth of cut if you can use it. I don't know enough about your job to play with the parameters much more.

Cheers,

BW

[Miksak]

Thanks alot guys! I will try it first thing tomorrow morning.

I can definitely benefit from a greater depth of cut, the job (probably more suited for a lathe, unavailable) is a hub for a pump pulley (to adapt a strain transducer to an existing outer pulley, automotive development stuff) and entails machining (from square stock) a circular profile 3.654" O.D. 2" deep and a bore 2.825" I.D. 1.5" deep with a bolt pattern at the center...

As far the condition (hot rolled, cold rolled, annealed etc.) is there an easy way to test? we have a Louis Smalls hardness tester for Rockwell scale hardness testing, I am not real familiar with Brinell but my guess is its somewhere in the low 30s HRC from the way it responds to the inferior tooling that I first tried...

You say not to exceed 75% engagement but is there a lower limit too? Was I being far too conservative? because I had only like 5% engagement previously...

Well anyway I am optimistic to try the settings you suggest and I will report back how it works out...

Thanks again!

Mike

[DareBee]

I make very little change in programming between cold rolled and 4140 (ann or HT).
Just give'r man.

[fizzissist]

...You didn't mention how long the cutter is.. You'll want that as stubby as you can get away with to keep that chip load up.

the 75% is an upper limit..obviously different parameters if you're doing a channel, and then it's a serious DOC issue, but still a function of diameter.

In looking at specs for my cutters, I'm seeing 300sfm as the high limit for 4140, so I'd probably dial it back to around 225 for openers, but increase the chip load to .003 /tooth...BUT....
What does SGS say????????

pg 3
http://www.sgstool.com/products/zcar...ROCHURE_LR.pdf

There's yer parameters...right from the horse's mouth. If it won't do that, then get your money back. And I mean it. Get your money back. Period.

Personally, I don't care for SGS. Maybe just me, but I broke an SGS early on in a grooving op and replaced it with a Dataflute. Ran the rest of the job with that single Dataflute. Same exact parameters. Ran rings around the SGS.

Maybe they're better now. They should be.

[Geof]

...and entails machining (from square stock) an circular profile 3.654" O.D. 2" deep and an bore 2.825" I.D. 1.5" deep....

Why are you using a 1/2"cutter, you are not space limited?

You could be using a larger cutter (for instance a 5/8" TiAlN coated five flute high helix), taking a much larger depth of cut (maybe 0.70") with an engagement of about 15% of the cutter diameter and feeding at around 0.01" per tooth. At 300sfm, which is feasible on 4140, you would be running at around 2000rpm, which is right near the top of the torque curve for your machine, with a feed of 100ipm and a powerful air blast, no coolant!!!. Your toolpath should be configured as a continuous spiral in from a diameter that just touches the original corners of the stock.

The hole is not so easy to do fast because it is more difficult to clear chips. Start with a drilled hole about 7/8" diameter then with the same cutter spiral out using a 0.5" depth of cut but with the engagement cut back to 10% of cutter diameter and possibly reduce the feed to 0.007" per tooth. Same sfm and again rig up a powerful air blast directed into the hole to get the chips out. (The reason for cutting back on engagement and chipload is to get a thinner chip because you will get some recutting.)

For machining something like this my choice would be a mill rather than a lathe. Chewing the corners off a square block to make it round is a ***** of a job and with 4140 the intermittent cut is murder on the tool.

[Miksak]

Thanks again for all the help.

Geof, the only reason I am using the 1/2" endmill as opposed to something larger is the price... $90 w/ our discount vs. $200+ for the larger Z-Carbs... (I have only been running CNC for 5 months, and when I break tools its usually due to a miscalculation, not wear or trying to achieve faster speeds thus smaller tools keep my idiot tax lower)

However I have been looking into trying some endmills manufactured by GARR Tool they advertise the same performance and cost 30% less...

Well I took your suggestions and settled on the following settings:

1600 RPM
209 SFM
.0025 APT
.125" DOC
.1875" stepover

And it works brilliantly! this increased the speed the project was moving at exponentially. Best of all, I am still on the same tool (I burned one up early on, probably due to work hardening)...

I am currently using flood coolant, is that the right choice? is an air blast better?

I have a lot to learn, I am going to look into getting GWizard...

Thanks again,

Mike

[Geof]

I agree there is quite a pucker factor when you ram a $200 tool into the work using the conditions I outlined.

If you use flood coolant with coated carbides, especially TiAlN coating, you are wasting money, you might just as well use uncoated. Particularly with TiAlN which depends on the chip temperature getting up quite close to red heat to correctly activate the properties of the coating. With TiAlN and an airblast you can get the chips coming off dull red and the workpiece and cutter stay relatively cool, cool enough to briefly touch the tool. This why an air blast works: It cools the tool a little during the non-cutting part of a revolution but does not chill the cutting area or cutting edge causing thermal shock and chipping. It also clears the chips away. It is likely your tool 'burnt out' not due to work hardening but micro-chipping at the cutting edge from thermal shock. When you cut slowly the cutting edge gets very hot in the cutting zone and then gets quenched when it hits the coolant.

I would still be tempted to modify the conditions you are using. Take the speed up to about 2500 rpm, increase the feed per tooth to 0.005", take the depth of cut to 0.25" (maybe even 0.30") and take the stepover back to about 0.05" (possibly a bit more). With air blast of course. This could boost your metal removal rate another 50% or more.

[Miksak]

Geof,

I increased the RPM, Decreased the stepover to .050" and increased the DOC to .250" and maintained the same APT...

so far so good, a little louder but a lot faster...

I guess this stuff isnt as simple as it would appear... I will do more research and possibly install some sort of air gun...

Mike

[Geof]

....I guess this stuff isnt as simple as it would appear... I will do more research and possibly install some sort of air gun...Mike

Yes get the air setup. With modern tool coatings fast material removal has changed greatly from what it was a few years ago. Have a look at this thread; http://www.cnczone.com/forums/haas_m...B_you_can.html I convinced myself only a couple of years ago that it was possible to do things that were unheard of when I was younger.

[RICHARD ZASTROW]

Make sure your air gun is capable of doing what Geof described. Blast the chips away, not gently blow air at them. Re-cutting air hardened 4140 chips can be detrimental to cutting tool health.LOL

Dick Z