[Advil]

Need some advise from those who have come before me. I've been having fine luck on my 770 with aluminum and titanium and even some 1018 mild steel but I'm working with making some 2" 4140 parts out of typical annealed 4140.

Tried 3/16 4 flute, 3/16 5 flute and 5/16 5 flute, all tialn coated.

I havn't found a DOC much above .010 that doesn't just high pitch scream with chatter and leave patterns when the cutter engages. HSM routinely tells me I can take a .32"+ DOC, but obviously more DOC doesn't help chatter. What's odd is that even a finishing pass at .3 is no good. DOC as little as .09 still chatters. I'm working with HSMAdvisor and GWizard and I can 'make' cuts with proper chip load and they may even make a decent looking chip I just can't do it without unbearable screaming chatter.

I've clamped the stock in my 5 inch vise securely with parallels and currently have it clamped hard with Mitee Bite Talon Grips.

What kind of recipes or end mills should I be using for this stuff?

Other things I've tried: I've checked my lost motion in all axis and it's still the same as my inspection report (roughly .0004 in x and y and about .001 in Z). Any chance that isn't enough of the story and I need to dig into the gibs and preload? I've also got the tool holders marked to line up with the spindle to minimize runout. These tools that I'm trying to make work are all checking to .0004 runout or better at the flutes.

[IMT]

*Check out NYCCNC videos on 4140 and Lakeshore Carbide's variable flute EMs. I've used the 1/4" 4 flute for lots of alloy steel parts (4130, 4140, 4340) as well as 17-4 and 15-5 stainless.
*Check your XY and Z gibs. I prefer the method of loosening the gib until there is slop, measure lost motion, tighten the gib a little, measure lost motion again. Repeat until the lost motion increases by around .001, back off a little.
*You have to use HSM tool paths in tough materials on these machines. Large DOC and small WOC. Also have to consider chip thinning when calculating the feed rate and what happens to the WOC and chip thickness on inside corners. The low depth of cut approach won't work for long, at .010 DOC the bottom .010 is doing all the cutting so it wears out really quick while the rest of the tool remains untouched.

The machine can do it but it has to be adjusted and maintained properly and the tool paths/feeds+speeds have to be spot on, just not a lot of wiggle room.

[nitewatchman]

Need some advise from those who have come before me. I've been having fine luck on my 770 with aluminum and titanium and even some 1018 mild steel but I'm working with making some 2" 4140 parts out of typical annealed 4140.

Tried 3/16 4 flute, 3/16 5 flute and 5/16 5 flute, all tialn coated.

I havn't found a DOC much above .010 that doesn't just high pitch scream with chatter and leave patterns when the cutter engages. HSM routinely tells me I can take a .32"+ DOC, but obviously more DOC doesn't help chatter. What's odd is that even a finishing pass at .3 is no good. DOC as little as .09 still chatters. I'm working with HSMAdvisor and GWizard and I can 'make' cuts with proper chip load and they may even make a decent looking chip I just can't do it without unbearable screaming chatter.

I've clamped the stock in my 5 inch vise securely with parallels and currently have it clamped hard with Mitee Bite Talon Grips.

What kind of recipes or end mills should I be using for this stuff?

Other things I've tried: I've checked my lost motion in all axis and it's still the same as my inspection report (roughly .0004 in x and y and about .001 in Z). Any chance that isn't enough of the story and I need to dig into the gibs and preload? I've also got the tool holders marked to line up with the spindle to minimize runout. These tools that I'm trying to make work are all checking to .0004 runout or better at the flutes.

Try a 2 flute EM.

[skrubol]

What width of cuts have you tried?
Is it possible the steel is mislabeled and actually hardened?

[Advil]

What width of cuts have you tried?
Is it possible the steel is mislabeled and actually hardened?

Quite a few WOC. Tried chip thinning .014 and also normal
Stepovers and feeds up to about .1

I just finished spending the afternoon doing the full adjustment on the x and y gibs. They're now a little tighter than the factory had it but still following tormachs guidelines. No change at all sadly. A bit frustrating.

Tested a piece with my shop file. The file would cut it fairly easy, but hard 4140 is what... 40-44 HRC? So I'd need a tester file set to be absolutely sure.

I'll try making a different part tomorrow out of a different metal just to save my sanity and make sure nothing else is up. I've got titanium feeds and speeds that cut up to .375 deep on adaptive paths and are smooth and quiet.

[Steve Seebold]

What’s your width of cut and your depth of cut?

It looks to me like you’re trying to remove too much material.

[popspipes]

My 4140 experience is limited, but I do know it will harden if your not careful, otherwise it cuts like leaded steel. I face the ends of small 1/2" tubes with a carbide cutter, get it a bit too hot and it will harden, carbide will still cut it but it will have shiny hard spots in it.

[Advil]

The plot thickens. I finished setting the Z axis gib. No change. But then I decided to do something I would normally never ever do. I ran the cut conventional direction. Perfect. So I started working up toward the full recommendation of HSMAdvisor. To my shock, pass after pass it sounded perfect and hogged through material in the conventional direction. Any time I tried climb, screaming.

Here's the last cut I took. This was more than adequate with a 3/16 and it tore through it effortlessly:
NOTE: I have 4140PH chosen instead of 4140 annealed just in case my material isn't what I think it is.

Material: 4140PH Alloy Steel 300 HB
Tool: 0.188 in 5FL Carbide TiAlN Solid End Mill
Speed: 324.0 f/min / 6603.8RPM
Feed: 0.0019 in 0.0097in/rev 64.26 in/min
Chip Thickness: 0.0010 in
Reference Chip load: 0.0010 in
Engagement: DOC=0.33 in WOC=0.01 in
Effective Dia: 0.188 in
Cross Section: 0.12 x Dia.
Power: 0.2HP
MRR: 0.27 in³
Torque: 0.19 ft-lb
Max Torque: 0.42 ft-lb
Cutting Force: 24.8 lb
Deflection: 0.0028 in
Max Deflection: 0.00667 in

So how about some more ideas why I can only do this conventional? Loose ballscrew or preload nuts? Machine just can't climb in steel?

EDIT:
I just punched the HSM toolpath and ran the hottest path I would let it calculate for my machine 10,000RPM and 97 inches per minute!!! It cut like butter. Still conventional direction:
Material: 4140PH Alloy Steel 300 HB
Tool: 0.188 in 5FL Carbide TiAlN Solid End Mill
Speed: 490.6 f/min / 10000.0RPM
Feed: 0.0019 in 0.0097in/rev 97.30 in/min
Chip Thickness: 0.0010 in
Reference Chip load: 0.0010 in
Engagement: DOC=0.33 in WOC=0.01 in
Effective Dia: 0.188 in
Cross Section: 0.12 x Dia.
Power: 0.4HP
MRR: 0.42 in³
Torque: 0.19 ft-lb
Max Torque: 0.42 ft-lb
Cutting Force: 24.8 lb
Deflection: 0.0028 in
Max Deflection: 0.00667 in

[skrubol]

Your deflection is higher than your chipload. I've never used one of those calculators before, so I don't know if that's normal, but that seems high/problematic. What's your stickout on these endmills?

[Advil]

I calculated it with a lot more stickout than I had. Calculated with 1in. Just checked actual stickout: .53". Deflection recalculated at correct stickout I'm at .0005. Just fine. The higher deflection number was still considered well within max deflection limits for roughing. I was using numbers that would keep things super conservative while I worked out the issues.

But the question remains, why do all cuts work conventional and none work until I get down to 1000RPM and under in climb?

[skrubol]

What range of chip loads had you tried with climb? You mentioned .1 feed earlier, but I assume that's a typo or units I'm unfamiliar with.

[Advil]

Chip loads (IPT) from .0007 up to about .002. That's pretty much the limit for either the 3/16 or the 5/16. IPT seems to have no effect at all.

FYI - I finished the prototype part using conventional milling. I may want to make more so still going to need to sort out this steel chatter problem.

Still hoping for someone with a specific tool and speed/feed doc/woc. I may have to break down and get whatever Lakeshore end mill was used in the NYC CNC video. What's needed here is a known good starting point.

[jwatte]

If you measure backlash and tighten your ballscrew nuts, I'd be very interested in hearing about the outcome!
If you don't, well, at least you have a cut that works :-)

[Bob La Londe]

I am curious to know what you learn. One of the reasons I decided to buy my 1100 was to cut 4140HT whenever I am having issues with my aging KMB1. Given that its about 35 years old that is more often than it used to be.

P.S. I actually found HT and QT to cut nicer than annealed.