What speeds and feeds for 3/8" 6-flute, 1018, trochoidal, in a 30-taper VMC?

[Finegrain]

I don't do a lot of big metal removal of steel in my 30-taper VMC, but I have a job coming up that will have me removing a couple hundred #'s of mild steel. I'm planning on using 3/8" x 1" LOC 6-flute YG-1 variable-index endmills. Axial DOC is ~3/4".

I have in the past used 8% stepover, 600 SFM (6,000 RPM), and ~200 IPM (.006"/flute with chip thinning). YG-1 recommends 1,000 SFM (10,000 RPM) and 340 IPM, at 5% stepover. YG-1's parameters are about 10% higher MRR.

What do you guys go with, for a 3/8" 6-flute EM in mild steel?

Thanks, and regards.

Mike

 

[cornerRad]

1018 is so soft you can push it really hard. The limiting factor is going to be horsepower and spindle connection of a 30 taper?

Is it a big plus spindle and holder?

 

[Finegrain]

Is it a big plus spindle and holder?

No, standard 16k spindle, 5 kW continuous.

Regards.

Mike

 

[MaxPrairie]

That's probably a good starting point. I typically do 10% step over on steel, but I use 4 flute on 3/8 and under, 5 flute on 1/2 and larger as my roughers.

 

[Nerdlinger]

That’s about where Im at with my 3/8” SGS em’s in 4140 x something like 5/8” deep. ~650SFM x 8%. Depending on how wide your slot is you may be leaving more than you think for a finish pass so adjust program accordingly. I Mastercammed leaving .005” on the walls of a .568” wode slot but with it going so fast with those little circles ot was really leaving like .020”! Good luck!

 

[BROTHERFRANK]

I've had better success roughing with 4 or 5 flute end mills in steel and other tougher materials on 30 taper. They like less flutes in the cut simultaneously. I think the higher flute counts are ok for very light finishing passes and will allow higher finishing feed rates due to the extra flutes...

 

[Wsurfer]

I don't do a lot of big metal removal of steel in my 30-taper VMC, but I have a job coming up that will have me removing a couple hundred #'s of mild steel. I'm planning on using 3/8" x 1" LOC 6-flute YG-1 variable-index endmills. Axial DOC is ~3/4".

I have in the past used 8% stepover, 600 SFM (6,000 RPM), and ~200 IPM (.006"/flute with chip thinning). YG-1 recommends 1,000 SFM (10,000 RPM) and 340 IPM, at 5% stepover. YG-1's parameters are about 10% higher MRR.

What do you guys go with, for a 3/8" 6-flute EM in mild steel?

Thanks, and regards.

Mike

FWIW,
I use the same end mill with nACRO coating. My max spindle speed is 10K, 5% stepover 400 IPM with air blast.
I use HSMadvisor which has worked well with my speedio. Held in a Maritool stubby side lock holder. I don't do production, so can't say on tool life in 1018. I did use the same tool(new) in 304 SS and got > 6 hours in the cut. 4670 rpm 110 ipm, .475 adoc, 5% rdoc with flood cooling. First time I ran a tool till failure. Got loud for 40 seconds or so before going POP.

 

[Finegrain]

Update ...

Running the job starting today. I have ~200# of steel to remove. Let's see how it goes

3/8" 6-flute YG-1 V7 Plus variable index
600 SFM (6,000 RPM)
200 IPM
8% stepover

Regards.

Mike

 

[Orange Vise]

3/8" 6-flute YG-1 V7 Plus variable index
600 SFM (6,000 RPM)
200 IPM
8% stepover

What's your axial DOC?

 

[Finegrain]

What's your axial DOC?

It varies over the part, but max .70"

 

[Finegrain]

Changing to 300 IPM and 6% engagement. Sounds better that way, more buzz and less growl.

 

[VTM]

I just got some tooling quoted for virtually the same application, but 5/16 cutters at 1" doc. But this is for a 40 Taper machine.
These are the speeds and feeds the sales guy recommended to me.

Walter MA377.7.93A4L038J-WJ30EM 5/16" EM, 4flt, .015" rad, 1" loc 1018 Steel HEM Toolpath .040" radial, full axial 7200rpm 78ipm high end of recommended info IMCO 9175644 M936 5/16 6F SQ POW-R-FEED Mill 5/16 x 5/16 x 1-1/4 x 3 1018 Steel HEM Toolpath .030" radial, full axial 10500rpm 183ipm high end of recommended info

 

[Finegrain]

YG-1 recommends ~1,000 SFM for their V7 Plus, but I'm not up there yet. Here's where I'm at right now:

800 SFM (8,150 RPM)
330 IPM
.023" radial
.70" axial

Still a 3/8" x 1" LOC 6-flute. Sounds fine. I'll have to wait and see what the tool life looks like.

Regards.

Mike

 

[Philabuster]

Try going to a 4 or 5 flute cutter and max out the SFM. 6 flute endmills on soft materials like 1018 tend to pack the flutes so you are limited on radial DOC. You are basically stuck taking a whole bunch of tiny finish passes.

 

[zero_divide]

FSWizard's numbers aren't that far off from manufacturer's suggestions.

That's assuming you chuck it at 1" stick-out.
Not sure how a 30 taper spindle would like that, though.

Running it with just the air blast is the way to go.

 

[Orange Vise]

YG-1 recommends ~1,000 SFM for their V7 Plus, but I'm not up there yet. Here's where I'm at right now:

800 SFM (8,150 RPM)
330 IPM
.023" radial
.70" axial

Still a 3/8" x 1" LOC 6-flute. Sounds fine. I'll have to wait and see what the tool life looks like.

Regards.

Mike

When the SFMs start getting up there, there's more trial and error involved in dodging the harmonics. You're doing it right by working your way up and going by sound.

6-flutes on a 3/8" is pretty dense. I'd venture a guess that you could achieve those same parameters or better with a 5-flute and get overall better tool life due to lower vibration. Variable pitch endmills work better with lower flute counts because the irregular flute spacing is more pronounced.

It's a myth that high flute counts work better because they have larger core diameters. While that's partially true, I can grind a 2-flute with a huge core. I just have to add a 3rd or 4th relief behind the cutting edge. Most cutters only have a primary and secondary. Also, when cutters get too dense, you end up with multiple flutes engaged in the workpiece at the same time, which adds vibration.

Since your axial is .700, the ideal cutter would have .750 flute length. Anything longer reduces rigidity. Happy to send you something to try out if this job repeats.

Any chip handling issues on this job?

 

[CarbideBob]

. Also, when cutters get too dense, you end up with multiple flutes engaged in the workpiece at the same time, which adds vibration.

Is this two teeth in the cut bad a bad thing?
Helix angle and .700 deep.
For sure there is a no mans land with doing such cutting.
Often we only look at the tip and ignore what is happening up near the top of the cut at the same time.

 

[BROTHERFRANK]

FSWizard's numbers aren't that far off from manufacturer's suggestions.

That's assuming you chuck it at 1" stick-out.
Not sure how a 30 taper spindle would like that, though.

Running it with just the air blast is the way to go.

Brother 30 Taper no problem!
This is 15-5 H900 with 3/8" 5 flute 1" Axial depth:

 

[Finegrain]

Since your axial is .700, the ideal cutter would have .750 flute length. Anything longer reduces rigidity. Happy to send you something to try out if this job repeats.

Thanks! I'll keep you in mind if the job repeats or something similar comes along.

Regards.

Mike

 

[Finegrain]

Any chip handling issues on this job?

Yup. Most of the chips knitted together up on the enclosure surfaces instead of getting down into the discharge troughs, even with the chip wash running full time. Had to coax them along every few parts.

I'm curious about using a serrated rougher in steel, like Frank's AlTiN rougher. I've had great success using his serrated ZrN roughers in Al. Anyone having success with serrated roughers in steel?

Regards.

Mike