[mountaindew]

nycnc just did a video recently on a shear-hog facemill single insert cutter, the MRR was impressive. Being a single insert, you can keep your RPMS up where your Tormach is happy, and push it pretty hard.

Shear-Hogs (Shank Style)

- - - Updated - - -

nycnc just did a video recently on a shear-hog facemill single insert cutter, the MRR was impressive. Being a single insert, you can keep your RPMS up where your Tormach is happy, and push it pretty hard.

Shear-Hogs (Shank Style)

That was a nifty demo!
I didn't see what was holding it. If not in a tts holder it adds more steps to set height. He didn't detail this that I seen anyway.
And not something that could go into a atc unless you put that puppy in a tts er32 collet holder.

[tmarks11]

nycnc just did a video recently on a shear-hog facemill single insert cutter

Pretty cool.

And then I went to their website...

Pretty cool, but not $200 cool....

... not something that could go into a atc unless you put that puppy in a tts er32 collet holder.

You can get it with a 3/4" shank, and than use the TTS adaptor that Tormach sells:

32432 - TTS Tool Conversion Kit


I used one of these on a JT3 arbor for my 1/2" Jacob Chuck, since Tormach (for some unknown reason) doesn't sell that size. Worked pretty good. I froze the arbor, heated the ring to 130º, and pressed it together with my shop press.

[dneisler]

On the tormach 4 flute face mill I run mostly 1 to 1.25 WOC and .05 to .075 DOC @ 2500 / 25 IPM and I get really nice results.

[mountaindew]

Pretty cool.

And then I went to their website...

Pretty cool, but not $200 cool....



You can get it with a 3/4" shank, and than use the TTS adaptor that Tormach sells:

32432 - TTS Tool Conversion Kit


I used one of these on a JT3 arbor for my 1/2" Jacob Chuck, since Tormach (for some unknown reason) doesn't sell that size. Worked pretty good. I froze the arbor, heated the ring to 130º, and pressed it together with my shop press.

That's a very cool solution, I never noticed this on their website.

I was thinking same thing pretty expensive , but if you need to machine a lot of material then I would look at such tools. That brings to mind the reason I don't have such high performance tools I made a tool makers vice the other day with half dozen different parts and I can say no way the machine cut 50% of the total material volume he cut in a minute and I made a tool makers vice with custom set of soft jaws even . Don't know how others get material but its not cheap around here and I live by a steel mill .

[tmarks11]

Gwizard:
.125" DOC
1.000" EWOC
1296 RPM
10.262 IPM

I have watched the depth of cut and feed rates people have posted that they got from GWizard, and they look to me like they would work quite well. IF YOU WERE WORKING ON A 20 HORSEPOWER MACHINE

Time to go back to the basics. We don't need a fancy calculator for this:

MRR= W X H X F

W = Width of cut
H = Depth of cut
F = Feed in inches per minute

HP = UHP X MRR

UHP = Unit HP (taken off chart)
MRR = Material Removal Rate

Aluminum .25
Steel 1.4-2.5
Alloys 2.0-3.3

so...

MRR=(0.125" DOC)*(1.000" EWC)*(10.262 IPM) = 1.28 cu in/min
HP = UHP X MRR = 0.25*1.28 = 0.32 HP

What was that you said again, Steve?

ok....now if he was cutting steel, this wouldn't work so well. And his choice of rpm (1300 rpm) does lead one to the natural conclusion he is cutting steel, so I guess I should cut you some slack... he didn't mention Aluminum until after your post, after all.

If this were a 20HP machine, it would be more like 400 ipm (although his choice of rpm and feed rate are less than optimum, and their DOC would be 2x+ his choice).

But, like everyone else said, why are you cutting so slow? Lets do some "classic" calculations:

speed = sfm * 4 / D = 800 * 4 / 1.5 = 2100 rpm
s = 800 fpm for Aluminum with carbide
D = tool diameter = 1.5"

feed = speed * CL * N = (2100 rpm) * (0.005"/tooth) * (3 flutes) = 32 ipm
CL = Chip Load (recommended by facemill manufacturer), lets assume 0.005"/tooth
N = # of flutes (I am guessing3 flutes, but YMMV)

Now lets work the HP formula backwards to find DOC (I based it on 0.75 HP to give you some power in reserve, with 1" WOC)
MRR = HP / UHP = 0.75 HP / 0.25 = 3 cu in/min
DOC = MRR / (W * F) = (3 cu in/min) / (1" * 32 ipm) = 0.0.093"

Same formulas that have been used for years, even before this new-fangled NC thing... Anyone want to post what gWizard says?

If I was just winging it, I probably would have dialed in 3000 rpm, 0.050" DOC, 1/2-2/3 step over per pass, 40 ipm. Increase DOC based upon sound/cutting load.