Chip load survey

[Thad]

What kind of chip load are you guys using? We typically use a 1" or 2" face mill (Ingersoll or Waukesha) for roughing 3D form or milling 2D pockets. A .010 chip load is about average. That goes for A2 & D2. How does this compare to the way you run your tools? What would you consider a heavy chip load?

 

For those who don't know,

chip load = feed / RPM X number of teeth.

 

Thad

[Paul McGarr]

This is going to be a long thread!

 

From my experiance, .010 is a decent cut for a 1" mill, (I actually average .009) but it just depends on too many things. You can take as much chip as your tooth and holder can handle without fracturing. I've seen .025 on an agressive 2" face mill, but I would not do that on my medium duty machines. Takes some serious horsepower.

 

I would consider .015 heavy...for me...in my shop.

 

Paul

[robk]

We try to stay around .010.. Until trying the Iscar Feed Mill. The damn thing is cutting @ .025 chip load . And according to the rep "this is only the beginning". The material is 420 Stainless (35 RC), and the cutter is 2.5" Dia. 5 flute. The thing is wild going @ 112.ipm with doc of .072. It's in a 40 HP Horizontal machine with a 50 Taper. The spinle load naver got past 40% yet.

 

Rob

[Thad]

quote:

---

I've seen .025 on an agressive 2" face mill, but I would not do that on my medium duty machines.

---

We've consistantly cut a .020 chip with a 4 flute 2" Ingersoll button cutter on all of our machines, including Fadals.

 

Thad

[Keith Graydon]

Let's just put it this way;

 

"I never met a machine that i couldn't stall"

 

really tho, I'm fairly conservative. .005-.015 or so. lighter for small cutters, heavier for larger or LONGER cutters.

[robk]

quote:

---

I never met a machine that i couldn't stall

---

+1

 

Rob

[Keith Graydon]

quote:

---

The thing is wild going @ 112.ipm with doc of .072. It's in a 40 HP Horizontal machine with a 50 Taper

---

HaHa YEAH! I love the sound of chips hissing off a machine

[Paul McGarr]

quote:

---

"I never met a machine that i couldn't stall"

---

I agree. I've also never met a machine that was incapable of friction welding. Well...maybe one.

 

Paul

[robk]

quote:

---

HaHa YEAH! I love the sound of chips hissing off a machine

---

That's the only drawback so far... Too much smoke from the chips hitting the coolant on the bottom of the machine. Today's forecast is pretty foggy

 

Rob

[Müřlıń®]

Chipload...what's dat???

 

J/K....I been wondering how to figure that.

Always just type in a feed and speed and cut it.

Never had a clue what the chipload was.

 

 

Murlin teh chipload retard

[Thad]

quote:

---

Never had a clue what the chipload was.

---

Chip load is the amount of material removed by each tooth.

 

We're in the process of testing new face mills. The recommended chip loads seem a little light (.004-.008) for the tools that are "the leader in the industry." I'm sure that's just salesman talk, but it got me thinking about how we run our tools compared to other shops. I realize there are MANY factors in how you run your tools. I am looking for general replies like I got from Paul and Rob.

 

I thought I'd get a few more responses to this thread.

 

Thad

[Hardmill]

I've used sandvik, ingersol, sumitomo insert

mills as well as a few others. They generally

tend to run in the 400-600sfm, w/ .01-.012

chip load. I've actually pushed some as hard as

.025ipt. It all boils down to the guy running

it. Most operators hear some noise and want to

slow down their feed(BAD OPERATOR), then proceed

to tell you its a piece of junk. I'm a control

freak if you treat these cutters good they'll

do you right back even better in most cases.

Do your homework on your tooling, material,

toolpath and workholding. Its well worth the

time and effort.

 

PEACE

[Ron Branch @ 5th Axis]

So Thad I assume you are running the face mills with postive rake inserts and no coolant. I think you have got good advice from the others as far direction goes. I have used Mil-Tec for years and some people like them some people dont. I have to agree it all has to do with the machine the holder the amount of tool sticking out of the shell mill holder and such. I think you will find if you go to the small chip load that you can increase the surface speed to as much 900 sfm and even though you are not taken the same depth if can sometimes be faster cause you gain it back the speed of the cut verse the depth. It is good to take care of faemills and not beating them to death which also beat your machine to death.

 

Good Luck

 

Crazy Millman

[Müřlıń®]

quote:

---

I am looking for general replies like I got from Paul and Rob.

---

Ok dude here it is....

 

2" future mill using TNMA 438's I think(.125 r).

.125 doc

5" min

4-fl

SS 383

 

Your formula gives me .003....which sounds way light compaired to all you guys.

 

But I am cutting high nickle alloy. I think SFM is around 80....

 

BTW....the reason I use such a stone age tool is that the inserts are 4 bucks a piece and have 6 sides. It will hold up to a heat checked, interrupted, work hardened surface that ranges from 35 to 55 RC.

 

Edit

my bad its a 3 fl

puts it about .005

still way light from what you guys run

Edit

Murlin

 

[ 09-15-2003, 11:11 PM: Message edited by: Murlin ]

[Chris Rizzo]

Ok Ok Ok,

 

You fellas are cuttin' the real stuff (D2,A2,SS,etc.), I'm just playin' with kid's toys now...

 

-Haas

-6061

-Mitsubishi 2.5" 5 flute/insert (ASX445).

-2500 RPM (1600 s.f.m.)

-Stepover @60%

-Chipload .005-.008

-D.O.C. .150

 

 

P.S. A previous shop I turned Waspalloy and Ni-620 forgings all day (and night). THAT was a real man's material!

[Ron Branch @ 5th Axis]

CMR kick that bad boy up to like 2400 sfm with .012 to .02 per tooth feed step-over of 75%. I know the fadal will grunt if I try it but since I keep hearing from the sales guy it is twice the machine of Fadals should be no problem. Let me know how it goes. I am really looking at the VF3 SS for something down the road.

 

Crazy Millman

 

Hey Murlin you ever looked into cermaic inserts from Greenleaf is suppose to be the real deal when it come to that techonolgy. Here is there contact information:

 

 

Greenleaf Corp.

Greenleaf Dr.

Saegertown, PA 16433

Phone: (814) 763-2915

 

[ 09-16-2003, 01:37 AM: Message edited by: Crazy Millman ]

[Fig sign]

One of my favourites Seco bull nose round inserts dia 12mm

25 mm dia 2 inserts end mill F25m insert material with aircoolant molds steel take off 1 mm full diameter cutting s3500 f4500 mm/min and it is 80% of recomendations due to not very strong VMC.

Chip load 4500/3500/2 =0.64mm/rev or 0.025inch/rev.

The spindel load upto 20 % and the inserts time of life is awesome

It roars like a tank but I can do a job in spare minutes comparing to conventional stile of cutting.

 

Iskander teh renegade : love my SECO .

[Müřlıń®]

Mill.....

I try to take it easy on my old machine tool.

It's the only one I will ever have and I wanna make it last till I retire

 

I will check out the ceramics, thanks

 

 

Murlin

[Joe6Pack]

I use a Sandvik 390 2" dia, 5 flute face mill, .180 deep, 60@ stepover, 800 sf, .005" per tooth. (1527 @ 38 ipm) 35% spindle load, on an Akira-Seiki V3XP.

Material is 3/8" A36 P&O plate, laser cut around outside profile.

[McRae]

quote:

---

Do your homework on your tooling, material,

toolpath and workholding. Its well worth the

time and effort.

---

Search for radial and axial chip thinning - this effect will save you money and give you added productivity...

[Chris Rizzo]

+1 Andrew,

 

Most simple feed & speed calc's don't take radial chip thinning into account, and assume over 50% cutter engagement. It is easier to calculate in your head, that's for sure. But doing a finish contour or the like, you need some serious feed rate overrides++++! Some of the better feed and speed calculators figure the REAL chip load out.

 

That would be a great feature for version X !!!