Feed Mills

[Avarillas]

I chewed up a 1.0 dia feed mill (iscar)

after I ran 8 17-4ph 11"x4"x4" blocks I was runing my tool like usual:

328 grade insert

1500 rpm

80. ipm

.050 max z steps

all of the sudden boom the pockets on the tool and the inserts flew away everywhere!!I went holly wacamole!!!! what happened? so I thought

maybe some of you guys might have some experience

with this kind of tool, or would recomend better

settings.

 

 

thanks.

 

(by the way it was scary to see pieces of the tool body flying everywhere!!)

 

[Tom Szelag]

That's nuts. I'm low man on the totem pole. I don't know crap, but 80IPM at 1500RPM seems high.

[Psychomill]

A few 'need to knows' first. Which mill were you actually using? 2 or 3 flute? We're you running dry (hopefully)? with or without air blast? What type of cutting,... facing, pocket, deep pocket, contour? horizontal or vertical? How were the chips looking? Any heat in the part? Any excessive heat in the tool? How were the inserts wearing? Was the material heat treated in any way? Whats your radial DOC?

 

I know this seems like "20 questions" but I'm just trying to give you some ideas to look into and something might come to you. I have this happen twice before. Interestingly enough, both times with Iscar. First time had problems with recutting chips in a deep pocket. I moved the part to a horizontal. Second time, my only guess was something was going on with the material. We had it normalized but I kept running into gummy areas. Tool heat would jump and then chip sticking and then... I switched it to a Sandvik 390 with a tougher grade and made it through the run but it ate alot of inserts for lunch. That job is back to running the Iscar with no problems since. Your feed and speed doesn't sound too out of wack... but then again, I don't have all the details.

 

HTH

[Mike Whitten CAD/CAM Contractors]

I have all of the same questions as Psyco.

 

But..

quote:

---

after I ran 8 17-4ph 11"x4"x4" blocks

---

How many minutes of feed time was this? Maybe the insert wasn't changed in time. Also, the feed seems heavy unless it was a light profile cut. In which case I would calculate the chip thickness etc.

 

Is there a way you can sink the tool deeper? .050 is not enough..

 

Mike

[Mike Whitten CAD/CAM Contractors]

Edit/

 

Armando,

 

I did a little studying on this subject and found that I was unaware of the constuction and usage of the feedmill. So..I take back what I said about the depth of cut and feedrate. These feedmills are new to me. I did not expect such a thing.

 

I will study some more about this.

 

Thanks,

Mike

 

[ 03-26-2005, 01:51 AM: Message edited by: Michael Whitten ]

[Storkman]

Feeds and speeds are actually low. You can run up to .137 chip per tooth with an Iscar feed mill.(I prefer .1 to .125) Max step down is I believe .078. try 908 grade inserts and 400 sfm.

[robk]

Storkman, Iscar feed mill is pretty impressive, but very unpredictable. We ran it here for a while with pretty good results. You're running it way too slow. The faster the better. We have also tested the feed mill from Ingersoll and it was a little better and safer than Iscar.

If you want speed and feed along with a warranty on the body of the cutter you need to get yourself a Mitsubishi AJX. A lot less vibration, a lot more predictable, inserts are cheaper, and if you break a body they will give you a new one for free. Check out this link. AJX

On the bottom of the page is a PDF file along with a video.

[MichaelJ]

are they for gust steel or will they cut allum. to

[robk]

All we're cutting is 400 grade stainless with it. Not sure if it's recommended for aluminum. I'm at home and for whatever reason I can't open the .pdf here (my wife's pc). Just to let you know though with the Iscar the operator had to stand next to the control in case something happened, but with the Mits. we're doing lights out machining and that's a pretty comfortable feeling.

[MichaelJ]

Ill have to look at them at work Monday

[Quickmike]

The AJX Rocks. Can't go wrong for roughing. They are scary at first, but they remove material fast. We have 2 2inch, 3 1.5inch, and 2 1inch of these things. I alsso like Mitsu's MBN ball end mill cutters for finishing or semi roughing. I think the free replacement policy is good for all of their indexable endmills.

[robk]

Also Psychomill mentioned Sandvik's 390 series at the top of this thread. It is a very popular cutter from them, but FYI we just swiched to Mitsubishi's APX series. The body is a little cheaper than Sandvik's (pricewise ), but the inserts are about $4.00+ less per piece from Mits. and last @ least twice as long with their VP15TF coating. And as always that warranty applies to all of Mitsubishi's inserted end mills... No I'm not their spokesman, but I'm a good client

Michael, I think that CMR does some aluminum work and he always mentiones Mitsubishi's AQX line. Maybe he'll chime in here.

[MichaelJ]

the Mits. rep was at the shop 2 weeks ago and didnt talk about them. we gust looked at the end mills.

[Storkman]

quote:

---

Storkman, Iscar feed mill is pretty impressive, but very unpredictable.

---

I agree rob, vibration causes Iscar's locking screw to loosen. And when they go you certainly can't stop them. I have heard good things about Mitsubishi. But the guy who orders cutters and bodys here seems to be married to the Iscar rep.

I have asked several times to check into the mitsubishi, but no luck. Maybe after he reads this thread it will sink in.

 

As for cutting aluminum, I don't know either. Be awful hard to get enough feed. In 400 series, a 3" feedmill will run almost 300 ipm.

[Tom Szelag]

.137 IPT?! Jeeeez.

[Chris Rizzo]

I've just been a bystander on this thread while you guys were talking bout the tuff stuff

 

MichaelJ, I'm not a fan of the carbide Mitsu endmills.. Too much $$$ and too many other good and readily available products out there for e.m.'s. However Mitsu' really shines with the insert mills. Maybe your rep has something else in mind pertaining to your application, but you should take a look at them. Hell, make him give you a demo cutter. With the replacement policy too, you really can't go wrong. It's a great incentive to really try and get the most out of the cutter, if it breaks, they'll give you a new one regardless.

 

We had a Iscar plunge mill that I ran on some cast iron a while back, and it did lack a certain "robustness". The insert seemed to cut very well, but the body and shank was nothing great. I usually find when using the mitsu cutter that the weak link is in the setup rigidity or machine H.P., seldom run into a problem or limitation with the cutter. Even when I run into stuff, literally .

 

For just about every cutter now they offer the hti10 insert, for AL. Max RPM (12K) and I feed it until I run out of H.P., or spit parts out of the fixture....1" & 1.5" AQX em, 2.5" & 3.00" ASX face mill

hth

[Storkman]

quote:

---

.137 IPT?! Jeeeez.

---

Tom, I found it hard to believe when they told me. To this day it still don't look right, a cutter spinning at 572 rpms and moving at 286 ipm. But it does work.

[Mike Whitten CAD/CAM Contractors]

OK,

 

You guys have taught me something! I have to get an AJX!

 

About Five years ago I was running a lot of 316 Prodec type stainless. As you guys know this stuff cuts like butter. You can really fly with indexable tools. We used Ingersoll 12J1-B's and Mil-tec face mills back then.

 

So..I do not have a whole lot of experience milling the standard type of 304/316 with indexable tools. I find myself just using coated fine pitch hog mills as most of the jobs I do nowadays are small anyhow.

 

So, the question is will the AJX mill normal nasty 316 SST fairly reliably?

 

Thanks,

Mike

[Thad]

quote:

---

a cutter spinning at 572 rpms and moving at 286 ipm.

---

It has 3.65 flutes?

 

Feed = RPM X # of flutes X chip load

286 = 572 X # of flutes X .137

286 = 78.364 X # of flutes

3.65 flutes

 

Thad teh Did you hear about the mathematician with hemorrhoids? He worked it out with a pencil.

[Storkman]

Thad, I use 3" feedmills 450sfm 5 flutes x .1cpt

[Tom Szelag]

So what exactly do you use these feed mills for? What kind of materials? It must cause a tremendous amount of wear on the spindle and consume plenty of horsepower. That's hoggin out a LOT of material. That's like gettin in there and hogging it out with a chisel!

[Chris Rizzo]

The depth of cut is relativly shallow, so it's not like a cutter buried in a part feeding at that rate. The general philosophy behind those feed-mills is light d.o.c., heavy f.p.t...

 

Lots of cutting motion and passes at high feeds, vs. slowly bury the cutter with one-pass and eat horsepower. I like to use that general stragedy (light fast cuts) for roughting on machines lacking h.p.. Mastercam's highfeed is great for that, along with paying close attention to your toolpaths- trying for smoooooth motion.

 

At least that's how I utilize the principal, don't want to speak for everyone's application and findings.

[thoskins]

WE use up to 4" feed mills here and we love them. There is a serious learning curve when it comes to using them. We also have an 8" that uses the round feedmill style inserts. Let me tell ya you need an umbrella made of steel to be around this thing when it runs. We can only use it for facing though. The round insert does not allow for pocketing. And before you ask we are running it on a 120HP toshiba floor mill.

[SLJ]

We've got a 1.5" Iscar doing 1273RPM and 153IPM in 15-5PH at .05deep on a 40 taper vertical. Works pretty well except the contour is on and off the part, so the heat isn't constant. So far it's the best process we've found for this part.

[Müřlıń®]

Type of steel you are cutting will greatly affect your settings. We cut high nickle alloy.

 

We have tried Iscar, Ingersol and a few others.

 

The max depth for the 2" Iscar is .05 and you must keep an eye on it.

 

The 1" should be run @ .03 depth of cut. If you look at the insert design, .05 on the 1" inserts puts the cut up on the secondary corner radius instead on the larger primary radius. Keep the cut below the secondary radius.

 

We like Ingersol the best because of the thicker center webb. The 2" 4-fl is a massive metal removal tool IMO..... 100 IPM @ .05 DOC 650 RPM...will run for hours at a time without fear of self destructing.....