how to hog out a pocket on a steel plate

[Santa Fe]

I allways use inserts for cutting the perifery of the parts and cut lots of chips that way.

My question is if I want to hog out a large pocket say 20" x 20" and 1.5" deep on a plate and I want to use an insert cutter, then what recomendations you guys can give me about plunge, RPM, IPM depth of cut, etc. or what ever you guys think is important to consider.

[cobra95kev]

If it is a closed pocket I would use either a Mitsubishi or Iscar 2.0" feedmill.

 

About 300sfm .040fpt and .040 to .06 depth of cut.

I have found feedmills rock if it is a closed pocket and you can keep the tool fully engaged.

 

Plunge at about 60%feed.

 

[Dowty123]

Feed mill is the way to go, other then inserts, there is 'variable helix' end mills (guhring serie 3114, destiny raptor DVH) that are pretty surprising, 1XD depth of cuts 'high speed pocketing method' with trochoidal off. For speed, I'd need to know what kind of steel it is.HTH!

 

Simon

[Redfire427]

Feedmills all the way. I have used both Iscar and Seco. Seco is unbelievable. Great tool life and not too abusive to the machine tool. Iscar seemed a little too aggresive to the machine tool for my liking.

On a 3/4 dia. Seco, we run 4000rpm .020 depth of cut and 350 ipm feed with a 50% stepover. I know they recommend a larger stepover but my experience has shown if you use a larger stepover, Mastercam leaves too many upstands in the floor for safe machining on the next depth cut.

[MotorCityMinion]

Cobra, .04 FPT? Seriously?

 

Prosin, 350 IPM? What material?

 

Both numbers are impressive, assuming were talking about mild steel, for tool steels, those numbers are amazing.

[J Coulston]

 

[gcode]

quote:

---

.04 FPT? Seriously?

---

seriously

We run 2in Mitsubishi feed mills at

1030 rpm, 84ipm and .055 DOC in mild steel.

Insert life is nearly forever.

The tools could go another 30/40% faster

but our but HBM's can't go that fast

accurately

[Thad]

quote:

---

.04 FPT? Seriously?

---

Dijet Feed Mills can do about .125 per tooth (so they advertise).

 

Search the forum for Feed Mill and you'll see what others have been able to do with them.

 

Thad

[sharles]

We use the mitsubishi high feed (feedmill) cutters. The first time we used it we all about died it was going so fast (compared to what we used to use). The thing is we've found they go just as fast in the harder steels as they do the milder steels. Definitely check them out.

[MultiAxGod]

Just like there's no substitue for cubic inches, there's no substitute for insert drills.

Use a large (depending in corner radius size) dia. insert drill (thru the spindle coolant if you have it) and drill the holes as close as possible to each other (don't know if mcam has a drill roughing routine or not, sorry). Then knock the stand offs and walls down with any good shell mill. Very quick, very efficient. Much faster than milling.

[robk]

This brings back memories. I have done a lot of work using feed mills in the past. We have done testing for Iscar when they were developing their feed mills for US release (ended up using Mitsubishi in the shop) They are the best thing since sliced bread for the right application. I don't use them anymore since most of my parts are nickel, waspalloy, inconel, etc...

Do not pre-drill your corners, roll the cutter around corners, ramp down @ 60%, and machine the pocket from outside-in.

Here is a link from 3 years ago with some cool testimonials Link

[Guest]

JCoulston.

 

Can that be done on a HAAS?

 

[gcode]

feed mill + Hass = Corvette for the service guy

[Redfire427]

Quote:

Prosin, 350 IPM? What material?

 

Both numbers are impressive, assuming were talking about mild steel, for tool steels, those numbers are amazing.

 

Reply:

We do this in H13, P20, Mild steel or anything else you can throw at it. Seco recommends up to .060 per tooth feed. It draws a crowd at the machine every time we run it. We even had a guy videotape it to send to a guy who works at another shop that thought we were full of sh--.

Don't forget, you have to have the right machine to accomplish this with a high speed control. The Makino's excel in these arenas. Forget old school methods, this is the future, now.

[Thad]

Rob, that's the topic I remembered too.

 

Thad

[Dave Ball]

I use SECO feedmills from 1.5" to 4" diameters for ruff facing, pocketing and they are great for helical boring large diameter holes, no start hole and fast as heck. A 4" feedmill runs at 750 SFM and .04 IPT with a .04 DOC in 1020 steel, it should go alot faster but my Mori aint got what it takes.

[Gary]

We a vf5 and cut 18 x 18 pockets in 4140ph plate and the mits rocks. I can only push a 7/8 to 1 inch tool though with machine because of the no balls factor. .035 deep 95ipm pocket outside in and I get a very reliable 3hrs of insert edge life. Feed mills outlast 90° cutters by a long shot

[TR Mfg.]

We use the Mitsibishi AJX feedmills

1" dia, 2100rpm, 80ipm, .03doc in 4340 plate, 38rc. We could go faster but it is as fast as the 1981 Hitachi Seiki can go. Insert life is messured in days.

[gms1]

Same here on the mitsubishi ajx mills. .05 doc .05 ipt for the 2inch diameter. We use the mitsubishi bxd mills on aluminum. I cant break that damn thing. Last test we ran on our okuma 56va was @ 14000 rpm and something like 350 ipm with .25 doc

[MotorCityMinion]

GMS1, I worked @ Metric right up the street from you. Also worked with Tom Nevel at 2 other shops in the past. The shop I'm currently at just got some of the Mitsubishi mills to try out on some Rex tools steels and the guys were adamant about running traditional speeds and feeds on a Tree mill. (Chickens). They never tried the 90 IPM like the rep said to start out at. I have access to a Makino S series VMC but no decent e-mill holders to use it with. Mostly shrink fit. Maybe I can talk them into buying some new holders for the Makino for a project I'm working on now.

 

http://www.emastercam.com/ubb/ultimatebb.p...ic;f=1;t=029938

 

How's business there?

[Torr Man]

Go to www.edgecam.com they have a free program that you can download. It requires you to draw the pocket in dwg or dxf. Once you have done this it will recommend which cutters to use and at what speed and feed. It was developed by some employee who did his doctorial thesis on this subject

[Teh Bear without Brains kinda idiot]

i WOULD USE Seco or Dijet

I prefer Dijet over Iscar -> much faster

I used Dijet 52 mm dia round inserts dia 16mm

S1400rpm f4000 mm/min on steels like armour steels.

Cooling air .

Great results

[Thad]

quote:

---

GMS1, I worked @ Metric right up the street from you.

---

Metric Punch in Taylor? I worked at Walt Industries on Delta in 1994.

 

Thad

[MotorCityMinion]

Yup, that's the one, Universal Dr.. 7 years there. Walt Industries, didn't they make some Harley parts for awhile? I applied there once, never heard back from them. I think there dead now though. That whole industrial complex is looking grim.

[Thad]

quote:

---

Walt Industries, didn't they make some Harley parts for awhile?

---

Harley parts is all they made when I was there. They closed shop some time ago. I don't remember exactly when. The last time I drove through there, there were a lot of vacant buildings. IIRC, even the Watson Engineering buildings (5 of them?) were empty.

 

Thad