HSS Turbo Mills Vs Insertable End Mills

[Don K]

This question is being posted to help resolve an issue in our machine shop.

 

Material: 6061-T6 Aluminum

We are running a pocket routine over a 5 inch length and roughly 2 inches wide.

This is a square aluminum billet being held in a vise.

 

Which tool would be better to use?

A HSS Turbo End Mill or an indexable insert cutter?

Which would be the best machining practice?

We are running this on a Haas with a 12,000 rpm max spindle speed.

 

I definetly would appreciate all input on this.

[gcode]

quote:

---

5 inch length and roughly 2 inches wide.

---

how deep??

[Don K]

quote:

---

how deep??

---

Roughly, 1-3/4 inches.

[mold100]

A pocket this small I actually use a 3 flute garr alumstar 1/2 inch dia 9000 rpms, 120 ipm at .2 DOC.

[iowajim62]

corner radius size ?

3/4 insert cutter for rough

3/8-1/2 carbide endmill for finish

[gcode]

Ø1.25 Iscar insert mill at 10K and 120/150 ipm

I'd use a profile cut set to spiral ramp @.200-.250 DOC

Its been a while since I ran a Haas.. this might be a little hot for 40 taper Haas, but it will rough your pocket in under a minute

[Robert Bell]

3/4 Dia. YG-1 Speed Freak 3 flute T-15 Powder Coated HS .06 Corner Rad. .005 -.007 per tooth.

My machine is 7500 rpm and I run 6000 @ 75 IPM .4 stepover .5 deep contouring. A little less depth for pocket maybe. I get great life contouring, bit less pocketing.

book says 10k rpm @ 200 IPM

 

I finish with solid carb

 

Hope this helps

[Don K]

I've been told that the turbo style cutter induces a lot of force on the spindle components such as the bearings, motor etc.

 

Any input on that?

[gms1]

We would run that cut with a 1" mitsubishi bxd mill 13000rpm 380ipm 1/4 doc on our Okuma 56va 40 taper.

 

Another thing to note for comparison purposes is you have to send the carbide mill out for regrind and when it gets back you have to deal with compensation for the tool. If you do any kind of 3D work with it after its been ground, good luck. The insert mill you pop in new inserts or turn the insert and away you go. And you can ramp heavier (18 degrees for the bxd) and plunge up to .200 depth. I'm not the tool order guy but I'd imagine the inserts are cheaper then the regrind especially if it has variable pitch flutes on it.

 

edit:: Forgot to add that with the Mitsubishi cutter you get a limited amount of warranty replacement cutters. You break it, send it back for a new one no questions asked. Each cutter is warrantied.

[Don K]

quote:

---

We would run that cut with a 1" mitsubishi bxd mill 13000rpm 380ipm 1/4 doc on our Okuma 56va 40 taper.

 

Another thing to note for comparison purposes is you have to send the carbide mill out for regrind and when it gets back you have to deal with compensation for the tool. If you do any kind of 3D work with it after its been ground, good luck. The insert mill you pop in new inserts or turn the insert and away you go. And you can ramp heavier (18 degrees for the bxd) and plunge up to .200 depth. I'm not the tool order guy but I'd imagine the inserts are cheaper then the regrind especially if it has variable pitch flutes on it.

 

edit:: Forgot to add that with the Mitsubishi cutter you get a limited amount of warranty replacement cutters. You break it, send it back for a new one no questions asked. Each cutter is warrantied.

---

This Mitsubishi cutter is the same exact cutter that I am using. There is a pissing match going on between the operators on the different shifts.

 

I ordered this Mitsubishi cutter to replace the older style turbo cutter which I used in the 80's. In my humble opinion there are far too many choices now in the insert technology not to be using the inserts. My tooling rep is the one who told me that the insertable cutter bodies cut more free and create less wear and tear on the equipment. Plus the benefits that you mentioned in your post.

 

I agree with all of this.

 

One other thing regarding the regrinds. You lose a tremendous amount of tool life regrinding tools. Probably near 50% of a new cutter maybe more.

[gms1]

I agree with the tool life. Removing material in aluminum like that is an easy choice for us with that cutter. That feed and speed isn't all that tool can do either. We run it there because we get good insert life at the rate on that machine. We have run it at 500 ipm we just didn't get the tool life we wanted.

The only down side I could see was the fact that you can't finish walls with it if it was a requirement.

[Don K]

quote:

---

gms1

Member

Member # 471

 

posted 09-26-2008 10:45 AM

--------------------------------------------------------------------------------

I agree with the tool life. Removing material in aluminum like that is an easy choice for us with that cutter. That feed and speed isn't all that tool can do either. We run it there because we get good insert life at the rate on that machine. We have run it at 500 ipm we just didn't get the tool life we wanted.

The only down side I could see was the fact that you can't finish walls with it if it was a requirement.

 

--------------------

Mastercam X3

Mill 3

Solids

---

It isnt a requirement. I am merely roughing with it and finishing with a solid carbide cutter.

 

Thanks for you input.