Recommend a roughing tool for 2.5" bores in 2" A514?

[Garwood]

Through holes will be bored to finish size. What's the best way to rough the holes?

Machine is Kitamura 5X with Big Plus Cat50 35HP. Hi/lo gears 10k max. Through spindle air and TSC, but I'd rather not use TSC because the rotary union needs replacing.

Thoughts?

 

[memphisjed]

annular cutter. punch. burn table (torch, not plasma in this case).

 

[Milland]

Not that much metal, 3/4" roughing endmill, helix down and spiral pocket? Two passes if need be.

Cheap 'n fast...

 

[sfriedberg]

Have you got enough thrust to run a 2+" spade drill?

 

[Philabuster]

I would run a high feed mill and spiral down the hole with your air blast.

 

[dandrummerman21]

High feedmill. A514 is nice to cut with one.

1.25" feedmill, no pilot hole of any kind, spiral down every ~.030"

I'm currently doing 1.75" holes in 321ss at 60ipm with a 1" feedmill. Works great.

I doubt it has enough Z thrust. I tried a 1.75" spade in this 321 job but the Z thrust was peaking out at 200% Z thrust, and the machine it is on (Kitamura hx400if) has dual Z ballscrews! Both Z and W were at ~200% at a measly .010" ipr


Does your kitamura have thru spindle air? Our HX400iF does, I forget the mcode for it. I believe it's M151. I believe M152 was the coolant purge code on our old 3x (which we scrapped) as well as H400, but that doesn't keep the air on for more than a couple seconds.

If you can't use thru spindle air, at least have an external air blast for chips.

I see that you do have thru spindle air. Do that.

 

[Philabuster]

High feedmill. A514 is nice to cut with one.

1.25" feedmill, no pilot hole of any kind, spiral down every ~.030"

I'm currently doing 1.75" holes in 321ss at 60ipm with a 1" feedmill. Works great.

I'm blasting 2.25" diameter by 3" deep holes in 316ss with a 1.25" feed mill spiraling down every .030" and running about .025" feed per tooth on a 2 flute cutter. Not hard on the machine either.

 

[Garwood]

I watched some YouTube videos in high feed mills. Definitely looks like the way! Thanks!

 

[EmGo]

High feedmill. A514 is nice to cut with one.

1.25" feedmill, no pilot hole of any kind, spiral down every ~.030"

I'm currently doing 1.75" holes in 321ss at 60ipm with a 1" feedmill. Works great.

I doubt it has enough Z thrust. I tried a 1.75" spade in this 321 job but the Z thrust was peaking out at 200% Z thrust, and the machine it is on (Kitamura hx400if) has dual Z ballscrews! Both Z and W were at ~200% at a measly .010" ipr

Interesting. I ran a few rough numbers and came out with a traditional machine being a good half minute faster per hole. And that was conservative.

On the other hand, a K&T or Ingersoll or Sundstrand would weigh twice as much, need a hefty foundation, cost a lot more, cost more to run; fixturing would have to be better, part would tend to be stressed more, so ... at least for job shopping, seems like the twinkie machine prancing around is a better deal than the hulk

 

[Garwood]

Interesting. I ran a few rough numbers and came out with a traditional machine being a good half minute faster per hole. And that was conservative.

On the other hand, a K&T or Ingersoll or Sundstrand would weigh twice as much, need a hefty foundation, cost a lot more, cost more to run; fixturing would have to be better, part would tend to be stressed more, so ... at least for job shopping, seems like the twinkie machine prancing around is a better deal than the hulk

This Kitamura's 44x22 travels and just 22k lbs. It's not a behemoth.

The holes in A514 are for a product. Speed isn't as important as process reliability to me.

 

[EmGo]

The holes in A514 are for a product. Speed isn't as important as process reliability to me.

Not complaining, just thought it was interesting. I bet it's something of a tossup when you figure in all the other factors, with the light weight machine maybe (probably ?) coming out cheaper.

But on a lathe, that's a different story

 

[dandrummerman21]

Not complaining, just thought it was interesting. I bet it's something of a tossup when you figure in all the other factors, with the light weight machine maybe (probably ?) coming out cheaper.

But on a lathe, that's a different story

In the case of my 2005 kitamura hx400if, it's a 400mm box way 40 taper HMC, 13k gear driven spindle, might be 20 or 25hp? 30? I don't recall. Has big plus spindle.

But looking at the load meters, Couldn't get close to the type of ipr that 1.75" drill needed. Was ~200% at .010" per rev, but I initially started out at .014 (which is also low) and spiked out at over 250%. Spindle load was ~90%

Not sure what the motors and drives are rated to but the machine was built to go fast and accurate (1968 rapids). And while the machine is stout and the spindle is pretty good down low, I would certainly not call it a powerful machine

And an 5X wouldn't be a lot beefier, if at all (besides having the cat50 spindle taper)



I almost wonder if the z thrust was pushing the tombstone back, causing the carriage to lift and get cocked on the ways, causing a lot more force to be required to slide it forward. It probably contributed to it somewhat.


I will say, I'm going 60 inches per minute, .030" stepdown, 1.75 hole with a 1" tool on that 321 stainless.
So the tool travels 2.35" per lap around. And I take 40 laps down to a depth of 1.2". That's about 94 seconds per hole.





Obviously you would tailor it to whatever feedmill you are going to run, but we run iscar, and my guess to start out at based on my a514 experience would be a 1.25 tool, 4 inserts, maybe 300sfm (900rpm), .025ipt, which would be 90 per minute.

 

[EmGo]

I almost wonder if the z thrust was pushing the tombstone back, causing the carriage to lift and get cocked on the ways, causing a lot more force to be required to slide it forward. It probably contributed to it somewhat.

Ja, just thought comparative numbers were interesting ... seems like the brute machines would be quicker at basic stuff like holes and facing castings, but for any contouring, the light fast mills would be quicker. And of course easier to fixture ....

Seems unfortunate that this approach has carried over to lathes tho - you can spin a 4" milling cutter slow, or a 1" cutter a lot faster, and the result comes out close to the same. And you get better accuracy with lighter machine components for profiling. But if you have an 18" diameter part in the lathe chuck, can't really spin it twice as fast and take smaller cuts

 

[Garwood]

This Kit 5X replaced a Mori MV-65B. That Mori was 38,000 lbs, 30HP and top speed was 4k RPM. Low range tapped out at 1000 RPM. The spindle itself was 3 feet long with 6 bearings. Z ballscrew was 2" diameter fine pitch.

That mill had the grunt to push and turn big old school tools. I miss it, but it was too cumbersome to make small parts on.

Lathes are a totally different story. Beef, HP and gears make things easy that are impossible on modern direct drive/belt drive machines.

 

[Orange Vise]

We use a lot of high feed mills around here. It's going to be your easiest way to get a highly reliable process for the least amount of effort/time.

For a 2.5" bore, I'd use a 1.5" Mitsubishi AJX 3-flute. They have a 4-fluters available with smaller inserts, but IME the beefier inserts always win in both tool life and cycle time. Also I don't like the double-sided feedmill inserts. The economy in the extra insert edges is not worth the degradation in performance.

An even more reliable process would be to use a 2xD indexable drill to punch a 1.5" hole (TSC not required for such a shallow hole), then spiral out with a premium endmill at 2.5-5% stepover. IME (YMMV) you'll get 3-5X more holes before having to swap tools. The thinking behind this is that the drill cuts uninterrupted unlike the feedmill, and solid carbide has a much sharper edge than the feedmill, and all of this is compounded by the fact that the work is being shared by two tools. You'll end up paying more for the tooling and it'll require more effort to dial in (not just cutting parameters but also chip management, which the feedmill excels at), but you'll save in the long run by reducing labor and potential error during the tool swaps. It'll also be easier on the machine... less hammering.

 

[SteveinAZ]

I agree with the insert drill. Generally speaking, drilling is the fastest way to get a hole, and an insert drill has little thrust requirements vs. a spade or standard drill point. Call up your favorite drill rep(s) and make them give/sell you a drill with some sort of performance guarantee, afterall, you have a 50 taper machine, I wouldn't be surprised if you can run a 2.5" drill in that machine, even at the low end of IPR, you'll still have a very stable process. You can also run most insert drills waaaaay faster than recommended sfm to help put heat in the chip and it does help to break the chips, but beware, when they don't break for a bit and are flung against the cabinet walls, it will make a pretty good bang. I actually have one, never had a use for it though, 2.5" diameter with a 2" shank, not even sure who makes it (and didn't do any checking either)...I'd let it go for a song....

Steve

 

[Garwood]

I've drilled a lot of 2" holes in 4140PH in a lathe with an indexable Walter drill. I've crunched inserts in that drill too many times to count. In 1045 it cuts like warm butter. Slams a hole right through 1045. 4140 is a careful balance of keep the SFM low enough for inserts to live, but not too low I stall the spindle. Basically get it all dialed in working fine then it unravels when it hits a slightly harder spot.

I haven't machined much A514, but I feel like it's closer to 4140 than 1045 and drilling a 2"+ hole with or without TSC might not be a walk in the park.

Never tried a feed mill before. I think I'm gonna give that a shot first. I like how the chips look. They look a lot nicer to deal with than 2" long razor blades from an endmill.

 

[Milland]

Never tried a feed mill before. I think I'm gonna give that a shot first. I like how the chips look. They look a lot nicer to deal with than 2" long razor blades from an endmill.

That's why I suggested a roughing endmill, a "corncob", which will give you broken chips rather than razor blades.

OTOH, you could sell the blades to Gillette - business opportunity!

 

[Philabuster]

Found a YouTube video showing a wimpy 40 taper HAAS cutting a 4" diameter hole in 4140 prehard, 2.5" thick using a high feed cutter. Cycle time shown on the video is 2 minutes, 35 seconds. They then increased the feedrate from 200 IPM to 250 IPM per the video commentary.

 

[memphisjed]

Agree with eg here. Going old school is faster. A annuallar cutter at 2 7/16” feeding at 3-4 ipm is a lot less than a minute/hole. These require low power and low thrust.
I recently tried a carbide tipped one- I like it on the mill because there is chip clearance above the tooth.
If a bpc can do a 1.5 hole without flexing your machine should be able to run salesman stated speeds.