Allied Spade Drill

[EmGo]

Our main customer is a gear house lol. We'll never be cutting gear teeth.

What ? you don't want to bite the hand that feeds you ? What are you, sensible or something ?

Yeah 12" deep for a 2" indexable won't be cheap.
Sandvik's DS-20 line for 2" drills only goes to about 10" cutting length.
But for 6061 they recommend 907sfpm (1730rpm) and .0061 IPR for a 10" deep hole taking 57 seconds per hole.
Not too shabby, but is the $1100 list price tag worth it?

So it wouldn't pay for itself ... at $60/hr, as I remember, the hole was good for about 5 minutes, so over 100 parts I'd have saved 400 minutes, say 7 hours, would have been $420 cheaper but cost $1200 (CA tax is 10%).

There's still a place for ye olde spade drille

 

[gregormarwick]

...

I'm just going to let you have this one, because I really don't care enough to rehash it all over again.

Congrats

 

[EmGo]

I'm just going to let you have this one, because I really don't care enough to rehash it all over again.

Congrats

Right. You wanted numbers, I bothered to look some up, you're wrong so you run away, as usual.

Congrats

 

[gregormarwick]

Right. You wanted numbers, I bothered to look some up, you're wrong so you run away, as usual.

Congrats

So it goes, at least I got you to do some mental exercise

 

[70olds]

Well duh, a thousand pieces

(btw, want to buy a hobber ? then you could do teeth, too !)

But okay, here's another place where the spade wins : had a bunch of aluminum parts, got a 2" hole about 12" deep. With a spade drill I was already close to maxing the machine out, do they even make good inserts for aluminum drilling ? And if they did, what would it give me ? Couldn't push the machine any faster, so what do I get for a bunch more expense ?

I think you really have to take this stuff on a case by case basis.

Couldn't push the machine any faster in what sense? RPM? Feed rate? Reach?

 

[EmGo]

Couldn't push the machine any faster in what sense? RPM? Feed rate? Reach?

RPM and horsepower .... 12" chuck, lathe top speed was 2000 but the blanks were 6 1/2" diameter and that's getting right up there for that big a chuck and jaws, jacked up the feed until the needle was well into the red ... I might have pushed a little harder but sometimes good enough is good enough

Was an SMW air chuck, too, which I don't trust as much as hydraulic.

 

[mmurray70]

Yes but then you'd have that drill body for other jobs and it would pay for itself in no time.
Not to mention that 50-100 pc job would get done a lot faster and you could be running a different job in the meantime.

The difference is not as much as you think sometimes. Lets say a batch of 100 parts with a 1" hole 2" deep in mild steel. 200" total to drill. And lets say a shop rate of $100/hr

Allied recommends 290 SFM in mild steel and 0.018 IPR. Works out to 19.9 IPM. Total of 10.1 min to run, $16.75 of shop time.

Sandviks calculator for a 870 drill in steel recommends 498 SFM and 0.0155 IPR. Works out to 29.5 IPM. Total of 6.8 min to run, $11.30 of shop time.

Thats a savings of 3 minutes or $5.45 of faster run time on the entire job. Hardly worth the investment of an expensive carbide drill in many cases.

 

[gregormarwick]

The difference is not as much as you think sometimes. Lets say a batch of 100 parts with a 1" hole 2" deep in mild steel. 200" total to drill. And lets say a shop rate of $100/hr

Allied recommends 290 SFM in mild steel and 0.018 IPR. Works out to 19.9 IPM. Total of 10.1 min to run, $16.75 of shop time.

Sandviks calculator for a 870 drill in steel recommends 498 SFM and 0.0155 IPR. Works out to 29.5 IPM. Total of 6.8 min to run, $11.30 of shop time.

Thats a savings of 3 minutes or $5.45 of faster run time on the entire job. Hardly worth the investment of an expensive carbide drill in many cases.

In your example you have to consider that those numbers are much more likely to be realistically achievable with the 870 than they are with the Allied.

Oranges to oranges in some basic free cutting mild steel (125Bn free cutting steel selected on the Allied calculator, 070M20 on Sandvik), thrust is more than double for the allied at approximately the same penetration rate:

870 surface speed: 120m/min - 394sfm
Gen2TA super cobalt: 84m/min - 275sfm

870 feed rate: 470mm/min - 18.5ipm
Gen2TA super cobalt: 447mm/m - 17.62ipm

870 thrust: 3850N - 865.5lb
Gen2TA super cobalt: 7971N - 1792lb

870 thrust with your cutting data: 4480N - 1007lb

 

[Rogue_Machinist]

In your example you have to consider that those numbers are much more likely to be realistically achievable with the 870 than they are with the Allied.

Oranges to oranges in some basic free cutting mild steel (125Bn free cutting steel selected on the Allied calculator, 070M20 on Sandvik), thrust is more than double for the allied at approximately the same penetration rate:

870 surface speed: 120m/min - 394sfm
Gen2TA super cobalt: 84m/min - 275sfm

870 feed rate: 470mm/min - 18.5ipm
Gen2TA super cobalt: 447mm/m - 17.62ipm

870 thrust: 3850N - 865.5lb
Gen2TA super cobalt: 7971N - 1792lb

870 thrust with your cutting data: 4480N - 1007lb

So im thinking about doing a peck. I know the drill isnt meant to be pecked. But it will limit the strain on the servo. But im thinking of doing a g73 where the drill never leaves the hole. But Its been years since I had to program one. I dont remember the values and all the examples refer to machine values which I dont have access to. So

 

[Mtndew]

Allied recommends 290 SFM in mild steel and 0.018 IPR. Works out to 19.9 IPM. Total of 10.1 min to run, $16.75 of shop time.

You're not getting that feed rate on your typical cnc lathe with a spade drill. No frickin way. You will get servo overload alarms.

 

[EmGo]

You're not getting that feed rate on your typical cnc lathe with a spade drill. No frickin way. You will get servo overload alarms.

Let's just use Mr Marwick's figures - max -

"Gen2TA super cobalt: 7971N - 1792 lb"

here's the numbers pulled out of an old American Tool brochure ... Hustler, their earliest nc lathe, flatbed, basically a Pacemaker with a control : 3 ranges 30 to 3000, only 12,000 lbs mass, 10" swing, 54" centers, front spindle bearing rating 17,680 lbs, z axis thrust 4,000 lbs.

50% load on z axis should manage these holes no problemo.

Ten years later cincinnati compact chucker, also 10" machine, 25,000 lbs mass and 40 hp mtd rated and 10,000 lbs thrust.

Gimme a real lathe and we'll make quick work of them holes.

If'n I wuz doing metal-removal kind of work ? It shore as hell wouldn't be on nuthin' modern.

 

[mmurray70]

You're not getting that feed rate on your typical cnc lathe with a spade drill. No frickin way. You will get servo overload alarms.

Maybe its an issue on some lathes. But even my shitty haas lathe would do that no problem on a 1" drill. Honestly I dont always push them to the limit like that. I ran a 1.343 allied a while ago on the Haas at 0.013 feed in steel and it was like 70% load in Z (out of 200%) so still had a bit of room too go.

Even if you slowed the allied feed down to work with a specific machine. Say it takes twice as long as an 870 drill. You still get the job done and it only takes 6.8 minutes longer, and costs $11 more shop time for the full job I mentioned above. Still lots of times the allied drills get it done with better economics. They are worth having around IMO for sure.

 

[gregormarwick]

Maybe its an issue on some lathes. But even my shitty haas lathe would do that no problem on a 1" drill. Honestly I dont always push them to the limit like that. I ran a 1.343 allied a while ago on the Haas at 0.013 feed in steel and it was like 70% load in Z (out of 200%) so still had a bit of room too go.

Even if you slowed the allied feed down to work with a specific machine. Say it takes twice as long as an 870 drill. You still get the job done and it only takes 6.8 minutes longer, and costs $11 more shop time for the full job I mentioned above. Still lots of times the allied drills get it done with better economics. They are worth having around IMO for sure.

Which Haas?

For sure my Victor would not care about that 1" drill either, but 1" is a small drill in there when I am regularly running 100mm insert drills in that machine. My 10" chuck Doosan that I used to have would have been less happy about it though.

 

[mmurray70]

Which Haas?

For sure my Victor would not care about that 1" drill either, but 1" is a small drill in there when I am regularly running 100mm insert drills in that machine. My 10" chuck Doosan that I used to have would have been less happy about it though.

SL30. Its a 10" chuck machine, but it cuts like an 8" lol.

 

[Ox]

So im thinking about doing a peck. I know the drill isnt meant to be pecked. But it will limit the strain on the servo. But im thinking of doing a g73 where the drill never leaves the hole. But Its been years since I had to program one. I dont remember the values and all the examples refer to machine values which I dont have access to. So

Good grief, you have asked that multiple times already.
You could have:

G1 Z-.75
W.1
Z-1.5
W.1
Z-2.25

....or one of many other options in the time that it took you to post the question the first time!
It is one hole in a lathe for Petey's sakes!

Would someone please learn how to hand code for once?!


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

Think Snow Eh!
Ox

 

[Rogue_Machinist]

Good grief, you have asked that multiple times already.
You could have:

G1 Z-.75
W.1
Z-1.5
W.1
Z-2.25

....or one of many other options in the time that it took you to post the question the first time!
It is one hole in a lathe for Petey's sakes!

Would someone please learn how to hand code for once?!


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

Think Snow Eh!
Ox

Relax my man, I got it done. Hand programming I know, I unfortunately do far more of it than id like. I came from a shop where the programs were all canned cycles. I got her done.

 

[wheelieking71]

Good grief, you have asked that multiple times already.
You could have:

G1 Z-.75
W.1
Z-1.5
W.1
Z-2.25

....or one of many other options in the time that it took you to post the question the first time!
It is one hole in a lathe for Petey's sakes!

Would someone please learn how to hand code for once?!


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

Think Snow Eh!
Ox

I can't finger-CAM profitably. Made too many mistakes in the past. Gun-shy? (among many other relavent reasons)
But, I can edit the hell out of some generated code I don't like! Thats for dang sure.

 

[Rogue_Machinist]

I can't finger-CAM profitably. Made too many mistakes in the past. Gun-shy? (among many other relavent reasons)
But, I can edit the hell out of some generated code I don't like! Thats for dang sure.

And this is the thing. I would say in the U.S. especially right now most shops dont hire machinist. They are hiring Operators with little actual skill. So much so that I get about 30-50 ads a day looking for "Machinists" but in the job description its basically has knowledge of G and M code and can make changes at Control. Canned cycles are for the most part significantly easier. Change a few values,youre done. Most of these jobs ask for set up experience. I can long hand program 90% of the stuff im working on but for some things like complex contours and such its just so much easier to draw in CAM and have it generate the code.

 

[EmGo]

I can't finger-CAM profitably.

On a lathe, wheelie ? You gots to be kidding. It's a pickanick. And you should be able to figger a few holes on a mill by hand, too

 

[wheelieking71]

On a lathe, wheelie ? You gots to be kidding. It's a pickanick. And you should be able to figger a few holes on a mill by hand, too

Ohh, I know. I can do simple 2X lathe stuff well enough. But, here are just a few of the reasons why I never got real proficient at finger-CAM:
I first started programming in '05. I was the lathe guy (set-up operate, there was 1 CNC lathe, pictured below). There was another guy doing all the programming.
He quit with short notice. Owner knew my work ethic. And when he turned me loose he simply told me "Figure it out. If you get stuck come get me (he was actually really good, just spread too thin). No matter what save your work. I don't want an NC file. I want a MasterSCAM part file". He didn't save any NC files, always posted from the last saved part file. This made a lot of sense to me. And I still operate this way to this day. He was extremely patient while I learned. Helped me a ton. And he knew I was 100% engaged to learn this new skill. It was my big break that I had been busting my ass to find for well over 10 years. But the fact remains. We always worked from the part file. Not the last posted G-code. That is just how I learned. And it stuck. Now I have been using FeatureCAM for over 16 years. I'm pretty decent with it, LOL. As fast as a guy can create geometry and curves in F-CAM? There is no way anybody is going to finger bang code and make chips before I can program and post. Maybe on the simplest of parts? I don't know. It would have to be pretty dang simple for me to bet against myself. And no matter what, I always have that master part file to look at. Hard to envision a complex part just reading code compared to opening a CAM file. I'm not saying I never do it. My lathe doesnt rigid-tap. So I have a generic cycle I finger banged to cheat it with a floating holder. And pulling bar, again, generic cycle, fill in the blanks. But if you hand me a print? Finger-CAM is simply not an option.