[riabma]

I have done a lot of small holes with the Tormach in aluminum with great results:

Diameter: 1/16"
RPM / Feed: 5100 / 8.3 ipm
Drill Peck: 1/3 of diameter
Tool: Low Helix Carbide
Depth: Up to 1"

Of course, center drilling before...

I hope it helps.

[Spinnetti]

looks like I need to do more research on this.. I have a part I'm doing now with 1/8, 3/16, 3/8 and 1/2 holes, 3/8 deep, flood coolant, no center drill, with one cut each (no peck), using plain ole' black drill bits in collets on my series III. Except for the 1/8, I think I'm running all the bits at 5100 speed and at least 16ipm... (will have to confim).... so far, it zips right through... The 1/8 and 3/16 size are silent when it cuts, though the 1/2" scares me a little and throws chips. The 1/8" I think I'm running about 4100rpm? I have lots to learn though, so this is an interesting discussion... I'm using gwizard to set my starting speeds and feeds, then tweak based on conditions from there. So far, clean holes, on size with no broken bits, though only have run a handful of parts. (seems to match Steve's findings pretty close?)

[Steve Seebold]

I do holes all the time that are .090 to .159 diameter, 4.5 inch minimum depth. I use ONLY Guhring drills. I don't even mess with anything else.

Yeah, Guhring drills are close to double the price of any other drills, but if I can drill 150 1/8 inch holes in the end of a piece of 3/16 aluminum, and not have any break out the side, it's well worth the difference.

I know of other guys who try to do what I do, and they will lose 1 part out of 6 because the hole breaks out the side of the part. The next job I do, I need to drill a .090 hole 4.5 inches deep in the end of a piece of material that is .156 thick.

[tbaker2500]

Thanks for the heads up, Steve. I'm going to need some precise holes soon, I'll try out Guhring. Where do you buy them from?

[BAMCNC.COM]

I must be missing out, I've always just circular interpolated holes, have yet to use a drill bit. Good thread, I'll have to look into those drill bits. Thx

[neilw20]

Observing the shape of the chip explains lots of issues.
Film: Securing tool alignment in non-rotating applications | Drilling

[Steve Seebold]

I must be missing out, I've always just circular interpolated holes, have yet to use a drill bit. Good thread, I'll have to look into those drill bits. Thx

Please explain how you would circular interpolate a .090 diameter hole that is 4.5 inches deep.

[SCzEngrgGroup]

First, you have to find about a 0.060" endmill, 4.5" long. I'd recommend carbide - you'll want all the stiffness you can get.... :-)

Regards,
Ray L.

[beanbag]

I do holes all the time that are .090 to .159 diameter, 4.5 inch minimum depth. I use ONLY Guhring drills. I don't even mess with anything else.

Yeah, Guhring drills are close to double the price of any other drills, but if I can drill 150 1/8 inch holes in the end of a piece of 3/16 aluminum, and not have any break out the side, it's well worth the difference.

I know of other guys who try to do what I do, and they will lose 1 part out of 6 because the hole breaks out the side of the part. The next job I do, I need to drill a .090 hole 4.5 inches deep in the end of a piece of material that is .156 thick.

Care to share your technique, or is that a trade secret?

[BAMCNC.COM]

Please explain how you would circular interpolate a .090 diameter hole that is 4.5 inches deep.

Wow, that's one way to take a compliment I guess...

[Rocco580]

An update on my parabolic drilling experiences.

[waltpermenter]

Wow, that's one way to take a compliment I guess...

you have no answer to his simple question about your dumb suggestion so you try to deflect attention, how old are you?

[Steve Seebold]

Care to share your technique, or is that a trade secret?

No trade secrets here.

First, run spindle at 4000 RPM.

Second, center drill your hole using G83 X?Y?Z?R.025Q.015 (you need a really good center) F6.

Third, use a Guhring Stub Drill (I'll post all the part numbers later today) and drill about 3/4 deep using a peck depth (Q) of 1/2 the diameter of the drill.

Fourth and probably most critical part (what I do anyway). Move to your X Y position, put the drill .100 into the hole, THEN and ONLY then turn the spindle on. If you turn the spindle on outside the hole with a drill that long, it will whip and you will NEVER get it in the hole.

The cycle I use is to drill a .125 hole 4.5 inches deep is:

S4000

G83X?Y?Z-?R-.1Q.0625F6.25

G83X?Y?Zfinish depth R-.1(don't forget to stay R-.1) Q 1/2 the drill diameter F 1/2 the drill diameter (.125 drill = 6.25 IPM, .09 drill would be F4.5).

It's a long slow process, but it has never let me down.

When I drill a .125 hole 4.5 inches deep, it takes 6 to 7 minutes just for the long drill.

When your hole is finished, turn the spindle off BEFORE you pull the drill out of the hole. G0G80M5 then and only then is it OK to pull the drill out of the hole.

It's not hard to do, it's just a very slow process.

You can Google Guhring to find a dealer close to you. MSC has them, but their their prices are crazy.

[neilw20]

Steve is not deflecting attention. He is stopping the drill deflecting !!
This is a sure fire way to learn to do coding and might be a challenge with some CAM programs.
Pilot hole always wins, and notice the peck drilling is not coming all the way out of the hole.

and Steve likes horsing around too..

[Steve Seebold]

drill bits. Thx

Please: DRILLS. A bit is something you put in a horse's mouth.

[beanbag]

Steve:
Why only 4k rpm?
What is the point of using a parabolic drill if you are still only going to take these tiny pecks?

That's an interesting trick regarding not having a spinning drill outside the hole.

[MetalZilla]

You want to try peck drilling with variable peck amounts as you get deeper into the hole. Here is an excellent drill peck calculator for just such a situation: Drill Peck Calculator for Deep Holes!

[SomeWhatLost]

fwiw, circular interpolated drilling, with an actual twist drill never ends well for me...
of course it always starts as inappropriate coding on my part... I never really meant to combine my drill processes...
but anyway, it really doesn't work as well as you think it wouldn't... at least not with small drills... maybe it works better with big ones?

[GJeff]

I think he meant specifically circular interpolating with an end mill. I don't think anyone does anything but straight up and down with drills, but I could be wrong.

[Steve Seebold]

Steve:
Why only 4k rpm?
What is the point of using a parabolic drill if you are still only going to take these tiny pecks?

That's an interesting trick regarding not having a spinning drill outside the hole.

It's something I started with my Haas TM1. It only had a 4000 RPM spindle and it worked really well that way, so I just kept doing it that way. Ya know, "if it ain't broke, don't fix it".

I take short pecks to avoid the drill drifting off. You may try it any way you'd like, but this way works for me.