High speed drilling

[lwells]

Running X3 with a new mori seiki nh6300. Drilling 8 .669 dia. holes 8" through 1020 h.r. steel. Simple bolt pattern. Just dropped some change on a guhring 17 mm solid carbide coolant through profile drill,9" flute. Plan to run in a r32 collet holder.Flange coolant though equiped with a chip blaster. 1000 psi I believe. I'm an old school bar guy so this should be interesting.I usually run drills between 50-100 sf. Would really like to see what my new baby can do. 8x8=64 holes. Thanks. Love the forum.

[Jack Neelands™]

lets see ...30 seconds for 3.5 inches...hmmm......best guess

 

 

1 min 20 seconds for 8 inches

 

the tool should pay for itself in machine time saved

[Leigh @ Kodiak]

Personally I would ask the tool supplier for their recommendations, that way if the tool goes boom on the first hole, you may have some recourse to get a replacement.

 

One rule of thumb I do go by when highspeed drilling is feed at 65% for the first %65 of the drill diameter.

 

Just for reference, we recently finished a job in mild steel where we used a solid carbide drill. No thru coolant though. We actually ran the tool dry, as per Kennametal's reccomendation (yea, it blew my mind to.) The holes were thru 1.5", and we ran at 1650 RPM, initial feed of 14 IPM, then a full feed of 21.5 IPM. We managed to do over 2500 holes before the drill needed replacing.

[mike_f]

Solid carbide, thru tool in 1020..you are close to 12x dia. to depth...I don't know which Guhring series drill you have but you should be somewhere around 300 - 350 SFM, but at 12x D you should probably be starting those holes with a shorter drill...+1000 for getting recomendation from your supplier, that's not a cheap drill.

have fun.

[Steve Hattori]

Definitely set it up to use that chip blaster- it'll be worth it!

[bm1983]

we use guhring drills up 1.5'' dia. make sure you get the reccomendations for speeds and feeds for the type of material from your local guhring rep. They are not very forgiving, and the inserts arent cheap!

[Guest CNC Apps Guy 1]

For 16x diameter and above I use a pilot hole .0005 larger than the drill about and 1.5-2x diameter deep. I turn on the spindle and flood coolant @ 500 rpm, feed from about .05 above the top at about 1-2 IPM. Once at 1x diameter deep I turn on the high pressure coolant and dwell for 2 seconds. Then I turn up the RPM to 25% of reccommended speed dwell for 2 seconds then 50% for 2 seconds then 100% for 2 seconds and go at it to full depth. Once at the bottom I dwell for 1 second turn the speed down to 500 RPM and pull out and stop.for materials that work harden, I'll come up .010 before turning down to 500RPM. I've used this method with 100% success in aluminum, steels, and exotics. If the hole is not blind, I shut off the high pressure coolant at the bottom of the hole before pulling out.the reason I go to 500 rpm is so the tool does not whip. I've done this with 50x diameter gun drill on an HMC and the drill was .09 dia.

 

HTH

[mike_f]

I appologize for the hijack here but I'm curious. I would pretty much handle a 16x D the same way James, with minor variations depending on many things. Do you have custom drill cycles to handle this ?..if so, would you mind sharing a sample of how you accomplish it ? I can fumble my way through a post but I haven't even tried to set up any custome drill cycles. I'm not exactly sure how to go about it. again, sorry for the hijack.

mike

[Johnny M]

Just Ran a .250 carbide drill coolant thru.

6061 Aluminum

Pilot hole .252 .100 deep

44 ipm,4900rpm straight feed thru 4 inch block

 

140 holes no prob.

 

as per instuctions by dealer.

Titex Prototyp drill

 

Cost $250 Canadian

[Guest CNC Apps Guy 1]

quote:

---

...Do you have custom drill cycles to handle this?...

---

No need to apologize for the hijack, it's pertinent. Anyways I have not created a custom cycle for this yet. I think it would be possible because there are enough custom parameters available to do it. It's just having the time to do it.

[Tim Johnson]

We run our 1/4" coolant thru carbide at 8878rpm, 101.458ipm in 2024 alum. (mitsubishi)

[lwells]

Dealer recomends 275 sf .012 ipr. which gives me abought 1570 rpm at 18.84 ipm . Reduce feed by 30% 2xD. Sound doable? I'm gonna let er rip.

[Jack Neelands™]

sounds about right actually...our .875 drill does about 1800 rpm at 22 inches a min....

 

ummm make sure you are out of the way of the chips....they come off like bullets.

[lwells]

Thanks guys.