Brother Speedio 16k spindle question

[bosmos_j]

I would try two drills, one 18mm or whatever, then another at 30. You can subtract out the power required for the 18 on the second drill and you might be there. I've done this on a couple parts. Chips can get long so I'd pause for chip breaks and pilot can't be too big or second drill will want to get pulled in. I've had that issue doing it on a manual machine, but have not had that issue on a CNC.

Dallas Yamazen apps guy told me he will red line the load meter on turnkey jobs for drills for what that's worth. I believe that was over brochure numbers, but job needs to be worth the risk.

 

[Orange Vise]

Since 30mm drilling is out, drill thru at 18mm and spiral out with a 1/2" endmill at full depth. I think it'll be faster than using a high feed mill for the 1" thick material you've described.

 

[TAIWA NUMBA WAAN]

Since 30mm drilling is out, drill thru at 18mm and spiral out with a 1/2" endmill at full depth. I think it'll be faster than using a high feed mill for the 1" thick material you've described.

This needs some serious air blast at the right angle to blow the needle chips out, otherwise you're gonna get what looks like a ball of thick steel wool volcano.

I didn't know S45/1045 steel could be pyrophoric but I just found out today.

 

[Finegrain]

This needs some serious air blast at the right angle to blow the needle chips out, otherwise you're gonna get what looks like a ball of thick steel wool volcano.

I didn't know S45/1045 steel could be pyrophoric but I just found out today.

They're thru holes, so hopefully OP can keep some airspace below the part to allow the chips to flush thru.

Regards.

Mike

 

[Mtndew]

They're thru holes, so hopefully OP can keep some airspace below the part to allow the chips to flush thru.

Regards.

Mike

Yeah there is plenty of space between the part and the vise for chips to be flushed out. I'm looking at a coolant thru bullnose end mill. This will allow me to bypass the drill and the finishing end mill, saving almost 1:30 in cycle time.

 

[gkoenig]

Yeah there is plenty of space between the part and the vise for chips to be flushed out. I'm looking at a coolant thru bullnose end mill. This will allow me to bypass the drill and the finishing end mill, saving almost 1:30 in cycle time.

I would definitely use a chip-breaking end mill on the major material removal, so you'll still need a finisher for the final pass.

 

[Matt@RFR]

I've been drilling .734" diameter 1" Deep in 1018 with a Walter insert drill on my 16k spindle. I absolultely would not want to go any bigger. I can't even push it hard enough to break the chips. I mean maybe I could but I've no desire to fuck around and find out. 5/8" and under is far more comfortable I'd say.

Pretty much my experience on our 16k spindles.
16mm (.630") Titex through coolant drill in 4140, 300 SFM (1819 RPM), started at the suggested .015" IPR and immediately stalled the spindle. Worked it down to .0045" IPR to get it reliable, but then had to start pecking because it wouldn't break chips.

That was a miserable experience.

 

[Pete Deal]

This needs some serious air blast at the right angle to blow the needle chips out, otherwise you're gonna get what looks like a ball of thick steel wool volcano.

I didn't know S45/1045 steel could be pyrophoric but I just found out today.

A rougher wouldn’t make needle chips and would flush nicely with coolant.

 

[Fal Grunt]

My recipe for shallow holes has been to pilot drill to approximately 1/2", and use a 3/8" 7fl chip breaker. 15% step over, full length of cut, 800 sfm, .0018 cpt. Using my inside diameter calculator, with a 1" diameter, that would bump the feed from 102ipm down to 64ipm.

7 Flute Baboon ChimpBreakers (inch) | Gorilla Mill

Based in Milwaukee, WI – Gorilla Mill has over 30 years experience manufacturing the best carbide drills, end mills and cutting tools in the industry.

gorillamill.com

I have found the tool calculators for these to be very conservative. IE, I made a left hand turn 100% width and 100% depth of cut with a 3/8" 1.25 LOC through a part at the above numbers, and the cutter lived for about an inch before it died, and I honestly believe it died, not because of the cut, but because the part started to come out of the vise.

 

[Micmac1]

IF you end up going the high feed index route, our haas mini mill 10k spindle loves the kyocera 3/4" raptor feed. worked more than surprisingly well for us and inserts lasted forever.