What's new
What's new
By:
Advanced search…

5/16 drill in 304 stainless

D

Dugtelal

Plastic
Joined
Aug 15, 2017
Have to drill twelve 1.75" deep holes using a 2 flute cobalt drill and I just keep breaking drills can't seem to find a good speed feed combo have tried 270 at 4 ipm 600 at 4 ipm all pecking at .150 with coolant I have turned the feed down I have turned it up I am at the end of my rope here any suggestions would be greatly appreciated.
 
Which specific drills are you using? Canned peck drilling or written out to avoid jamming the drill on reentry? Coolant rich enough?

And sometime the SS we get is crap, is yours from a reputable mill or anonymous?
 
HSS twist drill with Titanium Nitride coating,140 degrees, coolant is good, steel is nuclear grade so no problems there.
 
Dugtelal said:
HSS twist drill with Titanium Nitride coating,140 degrees, coolant is good, steel is nuclear grade so no problems there.
Click to expand...
Mystery make or known brand? Split point?
How many holes or inches on average before it breaks?
 
You should be around 45 sfm (about 550 rpm). A good quality drill with TiN coat and good coolant and you may be able to go up a bit on speed.
IPR should be around .0033...about 1.8-2.0 ipm.
These are the parameters I use in 316SS on a multi-spindle screw machine for HSS drills.
 
Milland said:
Which specific drills are you using? Canned peck drilling or written out to avoid jamming the drill on reentry?
Click to expand...

I find the biggest problem isn't the re-entry, its the pulling out.. When I'm dealing with crappy work hardening
material, I'll long hand it and feed out .010 or .020" before pulling out. Cuts the chips off clean. If I only
have a few holes to do, I'll just turn the rapids WAY down. Those chips are HARD and NASTY, you want to cut them
off clean, not try and rip them off, because occasionally you end up ripping the cutting edges off
the drill instead of ripping the chips off the part.

Slower retract(fast feed, or slower rapids) and entry gives everything a second or 2 to cool
back down before you start cutting again.

On the cooling everything down between pecks. Years ago, running a 1-5/16 drill in the lathe, going 9
inches deep or so.. Twisty drill.. By the time we got down to about 6 or 7 inches everything was
SMOKING HOT. The back end of the part was discolored and everything... The solution, turn the rapids
down.. Of course a well meaning employee saw the low rapids and turned them back to 100% and burned it
all up.
 
Bobw said:
I find the biggest problem isn't the re-entry, its the pulling out.. When I'm dealing with crappy work hardening
material, I'll long hand it and feed out .010 or .020" before pulling out. Cuts the chips off clean.
Click to expand...

It's a good policy, but I'd worry more about that with brittle carbide, not as much with a HSS. Do wish there was a broader range of G83 options at the cheap end of machine tools to allow this as a code line.

OP, you said cobalt drills in the first sentence of your opening post, HSS with TiN in a response, and they're different answers. Knowing if it's a "good" brand is helpful too. What others mentioned about slowing down feed is good, how about coolant status and whether it's clear chips are being flushed from the hole? A longer peck might help as long as the chips don't bird nest on the drill.
 
20170815_091109.jpg

I had the same issue in a 17-4 job using cobalt. Bought these and an the rest of the job out on one drill.


Sorry pic is upside down. I flipped it and its still upside down...


On edit. Thats what I get for posting from my phone. Cant see the number. Its a Morse EDP 60121 List 1360T
 
I didn't have time to read everything so if it's already been said.....Be sure to use a dwell, I used Cobalt drills and in work hardening material the cutting edges of your Drill can be chipped right off when retracting in rapid if the chip load is heavy. Use a dwell cycle and lighten the chip.

Good luck

Make Chips Boys !

Ron
 
Maybe this is going to sound light-weight but it works for me, especially since my American made cobalt drill sets and Cleveland drills are lasting a long time.

I use a Mobil Omicron cutting oil and I cut at the slowest speed for the situation and back out the drill to clear chips, drill has time to cool some, squirt some oil, feed drill, repeat.
 
plastikdreams said:
If done right bare cobalt should do many holes in 17-4.
Click to expand...

You'd think. I do wonder if the relatively simplistic split point of the standard cobalt drill isn't holding it back, as there's better point designs now that allow material to flow better while still giving great self-centering geometry. The two little vertical edges on a split point could be getting a lot of "push" resistance from harder/tougher materials where other point designs would pass the swarf through.

If I ever get a small CNC tool grinder set up, this is an area I want to play with.
 
You must log in or register to reply here.

Similar threads

S
4 X Diameter in 304?
Replies
5
Views
263
Orange Vise
Orange Vise
G
Variation in 1018 steel causing issues with insert drill
2
Replies
21
Views
587
Fal Grunt
Fal Grunt
N
Drilling SS 304 using HSS
Replies
12
Views
887
rjwalker1973
rjwalker1973
S
Drilling speeds and feeds for tool steels D2, H13, O1, S7, W2
Replies
9
Views
339
Dan from Oakland
D
I
drilling delrin without packing chips on the drill
2
Replies
39
Views
2K
triumph406
triumph406








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top