Drills breaking drilling through Grade 5 bolts

[cyanidekid]

Can you drill half way, flip it, and drill the other side?

I'd much rather make a bolt from scratch than modify cold-headed hardware.

as we have discussed at length in other threads (pun intended), cold headed and rolled threads are superior to cut threads and heads, considerably so in fatigue. aside from that, he's got 1000 of these to do.
a high quality fastener should be consistently in a fairly narrow range of hardness. a cheap fastener can be all over the place.

Holo-Krome or ARP....

 

[dnuccio]

Made some progress on this. Found a Kennametal carbide drill. Running at 1200 rpm 6.1 ipm about .005 ipr, pecking every .070". Still spotting but reduced the depth so the tip of the drill is cutting before the corners. I got through a little over 100 bolts before one of the corners of the drill chipped. Just going to order a handful of those drills and try to get through this job. As a few of you have mentioned, I'm thinking this is just a crappy material problem as grade 5 shouldn't be giving me this much trouble. We get these bolts sent to us from the customer so we have little control over their quality

 

[Booze Daily]

BTDT. Politely declined any future orders.

 

[Milland]

BTDT. Politely declined any future orders.

Or change terms to time and tooling...

 

[dnuccio]

BTDT. Politely declined any future orders.

I wish. Unfortunately this will be a recurring job as the customer is a friend of the owner. Might be able to get them to splurge on some higher quality hardware, but I doubt it.

 

[DDoug]

Look at the spec's for grade 5, and see if you can cross over to something similar like A325.

 

[Orange Vise]

Grade 5 is about HRC25-35, similar to 4140HT.

900 RPM is too fast. I'd cut it in half for starters and see where you get. Cut your IPM feed in half too, maintaining the same chipload as before.

Might have to slow down your rapids so there's enough time for the coolant to get down in there.

I have 1000 of these bolts to drill

Slow and steady wins this race. Make a simple fixture with a bunch of threaded holes as mentioned above and let the machine run unattended.

 

[Booze Daily]

Or change terms to time and tooling...

I’m a one man shop. I don’t have time to babysit a job.

 

[DanielG]

Still spotting but reduced the depth so the tip of the drill is cutting before the corners.

Why not use a 140 degree spot drill for your 135 degree drill?

 

[guythatbrews]

I'm surprised at all the talk about RPM. SFM is a better way to talk about this stuff.

If the drill sounds bad at 1" deep you need to start coming full out to clear the chips starting somewhat less than an inch. Dwell a bit to allow coolant to do the job before going back in. If the drill is showing margin wear the speed is too high.

Material likely an issue. Slow the sfm way down. 30 was mentioned start there. You gotta peck anyway I'd use a smaller feed too.

Not making headway with indications speed is too fast. Working yourself to death. Sometimes you just gotta slow it down.

 

[wmpy]

as we have discussed at length in other threads (pun intended), cold headed and rolled threads are superior to cut threads and heads, considerably so in fatigue. aside from that, he's got 1000 of these to do.
a high quality fastener should be consistently in a fairly narrow range of hardness. a cheap fastener can be all over the place.

Holo-Krome or ARP....

Yes, of course rolled threads are better. But we don't know if the customer actually needs that extra goodness. In my experience, a lot of times that a customer wants to modify some hardware, it's because they think that's easiest, cheapest, or it's just how their brain works. They need a bolt with a hole in it, so they ask if you can put a hole in a bunch of bolts they just bought and struggled to drill out in their drill press. It's rarely a highly engineered part.

It should be mentioned that the material used in a formed bolt was not chosen for it's machinability. 1000 pcs? If it were me, I'd definitely try to persuade the customer to let me make them from bar stock. I could even make it from ETD150 and roll the threads if they really wanted me to. I have the equipment to do so, though, and I know not everyone does. You wouldn't have the cold headed hex, but if they're putting a 5/16" hole through the part, how hard are they really going to be cranking on these?

 

[evil monkey]

i'm having a problem with drills breaking on this job. 1/2-20 grade 5 bolts, 1 inch long that I am drilling a 5/16 hole through the length of. I'm running this job on a Haas VF2. I'm using cobalt 5/16 drills, 135 degree split point at 900 rpm, 5.5 ipm in an ER collet holder pecking every diameter. Using flood coolant at a higher concentration than I typically keep it at. The drill appears to be getting very hot towards the bottom of the hole before it breaks through, the overall length of the bolt including the head is around 1.375 and the drill starts making noise around 1 inch deep. Stopping the drill before it breaks and checking it out, the cutting edge is very worn. I am spotting these holes with a 120 degree spot drill. I do not have thru coolant capability unfortunately. I have 1000 of these bolts to drill so doing it on the bridgeport (to get a manual feel for how the drill is behaving) is not really an option. I'm currently getting 10-15 holes out of a drill. Any suggestions would be appreciated

Stainless work hardens fast so I would slow the rpms down to about half what you are running . I have also had good success with adding blocks of ice to the coolant tank and reducing the tenperature as cold as possible. The colder you can get the coolant the fewer problems you will have rolling the cutting edge.

 

[Garwood]

I've done stuff like this. I used HSS and ran it stupid slow in a big heavy geared head Mori. Like 50 RPM for a 37/64 Drill 3" deep. Pecked about every 1/4".

It was slow going, but reliable.

 

[13engines]

The problem is started right off the bat with the120 degree spot drill The very edges of the drill that typically wear first in normal use are getting a big head start by hitting that too pointy spot before the tip does. Either switch to a 140 degree spot or forget the spot all together and use a Screw Machine drill. Sometimes I've also had better luck on tough stuff using coated HSS drills. Cobalts seem to give me trouble when I try them. Dormer drills come to mind.

 

[Scruffy887]

I have drilled some bolts before on a VMC in a threaded fixture that held 4 at a time. Totally amazed at what a PITA it was with feeds speeds tool life. Got very few done and realized I would need better tooling. Only needed about 40 of them but had to stop the job until better tools arrived. Still sucked.
I do drill .625 rolled acme shafts in batches of 620 every month or 2, and tap 1/4 20 form tap. Cobalt drill with pecking. full withdraw and flood coolant. This is part science and part Voodoo. Internal job that I have run for the past 20 years. Fixture holds 24 pieces. Once I got it to work I change NOTHING. Have boxes of the magic taps and drills that work. Throw them out after 620 pieces. And listen carefully near the end of the run as the drill sometimes complains. I toss it if it complains as the tap that follows will make a big noise without a hole to thread.
Feeds and speeds are set to be a trusted process as cycle time is a bit less than 15 minutes and for the most part I am doing something else until the last 100 or so pieces.
Piece 24 on the fixture is always inspected as a few times a corner of a drill got chipped and it kept drilling. Oversize hole that the bolt almost dropped into.

 

[DrHook]

Once upon a time, I did some similar drilling thru bolts on a manual lathe, although methinks it was 3/16 holes, and I damn sure didn't have flood coolant. After breaking 3 or 4 drill bits, it occurred to me I was gonna run out of bit budget if I didn't figure something out. I noticed that the last 1/4" or so was where the machine and or drill bit would begin "arguing", so I switched to a different bit for the last 3/8" or so, and made it thru the parts. I drilled most of the way with one bit, swapped chucks n bits, n finished the hole, and swapped back for the next one. PITA, but it worked. I did not have 1000 to do... I figured there must be some sort of hocus pocus involved in forming the very end of the bolt which caused it to be harder, and perhaps the drill bits were gradually failing, so my last 2 bits got me through. No fancy cobalt or anything, I'm sure, and probably dumb luck. ...anyway...

 

[Cole2534]

Slow and steady wins this race. Make a simple fixture with a bunch of threaded holes as mentioned above and let the machine run unattended.

This has saved me on some deeper holes.

 

[cyanidekid]

Yes, of course rolled threads are better. But we don't know if the customer actually needs that extra goodness. In my experience, a lot of times that a customer wants to modify some hardware, it's because they think that's easiest, cheapest, or it's just how their brain works. They need a bolt with a hole in it, so they ask if you can put a hole in a bunch of bolts they just bought and struggled to drill out in their drill press. It's rarely a highly engineered part.

It should be mentioned that the material used in a formed bolt was not chosen for it's machinability. 1000 pcs? If it were me, I'd definitely try to persuade the customer to let me make them from bar stock. I could even make it from ETD150 and roll the threads if they really wanted me to. I have the equipment to do so, though, and I know not everyone does. You wouldn't have the cold headed hex, but if they're putting a 5/16" hole through the part, how hard are they really going to be cranking on these?

if they are resistant to buying decent made in USA fasteners, I doubt they would possibly go for the custom bolt. also l'll add if you ever needed 10% extra strength, its going to be on this thin wall hollow bolt. the extra margin of pure tension strength for a rolled thread would I think actually be more in this case, maybe a lot more. you are leaving the workhardened material behind.

I will go so far as to say it's bad design/engineering to use a cut thread bolt for this, unless there is no reasonable alternative.

 

[Nmbmxer]

If you could get away from the spot drilling you could use a coolant inducing holder and poke a carbide drill straight thru. Id think the time savings would offset the toolholder cost. I built a basic coolant inducer using an extended ER toolholder and it worked pretty well for the job it was for. It was basically a slip on collar held in place with some snap rings and used teflon wear rings for seals. It leaked some but got enough coolant pressure to the drill to work fine. YMMV.

 

[dnuccio]

I'm surprised at all the talk about RPM. SFM is a better way to talk about this stuff.

If the drill sounds bad at 1" deep you need to start coming full out to clear the chips starting somewhat less than an inch. Dwell a bit to allow coolant to do the job before going back in. If the drill is showing margin wear the speed is too high.

It is fully retracting every peck