hardening while drilling problem?

C

celticpride2133

Joined
Jan 30, 2012
Messages
183
Im working on my first knife and ive run into a problem that I didnt think I would have. Im drilling my pivot hole and about half way through the steel (1080) the drill stops making progress and now I cang get it to drill through, or even drill it at all. Did the steal harden? What can I do? Thanks
 
That's called work hardening. It happens when you get the steel too hot while drilling. If you slow the drill down and take your time on the holes you should be able to avoid this problem.
 
Loo brick ant....

And yes, steel likes slower speeds. I'm usually one pully up from full slow on my old Milwaukee. The drill, not the beer...

Oh, and does it do the same thing on separate attempts with the same bit, or is the bit getting smoked? What kind of steel also. 304 for example work hardens if you look at it funny.

-Eric
 
What type of cutting fluid are you using? What size bit and what speed?

I would guess too little feed pressure. Fill us in so we can help. We were all in the same boat one time wondering wtf....
 
Even with cutting oil, I find that I get work hardening toward the bottom of my small holes in high carbon steels. I can mitigate the issue to some degree by being very diligent in peck drilling but often it is still an issue. Lately, I've been using carbide drills for my small holes and found that they can cut quicker thereby reducing hardening and if the material does work harden, they don't really care.

Bob
 
Im using a 1/4 inch bit, just using water while drilling, the drill hole gets crazy black before it stops drilling, can I save this knife or no, its 1080 steel and drill is running 1500rpm?
 
celticpride2133 said:
Im using a 1/4 inch bit, just using water while drilling, the drill hole gets crazy black before it stops drilling, can I save this knife or no, its 1080 steel and drill is running 1500rpm?
Click to expand...

Speed seems about twice as high as I would go at it. Is the bit hss, cobalt? Is it sharp? Try a cutting oil, Home Depot has a dark cutting oil by a Oatey if you need something ASAP. Are you pecking? How heavy is the drill feed?
 
celticpride2133 said:
Im using a 1/4 inch bit, just using water while drilling, the drill hole gets crazy black before it stops drilling, can I save this knife or no, its 1080 steel and drill is running 1500rpm?
Click to expand...

For starters, I think fifteen hundred is too fast for a 1/4" drill

The rule of thumb I use is 500 rpm for a .500" drill

Half the drill size to 1/4" is double the speed to 1,000rpm

so according to that, you're 50% too fast.


Now those rules of thumb were designed for maximum production in mild steel


My real life speeds are even lower for a hardening steel, and a bit lower yet, just cause I ain't in that much of a hurry.



You're going to have to sharpen that drill

You're going to have to probably grind out that hardened part with a carbide burr, or dremel stone until you get to soft steel again.




If your first knife is a folder, try a little fixed blade first.
 
Slow your speed and increase the feed rate ! There are lots of alloys that workharden more than 1080.The worst of the steels I found is 301 stainless.
 
Hardening while drilling has nothing to do with heat, nothing to do with cutting oil and everything to do with inadequate and uncontrolled feed rate.

If you're using coolant and drilling something as thin as a knife you don't necessarily need to peck. Pecking makes work hardening worse but allows your cutting edges to cool if you're running dry.

This is video of drilling 1/4" A2 at 916 RPM and 4.6 IPM. No pecking because of coolant and only 1/4" deep hole.

[video=youtube_share;bGZqqo2r2Ec]http://youtu.be/bGZqqo2r2Ec[/video]

No drama. Sounds a little like cooking bacon. :)

That was A2, but I just ran that pattern in 3V and drilled about 300 holes (works out to about four feet) with that same drill without needing to resharpen it. It is a cheap basic 118 HSS, USA made drill, probably three or four bucks. Then I had to run that many holes in Elmax, which actually does work harden extremely badly, so I split the point to reduce work hardening and had to resharpen it a couple times during the run because Elmax (1.7% carbon, 3% vanadium) is abrasive. But think about that, a properly fed inexpensive (not even cobalt) drill can go through two feet of something like Elmax without a problem.

I see the problems people have drilling holes and the things folks do to improve it and some of it helps, most doesn't hurt, but at the end of the day, 99% of the answer is to feed it right.

1,500 RPM is pretty fast, you'll reduce reasonable cutter life to perhaps 100 holes, but fed right it would still work.

There is no good reason to use carbide here.
 
Nathan the Machinist said:
Hardening while drilling has nothing to do with heat, nothing to do with cutting oil and everything to do with inadequate and uncontrolled feed rate.

If you're using coolant and drilling something as thin as a knife you don't necessarily need to peck. Pecking makes work hardening worse but allows your cutting edges to cool if you're running dry.

This is video of drilling 1/4" A2 at 916 RPM and 4.6 IPM. No pecking because of coolant and only 1/4" deep hole.

[video=youtube_share;bGZqqo2r2Ec]http://youtu.be/bGZqqo2r2Ec[/video]

No drama. Sounds a little like cooking bacon. :)

That was A2, but I just ran that pattern in 3V and drilled about 300 holes (works out to about four feet) with that same drill without needing to resharpen it. It is a cheap basic 118 HSS, USA made drill, probably three or four bucks. Then I had to run that many holes in Elmax, which actually does work harden extremely badly, so I split the point to reduce work hardening and had to resharpen it a couple times during the run because Elmax (1.7% carbon, 3% vanadium) is abrasive. But think about that, a properly fed inexpensive (not even cobalt) drill can go through two feet of something like Elmax without a problem.

I see the problems people have drilling holes and the things folks do to improve it and some of it helps, most doesn't hurt, but at the end of the day, 99% of the answer is to feed it right.

1,500 RPM is pretty fast, you'll reduce reasonable cutter life to perhaps 100 holes, but fed right it would still work.

There is no good reason to use carbide here.
Click to expand...

Thanks for chiming in. Your experience is greatly appreciated.
 
Nathan, do you have any opinion oh hi molybdenum bits that supposedly work better in material that tends to work harden?. It has been marketed as able to cut quicker and under the the material that is hardening compared to cobalt. Also has thinner web compared to cobalt since cobalt needs this since it is more brittle.
 
PT Doc said:
Nathan, do you have any opinion oh hi molybdenum bits that supposedly work better in material that tends to work harden?. It has been marketed as able to cut quicker and under the the material that is hardening compared to cobalt. Also has thinner web compared to cobalt since cobalt needs this since it is more brittle.
Click to expand...

I have no opinion on those. I use high dollar drills on aluminum where I'm feeding a 1/4" an inch deep without pecking at over 40 IPM, and carbide on wood and plastics, but for steel I've kind of settled on old school 118 degree M2. That's about as low tech as you can get. For materials that work harden a 135 deg split point fed in one shot is a good bet, but honestly a properly fed sharp 118 drill doesn't work harden too bad.
 
Nathan the Machinist said:
I have no opinion on those. I use high dollar drills on aluminum where I'm feeding a 1/4" an inch deep without pecking at over 40 IPM, and carbide on wood and plastics, but for steel I've kind of settled on old school 118 degree M2. That's about as low tech as you can get. For materials that work harden a 135 deg split point fed in one shot is a good bet, but honestly a properly fed sharp 118 drill doesn't work harden too bad.
Click to expand...

Now that we have you here talking about drills can we talk about sharpening ?


I can hand sharpen, but it takes a long time and it's never as perfect as a factory edge


I have been thinking about a drill doctor 750 to do split points with, but they only go to 3/4"


I use some big drills for fabrication maybe 1" or 1 1/2"
That's where the drills are expensive and that's where my hand sharpening flaws really show up.

Can you recommend or comment on drill sharpeners?
Is there a good system that won't cost a few thousand, or a particular one I should be looking for at industrial auctions

or maybe a good set of plans that I can diy

It would be swell if it could sharpen endmills too
I'd love to make up some form cutters
 
12345678910 said:
Can you recommend or comment on drill sharpeners?
Is there a good system that won't cost a few thousand, or a particular one I should be looking for at industrial auctions
Click to expand...

I'm sorry, I can't. I sharpen by hand. From 1/8" to 1/2", though as my eyes aren't as sharp as they once were the little guys aren't working out as well as they once did. I've tried to teach people how to do it but I can't.

I don't even use the little gauge anymore. I don't think I could even put hand to one right now if I wanted to. I eyeball it, but 9 times out of 10 even after eyeballing it I don't tweak anything. The point should be centered, the shoulders should be level, there should be some rake back from the cutting edge, but not more than you need. That's actually a common flaw in new drills is more clearance than you need or want. They make them general purpose so they'll work in aluminum too, but for steel you don't need or want that much clearance.

Sharpening drills is not that hard. A dumb 20 year old machinist still in school can do it. If you can make a knife you can sharpen a drill. You grind a cutting edge and it diminishes in a slightly angled cone for clearance. Most of the time a 1/4" drill can be sharpened in four seconds. Splitting a point is easy once you wrap your head around the concept - you're not grinding clearance behind a cutting edge, you're removing the web to extend the cutting edge to the center of the drill. It's kind of a blind cut, but as long as its even it almost doesn't mater how it turns out, almost anything will cut better than that web.

I don't use drills larger than 1/2" much.

You ought do it on a stone wheel, but I don't have one anymore so I just use a contact wheel. A platen would probably work too, but I've never tried it because I learned on a wheel so I do it on a wheel.

My approach is stupid monkey simple and crude. And when you consider I'm putting these regrinds in a CNC machining center where there is no tactile feedback if there's a problem and a drill could break and wreck a workpiece or a $$$ drill chuck it's remarkable it has never backfired on me, but it just works.

Sorry not to be more helpful.
 
I am not going to disagree with what Nathan says. I think he is a fine machinist and knifemaker and knows what he is talking about. I will instead, provide a counterpoint. I would not call myself a machinist though I have been machining for 30+ years including a couple years of production CNC work. Some materials are finicky and will harden if you look at them wrong. Since I started knifemaking, I've been using 304L for my guards and bolsters. I certainly understand proper feeds and speeds and I have the skill to hand sharpen my drills to proper geometry. That said, I've found that a guard of small size, that can't easily dissipate heat will harden pretty readily while drilling pin holes. Once it is hardened, what is the fix? Should I pull it out of the vise, and anneal it? Should I start over, slotting, fitting, and shaping a new guard? Or, does it make more sense to just drill it through with something that will work? Carbide drills work! Yes, they are ridiculously expensive but so are many of the tools and tooling that work well and make life easier.

I am all about finding a good efficient workflow. I have found that if I start out pre-drilling all my holes with a 1/8" carbide twist drill. Everything goes easily. I can step up to a larger size in a HSS drill and have no issues bringing holes to final diameter. The carbide drill stays sharp far longer than HSS but is easily re-sharpened on my belt grinder using a old 120 grit Blaze belt.

Finally, there are some vendors on Ebay that sell 1/8" USA made carbide twist drills for as low as $4-5. If you are having trouble with your material work hardening, and you are using correct technique, why not give them a try and see if the headache goes away?

Bob
 
Something to think about with 304. It is an austenitic stainless, meaning that even at room temperature it is in the condition (face centered cubic) of really hot steel. Getting it hotter won't make it get more austenitic, it's already completely austenite. That's why it's non-magnetic. And, no matter how fast you quench it, it's going to remain austenite. You can't increase its hardness with heat. It gets hard through work hardening and that's pretty much the only mechanism to harden it.

When machining conditions are bad, things tend to work harden. And things tend to get hot. So there is an association there and it is a commonly held belief and is even mentioned in some tooling books, but in reality the heat is not causing the problem, it is a symptom of a problem.


EDIT:
I tend to be guilty of a mindset that there is a right way and that is the only way and therefor you shouldn't use carbide drills in stainless, you should use regular drills and feed them right. But, in reality, if it works, who cares. Use what works for you. *shrug*
 
Last edited:
Nathan, I have to say I open every post I see your name in. I learn so much from you and your knowledge of metal working. Just wanted to say thank you.

Warren
 
I , too ,open every Nathan the Machinist post .I have learned a ton of things from him.
Makes this forum what it is.
 
Of the 300 series 301 work hardens the quickest .It makes great springs ,just roll it to desired hardness. 305 work hardens the least, best for making rivets
. 303 is a free machining grade. As I understand most makers prefer 416 for bolsters to eliminate the 'gummyness' when machining
Nathan is usually right.LOL
 
You must log in or register to reply here.
Back
Top