Breaking TiN coated carbide step drills

Trying to use a TiN coated carbide step drill for a 1018 steel part. Step drill diameters are .245" at the tip leading to a .427" diameter. The drills are breaking on the lead angle (118°) between 1-6 thousand cycles. We have tried changing the RPM's up and down with no positive results and would prefer not to slow the cut down as it is a very high volume machine.

Currently we are running at 850 RPM's with a .300" feed and a 12 sec cycle time. Originally was set to 1160 RPM's and have also tried 1500 RPM's. We are looking at changing the coating to AlTiN. Does anyone have any other suggestions to prevent the tool breakage?

Is it a blind or through hole?

2nd thought 850 rpm at 0.300'' / minute = 0.00039'' /rev .................that drills not cutting - it's rubbing and possibly blunting the point causing breakage,.............. try somewhere around 0.003'' / rev - which at 850 rpm is 2.55 ''/ minute.

3rd thought 850 rpm is very slow for 1/4'' HSS but about right for 7/16.

I think you need to look in to your feeds and speeds for the type of drill you are using, and possibly slow down when you hit the larger diameter.

Breaking how? Chipping or actual fractures along the edge? 1-6k parts is quite the variance in tool life. Are you sure they are not inclusions or flaws in the material leading to sudden failure?

It's not what you want to hear but have you considered firing a stubby cobalt #7 (.201) down first to take the pressure off the tip and let the pilot act more as a reamer? I don't imagine you'd add more than a couple seconds to the cycle time per hole.

Your RPM says HSS, but your title says carbide?

WAY too slow on the speed.
kick it up to around 2,800 rpm or more and go .006-.008 ipr

IMHO thats part of the problem with step drills, i only like em were its possible for the smaller size to drill through then bang the speed down for the larger size adjusting feeds to suit. Few of em do well if the small size is still drilling when the step comes into play, one piece of swarft under the flute and they flex and snap the small drill tip off time after time.

RPM wise i would be using more with 8% cobalt HSS, but then im a animal when it comes to drilling mild steel. A good coated Hss cobalt bit of 1/4" diameter i will oftern spin nearer 1600rpm, dropping more down to your 800 ish rpm for a 1/2" drill

Altin does help a bit in mild steel too, but it all depends on how good the tin coating is, if its very good the difference is not much. If its a crappy cheap coating then its a lot more of a difference. Thing to watch for is the swarft sticking in the flutes between holes? If it is, its time to regrind - recoat it.

If your machine can do it it may make more sense - be faster to just use 2 drills and hit each hole twice. A good carbide drill in a VMC thats capable of fully driving it will be border line as fast as punching holes on a iron worker at these diameters. Oh if you do that, definitely big hole first then little hole. Other wise you just chip the big drill!

If you have a tool changer on your machine go with two carbide drills. With the feeds you are at now your cycle time may even go down even with the tool change. I am running around 6k at 22-25 ipm in 1018 right now with thousands of holes with each coated carbide drill. That is with flood coolant though. If your using a bridgeport type mill well then what your doing makes more since to me.

Would love to add another drill. Unfortunately we are machining this part on a 12 station rotary transfer machine and every station is occupied without the ability to make more space. It is a Blind Hole.

The tip is chipping/breaking off on the point of the drill. We believe it is caused by the tool heating up because coolant struggles to reach the drill tip because of chips wrapping around the tool. That in combination with the wear on the tool causes it to break off. We have numerous machines running the same step drill and have noticed that the lower the sulfur content on the material the more breaks. There is no damage on the side of the small Dia just on the point which leads me to believe it occurs when the tool first hits the part.

Right now the SFM is 54.5 (small) 95.0 (large) and the feed/rev is .0018 ipr. We tried raising the RPM (up to 1500) to get the feed/rev even lower (.001) and the surface footage up but it did not help. We could try raising it even more but I think we might just burn the tool out faster.

Count to 10 Sami

Please read the replies carefully,

I repeat, you are not pushing that drill hard enough, unless the spindle driving it is that shagged it drops on to the workpiece - the point / tip damage is not occurring when it ''hits the part'' it's caused by the drill over heating through rubbing, drills, like all cutting tools have to CUT.

Drills are designed to work within given parameters in relation to their diameter, within those parameters feed must be maintained whatever the spindle speed. ergo if you increase the speed the feed rate must also be increased, and vice versa.

The sulphur content WILL have an effect of tool life as it is used as an additive to promote free cutting.

You misread the original statement. The .3" feed isn't per minute it is how far the tool goes in the 12 second cycle time. This equates to .0018" per rev. If you really think speeding up the feed of the drill so that it has a .003"/rev we can try that. That would bring the cycle time down to 7 secs. Seems contradictory to move the drill in faster to prevent it breaking but I see where you are coming from.

Would you also recommend speeding up the drill and decreasing cycle time even more? If so what speed would you recommend for the cut?

Maybe TiCn. At this speed AlTiN makes no sense but often this gets a TiCn under-layer to help with bonding and it works at the lower speeds where you can not convert the AlTiN.
You are way slow. Chip load is light but workable. Somewhat demands on edge condition.
Mostly I suspect a tip geometry problem which is often vendor specific. Maybe a base carbide grade problem.

Where is your tool supplier in helping with this problem? Tell them you want a solution. That is their job, not yours.
Get out your monkey bat and give it a good swat to get it of your back an onto the people selling you tools.
Bob

Any suggestions on tip geometry? We design and make all of our own cutting tools. Right now it is just a 118° point, straight flute, step drill.

Also you said way too slow. Would you agree with Sami and suggest a .003"/rev feed? What RPM would you recommend?

UPDATE: We actually advance this tool .600" with a 10s cycle time at 850 rpms. That results in a .0042" feed/rev. Which seems to agree with what many of you are saying. Should we try to speed the drill up then. Or maybe even slow down the feed rate?

I did not take time to read all the responses so this may have been brought up. Depending on how heavy your chip is the drill could be chipping on the way out. I recently had a 3/4 thick 316SS plate job with over 20 drilled and reemed holes in each. The order was for over 200 parts so I went with a carbide drill. I was losing drills the lead edge was chipping or the drill was braking off clean.

The chip was heavy and the damage was occurring as the drill was rapid'ing out during the peck cycle.

Make Chips Boys !

Ron

cbarish said:

Should we try to speed the drill up then. Or maybe even slow down the feed rate?

Click to expand...

You've had multiple people telling you to speed up the rpm's and feed faster.
Yet you're still asking what to do.
I run my carbide drills in 1018 at 370sfpm and for a .500 dia drill I go .011 ipr

Your way of calculating feed rate is strange....

*IF* this drill is Carbide I would go with 200SFM and .004" per rev.

How much run-out does the drill have? I am assuming it's in a Quality tool holder?

Whats the geometry on this like?
Is it 0 rake like a cheap Irwin step drill for a hand drill?
Or does it have some positive geometry so that it actually CUTS and doesn't just smash the material out of the way?

cbarish said:

Any suggestions on tip geometry? We design and make all of our own cutting tools. Right now it is just a 118° point, straight flute, step drill.

Also you said way too slow. Would you agree with Sami and suggest a .003"/rev feed? What RPM would you recommend?

Click to expand...

Ok, that presents problem.
A) I would not put the same rake and clear angles on carbide as HSS. Does your design account for this.
B) edge prep? any, none?
C) type of Tin coat, PVD, CVD, thickness?

I'd be up above 400 SFM on the minor diameter and way past your feed per rev. but tool geometry of the flute and clearance behind the cutting lips matter.
I could give a shit about point angle but it does interact with the clearances on standard grinds or the front rake and belly/hook if your flute is fixed.
Not even sure if you are in a C-2 or C-5 carbide,

For sure I'd try faster and harder. Pull the tool very early and look at the wear under a microscope. What is happening?
Which is pissed off the flank or the top? Weld? Coating gave up the ghost? Tip (flank) shows signs of rubbing? Micro-chips which a buff hone may fix?
I don't think you will see thermal cracks as you are not in this range for speed.

As a random wild guess I'd think small chip welding that pulls out pieces of the carbide as it is forced to cut. Good news is that this only happens in a fairly small range of speeds.
Going faster gets you out of this badland. Going slower also does but slow is rarley a good option.

The real trick here is to pull tools way, way before they go bad and look at them.
On a 6000 pc tool I like to see it at 10, 500, 1000, 3000.
Nobody wants to pull a tool still working but it's the only time you see anything that lights up that little bulb.
Chip the crap out of end, give me 1/2 of a broken insert. I can't tell you anything at this point and can simply pass out wild guesses of things to change.

There is a whole nother way out of this problem and for sure this is common.
Try lots of feeds and speeds, try lots of coatings and carbides. You will hit a "works for you" combo at some point.
Sometimes the shotgun approach is faster to the finish line.
Bob

cbarish said:

Any suggestions on tip geometry? We design and make all of our own cutting tools. Right now it is just a 118° point, straight flute, step drill.

?

Click to expand...

My italics !

You're running a straight flute step drill in soft steel, and getting at least a thousand holes? ...............I'd call that damn good going.

Soft steels ''need'' spiral flutes, ....especially if the drill axis is vertical.

Mtndew said:

You've had multiple people telling you to speed up the rpm's and feed faster.
Yet you're still asking what to do.
I run my carbide drills in 1018 at 370sfpm and for a .500 dia drill I go .011 ipr

Click to expand...

Correct. Then I noticed that our feeds in our machine layout were not the same as what we had on the floor. I then updated the feed in the post which was now higher than what most recommended and was asking whether this should be slowed back down.

Also i'm trying to get as much information as possible. Clearly there are some differing opinions on what the "ideal" is. The nature of the plant I work in doesn't lend itself to playing around with speeds and feeds. Machines run 24/7 365. A stoppage for 5 minutes needs to be justified. This is why I was trying to get as much information as possible before just blindly speeding up the machine.

Thank you everyone for your help I am very new to the manufacturing world and your insight has been greatly appreciated.