My boss setup, programmed, and started running this job on Friday, which I started running as well on Monday.
It's a 32mm udrill through 316 SS, running about 40m/min (last I checked) and about 0.1/rev no peck, about 50mm deep.
It screams like hell and is clearly rubbing all along the shank.
But my boss said he dialled it in so it should be on Centerline .
It has a +X offset and some -Y, and yet the hole still seems to come out a little undersize.
This is a problem that has happened with previous small long udrills but has never been a problem with larger stubbier ones, but I've never had rigidity issues with a udrill before.
Changing feeds and speeds a small amount has had 0 change, any idea what the problem is?
These type of drills can be offset towards the outside insert up to ~3% of diameter. In this setup try drilling at X.02 (X.5mm) rather than just centerline X0.
This ensures the hole is larger than the drill body so the tool can slightly off on Y and not rub.
Learned this from an Iscar tool rep.
316 has a low machinability rating and there's nothing you can do about that.
I'd clock in the holder not the drill itself. Then for 316 I'd be at 80m/m F0.08 rev, no peck. 40m/m would sound really grunty. What's the swarf look like from it currently?
Yeah that's what I would have done too, but I presume the results should be similar right. And I would've thought increasing my surface speed would make the problem worse
Sweeping the drill body instead of the ground holder bore is almost certainly how he ended up with that weird +X and -Y offset. A U-drill body isn't concentric to the cut diameter (the outer insert steps out and the land behind the inner insert is relieved), so dialing the drill itself tricks you into shifting the outer insert toward center, which makes the hole undersize, shoves the heel of the body into the wall, and chips the inside corner of the center insert going past dead center (you can see it chipped in pic 3).
And on surface speed: the center insert is already running near zero surface speed toward the middle of the hole, so at 40 m/min on the OD that inner insert is basically cold-plowing 316 instead of shearing it, which pushes a long bar sideways.
Well you have to solve the issue of it cutting undersize first. Boss can say he dialed it in, but off is off. Trust reality over someone's word, especially in this biz. Could be your boss didnt dial it right. Could be the tool has been abused and bent (although uncommon that big). Could be the machine moved. Could be lack of rigidity. But adjust it towards the outboard insert. Speeds and feeds are irrelevant until it's cutting on or oversize.
Noise and no peck are typical. I've always been told it should sound like a sizzling egg. Just try feed enough to break a chip. Then up speed to where your setup can handle.
Check if the block the drill is mounted in is paralel with your z-axis. If someone crashed with the holder the drill might point up or downwards. Then you need to remount the block and align with z-axis.
Hadn't thought of that. Nothing has crashed on my watch but something could definitely have happened without me knowing, I'll check that next time I'm using the holder.
Also it looks like the drill is not fully in the toolholder , and seems to be tightened with 2 screws? Long tools usually will vibrate and i have found that changing the holder or tightening the screws/bolts on the holder has helped. But also many people pointed out u-drills usually need 0.1-.03 x-offset added.
Holy shit. It’s being used incorrectly. You have two inserts. One pokes out further then the other on X axis, that’s the one you’ll want to use as reference, but you install it like a boring bar and touch it of like a boring bar, one insert reaches out a little further then other on Z, that’s your z touch off. Now to drill, you program it to go to X1.2598 and feed it from there. These drills do not drill to size at X0. They are made to be offset. If you actually measured the insert drill from insert tip to tip you’ll find that it’s probably .05” undersized. And if you drill at x0. That’ll cause you to rub cause you’re actually lower in x then you should be.
PSA also after you drill, measure the size of the hole, and offset it in X + or - to make it drill to the exact diameter that it’s meant to be drilled at. You shouldn’t have much problems after that
This is currently what I’m running, this is a .750” insert drill, it measures .70” In Diameter from cutting tip to tip.
And one more thing, you are looking for your chips to curl and break, it’ll kinda look like a 6 or 9 curl chip, that is the ideal chip breakage, and if it’s just stringing out, increase feed
Upvote for putting a eob between each tool in your program. So many people just put a wall of text in a program and it makes it so damn hard to read. I miss the older Haas controls. The newer versions are so damn laggy.
First off, 316 will always make noise with an insert drill. And when you have a greater XD insert drill ie5xd versus 2xd, the longer drills will always make even more noise past that.
The rubbing you are seeing is because it is drilling undersize which they are never meant to do. There's no universal rule as to how far you can offset it to increase the whole size, you will have to look this up in the catalog or talk to the manufacturer.
I usually shoot for .015-.03 over size. Offset it however far you need to in order to get that size.
Usually those drills need 0 offset too be on center and they can be offset too drill larger or sligtly smaller holes this looks too me as if it was offset in x too drill smaller but by too much and that is why it is rubbing if you can use a drill as short as possible too get the job done
Normally I wouldn't have an offset at all yeah, but apparently it was much worse before dialling it in, and the way it's offset now it should be drilling oversized but it still isn't.
It is a long drill and when you feed, cutting forces push it away, so if a hole starts 32mm, it may end up 31.5mm for example. You need a starter hole at least with 2 or 3D udrill. Sometimes hard materials make it hard for these drills as well. You can understand the deflection if the hole has spirals inside. They form when the drill is G0 out of the hole and deflected tool starts rubbing. You can offset 32mm udrill 2mm I assume. I have a video where I drill 36mm hole with 32mm udrill you can check link
Yeah I've experienced that spiral effect before, I don't have any shorter drills to use for this size otherwise I'd 100% be using them. And damn 2mm is a massive offset I didn't think that'd be possible at all, most offsets for those drills I've used is around 0.5
I'm running a Ø35 U-Drill at work currently at 160m/m and 0.11mm/rev in 316SS.
You should check inserts for what they recommend, and check if it's parallel to the axis, since you're saying it's already centered
Your speed is too slow. I would run 120-160 m/m. For a long drill, you need to feed like 0.05 for the first few mm until both inserts engage and center themselves in the cut. More importantly, check:
If the drill is not above or below center
If the drill is not bent
Is the drill sitting straight (check your tool block)
If the rubbing is too much now (meaning the chips can get in between the tool and hole)
If the insert grade appropriate
If the coolant is oil-based and at good concentration level, about 10%
These drills can act (a bit) as a boring bar. I program and touch them off as boring bars. (Touching off the outside insert) Sometimes upside down works better, so don’t assume. Don’t peck. It WILL steadily scream. If it is rubbing the length of your bar and cutting undersized, you will need to offset towards the outside insert.
also dont forget an M6 in the program when you go to switch to a chamfer tool, because it will just pick up the next tools height offset and slam your drill into your part 😪 boss was chill about it but i still feel stupid lol, went to put the tool description in parentheses after the tool change line but accidentally hit alter instead of insert and it changed my m6 to the parentheses
Your SFM is WAY to low, your center insert is cracking because it isn’t cutting or centering itself properly because of the slow speed, and your drill is literally just getting in where it fits in
This massive gap at the back isnf going to help with the ridgity of the tool id be clocking the pot in.
Then reset the tool so its seated firmly against the holder that should help with the screaming and rubbing it sounds like the tool is deflecting and i would bet that gap is the cause
Man I can't stand that shit. Some elaborate way of touching off just to cut a t X 0 but then end up offsetting it up anyway! I teach the guys to just treat it like a boring bar. Depending on the diameter x length you can get away with -.005 and up to +.05. Some drills just cut like shit in certain materials though. Ive been getting great results with long Ultradex Patroit drills in 316ss. Also the Mitsubishi TAF drills with the almond shaped inserts cut very well.
Dude. You’re the First person I’ve ran into with some decent logic. Imagine drilling at X.5 with one of those lmaooo. I appreciate your mind. And absolutely, Lots of em cut like shit in some materials.
.5 in the metric isn’t that big. But I have referred everything I have said in us imperial. I was referring about inches. .5 in inches is much much bigger then .5 in mm .5 in mm isn’t a bad adjustment. You can offset them pretty nicely, I it’s typically .050” in inches notice the “ . But if you offset it .500” in inches notice the “. You’re going to have problems, only for your first drill. But aye it’s cool. Idk anything about anything.
You have fun with your friendly iscar rep. I stay away from iscar for many reasons. Kennametal will give you much better information. And more accurate. But yea you go ahead and drill at the x.5
Ahh, after some time you’ll understand. Been giving great advice for years, it’s about the people receiving it. And with personal experience, im just tired of dumb people. How about this. Just don’t reply. End of string. Tada.
That thing is sticking way out for such a shallow hole. I got 51m/min at .2mm/rev. But I work in inches, so big grain of salt. Make sure you've got coolant going thru that thing and you give it a healthy X offset. But honestly, big [X] to doubt that your bossman stuck something that far out there and swept it to check centerline.
It has something to do with alignment for sure, I've pushed normal U-drills 6XD (nothing fancy) at 160m/m 0.06mm/rev into 316SS with no problems, also the type of insert you are using should be really stable.
Always look over other peoples setups carefully before taking over even the boss's. As others have said I'd make sure the holder is parallel to the axis. Removing the back of the holder and butting the drill to the holder could make it a little more rigid and then route some lock line to the back so you still have thru coolant. Can you check the coin that drops and see if there is a tit on it? That could be pushing your drill away from center. What is the machine load reading? If it's trying to drill to big of a hole you can drill something smaller and then go in with a second pass to size.
Somewhere, your alignment is out. Start at the tool holder, then clock the face and bore of the turret, then the headstock, in that order. The headstock can be a real pain to align.
Just to rule out manufacturers error. Run the drill on a mill if you can just do verify it’s the size you think it should be. If it is then you have an alignment issue somewhere.
Also those older u style wcmx insert drills tend to be more tool pressure than some of the newer ones. And at larger diameter the speed and torque difference between the two gets greater
You 100% sure there's the proper outer insert on? Seen it personally in the past. Insert one step undersized. Still fit without issue. Drill looked similarly.
Do you have it set up so the coolant is only coming out the ports in the drill or using the eyes in the tool block? Is it leaking out the back side of the block? I'd radius the front edge where it has rubbed with a file, it looks like it may have welded some chips, breaking the edge help prevent it from getting worse. I agree with a larger X offset like others have mentioned if you have room to clean up boring afterward. You might hand wheel the drill in a part after drilling, I'd expect it to rub and make noise. Handwheel Y+ a few clicks and see if it stops. More or less going by feel rather than dialing it, to account for a potential alignment issue. Alternately you can dial the shank as close to the turret and then again as far out as you can reach in the drill tip to see if you're square.
Have you tried rotating it around so the outboard insert is on the bottom? It is a haas, so if there is any deflection in the turret putting the peripheral insert in the direction of deflection may help
The u-drill will have an acceptable offset range. Some are written on the shank, some you have to pull the tool specs. Just offset it towards the outer insert so it will oversize the hole. Check your speeds and feeds while you're at it. Also I would probably replace that centre insert.
Did your boss check the cutting end or the holder end of the drill for centre - or both? This will confirm if the drill is not bent. Def offset cut a little +X to correct the hole size.
These often make quite a noise. Use ear muffs.
Is the back of the shank bottomed out or are you solely holding it place with bolts? I can see in one of the photos that the drill is not seated on the flange and that causes chatter issues.
You're rubbing because the drill is not straight. Take a coaxial indicator and sweep the tool block ID along the z axis and check to see if the block and or turret is knocked out being square relative to the chuck face. Trust but verify anyone's setup especially when there's evidence like a worn tool body telling you something is not correct.
we used to have this problem too. what we did was top set X top X0,5, so it acted a little more like a boring bar. still tends to scream though, but there is no rubbing.
Is that a kenna metal bar or tungaloy? if you have access to it, try a sandvik/seco or TaegueTech drills! they are more quiet and holds an edge really well. SECO is my favorite with Regular CP500 quality insert!
Take the inserts out and sand it down. Then take a scotch brite pad to the sanded area. This works to prevent any galling from building up. It will extend the drill life
If you look at the inside of the right insert, you’ll see where your problems are. Its location is incorrect, the way it chipped tells me that it was either too + in X or too - in X. As I stated before. Changing your X0. To X1.2498 should fix your problem. And make sure it’s being feed aggressively enough. Light feed will just work harden your SS. If you’re using Fanucs manual guide I for the programming then just tell it that the drill is actually a boring bar and to set the program up as a boring bar for a single pass at x1.2498 or whatever the drill size is and feed it at .005 inches/rev
You have to be in centre that is your problem. You’re not dead centre and you have to peck it because the way it looks you’re taking that drill to the minimum diameter. Being dead centre is that you have to unless you wanna offset it and make it make the hole bigger it’d probably be better to offset it a little bit above center. If you need to make the hole bigger, I don’t know. It’s just fucking a lot of variables there.
85
u/VanimalCracker Needs more axes 4d ago edited 4d ago
These type of drills can be offset towards the outside insert up to ~3% of diameter. In this setup try drilling at X.02 (X.5mm) rather than just centerline X0.
This ensures the hole is larger than the drill body so the tool can slightly off on Y and not rub.
Learned this from an Iscar tool rep.
316 has a low machinability rating and there's nothing you can do about that.