What's new
What's new

Drilled hole repeatability issue

DBcooper

Aluminum
Joined
Jul 7, 2017
Location
Kaufman
I'm running a family of parts that get a 14.5 mm drill thru on a lathe. I'm using an replaceable tip YG1 'i-one drill' in A2. Tolerances are +/- .05mm. about half of the parts are coming out just barely undersized, with the occasional oversized hole. New insert, and in my opinion pretty conservative feeds and speeds, 700 RPM, 2.5 IPM, with a spot drill first. Also, when the hole is oversized, it leaves a pretty nasty swirl mark that doesn't make sense to me.

The undersized ones open up to tolerance easily with sand paper in a die grinder, but it's certainly inconvenient and inefficient. I appreciate any ideas y'all have
 
Wasting time inspecting and hand grinding some, it might be better to pre drill. or finish with a reamer.
Might you spot drill 19mm deep with a carbide 14MM and the follow with your !4.5
A 14.5 drill can not make an undersize hole unless the part is getting hot and expanding, it would get stuck and break..
A perfect drill will make a hole .0002" larger (.0051mm or more) than its micrometer check size.
 
Last edited:
A 14.5 drill can not make an undersize hole unless the part is getting hot and expanding, it would get stuck and break..
Another possibility for undersized holes is the drill not making a cylindrical hole, usually three or five lobes if the drill has two flutes. A pin gage the size of the drill won't pass through the resulting non-circular hole.
 
A 14.5 drill can not make an undersize hole unless the part is getting hot and expanding, it would get stuck and break..
But, a drill can make a raggedy-ass hole that won't gage because the walls are a mess.

As for drilling 14mm then 14.5mm, sending a drill down a slightly smaller hole than the drill size can make the drill chatter and go all sorts of crazy. Maybe a stub carbide 14.5mm would be OK, acting more like a reamer than a drill.

Regards.

Mike
 
Are you using a spot that matches the tip angle of your drill? I'm wondering if your drill is walking a bit when it engages the material which could create the inconsistency.
 
I'm running a family of parts that get a 14.5 mm drill thru on a lathe. I'm using an replaceable tip YG1 'i-one drill' in A2. Tolerances are +/- .05mm. about half of the parts are coming out just barely undersized, with the occasional oversized hole. New insert, and in my opinion pretty conservative feeds and speeds, 700 RPM, 2.5 IPM, with a spot drill first. Also, when the hole is oversized, it leaves a pretty nasty swirl mark that doesn't make sense to me.

The undersized ones open up to tolerance easily with sand paper in a die grinder, but it's certainly inconvenient and inefficient. I appreciate any ideas y'all have
You haven't said how deep you're going, I personally would drill undersize and bore it if the depth is less than 3xd.
 
Are you using a spot that matches the tip angle of your drill? I'm wondering if your drill is walking a bit when it engages the material which could create the inconsistency.
That's a good thought, I'll try to find another spot drill. 14.5 mm modular drill tips are surprisingly difficult to find (seems like they're 14.4 or 14.6) so I couldn't be terribly picky on that. I am now thinking it is a 140° and the spot is probably a 120°

Thanks for your input
 
ordered a 142 degree spot drill, while im waiting for that, i adjusted the program to feed in the first 1/4" at 1 IPM and from there it goes up to 3 IPM, that seems to have fixed it. Thanks fellas
 
I've been advised in the past to spot with a short series holder using the same inserts. Seems to work well for me although I'll get the odd one where the hole has wandered presumably due to chip packing throwing things off slightly. That being said I wouldn't be expecting a drill to achieve that tolerance at any depth unless solid carbide. As others have suggested I'd probably ream. What you lose in cycle time you regain in downtime not having to rework parts.
 
New insert, and in my opinion pretty conservative feeds and speeds, 700 RPM, 2.5 IPM
Yeah that's about 1/2 as fast as I would run my Sandvik 870 drill in A-2.
Why are you going so slow?
1518rpm and 10.9ipm is what I would run it at.
 
If you spot perhaps 19mm deep with 1/2" mostly solid spotting drill then the finish drill will have its OD circle grind margin in the bore before its point hits, so having better size control with not including point error included in hole size.

With a simple drill sharpening device, you might buy solid drills and get multiple uses, likely beating the cost of insert drills with perhaps getting 1/2" or more sharpen-off @.030 and still make size..
Measure your insert drills at intervals to see if used one are going undersize. fresh they shold micrometer about .5709
Dull drills may over heat the part so it goes undersize when cooling.

Materils that can work harden can act odd to hold drill size.
QT Op: (Going about 3.25" deep) how hot does the part get?
 
Last edited:
If your spot drill angle doesn't match
That's a good thought, I'll try to find another spot drill. 14.5 mm modular drill tips are surprisingly difficult to find (seems like they're 14.4 or 14.6) so I couldn't be terribly picky on that. I am now thinking it is a 140° and the spot is probably a 120°

Thanks for your input
If your spot drill angle isn't equal or greater than the drill diameter it can cause the drill to walk. However from what I can tell the real issue is poor chip formation and poor chip evacuation. Are you chips coming out looking like a 6 and slightly burnt? If they're not your not pushing the drill hard enough for the drill to form a proper chip, if your not forming a proper chip it won't evacuate properly causing chip packing, chip packing is causing a non cylindrical hole which is why it wont gage correctly. The next issue would be the heat management. What coating is on your carbide tip? For A2 I would advise a AlTiN coating with through coolant. SFM= 230 IPR= .008 with no spot drill. A 140° tip angle is self centering and doesn't need it.
 
Yeah that's about 1/2 as fast as I would run my Sandvik 870 drill in A-2.
Why are you going so slow?
1518rpm and 10.9ipm is what I would run it at.
why so slow? i suppose im afraid of grenading a $500-700 drill lol. i'll bump up the feed and speed and give it a go. thanks
 








 
Back
Top