circular interpolation of small deep holes

[rchprks]

help!
our die designer has declared that i should be able to interpolate a.250 hole 1.5 inches deep location +-.0005 with no taper. using .188 4 flt carbide e.m.2" long matierial is boiler plate. is this possible ?

[HuFlungDung]

If he is trying to establish position, just rough drill it full depth with .156 drill, redrill it again with the extra long .188 endmill to straighten it up a bit (like a boring operation in case the drill wanders), redrill again with the .236" to full depth then interpolate the top 1/2" of depth with a regular length endmill for position accuracy. Leave .005 at the top to ream, and finally ream to full depth. This should get you a pretty good hole in all respects.

[little bubba]

No offense, but your die designer sounds like an idiot. You probably could do it, but why? I guess it could be done with a slow enough feed and a couple of spring passes.

I think Hu flung went a little overboard on getting position. I find that a heavy fed drill tends to walk more than a light fed one, and also HSS tends to walk more than carbide. I would use a D carbide drill with a light feed of about .002-.0025 per rev and then ream it.

I couldn't even fathom trying to interpolate that, I would invite the designer down to the shop floor and have him show you how its done.

[HuFlungDung]

I dunno, a half thou accuracy for a hole position requires some pretty careful work. Where a drill feels like heading is a crapshoot, and must be followed by a boring operation before reaming, if you expect the hole to be vertical after you are done.

[motomitch1]

The big dogs would spot drill,drill.236,then it would be qualified or bored to .243-.245 using a under size or reground carbide endmill,and reamed .250.

Are jig grinder

[little bubba]

I'll give you, .0005 on position is tight, absurdly tight, but is boring with an endmill really going to be any better than an easy feed with a carbide drill? Assuming the machine is good on postion, little to no tool runout etc.. I can sort of see drilling twice, but why the endmill? I've found that a very light feed on a carbide drill will give the same result. I'm not trying to argue, just trying to gain a little knowledge.

[DieGuy]

This sounds like a job for a Jig Grinder. That designer is smoking crack (pretty good quality crack I might add). If it has to control size for full depth and position (location and geometry), the Jig Grinder is the only way to really get those tolerances, the reach is just to long for much else.

[HuFlungDung]

Originally Posted by little bubba I'll give you, .0005 on position is tight, absurdly tight, but is boring with an endmill really going to be any better than an easy feed with a carbide drill? Assuming the machine is good on postion, little to no tool runout etc.. I can sort of see drilling twice, but why the endmill? I've found that a very light feed on a carbide drill will give the same result. I'm not trying to argue, just trying to gain a little knowledge.

My thoughts are that the lands of the drill flutes have no cutting clearance, so if there is any deflection, the drill is unable to correct its position because the flutes cannot cut sideways. So any slight deflection builds on itself and gets steadily worse.

So if you open the hole with a drill, then drill it with an endmill, this emulates a boring action because the endmill is not constrained to follow a crooked hole. The sharp cutting edges on the flutes of the endmill can and will cut through the unequal wall thickness conditions of a wandering drilled hole.

[little bubba]

HuFlung The relief thing makes sense. Just finished running a job on the worst castings ever seen, literally. .375-.381 holes, .010 on position and they decided to cast the holes into the part, .010 undersize. Needless to say, these holes are not straight, not on position and far from round. In this instance, picked up visually on one hole as zero with a .374 pin in a tool holder and then plunged with a 3/8 endmill, chamfered excessively, and then reamed really slow to .378(needed a tight tolerance on the hole for a 2nd op). To me in this instance the endmill made sense, interupted cut, porosity, hard spots, did I mention that a 3 year old could make better castings.

For the OPs application, I can see where you are coming from, but I think that a carbide drill, short as you can get it, on a tight rigid machine, fed light will give you a nice straight hole, as long as there isn't any crossholes or anything.

I'm going to file your suggestions away in my might need it some day file.

[Dan Fritz]

I think HuFlungDung is giving some good advice. You may be able to hold a pretty close tolerance with a short carbide drill, but any drill point can be slightly asymetrical, causing some drift. Even a drill that's ground perfectly can still run off-center due to errors in the tool holder. This can cause your spindle to wobble if there is any bearing play or if the tool holder's taper isn't perfect.

I was always taught that you should bore for position & straightness, ream for size, and use a drill to just make a hole someplace. An endmill comes pretty close to the performance of a boring bar, although there can be problems with endmills too. Basically, you want to sculpt a hole around the theoretical axis of rotation of the spindle without putting much sideways pressure on the tool or the spindle. A single-point boring tool taking a light cut does that best on a machining center. A gig grinder is designed to give the best possible hole location, but they're pretty slow by comparison.

For that tight a location tolerance, I'd drill first, then endmill (or bore), then ream if you need to to get the size you want. I'd also look to see if your CNC control has a "uni-directional positioning" feature. Uni-directional positioning always approaches the position from the same direction in each axis, even if it's got to overshoot the position and back up. It removes some positioning errors due to backlash, ballscrew wind-up, and stick-slip. Some Fanuc controls use G60 for this.