Lets Get Basic- Drill Bits For Lathing

erichmatt said:
Sure drilling first then boring will get you a straighter hole than drilling but how are you going to bore a 3/8 hole that is 4 inches deep?
Click to expand...

One way would be boring bar. Boring bars don't always have to be single point, either.
Another way would be to plunge a 4 flute endmill. Need a clearance hole, usually, for 4 flute. Lots of long endmills out there.
Core drills are about as precise as reamers. Like a reamer, they'll tend to follow the hole, though. But they move material nicely.
Then there's always a gundrill. They make very deep and very accurate holes.
What are the feature requirements? Cylinder, diameter, etc.?
I guess it depends on several questions like material, how accurate, and how many $$.
Certainly not impossible.

Wrat
 
wrat said:
One way would be boring bar. Boring bars don't always have to be single point, either.
Another way would be to plunge a 4 flute endmill. Need a clearance hole, usually, for 4 flute. Lots of long endmills out there.
Core drills are about as precise as reamers. Like a reamer, they'll tend to follow the hole, though. But they move material nicely.
Then there's always a gundrill. They make very deep and very accurate holes.
What are the feature requirements? Cylinder, diameter, etc.?
I guess it depends on several questions like material, how accurate, and how many $$.
Certainly not impossible.

Wrat
Click to expand...

Most of those options require a hole to be drilled first and would benefit from have a relatively straight hole to start with.

A 4 inch long boring bar that is thin enough to cut a 3/8 hole is going to chatter like crazy and require a very light cut and slow feed. I looked on msc for long boring bars and the only one the comes close is one that has a minimum hole size of .360 in and a max depth of 3.125 inches. So it's not quite long enough, guess how much it costs? $339. More than a whole set of decent number, letter, and fraction drill bits. If you went for a boring bar that is supported at both ends with a tool cutter in the middle (like a line boring machine) you would have better luck but I can't think of a easy way to support both ends of a boring bar and hold the piece in a lathe. I am sure there are ways to do it but it would require a special jig or a whole different machine.

A gun drill would be great but I don't know anyone who has one let alone any one who would let me use it.

Cheap drill bits have their place. I am going to keep my cheap set for doing things that are likely to break a drill bit, like hand drilling in an awkward place or some other thing. If I am going to do something that pushes the limits of how accurate drill bit can be I am for sure going to use the best drill bit I have.
 
erichmatt said:
Most of those options require a hole to be drilled first and would benefit from have a relatively straight hole to start with.
Click to expand...
Not necessarily. Plunging an endmill only requires a clearance hole for the flute centers. It doesn't care how straight the hole is.

Look if I can help out a little, cool. You're obviously closer to it than me. But a few things i can tell you:

I have used boring bars of that length and smaller diameter. But then, that was in the days of more tool grinders and fewer purchasing agents. So no, it might not be readily available off the shelf because it probably never was.

I can also tell you it still comes back to material, feature, and tolerance, which we still don't know, and hey, it doesn't much matter if you tell me or not. But the entire process revolves around that. The entire process. If those are unknown, then the part isn't designed yet and no real requirement exists. If those are known, then the process is a simple matter or at least simple decision.

Granted, those factors drive price. So if you need 0.0001" over 4" in stellite, then it will cost more than 1.0" over 4" in white pine. This may sound obvious, but it's still inescapably the driver and the more we know about material, feature, and tolerance, the more we know about process and therefore cost.

And cost is not just $$. Because we know that Time = $$, we can then conclude that if you don't want to throw a lotta money at it, then you'll hafta throw a lot more time at it. There's no free lunch. Those are Rules of The Universe that cannot be changed.

If the tolerance is "the best hole i can put in with a drill bit i can buy" then you really don't have a question. Drill, baby, drill! Done and done. If there is no declared tolerance, then it's time to start understanding holes and other machined features. If the question is about "which drill bit?" then it's a discussion of superstition like asking "which is the best pickup?" or "what's the best beer?" Starts good arguments (uh... discussions ;-) but yields little useful information other than the identities of argument participants.

Regardless, none of this is new or unique and has been well-studied and published since before either of us were born.


Wrat
 
erichmatt said:
For a project I was working on recently I needed to put a 3/8 hole in the middle of a 4 inch long 1/2 inch piece of round. We were going to ream it later to get a more accurate size but the hole needs to be pretty close to down the center of the piece. Sure drilling first then boring will get you a straighter hole than drilling but how are you going to bore a 3/8 hole that is 4 inches deep? A reamer will give you a good size but it will want to follow the hole that was drilled. We could drill it crooked put it on a mandrill and turn the outside, or leave it long and turn it between centers put in the ends of the hole but those options are harder than drilling a straight hole to begin with. Drilling a straight deep hole with a bent drill bit probably isn't going to happen. Sure the mandril option or the centers option would probably give us better results than drilling with a good drill bit the good drill bit is good enough and takes less time.
Click to expand...
Drill from both ends with a 23/64" stub bit. Drill through with a 23/64" jobber bit. Ream to size.
 
John Hasler said:
Drill from both ends with a 23/64" stub bit. Drill through with a 23/64" jobber bit. Ream to size.
Click to expand...
Good idea, I would still rather use good drills to do that process rather than cheap ones.
 
erichmatt said:
A 4 inch long boring bar that is thin enough to cut a 3/8 hole is going to chatter like crazy and require a very light cut and slow feed. I looked on msc for long boring bars and the only one the comes close is one that has a minimum hole size of .360 in and a max depth of 3.125 inches. So it's not quite long enough, guess how much it costs? $339. More than a whole set of decent number, letter, and fraction drill bits.
.
Click to expand...

as someone else mentioned, The material and the tolerance are important. The tool geometry is also pretty important.

if the tolerances are tight, it must be bored, or bored and then reamed.

The cheapest way, would most likely be to buy a solid carbide bar like this one, and then braze/solder a cutting bit onto the end. The bar itself could also be ground into a solid carbide boring bar.
http://www.mscdirect.com/product/details/48611305

This thread shows a custom brazed bit.
http://www.hobby-machinist.com/threads/homemade-boring-bar.18364/


erichmatt said:
If you went for a boring bar that is supported at both ends with a tool cutter in the middle (like a line boring machine) you would have better luck but I can't think of a easy way to support both ends of a boring bar and hold the piece in a lathe. I am sure there are ways to do it but it would require a special jig or a whole different machine.
Click to expand...

You just clamp v blocks to the carriage (shimmed as needed), and then turn the bar between centers.


The third option, would be the Kelly Johnson (SR-71 designer) method, don't let the engineers design difficult to produce parts.
 
Last edited:
Right from Wikipedia:
  • The spiral (or rate of twist) in the drill bit controls the rate of chip removal. A fast spiral (high twist rate or "compact flute") drill bit is used in high feed rate applications under low spindle speeds, where removal of a large volume of swarf is required. Low spiral (low twist rate or "elongated flute") drill bits are used in cutting applications where high cutting speeds are traditionally used, and where the material has a tendency to gall on the bit or otherwise clog the hole, such as aluminum or copper.
Bill
 
planeflyer21 said:
Will it be straight?
Click to expand...
Fairly. The stub drills will make pretty straight holes (if they are good ones). The one on the entry side will act as a drill guide for the jobber-length one so that it will start straight into the middle section, which will be much shorter than the total hole length. The reamer will take out any irregularity under a 64th. I suppose you could drill at 11/32", core drill at 23/64", and then ream. That's a lot of operations, though, not to mention the cost of the core drill which you will probably never use again.
 
John Hasler said:
I suppose you could drill at 11/32", core drill at 23/64", and then ream. That's a lot of operations, though, not to mention the cost of the core drill which you will probably never use again.
Click to expand...

This was very close to the process we ended up using. We were making sleeves to repair very worn out valve guides that were part of the block. The first few we did stub drill and then the rest of the way with a jobber. It worked ok but could be better. Today we switched to stub drilling from both sides then finishing the middle with a longer bit. They came out quite a bit better, sighting through them you could barely see were the holes met. We then installed them and core drilled them and then reamed them to the final size. When we drop a valve in it bounces nicely so the new guide is lined up with the old seat.
 
You must log in or register to reply here.
Back
Top