How true are drilled holes on a lathe?

[triumph406]

More accurate spinning the work than the drill, caveat
New drill, properly ground,

Ok- I hadn’t known that.

In 40+ years never heard that.

----------------------

If it was me I'd set up the BP or VMC, drill undersize, straighten and locate the hole either with an endmill or boring bar, If the endmilled or bored holes are correct the drill has a fighting chance of staying straight.

 

[eKretz]

Holes drill straighter with the work doing the spinning, that is true. They drill even straighter with the work *and* the drill spinning. There are gun drills that use that setup. At any rate, if you want the straightest hole possible in any given setup, start the hole with the shortest, stiffest drill (preferably carbide) you can. Then switch to the longer drill. You can take a step up by substituting drilling undersize and boring the starter hole to the drill size. Of course, the straightest hole will be single point bored all the way through. But he didn't ask about that, he asked about drilling.

I would also add that you ought to monitor the pressure on the drill feed. If the drill is being pushed very hard it is very much more likely to drill a crooked/wandering hole. Even worse if it's a very long drill. A nice free-cutting point is much more likely to drill a nice straight hole.

 

[michiganbuck]

I would think that the slight wobble in a 4-jaw lathe chuck might wobble differently if the part had to be relocated for the second hole/bore.

So, I would mark the part sides to match them with the same jaws so the wobble might be similar.
but who knows if the holes would be parallel to the part sides.
On a BP (or other mill) one could indicate/tram the sides to be straight to near zero, and then only have to worry about the location.

One maght put a 6" long round part in the lathe 4 jaw, then indicate it for straightness in 4"of length to get a ball park idea of runout from wobble.

 

[Superbowl]

I like to drill from both ends. Spot, drill half way with an under size carbide drill (they are stiffer), then increase the hole size with a larger drill. Flip the work, spot, then drill with the smaller size drill until the holes meet, then use the larger size drill on the second side. Ream to clean up and come to size.

 

[boslab]

You can help a hole, pilot then ream a section about 1” deep, the pilot then helps guide the drill on its journey.
I think I read that in a Moore jig borer book ( a beautiful machine, even the scraping is art)
The deeper the hole the harder it is to control, there are drills like those fancy helical ones that can go 10+ x diameter easily, I’ve only used them once, but drilling thermocouple holes in a copper or beryllium copper mould, did not enjoy that.
Mark

 

[Joe Gwinn]

Ok- I hadn’t known that.

In drilling aren’t the cutting aspects of the flute which will cause wander equal in both approaches.
I am struggling to get my head around why it’s different.

My feeling has always been to use boring bars on the lathe or boring heads on the mill to get best and equal work while they differ- one being work spinning and other fixed.
Am I mistaken?

One way to think about the difference is to consider two cases where the drill starts slightly displaced from the desired path.

If the drill rotates and the work doesn't, the result is a cylindrical but off-location hole.

If the work rotates but the drill does not, there will be on average a very strong centering force trying to pull the drill towards the rotation center. If the offset isn't too large, most of the hole will be on the rotation center, but the entry hole will be bell-mouthed.

One can also rotate both, but in opposite directions. This is often done in traditional gun drilling. @eKretz makes this comment earlier (while I was typing.)

 

[Joe Gwinn]

I would think that the slight wobble in a 4-jaw lathe chuck might wobble differently if the part had to be relocated for the second hole/bore.

So, I would mark the part sides to match them with the same jaws so the wobble might be similar.
but who knows if the holes would be parallel to the part sides.
On a BP (or other mill) one could indicate/tram the sides to be straight to near zero, and then only have to worry about the location.

One might put a 6" long round part in the lathe 4 jaw, then indicate it for straightness in 4"of length to get a ball park idea of runout from wobble.

True enough, but no requirement on parallelism et al was stated.

 

[jim rozen]

This part honestly could benefit from a re-design.

1) put the brass blocks in the mill. Mill two slots across the block separated by your desired center distance of the shafts.
2) turn four bushings to fit the slots, two at each ends. Make the bushing ID equal to the shaft diameters.
3) solder or clamp (block across the top of the slots) the bushings to fix them in place.

Yes you will need to do some design work to get the bushing OD, ID, length just right. When you are done you can set the centerline distance within one thou easily, no extreme effort.