What's new
What's new

How true are drilled holes on a lathe?

Trboatworks

Diamond
Joined
Oct 23, 2010
Location
Maryland- USA
I have to drill two 3/8" holes lengthwise into a 3.5" long stick of brass on the lathe.
I need decent location and the bores to run true- how likely is just drilling them in going to be good?
The top hole is right through the length while the bottom one is 3" deep.
The bores will carry gear rack elements with a gear in-between so need to be on station well enough so that the gear run of ~1" will not bind.
The gear is 32 TPI 20^o.
The gear travel is at between 1.75 and 2.75" depth so at that location the bores need to be true enough for that 1" of run.

I have to check the shop but I am pretty sure I don't have a long enough bar in this size or if it would cut at that depth anyway.
Drill just under and then run a drill in at diameter?
Ream final?
Approaches to get these bores done well?
The get out of jail card is I can mill in the rack teeth at different depths just so it is under rod diameter so a bit closer bores can be accommodated- tight clearance on the gear/racks is not required so some engagement play I can live with.

Screenshot 2023-12-24 at 8.38.01 AM.png
 
Last edited:
Not too likely they'll be concentric if done with a twist drill. People tend to push it with brass also, and that aggravates drill wander. I'd plan on at least .005" of center on the through hole, proportionally less on the short one. But... you might get lucky!
 
Ah- I came to the right place.
I didn't even think of the mill and that is a much better ideal- I can have one clamp up and travel to the location to bore the second one.
I am running out to the shop to see what I have in tooling- I am pretty sure I have correct reamer and may have an end mill?
I skim shallow bores with end mills routinely but I am sort of a peasant- a no go for this depth?
The longer bore carries a sliding rack element in brass so needs a reasonable finish.

I will look.

The mill is a Deckel FP1 with a good quality DRO I would lay this down and use the Y spindle to bore.
 
Last edited:
How would you offset accurately in the lathe? 4-jaw? Not good. Start the holes with a boring head. Drill won't start accurate unless you've done this a lot. Reamer will just follow the drilled hole - reamers don't locate, they *size* an existing hole.
 
How would you offset accurately in the lathe? 4-jaw? Not good. Start the holes with a boring head. Drill won't start accurate unless you've done this a lot. Reamer will just follow the drilled hole - reamers don't locate, they *size* an existing hole.

Yeah- before enlightenment I was thinking four jaw and have to admit I was not confident with the PITA of locating holes - indexing stock straight etc .
In this instance I lacked courage and wisdom but thankfully realized that before wasting time and material.
Thanks for tip on boring to start and no I don't find myself needing to hit bores like this much and am no expert on dropping holes on really good location.
 
Last edited:
My biggest issue with getting nice a straight holes in a lathe is the tailstock is never that straight with the spindle. No matter how much I avoid trying to adjust it in hopes it will eventually fix it self, the problem never goes away.
 
Back before I had a mill etc etc (yeah, it's that old fart again) I'd use an angle plate on the lathe (easy enough to set the centres with a square edge and a job locks for the spacing,

Drill 23/64 then bore as deep as poss to leave say 0.005 for a reamer, then use that bored & reamed hole to guide a drill with the cutting edges dubbed and corners gently rounded, - which will stop dig in and wander, and cut ''tight'' then finish with reamer.

Just my 2 cwents, YMMV
 
Last edited:
My biggest issue with getting nice a straight holes in a lathe is the tailstock is never that straight with the spindle. No matter how much I avoid trying to adjust it in hopes it will eventually fix it self, the problem never goes away.
That is where a floating tailstock tool holder comes in handy. I believe that a 4 jaw chuck could do this job if certain things were done first.

Make sure that all long sides are parallel to each other and the ends perpendicular.

Spot drill one hole on a mill.

After indicating in the spotted hole on the lathe make sure to mark 2 jaws as reference so the other 2 are the only ones loosened and tightened.

Drill and ream that hole and then reverse the piece in the jaws and spot drill the second location before drilling and reaming.

I 100% agree with Limy that an angle plate would give better results than a 4-jaw.

I also agree with DanASM that a half round drill would follow the axis better after initial shallow drilling. That is how I drilled a small brass cannon casting years ago to make a miniature BP cannon. I made the drill out of drill rod per an old Popular Science article carefully honed it after hardening with a torch.
 
That bit of brass rectangle would nest quite nicely in the jaws of a 4-jaw chuck, so one can drill those holes on a lathe in two steps, one hole per step:

Put rectangle is the chuck displaced so the first hole is on the lathe rotation axis. Using a slightly undersized drill held on the carriage and well centered, spot-drill the start dimple, then drill the hole, then ream it to dimension. Flip bar over in the chuck and center such that second hole is exactly on rotation axis, drill and ream as for the first hole. As @DanASM suggests, given that this is brass, a dubbed or half round drill would be useful or essential.
 
Drill under size in the vertical mill, then bring to size with a boring head.

rnHpwOs.jpg
 
The mill is the right tool for the job, though it can be done on the lathe with enough care in setup. Finish by boring, as above. You'll want a boring bar that just passes the hold, given the depth. Finish pass of maybe 0.003" on the diameter, though others may suggest more or less.
 
More accurate spinning the work than the drill

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?
 
Last edited:
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?
RIDER ;- Assuming the tools are cutting as they should!!!

Don't forget a static single point boring tool can (due to machine alignment etc etc) bore a taper, a boring tool rotating around a fixed centre can only produce a straight bore
 
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?
I was always told that any drill wander changes the effective cutting angles on the tip. So one side takes a deeper bite than the other. Resulting force pushes or bends the drill sideways so the flutes on one side stop out a bit from the sides of the hole hence the hole is not only off a bit but larger. Doesn't help the the centre chisel edge off an ordinary drill doesn't actually cut.

Milling cutter is intrinsically stiffer and better behaved due in large part to the grinding process, if properly done, producing effectively identical cutting edges. Theoretically an accurate four facet grind ought to be almost as well behaved as a milling cutter. But an inaccurate four facet is going to wander.

Clive
 








 
Back
Top