Keeping a small hole on track?

BHolcombe · Dec 30, 2019

I have a task coming up in which I plan to bore a 3/32" hole. Normally I would do this with a carbide spade or other carbide tool that will not deflect much.

However, this hole is 1" deep and it's in an awkward location. End mill holders won't gain me enough space so I plan to use an Albrecht mini chuck. Only trouble there is that a chuck won't grip carbide.

So in situations like this what is your preferred method?

Thank you.

BugRobotics · Dec 30, 2019

What material are you boring and what is your hole tolerance?

Scottl · Dec 30, 2019

Bore/ream a hole in a piece of larger diameter stock to accept the drill and then mount that in a collet or milling holder. That will be more rigid than the chuck.

Might have to use something like permanent Loctite and then heat it to release the drill.

Thunderjet · Dec 30, 2019

BHolcombe said:
I have a task coming up in which I plan to bore a 3/32" hole. Normally I would do this with a carbide spade or other carbide tool that will not deflect much.

However, this hole is 1" deep and it's in an awkward location. End mill holders won't gain me enough space so I plan to use an Albrecht mini chuck. Only trouble there is that a chuck won't grip carbide.

So in situations like this what is your preferred method?

Thank you.

I would do the tool holder thingy as stated above, probably use brass as the holder.

1" deep isn't really that bad. Use a milling machine, spot with a known good spotter, and drill thru with a new .078 drill.

Then I would go as deep as you can(probably 3/16 or so) with a carbide endmill, then use your new 3/32 drill for the finish up thru.

If you need to be closer than that, you can find an old dull 1/8 carbide endmill and grind down the O.D. to your size, and it would probably get all the way thru the 1" depth.

Good luck.

guest · Dec 30, 2019

I do 3/32" dia. by 1.150" deep in SS all the time. I don't like the little carbide drills. I'd use cobalt unless it's some exotic material. If this is a BP job, you don't have the RPM for carbide anyway.

I like collet extensions to get a longer reach, assuming I'm not right up against a wall.

1/2 Straight Shank ER11 Collet Extension

WizardOfBoz · Dec 30, 2019

1" deep with a 3/32 hole is a 11 to 1 length to diameter ratio. For a boring bar, that ratio is pretty high. For larger holes you'd use a carbide devibrator type bar for up to 10:1. I'd be suspicious that the tolerances you think you are getting by boring would be lost by bar flexibility. At least one mfr (here) offers a carbide bar that would work for diameter, but specifies that the max hole depth is 1/2 inch.

To go back to another's questions and to add to them
1) What material (and what HT state) are you boring this hole into?
2) What are your tolerances?

Depending upon tolerances, I'd be tempted to use an undersize carbide drill to get the hole started, and to ream with a precision reamer. A drill-reamer might work, but I think that the flute length would be less than 1 inch, and you'd have to allow the drill to drill in more deeply than 1 inch.

Not sure if they make gun drills in 3/32. That might work, but given their length and your geometry constraints I think you may be limited to the drill and ream paradigm. Others have indicated how you might hold those tools.

Another approach to tool holding could be boring a slightly undersized hole in stock, then heating and allowing the thermal contraction to hold the tool.

BHolcombe · Dec 30, 2019

This is for an rotational alignment pin, so it must operate smoothly but the tolerances are not super tight. I'm planning to ream .003" oversize.

Drilling into aluminum.

That ER11 collet is brilliant, that will do the trick.

EPAIII · Dec 30, 2019

Why not? You aren't going to be using a lot of torque with a 3/32" bit. It should hold well enough to drill a hole in aluminum. I would at least try it before saying it will not work.

And you could use a diamond wheel or burr to make three flats on the shank, using a simple indexer. That would give you a positive grip.

BHolcombe said:
I have a task coming up .....<snip>.....

Only trouble there is that a chuck won't grip carbide.

.....<snip>.....

Cole2534 · Dec 31, 2019

EPAIII said:
Why not? You aren't going to be using a lot of torque with a 3/32" bit. It should hold well enough to drill a hole in aluminum. I would at least try it before saying it will not work.

And you could use a diamond wheel or burr to make three flats on the shank, using a simple indexer. That would give you a positive grip.

I've gripped, and milled with, larger carbide tools in an Albrecht chuck before when I didn't have the right collet. Not ideal, but it works in a pinch.

Sent from my SM-G973U using Tapatalk

BHolcombe · Dec 31, 2019

I may well give it a shot but wanted to have a backup plan in order and also given that I don't drill many accurate small holes I wanted to see what people are using for such things.

Terry Keeley · Dec 31, 2019

The 135* split point cobalt drills from Dormer are fantastic.

http://selector.dormertools.com/web...e-data-sheet.pdf/R10CO?searchaction=Technical

I did some very straight 2" long 3/32" holes in 6Al4V with them no problem.

CarbideBob · Dec 31, 2019

EPAIII said:
....
And you could use a diamond wheel or burr to make three flats on the shank, using a simple indexer. That would give you a positive grip.

Sometimes when "you can't get a grip" sandblasting the shank of the carbide tools works.

Mike1974 · Dec 31, 2019

Can you drill from both sides? We use .0635" carbide circuit board drills all the time to roughly 6x diameter. .093" sounds like a big step up for us.

If you can drill from both sides much more manageable. Maybe even drill undersize on one side, drill other side undersize, then bore (http://www.harveytool.com/ToolTechInfo.aspx?ToolNumber=35490) and ream to size

BHolcombe · Jan 2, 2020

This is a blind hole. I have another ‘long’ bore on the same part and I have been debating wether to bore both sides toward center.

I plan to ream to final sizes so very minor deviations in position should be manageable but I still hesitate to flip parts and add errors.

BHolcombe · Jan 5, 2020

Figured I would update this thread. One the larger of the two holes for this part I decided to bore the hole with a center cutting solid carbide mill then ream to size. Worked nicely.
That hole has a step to it that I will prep next, I bought a boring head (finally) for this purpose.

For the smallest hole I bought a solid carbide twist bit and reamers.

I recognize that reamers follow the path provided for them, but I suspect .125” is too small for the boring head.

I’ve been clearing chips with air as I bore and that’s been helpful.

This is what I get for designing the longest possible bearing support for a small part.

Limy Sami · Jan 5, 2020

FYI Internal Tool - All Lathe Tools

There are others.

BHolcombe · Jan 5, 2020

Thank you, nice to see that they do in fact make boring bars that small.

BHolcombe · Jan 16, 2020

The drill chuck worked fine for this task. The pin did not introduce any drag on the part, so happy with the result. I reamed for one thousandths clearance so I did have some room.

I do plan to add a small extension collet to my tool kit.

Keeping a small hole on track?

Aluminum

Stainless

Diamond

Stainless

guest

Guest

Diamond

Aluminum

Diamond

Diamond

Aluminum

Titanium

Diamond

Diamond

Aluminum

Aluminum

Diamond

Aluminum

Aluminum

Similar threads