What's new
What's new

How to mill a 1.8504 bore with .0004+/-.0000 tolerance

plutoniumsalmon

Hot Rolled
Joined
May 27, 2014
Location
Los Angeles
Howdy.
I have a possible client asking me if I can cut apart for them that has this feature. The thickness is .75 and besides this its a pretty simple part. I do mainly art stuff thats feature rich but not super high tolerance. How do I even measure this. The material is steel.

Thank you
 

Attachments

  • .0004.jpg
    .0004.jpg
    7.9 KB · Views: 290
If I did that I would rough out, run a boring bar thru leaving .002-.003 and finish hone. If you don't have a hone you could bore the part taking light passes and checking after each pass. You obviously have to be confident you can measure that tolerance.

I make go/no go gages for very tight tolerances when honing or use a dial bore gage
 
That ID should be bored, not milled (/pedant), and measured with a .0001" reading dial bore gage checked against a precision setting ring (or, stacked gage blocks as per a current thread). And you have to watch part and measuring instrument temps to ensure they're not allowed to drift due to CTE.

Not a trivial part if you're mostly an artsy type, either come over to the grimy industrial side and buy some tooling, or farm it out to a proper job shop.

I should add that even surface finish matters with bores like this, a rough finish can give false readings that are meaningless as you're just contacting fragile "peaks" of the material, rather than a smooth, uniform surface.
 
You don’t mill such a bore. I mean, you can mill out or drill through or make the opening any way you like but to stay within four thou you climb the ladder of processes. Turning, reaming, EDM, honing, lapping, rolling. You measure with an internal micrometer which typically has three points. Plug gauges are more reliable, though.
 
47mm bore, could be a slip fit for a 6204 or 60005 bearing.

1.8504" is 47mm, so plus .0004 means most 6204 or 6005 bearings will slip into that bore without difficulty if the surface finish is good and roundness.
 
47mm bore, could be a slip fit for a 6204 or 60005 bearing.

1.8504" is 47mm, so plus .0004 means most 6204 or 6005 bearings will slip into that bore without difficulty if the surface finish is good and roundness.

I asked. Does slip fit really have to be this precise. I did other stuff that had bearings and it was not that exacting.

Ok. Apparently its for one of these Keyless Bushings - Straight | MISUMI | MISUMI USA
 
Well, that's silly - the whole point of a bushing like that is to have a fair bit of "wiggle room" when connecting a shaft to a pulley or other bored item. Should allow for a +.005" on the bore and still be fine, crazy to ask for +.0004" on that.

OK, just checked here: http://www.tribology-abc.com/calculators/iso_holes.htm and with the 47mm bore an H7 tolerance gives +25u, or .001". Still close, but not .0004" close.
 
I'm guessing it's a Bridgeport you have...gonna need a boring head and a inside mic that probably costs way more than the part lol...unless you have a cmm, in that case have at it.
 
If it were me, in my primitive garage shop, I'd make a plug gage or two, measured with a good mic. Then I'd bore the hole, the hard part being the resolution of the adjustment of my boring head. I'd get within the tolerance, but just barely. It would be way better to do it undersize by 0.003" or so and have somebody hone it. It's an easy job for somebody with a micro-adjust boring head, but you probably don't want to pay for that.
 
If the part is not long... (which it probably is) (don't know).


Plutonium Salmon has an Okuma LB 3000 EX II lathe/ turning center… If it fits on a face plate etc. would it not be more accurate to use his turning center to make the bore (+ better surface finish) than a comparatively more rickety mill (+ more spindle runout) doing said "boring" operation (to said tolerances).


Maybe I'm missing something here ?

@Salmon how many pieces ?
 
0.0004" == 0.01 mm.
That is easy, and any excellent modern tool or average cnc machine can do that as-is.

Industrial diamond-plated hones size car engine bores to better than 0.01 mm, quantity 300.000 per year, one tool.
A 15 sec op.

Any decent cnc machine can bore, or interpolate, a shallow hole == 40mm++ to less than 0.01 mm TIR error.
 
If the part is not long... (which it probably is) (don't know).


Plutonium Salmon has an Okuma LB 3000 EX II lathe/ turning center… If it fits on a face plate etc. would it not be more accurate to use his turning center to make the bore (+ better surface finish) than a comparatively more rickety mill (+ more spindle runout) doing said "boring" operation (to said tolerances).


Maybe I'm missing something here ?

@Salmon how many pieces ?

Nah. Not missed. You're onto it. Tolerances are but a small part of it all.

Where one has "scarce resources" - tooling, metrology, and experience included, a good lathe, single-pointing, is the sneaker-upper-on of choice for round stuff. Always has been. Time and tedium substituted for money invested. Making yer own ID gages even for but the one part, 'coz good OD metrology is all you presently own, etc.

And then.. how many do they want THIS time, how many will they want in the next 6 months? What's the future prospect for more of this work in the next several years? What sort of deadlines and turnaround times apply? Is there product liability exposure?

Can you even recover your COSTS?

Do you want to chase that type of work AT ALL?

If those are not a "fit", just send it out or refer the client directly to someone who IS set up for all that stuff, same as you would if they asked for open-heart surgery.

(Or so one hopes.. yah gotta know hobbyists..).

:)

"Beyond my current resource set", is honesty, not cowardice.

Don't waste your time or the client's time.
 
Just rough it as close as you can and give it to a honing shop to finish.
Not only is it a close tolerance to hold and you also have to have the equipment to inspect it. A hone shop has all that. To those that suggested plug gages, how do you know your hole is round? It could be out of round and out of tolerance.
 
Just rough it as close as you can and give it to a honing shop to finish.
Not only is it a close tolerance to hold and you also have to have the equipment to inspect it. A hone shop has all that. To those that suggested plug gages, how do you know your hole is round? It could be out of round and out of tolerance.

"Honing shop" will give you a serious invoice, too!

:)

Plug gages are one of the FIRST type yah learns to MAKE! And "vet". And use. Because you CAN.

Most ever'body gets hands onto decent 0-1" and 1-2" and, and . OD mic's early-on. Still "at school", even.

Good ID mics, only later. Proper bores gages later yet, if ever.

And they are sore harder to get true readings from, quickly.

Learn to USE bespoke ID gaging and consistent holes get easier.

You got the lathe. You got good OD metrology. You don't need enough metal value in it as would buy a cheap lunch.

Sanity check:

Just how much pickier is a bearing or shaft going to BE than a decent DIY plug gage, anyway?
All b'long "right circular cylinder" tribe, hair and eye colour notwithstanding. Tapers, to a different race - truncated right-circular cones.

And while steels don't wander around aimlessly with the weather quite as much as shiney-wood, all metals still do MOVE too, yah?
 
Good boring head and Sunnen GR9121 bore gage you should have no problem doing this part.
 
Good boring head and Sunnen GR9121 bore gage you should have no problem doing this part.

Large enough bank balance of "play money", and yer Mistress's prior-relationship kid could just hire a few thousand done as interesting ballast for a Feadship motor yacht, too.

Other times it is all about getting a job done with the resources one HAS.

Not the ones one WISHES they had.

More than one way to prevail in business, and a sore DEVIOUS lot, PM'ers can be!

Some weeks it seems y'all keep coming up with "nice to have" s**t just to drive yer competitors broke buying more tools!!!...

:)
 
i measure bore with a indicating bore gage set to a ring gage or use gage block with gage block jaws
.
preferably you would want a short length boring bar devlieg ones i prefer a spring washer as its easier to fine adjust roughly .010 range. they sell gear fine adjust type which is easier to set to .0001" normally. just saying some types are a lot easier to fine adjust
.
1) shallow test bore -.005" and meassure
2) bore full depth -.005 and measure
3) shallow test cut -.002 and measure
4) bore full depth -.002 and measure
5) shallow test cut to size
6) bore full depth to size
.
devlieg boring bar - Google Search
 








 
Back
Top