# Drilling a straight hole



## Mitch Alsup (Jun 17, 2021)

Hey guys,

I need to drill a straight hole through 3/4" 6061 T6 aluminum. Dead straight.
The hole needs to be about 0.201 and there needs to be a 0.246 hole on each end of this hole 0.183 deep. 0.246 allows for a thumb press fit of a small ball bearing in the hole.
Although I do have a boring head, I don't not have anything small enough to bore the hole.
I do have drills of the appropriate size.
The 0.201 hole is simply clearance to the 0.125 shaft--anything from 0.140 through 0.230 would work just fine.
The 0.246 holes on each end are for a press fit ball bearing
The pair of holes have to be less than a couple of tenths from absolutely normal to the aluminum bar.
I have tried this more than a dozen times and not gotten any closer than 0.001,8.

The location to put these features is determined off of two bored features, moved to the edge of the bar with a machinists rule and scribe, taken down both faces with the machinist rule. The thickness of the part is measured with micrometer, the edge picked up with a edge finder, and the spindle moved ½ the edge finder and ½ the thickness. The spindle is moved to the scribe line with a center finder and verified that the center of the finder touches the scribe line. To my not so trained eye, the scribe lines are within a thou (often better) as they traverse the edge.
I start with a #2 center drill, drill half a bit more than ½ way with 0.201, drill the 0.246×0.183

I have tried both drilling all the way through and drilling ½ the way through both fail by about equal amounts

The head is trammed to less than 3 tenths over 18 inches and a fly cutter cuts true with just a scratch on the back side.
I suspect the drill is wandering as it traverses the 3/4" rod.

What do I need to do to make this set of features ??


----------



## Ulma Doctor (Jun 17, 2021)

A drill bushing and a fabricated drill fixture can reduce drill drifting


----------



## Ulma Doctor (Jun 17, 2021)

duplicate post


----------



## benmychree (Jun 17, 2021)

Drills are not precision tools to the extent that you require them to be, that sort of accuracy can be attained only by boring.


----------



## tq60 (Jun 17, 2021)

Get a stub or screw machine length.

Or, cut your drill so only 1 inch or less of flutes are left and share correctly and or cut shank of bit so you can place it in your Chuck with only 1 inch or less extended.

This way the bit cannot bend.

Drill one side only.

Last option is locate an end mill that is end cutting smaller than your hole.

Drill first with small drill to remove excess then use end mill.

Ream to final size.

Sent from my SAMSUNG-SM-G930A using Tapatalk


----------



## JimDawson (Jun 17, 2021)

Yup, what @tq60 said. ^^^^^^^


----------



## RJSakowski (Jun 18, 2021)

I am curious as to how you will determine the hole is straight to better than .0002".  Also, are you talking about straightness rather than perpendicularity?  Dealing with the kind of dimensions and tolerances you are talking about, I would never use a rule and scribe for layout,  In the past, I did a lot of that type of layout and +/- .020" was a reasonable expectation.  

A better drawing would be useful, as would a description of intended use, if possible.  Many times changing the machining order can simplify the task.


----------



## jmkasunich (Jun 18, 2021)

If this is something where you control the design I'd look for flanged bearings so you don't need the reduced diameter in the middle.  Then just drill thru undersized and ream to fit the bearings.

If you have a boring head that can hold 3/8" shanks and you have an old 1/4" HSS endmill with a 3/8" shank you can bore it.  Just grind one flute off of the endmill and orient it so that the other flute cuts like a boring bar.  But aligning the bores in both sides of the part will be very tricky - hence my preference for boring or reaming all the way thru in one setup.

If you are talented at tool grinding you could remove all of one flute and all but the first 1/4" or so of the other flute, then give the upper edge of the remaining flute segment some axial relief.  The resulting tool could bore the upper recess to the proper diameter using the original cutting edge and clockwise rotation.  Then wind the boring head toward the center enough to pass thru the smaller hole (I'd make it as big as possible), move down so it sticks out the bottom of the part, reverse the spindle rotation, and bore upward to make the back hole.  Gradually wind the boring head back out until you reach the setting that gave you 0.246 on the top recess.


----------



## Karl_T (Jun 18, 2021)

Is the part too big to mount in a four jaw chuck on your lathe?

lathes excel at accurate diameter bores.


----------



## RJSakowski (Jun 18, 2021)

jmkasunich said:


> If this is something where you control the design I'd look for flanged bearings so you don't need the reduced diameter in the middle.  Then just drill thru undersized and ream to fit the bearings.
> 
> If you have a boring head that can hold 3/8" shanks and you have an old 1/4" HSS endmill with a 3/8" shank you can bore it.  Just grind one flute off of the endmill and orient it so that the other flute cuts like a boring bar.  But aligning the bores in both sides of the part will be very tricky - hence my preference for boring or reaming all the way thru in one setup.
> 
> If you are talented at tool grinding you could remove all of one flute and all but the first 1/4" or so of the other flute, then give the upper edge of the remaining flute segment some axial relief.  The resulting tool could bore the upper recess to the proper diameter using the original cutting edge and clockwise rotation.  Then wind the boring head toward the center enough to pass thru the smaller hole (I'd make it as big as possible), move down so it sticks out the bottom of the part, reverse the spindle rotation, and bore upward to make the back hole.  Gradually wind the boring head back out until you reach the setting that gave you 0.246 on the top recess.


You can't reverse spindle rotation.  Your cutting edge would be trailing.


----------



## jmkasunich (Jun 18, 2021)

RJSakowski said:


> You can't reverse spindle rotation.  Your cutting edge would be trailing.


You're right - total brain fart on my part.

If you can't change the design to allow for boring all the way thru, you have to either grind a back boring tool from scratch AND be able to measure the back bore as you bring it to diameter without messing up your setup, or you have to flip the part.

Making a boring bar from an endmill would still work for boring the top recess.

Drill about 0.220 all the way thru, then bore to 0.230 all the way thru, and then bore the upper recess to 0.246.  Since the 0.230 and 0.246 are bored in the same setup they will be concentric.  Flip the part over and indicate it in using the 0.230 bore as your reference and then bore the bottom recess (which is now on the top).

The important part in this project is to stop thinking about drilling an accurate hole.  There is no such thing as accurate drilling.  If you need accurate diameter, you need to ream or bore.  If you need accurate location, you need to bore.


----------



## Papa Charlie (Jun 18, 2021)

To get the accuracy that you desire for the bearings, you will need a ream. Drill undersize and then use the reamer to final dimension. 

As for drilling the shaft I would purchase several drill bits. From very short to aircraft length. Start with a center drill to give the bit a good start. When drilling, you will need to not drive the drill but let the drill drive. Pull often and clear the chips, it does not take much in chips to throw the bit off. Do not let the bit get too warm or the base material. Once you have drilled the length of the first bit, then switch the second and repeat and follow up with the aircraft, again repeating the process. 

It is possible to drill from both sides if your fixture is good enough to allow you to flip the part and the hole is centered from top to bottom.


----------



## Mitch Alsup (Jun 18, 2021)

RJSakowski said:


> I am curious as to how you will determine the hole is straight to better than .0002".  Also, are you talking about straightness rather than perpendicularity?



I am really concerned with the perpendicularity, not straightness. You are correct, here. Sorry for the poor description.



> Dealing with the kind of dimensions and tolerances you are talking about, I would never use a rule and scribe for layout,  In the past, I did a lot of that type of layout and +/- .020" was a reasonable expectation.
> 
> A better drawing would be useful, as would a description of intended use, if possible.  Many times changing the machining order can simplify the task.



The bar is going to be an unequal length balance beam. I did a couple of these (6) a few years ago for a telescope I was building and every single one was "crooked" usable but crooked--visibly crooked from 20 feet away.

The harder part is to get the bearing axis such that a shaft can be inserted  with the bearings held in circumferal tension in the holes* and the shaft held in circumferal tension in the bearing races** -- or else I have to figure out how to put a 2-56 threaded hole in 4140. When I did this for my previous telescope I had to lap the 4140 down until it had a slip fit through the bearings in order to get the bearings to turn at low force levels. This is to be a balance beam where I want a strand of hair to move the beam under gravity on the strand of hair. "delicate"

(*) I did experiments and 0.246 is enough to hold the bearings in the holes and I can press the bearings in using my thumb as a press.
(**) My ground 4140 rod actually measures 0.125,2" and I will likely have to lap it down to fit the bearing inner race anyway.
But if the two bearings are not absolutely square with respect to each other the shaft will not turn at low friction levels.

If you look at the attached picture, you can visually see that the balance beams are not exactly 120º and the points of mirror support are a couple of hundredths from where they should be.


----------



## jmkasunich (Jun 18, 2021)

Mitch Alsup said:


> The harder part is to get the bearing axis such that a shaft can be inserted  with the bearings held in circumferal tension in the holes* and the shaft held in circumferal tension in the bearing races** -- or else I have to figure out how to put a 2-56 threaded hole in 4140. When I did this for my previous telescope I had to lap the 4140 down until it had a slip fit through the bearings in order to get the bearings to turn at low force levels. This is to be a balance beam where I want a strand of hair to move the beam under gravity on the strand of hair. "delicate"
> 
> (*) I did experiments and 0.246 is enough to hold the bearings in the holes and I can press the bearings in using my thumb as a press.
> (**) My ground 4140 rod actually measures 0.125,2" and I will likely have to lap it down to fit the bearing inner race anyway.
> ...


This looks like it will be lightly loaded.  Might be a good candidate for retaining compound, something like Loctite 609.




__





						LOCTITE 609
					

High strength methacrylate ester acrylic retaining compound designed for the bonding of cylindrical fitting parts.




					www.henkel-adhesives.com
				




Lap the shaft until the bearings are a nice light press fit.  Put the bearings on the shaft.  Drill then bore or ream the aluminum part a couple thou oversized so the outer races are an easy slip fit.  Insert the shaft with bearings and apply a drop of 609 to each outer race - it should wick around and lock the outer races in place while allowing the alignment to be driven by the shaft only.  609 can easily fill a gap of 0.002 or more.

Update:  looks like Loctite 630 or 620 is better for this application - they are designed for slip fits.  Gap fill up to 0.2 or 0.25mm (0.008-0.010").  Also, after looking at the Tech Data Sheet, seems like it is better to pre-apply rather than adding after and hoping it wicks around.  Just make sure it doesn't get inside the bearings


----------



## RJSakowski (Jun 18, 2021)

An interesting project.  The "weight of a human hair" presents a pretty tough requirement.  I would think that bearing friction would be a deal breaker. 
Something to consider would be a different bearing mechanism.  A jeweled bearing as used in mechanical watches or microammeter movements might prove to have less friction.  If they aren't capable of carrying the load, another mechanism might be a knife edge.  Old dual beam analytical balances use agate knife edges and have sensitivities to better than .1 mg.


----------



## Mitch Alsup (Jun 18, 2021)

RJSakowski said:


> An interesting project.  The "weight of a human hair" presents a pretty tough requirement.  I would think that bearing friction would be a deal breaker.
> Something to consider would be a different bearing mechanism.  A jeweled bear as used in mechanical watches or microammeter movements might prove to have less friction.  If they aren't capable of carrying the load, another mechanism might be a knife edge.  Old dual beam analytical balances use agate knife edges and have sensitivities to better than .1 mg.



I got the 13" telescope beams to respond at the "strand of hair level" with the shaft in the bearings a cozy slip fit. I could not get the bearings that responsive if the shaft was not a slip fit. So, this tells me the bearings are capable of "getting it done" if I can get them positioned properly.

Also note, the beams are going to be dynamically balanced so if set to point horizontally and moved to another orientation the beams do not move under the influence of gravity necessarily.

This is an experiment in the "how low of friction can one build a telescope mount to". There is every reason to believe that the telescope will end up working even if I miss my target by a factor of 10.


----------



## Mitch Alsup (Jun 18, 2021)

jmkasunich said:


> This looks like it will be lightly loaded.  Might be a good candidate for retaining compound, something like Loctite 609.
> 
> 
> 
> ...



My other idea was to make 2 bearing housings and mill a slot in the beam and use screws to set tension between the housings to hold the bearings while checking the friction on the shaft. Then it becomes an assembly problem rather than a machining problem.

But thanks for the 609 reference.


----------



## Zack (Jun 18, 2021)

Karl_T said:


> Is the part too big to mount in a four jaw chuck on your lathe?
> 
> lathes excel at accurate diameter bores.


Yeah I was going to say that.  Chuck it up in a lathe and go after it with a little boring bar.


----------



## Mitch Alsup (Jun 19, 2021)

So, for fun today, I drilled a hole with a 2-flute 3/16 end mill from "Little Machine Shop". Hole was drilled nice and slow at 1120 RPM.

The hole ended up where a 0.205 drill would fit in it with negligible slop, a 0.204 drill with significant slop.
For the math challenged, 3/16 is 0.187,5"

The hole also ended up about 1º off of normal.

Grrrrrrrrrrrrrrrr..........


----------



## Iceberg86300 (Jun 19, 2021)

Mitch Alsup said:


> My other idea was to make 2 bearing housings and mill a slot in the beam and use screws to set tension between the housings to hold the bearings while checking the friction on the shaft. Then it becomes an assembly problem rather than a machining problem.
> 
> But thanks for the 609 reference.


You can press one bearing in & clearance fit the other. Use a cap on the clearance side to pinch the bearing in place after you get it into the position that allows the bearing l bearings to run sufficiently free.

Retaining compound was my thought before you explained the application.

Otherwise, back boring in whatever fashion you can manage would be the ideal operation if you didn't want to shift this to an assembly issue.

Are the tolerances & sizes you've come up with from the bearing manufacturer?

They might have something with a larger clearance that is more forgiving.

Sent from my SM-N975U using Tapatalk


----------



## Mitch Alsup (Jun 19, 2021)

Iceberg86300 said:


> Are the tolerances & sizes you've come up with from the bearing manufacturer?



In true hobbyist form, I bought a bunch of bearings, and fiddled around with them until I got a nice low friction setup. Now repeating is the hard part,

The bearings are likely from an R/C racing car/truck application.


----------



## Flyinfool (Jun 20, 2021)

How accurate is your machine?
What is the run out of the mounting system you used for the 3/16 end mill?
Even center cutting end mills are not real good at center cutting. You are better off drilling a clearance hole first and then coming in with the end mill. The clearance hole for the shaft does not need to be close to the shaft size, The bigger the through hole the stiffer the drill and the straighter the hole. Drills are not accurate enough for precision fits of bearings. Ream or bore is the only way close enough, repeatably.
Once you have located the hole, LOCK the X and Y axis to be sure the table does not move. You would be surprised at how easy it is to bump a table a few tenths with just your hand. To try to do the 2 sides from each side would require a precision ground bar to start with and an incredibly accurate setup. As mentioned above your best bet is to do both bores from one side. Better would be to put the bearing bore all the way through from one side and use flanged bearings. If the bearings need to be flush then C'bore for the flanges. You can buy little solid carbide micro grain boring bars that will bore a hole that small. You may have to make an adapter sleeve to fit it into your boring head.

I doubt if any piece of AL stock is as square as you need. You will have to make the material square before you can put in a hole square to a specific surface. Right now you are making a hole square to one of the faces of the vise and then drilling a different surface and hopping it comes out square to the surface that is not indicated in. It does not take much of a piece of dust between any of the parts involved to make for .0003 of misalignment. Any slight nick or scratch can also put you out by .0003. Even though the table is trammed to .0003 over 18 inches how accurate is the reference surfaces of the vice on that table, then how good are the parallels that are setting the height of the bar. You are working thru at least 7 surfaces that all have to be clean and perfect as each one can add some small error to the final setup. All those little errors add up and show in the final part.

I also would be interested to know how you are measuring the accuracy of your hole?


----------



## SLK001 (Jun 20, 2021)

I'd use a center drill to drill this - much less deflection.  You have to clear quite often, but once the body is inside the hole, a center drill tracks true.


----------



## RJSakowski (Jun 20, 2021)

Sixteen years ago, I had a need to make this part.




While perpendicularity was not a specified requirement, it was implied by virtue of the requirement that the two .008" diameter holes in the c/bore intersect exactly.  This was accomplished by using an RT mounted vertically so the the work could be rotated 90º for machining four sides.  Additionally, I could face the side parallel to the table surface, enabling machining five axes on a single setup.  The sixth face was machined in a second op.  

Extreme care was taken in setting up the RT to ensure that RT axis was parallel to the x axis ways and the surface vertical.  The task was made easier due to the use of a newly installed three axis DRO.  To accomplish the task, an Excel spreadsheet was set to exactly specify each of the 75 steps in the order of work, including tooling, orientation of the work, and machining distance.

While your part is different, the same approach could be used.  An over sized bar could be mounted between centers on the RT and the tailstock, faced on four sides and the c/bore and through holes machined.  Then rotate the RT 90º and machine the bearing holes.  The work would be removed and the end faces machined in a separate op.


----------



## Iceberg86300 (Jun 20, 2021)

Mitch Alsup said:


> In true hobbyist form, I bought a bunch of bearings, and fiddled around with them until I got a nice low friction setup. Now repeating is the hard part,
> 
> The bearings are likely from an R/C racing car/truck application.



Not just hobbyist form!! It happens A LOT on the professional side as well.

I only know to ask b/c of the countless bearing catalogs & engineering guides I've poured over as a machine design engineer.

The hobby grade bearings you have are likely nothing special at best, atrocious at worst, and if it's the latter it's entirely possible for high precision low tolerance work to actually cause problems.

What you have is likely ABEC 1 or the equivalent p0 on the scale used by everyone but ABEC, and normal clearance of CN/C0.

For an ABEC 1/p0 bearing of your size the ID & OD tolerance is roughly +0 -.0003" (8 microns), and center of the unassembled normal clearance range is roughly .0002" (range is 2-13 microns).

As you can imagine there FAR more specs. Runout, width, possible taper, etc, etc. To make it more interesting p grades don't go in order. It's p0, p6, p5, p4 in order of increasing precision. Internal clearance increases C2, CN, C3, C4, C5.

For your app I'd probably spec unshielded p5/ABEC 5 instrument bearings, which comes close to halving p0 tolerances. Clearance grade would be determined by how accurate you can get the bore.

With that said, you've already proven that what you have will work, but I just don't know if you'll be able to get away with removing the inherent adjustability you have right now. Also, if you're in a clean environment I'd pull the shields & clean the grease out & switch to oil if you haven't already. But that does come with the trade-off of requiring regular lubrication & cleaning depending on environment & any sealing/shielding you can add.

A bunch of fine suggestions have been given to get the geometry your require for the current design, but the capabilities at your disposal, I'd probably go with something like this:

Which would allow you machine everything in one setup. Bore hole for a slip fit & get locating shoulder inside the bar & face off the top + drill & tap holes to accommodate a cap.

Turn shaft in one setup to get a shoulder to locate both bearings & ensure the features share the same datum. Not sure on press fit here. Probably go with a slip to maximize the amount of alignment error that you can handle.

Assemble it all using a cap & VERY light wave washer if you can get away with it. Or not. Probably an assembly time decision. Or just leave it out if this doesn't need to be captured.

Hopefully the description with drawing make it a little more clear.
	

	
	
		
		

		
			





Sent from my SM-N975U using Tapatalk


----------



## RJSakowski (Jun 20, 2021)

One source of better grade of bearings is the motors from computer hard drives or floppy drives.  For smaller sized bearings, laptop hard drives would be a good bet.


----------



## Mitch Alsup (Jun 21, 2021)

Iceberg86300 said:


> The hobby grade bearings you have are likely nothing special at best, atrocious at worst, and if it's the latter it's entirely possible for high precision low tolerance work to actually cause problems.



Nothing special, but I got 100 of them for maybe $10.00 and about 1/10 does not turn with adequate smoothness so it gets tossed.


----------



## Boswell (Jun 21, 2021)

Mitch Alsup said:


> Nothing special, but I got 100 of them for maybe $10.00


Well at 10 cents each, at least you only have your time invested when if you can't get them to work.


----------



## nnam (Jun 22, 2021)

I am wondering how you established 1 degree off  perpendicular.  Drill bit point not centered also cause the problem, as well as bent drill bit.

I wonder if you considered carbide bit instead of HSS bit.
In addition to your suggestion of adjustable bearing location, 3 more things I would like to add.

1.  Did you check the alignment of your milling table and the head?
2.  How about drilling a bigger hole, the use epoxy to sit the bearing to make it lined up perpendicularly, similar to your screw adjustment  method.
3. Make a powered rotating vise while drilling with a hard bit or boring bar. (crazy idea).  This may work with a lathe and a drill holder.


----------



## Mitch Alsup (Jun 22, 2021)

nnam said:


> I am wondering how you established 1 degree off  perpendicular.  Drill bit point not centered also cause the problem, as well as bent drill bit.



I found a 0.204 drill loose, and a 0.205 drill properly snug (the 0.209 drill did not fit). 
Then I used a 45º angle plate (the 90@ corner side) and looked at the drill bit sticking up.
.....if fell away on one side
.....it was nearly coincident on the other.



> I wonder if you considered carbide bit instead of HSS bit.



I had a HSS end mill in 3/16 (although it drilled a 0.205 hole ?!?!) I did not have anything in cobalt nor carbide in that size.



> In addition to your suggestion of adjustable bearing location, 3 more things I would like to add.
> 
> 1.  Did you check the alignment of your milling table and the head?



head is trammed to table within 0.000,3 over 15" reach side to side.
In the distant past, the vise on the table trams out in the 0.00,3 range on the surfaces that hold parallels.
I have not trammed the vise on the rotary table.
I was tappy-tap-tapping the part onto the parallels and the parallels were tight..



> 2.  How about drilling a bigger hole, the use epoxy to sit the bearing to make it lined up perpendicularly, similar to your screw adjustment  method.



This may end up being the fall back point, but thanks for mentioning epoxy, I had not thought of that--and it seems and easy way out.



> 3. Make a powered rotating vise while drilling with a hard bit or boring bar. (crazy idea).  This may work with a lathe and a drill holder.



I am not at the stage in my machinist hobby where a boring bar small enough for these features would survive long enough to be worth the money.


----------

