[4]

How to accurately bore on the lathe?

[3]
[10] Like what you see?
Click here to donate to this forum and upgrade your account!

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Mar 26, 2018
Messages
184
Likes
124
#1
I am finishing a number of timing pulley bores on the lathe and want to achieve a finger press onto a ground 16mm motor shaft. The pulleys are aluminum and currently have a 12mm bore. Before starting the actual pieces I ran half a dozen test pieces in 6061-T6 bar stock. I attempted to use a very cheap (I mean ~$4 cheap) 16mm reamer but not surprisingly it cut like crap (it also has a significant amount of taper along it's length (~0.001-0.002")). My next attempts were fine feeding an indexable boring bar (TCMT21.51 insert) working my way up from the 12mm to 16mm and cutting the last pass at 10 thou off the diameter. It gave an amazing finish and was on size easily within +/- .001 (.0254mm) or less.

My issue is that 15.98mm is quite a bit tighter than a finger press and 16.02mm is a sliding fit. I did hit a few of my test pieces around 16.004mm which went on very nicely, but I'm struggling to get a reliable process to cut them like that every time. Here's my thoughts which I hope someone can chime in on!

1) My roughing cuts going from 12mm to 16mm are not always the same and might be leaving variable amounts of stock for the two finishing passes. Not surprisingly this would change the cutter deflection and change the finished diameter. Is there some magic way to approach a bore size so you don't have to do anything crazy to hit a nice tolerance?

2) If a part came out undersized and I tried to just kiss the diameter with a few tenths, my cutter would rub rather than cut. Eventually I would bump it enough that it would "bite" and blow the hole way over sized. I think a aluminum specific sharp insert (like a TCGX) would avoid the rubbing? Would a smaller nose radius improve this (like a TCMT21.50)? What about those cheap brazed carbide boring bars?

3) Suck it up and buy a better reamer...


I know there are many tricks of the trade for more precision operations, so I'd love to hear anything you guys can share!

Thanks!
 

RandyM

H-M Supporter - Commercial Member
Staff member
H-M Supporter - Commercial Member
Joined
Apr 12, 2011
Messages
2,359
Likes
2,307
#2
What is your definition of a "Finger Press"? You'll need to define your required tolerances in terms of decimal places. Basically, there are press fits and sliding fits and you'll have to determine what it is you want.

And with the tolerances you are talking about, I am thinking you are in the realm of grinding and not boring.
 

Dave Paine

Registered
Registered
Joined
May 10, 2014
Messages
813
Likes
589
#3
I would not make the final pass 10thou, too much spring in the boring bar. I would want to sneak up on this and make the final pass perhaps 1 thou then measure and if needed make a final spring pass without changing the carriage setting.

The tool should be able to cut without needing to be bumped. Perhaps a dull cutter.
 

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Mar 26, 2018
Messages
184
Likes
124
#4
Fair enough. I'll be honest, I'm not great at relating shaft fit identifications (eg. ANSI LT3) to how they actually "feel" but lets say i'm aiming for 16mm (0.6299") +/- .013mm (0.0005"). I got nice fitting bores when they were in the 16.000 to 16.010 range.
 

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Mar 26, 2018
Messages
184
Likes
124
#5
I would not make the final pass 10thou, too much spring in the boring bar. I would want to sneak up on this and make the final pass perhaps 1 thou then measure and if needed make a final spring pass without changing the carriage setting.

The tool should be able to cut without needing to be bumped. Perhaps a dull cutter.
That sounds reasonable! The cutter is a new TMCT insert, but some grades of inserts sacrifice sharpness for strength. I'm thinking a different insert or a sharper corner radius would help the rubbing.


EDIT: I also have a pile of brazed carbide boring bars which I could try honing to a razor edge. I've never used them as I've been spoiled from day one with indexable cutting tools.
 

roadie33

Active User
Registered
Joined
Dec 11, 2014
Messages
826
Likes
628
#6
I lucked out and picked up a set of Metric Chucking reamers at an auction from 8mm to 30mm, Over and under sized by .02mm
They are a mixed brands of Cleveland, Hertel and Made in USA.
Had to do the same thing on a 10mm motor shaft. Used a 10.02mm reamer on pulley and it was perfect finger press fit.
Reamers are costly but just buy the one size you need for the job and before you know it you'll have a set.
 

westsailpat

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Feb 14, 2016
Messages
558
Likes
331
#7
If you are rubbing you need to fix that , you might try setting the bar at above center . One thing I used to do was once I was happy with how the bar was cutting I would feed in and then feed out check the size then dial in and do it again , now you have established how much the machine is taking . Also you could wrap some fine sand paper around a precision diameter and "hone" in your bore . Hope that helps .
 

pacifica

RGL
H-M Supporter - Gold Member ($25)
Joined
Jan 2, 2018
Messages
149
Likes
75
#8
Dont forget thermal expansion of steel: if you measure at 140degrees(right after you finish boring) and ambient temp is 70, the piece will be about 5 ten thousandths difference per inch. expansion.

If you use a reamer under power then you have to factor in runout from your machine also.
At .02mm you probably want to ream by hand.
 

RollingPin

Newbie
Registered
Joined
Nov 26, 2015
Messages
10
Likes
9
#9
What Mr. Paine said and may I suggest hss instead of inserts. It’s not that difficult to grind tools and in MHO they provide a much better surface on aluminum.


Sent from my iPad using Tapatalk
 

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Mar 26, 2018
Messages
184
Likes
124
#10
I have heard about setting your boring bar above center to increase the effective rake and make it "sharper" although I haven't tried this. That might be my first line of attack. I don't have any HSS boring tools, but I will also try a sharp brazed carbide bar.

Lapping or honing would be a good way to tackle this I think. Maybe some fine lapping compound and a 5/8" carbide endmill shank would do it.
 

petertha

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Jan 15, 2016
Messages
557
Likes
371
#11
I've settled on a few tricks that might help.

- try to converge on the target bore by the same increment, say 0.005" per pass. Some materials are not as forgiving for sneaking up on a dimension, especially if they work harden or don't play as well with the cutter type/nose geometry/rigidity.... So for example 0.005 + 0.005 + 0.005" (measuring in between of course) might get you to closer to the target than 0.010 + 0.003 + 0.002

- make the boring bar spring passes at different feed rates on your lathe. It does make a difference because you are changing the traversing pitch, so stand a better chance of cutting off the hilltops vs. the tool following along in the same path like a record player. So my ritual is 3 identical spring passes with carriage locked at the 3 finest feeds on my lathe.

- use the heaviest most rigid boring bar with shortest stick-out. Listen/feel for any harmonics, adjust rpm/feed accordingly

- make sure your carriage is locked every pass & ideally using something like a DRO. Even the act of locking the carriage can be enough to move it slightly (+/- 0.002" is not uncommon) depending on your lathe wear & how the clamping mechanism imparts itself against the dovetails or whatever. A DRO sees this because its measuring independently whereas a dial machine will not.

- if you can find a reamer to match your bore, it can save a lot of work. Now boring means just getting it appropriately undersize so the reamer can do its job with more consistency. Ensure your tailstock is very well centered.

- assuming you are not into toolpost grinding, that then leaves lapping. Its best to use the correct tools & the don't have to be expensive. These brass laps work well & are reasonable. Ideally you want a softer material (brass or some folks use copper for home made ones) which will embed the grit. This is somewhat messy & time consuming work. I would recommend not being much more that 0.002" undersize because it takes a lot of lapping to get that final amount down. http://www.acrolaps.com/
 

GoceKU

Brass
Registered
Joined
Jul 14, 2017
Messages
603
Likes
1,062
#12
If you take your time you can achieve any size you want, smaller holes are more difficult because boring bars have more deflection, i usually finish smaller bores with DIY flapper wheel to take the last few thousands off
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
498
Likes
323
#13
.004 MM is 0.00000159", how did you measure this?
 

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Mar 26, 2018
Messages
184
Likes
124
#14
.004 MM is 0.00000159", how did you measure this?
0.004mm is 0.000159”. Measured with a telescoping bore gage and mitutoyo half tenths mic. Admittedly this tolerance is rather unnecessary, but the exercise in hitting repeatable tight tolerance dimensions on a lathe is not.
 

MarkM

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Apr 23, 2017
Messages
243
Likes
178
#15
Your tool geometry is everything when it comes to boring. It s not only the insert but also the insert holder that gives you your tool geometry. A small radius and rake on your tool helps offset deflection. Brazed Carbide can be used for these tight tolerances if ground with the right geometry. 6061 loves rake and a sharp angle of keenes. Plenty relief up front and your side clearance. Myself when i am in to the tenths its hss all the way for boring. Carbide especially inserts don t like to sneek up on a dimension. Brazed Carbide if ground with the right geometry but I still prefer hss when I need to be that precise. I'd go for a 001" if it were me. It s 6061 and a metal shaft. Heat your pulley up if you don t have a press or can t use your lathe (tailstock) or a vise to help press it on. Finger press may not hold your parts. Disimilar metals and your pulley may heat up from your belt friction.
 
Last edited:

pacifica

RGL
H-M Supporter - Gold Member ($25)
Joined
Jan 2, 2018
Messages
149
Likes
75
#16
.000159" is Better than I can do with a stand and german steinmeyer snap micrometer! Screen Shot 05-16-18 at 03.07 PM.PNG
 

markba633csi

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Apr 30, 2015
Messages
2,811
Likes
1,458
#17
MarkM said it as well as I could- with a sharp tool you should be able to shave the eyelash off a gnat
MarkS
 
U

umahunter

Guest - Please Register!
Guest - Please Register!
#18
If you need a reamer check Amazon I got a Morse 3/4 carbide tipped chucking reamer for 29 bucks
 

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Mar 26, 2018
Messages
184
Likes
124
#19
Thanks again all!

I just finished another half dozen test pieces and two of the pulleys. Here is what I found really helped!

I did my roughing passes at 20 thou until i was 40 thou from the final diameter. Then I switched the power feed to the finest setting and took a finishing cut at 10 thou. I measured this and took a second 10 thou cut. Measured again and took a third. At this point I knew how the final cut would work and I adjusted the final depth as needed (roughly 2 thou deeper). I liked this because it tended to risk an undersized bore rather than an over. My first piece wasn’t great but after that I got the 4 remaining test pieces and two of the pulleys within +/- 0.0004”. I’m happy with this! It’s amazing how much of a difference in fit there is between a .6295” and .6303” bore on a 16mm shaft. One pulley is a little to tight to hand press so I might lap the bore or heat it up before putting it on.

My finish pass was made at around 12 thou off the diameter and produced a nice finish and consistent diameter.

Still have a few more to go so we will see how it finishes up.
 

pacifica

RGL
H-M Supporter - Gold Member ($25)
Joined
Jan 2, 2018
Messages
149
Likes
75
#20
Nothing like a 350 degree oven and air in a can to freeze the shaft. a 400 degree differential in parts , with a16mm bore will add an extra .0016" or .04mm.Once it cools off it may be difficult to remove!
 

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Mar 26, 2018
Messages
184
Likes
124
#21
Nothing like a 350 degree oven and air in a can to freeze the shaft. a 400 degree differential in parts , with a16mm bore will add an extra .0016" or .04mm.Once it cools off it may be difficult to remove!
So I may or may not have been screwing around doing just that and got my pulley stuck halfway on the shaft (motor not yet installed) :rolleyes:
 

P. Waller

H-M Supporter - Sustaining Member
H-M Platinum Supporter ($50)
Joined
Mar 10, 2018
Messages
498
Likes
323
#22
0.004mm is 0.000159”. Measured with a telescoping bore gage and mitutoyo half tenths mic. Admittedly this tolerance is rather unnecessary, but the exercise in hitting repeatable tight tolerance dimensions on a lathe is not.
Old machine shop joke, add a 0 to the right of the period, add a 0 to the cost left of the period (-:
 

cascao

Active User
Registered
Joined
May 24, 2012
Messages
353
Likes
810
#23
For this kind of job I have grind a boring bar from a carbide rod. Very sharp and way less deflection than any steel.
What is the each shaft real dimension? At this tolerance maybe there some variation on shaft too and each shaft will match one specific pulley.
 

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Mar 26, 2018
Messages
184
Likes
124
#24
Shafts are 16.000mm +.008/-.003 so that easily could play into these fits! I'll see if they actually vary and maybe match pulley to shaft. I'm going to try to finish the rest tonight and see how they turn out. Thanks again everyone
 

higgite

General Manger - Proofreading Dept.
H-M Supporter - Gold Member ($25)
Joined
Aug 15, 2013
Messages
818
Likes
862
#25

petertha

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Jan 15, 2016
Messages
557
Likes
371
#26
My close tolerance boring experience is confined to model engine liners in various kinds of steel & cast iron. The target has to be within 0.0005" but more importantly, of a specific finish at that final bore. That's not exactly an easy combo to hit. I have a super stiff boring bar that has a shank diameter probably 70% of the bore ID. I tried HSS but preferred sharp inserts for consistency. Part of that was likely my inability to dress & set up HSS properly & maybe cheapo import HSS boring bar. They just aren't as common anymore.

What I think you will discover if you get into lapping after turning is bore gages are measuring an average of whatever hill tops they are residing on. That may be fine for your purpose, in fact maybe even desirable if you are using retainer type adhesive. Lapping its quite revealing. Your beautiful boring bar finish at 0.0005" tolerance inevitably turns into 'micro-stripes' where the lapping has flattened the hill tops with a matt finish but the troughs are still shiny. My pics don't do a great job of showing this properly but I'd recommend you try yourself. This is why I was recommending you change up your traverse feed selection on final spring passes. If you don't, you are just spring passing the bottom of the vee. But that has little to do with the dimension across the crests (think of it as threading which is essentially what is happening). Yes a more rounded tool tip minimizes this effect, but I feel also at resisting DOC so even more need for spring pass. Lapping also reveals other effects like ever so slight bore difference between the opening of the hole & closer to the chuck. Lapping (if done properly) doesn't lie, its visually quite apparent until the whole surface is entirely matt & now removing native material.

Of course all this is very material + cutting tool + machine rigidity dependant. The recommendation to stabilize temperature prior to measurement is very important at these tolerance levels. Re measurement, I like snap gauges too but I would recommend a good quality bore gage set against a known standard. Not only can you get good consistent direct readings without in-between-device chances of error but you can repeat this many times & at different positions down the bore, 'mapping it' so to speak.

If you can get to within 0.0001" using lathe tools & no grinding/lapping secondary finishing, you are a better man than me. The way I think about it, if every commercial 'cylinder bore making' company could hit the appropriate tolerance /finish with cutting tools alone & mitigate grinding / lapping / honing operations, why would they go through all that added expense?
 

Attachments

pacifica

RGL
H-M Supporter - Gold Member ($25)
Joined
Jan 2, 2018
Messages
149
Likes
75
#27
My close tolerance boring experience is confined to model engine liners in various kinds of steel & cast iron. The target has to be within 0.0005" but more importantly, of a specific finish at that final bore. That's not exactly an easy combo to hit. I have a super stiff boring bar that has a shank diameter probably 70% of the bore ID. I tried HSS but preferred sharp inserts for consistency. Part of that was likely my inability to dress & set up HSS properly & maybe cheapo import HSS boring bar. They just aren't as common anymore.

What I think you will discover if you get into lapping after turning is bore gages are measuring an average of whatever hill tops they are residing on. That may be fine for your purpose, in fact maybe even desirable if you are using retainer type adhesive. Lapping its quite revealing. Your beautiful boring bar finish at 0.0005" tolerance inevitably turns into 'micro-stripes' where the lapping has flattened the hill tops with a matt finish but the troughs are still shiny. My pics don't do a great job of showing this properly but I'd recommend you try yourself. This is why I was recommending you change up your traverse feed selection on final spring passes. If you don't, you are just spring passing the bottom of the vee. But that has little to do with the dimension across the crests (think of it as threading which is essentially what is happening). Yes a more rounded tool tip minimizes this effect, but I feel also at resisting DOC so even more need for spring pass. Lapping also reveals other effects like ever so slight bore difference between the opening of the hole & closer to the chuck. Lapping (if done properly) doesn't lie, its visually quite apparent until the whole surface is entirely matt & now removing native material.

Of course all this is very material + cutting tool + machine rigidity dependant. The recommendation to stabilize temperature prior to measurement is very important at these tolerance levels. Re measurement, I like snap gauges too but I would recommend a good quality bore gage set against a known standard. Not only can you get good consistent direct readings without in-between-device chances of error but you can repeat this many times & at different positions down the bore, 'mapping it' so to speak.

If you can get to within 0.0001" using lathe tools & no grinding/lapping secondary finishing, you are a better man than me. The way I think about it, if every commercial 'cylinder bore making' company could hit the appropriate tolerance /finish with cutting tools alone & mitigate grinding / lapping / honing operations, why would they go through all that added expense?
Beautiful work!
 

pacifica

RGL
H-M Supporter - Gold Member ($25)
Joined
Jan 2, 2018
Messages
149
Likes
75
#28
I've been using dpmt (positive rake) inserted,size 32.52 and they give an excellent finish,only 2 edges,though.but worth it.finnish is better than my hand ground HSS!I use a belt grinder with an angled,clamped holder for accuracy of the angles.
 

petertha

H-M Supporter - Gold Member
H-M Supporter - Gold Member ($25)
Joined
Jan 15, 2016
Messages
557
Likes
371
#29
Thank you. And just for completeness, here is a reamer finish (6061-T6 Al). Lathe bored about 0.005"under size, then in goes the reamer. They are not exactly cheap in larger diameters, but if you are doing a bunch of similar parts, they may be worth it.
 

Attachments

macardoso

H-M Supporter - Silver Member
H-M Supporter - Silver Member ($10)
Joined
Mar 26, 2018
Messages
184
Likes
124
#30
Petertha, beautiful work! I have some more practice to go before I could hope to hit .0001"!

The good news is that all 4 pulleys are done, 2 are a light press fit, I think I will do a thermal shrink, and 2 are a very tight slip fit, only about .0005" difference between the bore sizes! I'm very pleased that I could hold +/-.0003" on my target without too much trouble. I'm sure with a better insert selection and a stiffer (larger) boring bar I could do even better. Thanks for all the advice.

The last step is turning some 1/8" x 1/8" brass slugs and inserting them into the tips of the setscrews on the pulleys. I got one installed on my motor and it is not going anywhere!
 
[6]
[5] [7]
Top