What's new
What's new

Interpolated bore circularity

vmipacman

Cast Iron
Joined
Nov 21, 2014
Location
Virginia, USA
This is a theoretical question. If I had a large diameter hole with a tight tolerance and the machine has axis backlash, would a larger cutter with smaller interpolated movements give better results than a smaller cutter with larger interpolation moves?
For example, a 4” hole milled with a 1/2” em versus a 4” hole finished with a 3” shell mill. Would the would the hole with the bigger endmill have better circularity? Or the same?
Thanks
 
This doesn't answer your question but boring bar would minimize the machine backlash inaccuracies to end up with a round hole as long as it would hold still while doing it. Boring bar instead of end mill be my first thought knowing the machine had issues.

Brent
 
Thanks for acknowledging that wasn’t the question :) but yes boring bar would be ideal. But also a pain in the butt to dial in and deal with harmonics and balance and rigidity and chipload etc. I was thinking this might give results somewhere in the middle.
 
This is a theoretical question. If I had a large diameter hole with a tight tolerance and the machine has axis backlash, would a larger cutter with smaller interpolated movements give better results than a smaller cutter with larger interpolation moves?
For example, a 4” hole milled with a 1/2” em versus a 4” hole finished with a 3” shell mill. Would the would the hole with the bigger endmill have better circularity? Or the same?
Thanks


I don't know the exact answer to your question,

But the reversal spikes are going to be the same magnitude regardless of tool diameter.

For example on ball bar plots reversal spikes show up separately as cardinal "spikey" points as distinct from the plotted circularity.

You can almost have a peanut shaped ball bar plot with reversal spikes or you can have a more circular plot with the same magnitude of reversal spikes. You can have bad circularity and yet have no reversal spikes / backlash at all.


Kinda depends what and how you define circularity as being independent of reversal spikes or reversal spikes not being lumped in with circularity.

Visually not 100 % sure how your part will look with the two massively different diameter tools... One would think that the lobeing of a cam like "circle" would be less pronounced visually with a larger diameter tool maybe … But that again statistically is different / maybe independent of measures of "circularity".





Practically a boring bar from a static point makes for a better "bore" / circle like what Yardbird just said If your machine has trouble interpolating round circles and has additional backlash / slop in each axis or on one axis only.

In your theoretical example does each axis have equal backlash / slop or just one axis ?
 
Thanks for thinking it through about “ovality” vs reversal spikes. I was thinking if you say used a tool large tool in a large hole it must be better.
Oh well, I’ll put my theoretical question in context :)
I have a 4.5” bearing bore I need to hold 2 thou on. I get 1 thou difference measuring across the hole at various points just in diameter. So without knowing what it actually looks like in circularity it may impinge on a truly circular bearing race. Plus factoring in the 1 thou of error it only leaves 1 thou of tolerance. Needless to say I finished bored the first two parts and they passed inspection ok. But The boring head sucked btw. The other 6 I don’t want to bore if I can help it. Was thinking of trying a single point fly cutter set at about 4” and programming a tight boring cycle. Was thinking that would be a compromise between the cnc and boring strategies...
 
The small EM >might< be better because one would probably want to feed it more gently.

Beyond that, I'm not sure there would be a difference.

Sent from my SM-G973U using Tapatalk
 
Thanks for thinking it through about “ovality” vs reversal spikes. I was thinking if you say used a tool large tool in a large hole it must be better.
Oh well, I’ll put my theoretical question in context :)
I have a 4.5” bearing bore I need to hold 2 thou on. I get 1 thou difference measuring across the hole at various points just in diameter. So without knowing what it actually looks like in circularity it may impinge on a truly circular bearing race. Plus factoring in the 1 thou of error it only leaves 1 thou of tolerance. Needless to say I finished bored the first two parts and they passed inspection ok. But The boring head sucked btw. The other 6 I don’t want to bore if I can help it. Was thinking of trying a single point fly cutter set at about 4” and programming a tight boring cycle. Was thinking that would be a compromise between the cnc and boring strategies...

LOL that's cool,

I didn't know how theoretical you wanted to go with this so I actually stopped short for me.

Literally one could build formulae and equations for your question, with Brent's / Yardbird's point in mind it almost a calculus problem as one of the limits i.e. a tool that has the same diameter as the bore and makes an interpolated circle that tends to 'Zero" versus cutting tools of various smaller diameters with their respective interpolated circle radii + shifting from backlash + phase angle shifts...


I'm actually having to look at similar problems at higher tolerances so I will try to put a better thinking cap on maybe over the next few days.

Right now it's cool enough (temperature wise) for me to muck the barn out (rather than earlier)… To the barn !

Meanwhile I was thinking also some kind of epi-cyclic or trochoidal tool path that processes (like as in procession) might cancel out some of what you are talking about (quadrant) errors on the machine here to deliver a smooth and round and circular bore (probably for a smaller diameter tool). Caveat being depth of bore + surface finish considerations, but for "bearings" . The motion a bit like spirograph (just a left of field idea). Could look terrible but actually seat your bearing perfectly well with multiple good contact points and surfaces ?


94950c12cd077b1a7df28cffe4ed5683[1].jpg

^^^ kinda like a "spirograph" that but with less pointy tool path (broader smoother arcs) and maybe a larger endmill than 1/2" depends what the repeatability of your backlash is ?




What depth are you boring ?

'Circularity" how is your inspection department defining that / determining what they consider criteria for circularity i.e. procedures ?

Flycutter 4" down into a bore ? You grind your own tools and are completely 'Chill" with that ?

I don't know your set up and safety considerations blah blah blah…

Was wondering whether the single insert on a shell mill idea works for bores but I'm not the guy to ask whether the angles and geometry on the insert are 100% appropriate for that ???? Versus an actual boring tool.
 
I always just mill it as round as it gets to .006 under or so then switch to the boring bar to finnish. Once the bar is set you never have to mess with it, dead easy to hold your tolerance.
 
Cameraman, very cool idea with the procession toolpath. Never would have thought of trying that!

The bore is only 1" deep btw, and 4.5" round. So a tight spiral boring cycle would not be too bad.
I don't have a good way to check these on the machine other than telescoping gages and mics. I turned a 4.499 diam go-gage on the lathe for this bore that is 4.500 to 4.502.
On the customer end, it just needs to work. But with them, when it doesn't, it needs to be right per the drawing :) They have way more inspection capability than my little shop. Plus I'm trying my best to get it right and this big tool boring hack would come in handy.
 
I think the best would be a .75 endmill so it would have less taper 1 inch down. And feed at or below 20 ipm
Don


Sent from my iPhone using Tapatalk Pro
 
Another thing to consider (whether it matters or not depends on you & the customer...) is how the bearing is used. High rpm, low rpm, loaded, side loaded, hot-cold, etc. And the style of bearing, shielded, un-shielded, closed, open, grease pack, etc.

If your end of the assembly is the press fit, and depending on bearing needs/style, circularity could not be as important, as long as it stays in place and works...


To your original question, I would use a smaller, relative to finish size, (3/4-1") endmill, if the boring head was a no-go*.

* Why do you say the boring head is a problem? Theoretically (I know haha), once set you should be able to mill all of them .01 under or so and have at it. Do you have a good boring head? Would this job facilitate buying a good boring head? Might be a good time to tell the boss "here are the problems I am having, this xxxx boring head would solve that"

BTW, I recommend this for a precision head/kit, used them and loved them, very repeatable!

Techniks BohrSTAR 43 Triangular Insert Boring Kit – Range .314" up to 1.962"
 
first off, you need a bore gage. These are all just mute points if you have no way of measuring it. If your machine has any measurable backlash, you shouldn't be interpolating bearing bores at all.

But to answer your question, the size of the tool will not affect circularity.
 
This is a theoretical question. If I had a large diameter hole with a tight tolerance and the machine has axis backlash, would a larger cutter with smaller interpolated movements give better results than a smaller cutter with larger interpolation moves?
For example, a 4” hole milled with a 1/2” em versus a 4” hole finished with a 3” shell mill. Would the would the hole with the bigger endmill have better circularity? Or the same?
Thanks
.
4" dia hole with 3" mill leaves rougher surface but you dont mention depth. obviously a 1/2 dia end mill would have trouble over 2" depth. at 3" depth the 1/2" end mill would leave a bad finish too.
.
it aint theoretical i see it every day. if feed programmed from cutter center and dia comp is really wear comp than actual feed at cutter circumference is much higher than feed at cutter center. so a 20.0 ipm feed might be way too high for the 3"dia mill to get a good finish. when I or J is small most experience operators in a millisecond can tell if feed might be a problem. for example 4"dia bore to IJ would be 2.0 if feed at circumference but 3" mill IJ is .500" (wear comp) so you got a 2.0/.5 = 4x ratio so 20 ipm feed really like a 80 ipm feed. gives a rough surface obviously. like using .625 dia end mill for a .75 bore tends to give a rough surface unless slow feed down
.
obviously if depth is 4" or more than that becomes important. not unusual to have 6 to 12" depths. when length to dia ratio of cutter over 5x so 3"dia mill thats 15" long any longer you get vibration finish. many times if roughing it dont matter if finish is rough. might use 30 to 40 ipm feed with 3" dia mill. if leaving .020 for finishing it dont matter if dia is -.018 to -.020 in spots
.
longer tooling often uses slower rpm so vibration aint as bad. if using 15 to 20" gage length tooling obviously feeds and speeds depend more on vibration limits. even 10 to 15" length tooling have some vibration limits if trying to get a very good finish
 
Well, not interpolating is the obvious answer on a machine with backlash......

Most controls have backlash comp......

wonder what would happen if you drew the bore as machined in CAD and inverted it..........
 
backlash you see if measuring bore at different clock positions. not unusual to see .001 difference
.
cutter size dont really effect backlash its same. 3.3" dia bore with 3"dia mill gives rough surface but if trying for 6" depth good luck doing that with a 1/2" dia end mill
 
I disagree with all the responses related to "bearing bores need to be perfect", it is a matter of function plain and simple. Will it work?

That is what you need to ask the customer, but if it is aero or gubmint, well you are screwed LoL! They may want/require .0001", too bad if it is actually needed or not....
 
many machines not only have backlash but have slide tilting. that is when Y reversed it can show as Z or X movement. hard to describe.
.
even when less than .0005" slide tilting can cause problems
 
I disagree with all the responses related to "bearing bores need to be perfect", it is a matter of function plain and simple. Will it work?

That is what you need to ask the customer, but if it is aero or gubmint, well you are screwed LoL! They may want/require .0001", too bad if it is actually needed or not....

.
bearing bore depends on tolerance if +/-.0001" that includes circular tolerance. if +/-.0010" than obviously it can be more out of round. boring bars are normally required when bore must be circular less than .001" circular error
.
many larger parts go out of round .001" when unchucked and have had some time to think about it. i see that almost everyday. depends on bore wall thickness and part shape
 








 
Back
Top