Tips on finding centerline? Y axis subspindle lathe

I don't really have much experience on lathes besides a benchtop CNC sherline thing 15 years ago. All my (relatively low) experience is from my Hardinge VMC with a Siemens control, vs. this Feeler HT-30SY lathe with an oddly-implemented Fanuc 18i-TB control. So, I could definitely use some help from the experts on here.

My current task, while I slog through trying to substantially modify a Fusion 360 post for this slightly odd machine, is to get the tooling offsets dialed in. So, what are some good techniques to find an accurate Y axis offsets for turret tools on a Y axis lathe?

I've got a coaxial indicator and I've dialed in the bore and axial live toolholders... I found several resources online demonstrating that. However that's about as far as I've got with any confidence. Now, I'm trying to find the offsets for the rest of the tools.

I've tried the scribe-a-line-on-a-face method... I'm not really sure how close that's really getting me. It also certainly wouldn't help rotate a boring bar into the correct orientation aligned on the XZ plane.

I've also tried stepping Y up and down and facing off a part until I get as smooth a face as possible... however I'm not even sure if that's actually a valid method.

I'm currently trying the "ruler" method, where you move Y around until a ruler held between the insert and the round stock is perpendicular... but measuring perpendicular accurately may be a problem. Maybe put round stock on my mill to cut a flat reasonably parallel to the stock centerline, and in the lathe use a good square on that face to find when the ruler is perpendicular?

Actually, even the positions I've indicated the bores for won't be right for boring bars or other tools not axially aligned with those bores. It'd be better if I had two sets of offsets for those cases... I suppose one could use the geometry and wear offsets that way, but that's probably a misuse and not a good practice. I could certainly try to maintain higher tool offset numbers for the true axial offsets, and copy them down as starting points when setting up a new tool.

It's a 12 position turret. I've currently defined offsets 1-12 as main spindle tool offsets, and 21-32 as the subspindle tooling offsets. Tool offsets for turret positions that are only for one spindle or another are copied into both sets.

So, how would you do it? What other good practices should I be considering/aware of?

I think you're overthinking this. If you dial in a boring bar holder so that it's at X0 and Y0 at one turret position, all the other turret positions should be the same. If you're finding a large difference in the X0, Y0 between turret positions, your machine has a problem. I don't doubt that there might be small differences, but they shouldn't be enough to make a difference to your machining. Spending a lot of time indicating every single holder in an example of perfection being the enemy of good.

So, I would indicate an I.D. holder to make sure that Y0 really is Y0. If it's not, then reset your Y 0 position. Check a couple holders just to make sure that the first one you checked wasn't damaged from a crash or something. I would not have separate Y offsets for every position. Once your Y0 is set that way, assume that your turning tools, radial live holders, etc are all at Y0 unless your machining tells you otherwise (e.g. turning tool leaving a nib, Y-axis milled feature not on center).

For the X offsets, I would make a cheat sheet for the X0 position of all the ID holder and axial live holder types. Don't do it for each individual holder, just the holder types. Maybe all your ID holders are the same, which are the same as all your axial live holders. Then, you would just have one number to write down.

This should be good enough for most jobs. Take a test cut and adjust accordingly. If you really need to nail it the first time, you can indicate that specific tool, but I think it's a waste of time to indicate every holder now when you're most likely going to be removing and adding holders to accommodate different jobs.

I think having offsets 1-12 for the main spindle and 21-32 for the sub is a good idea. I wouldn't have two sets of offsets for center cutting and boring bars, though. I think that would get too confusing. Just write down the offset for a center cutting tool.

concerning offsets, I would add say 30 to what ever offset for a the secondary position. say your using a grooving tool, the leading edge would be 1 and trailing edge would be 31. Or say a insert drill, 5 would be the center drilling position and 35 would be the turning edge.

One trick I use when I'm on a machine without a probe is get a round bar about 5 or 6 inches long and mill the last inch or so down to the center line. Basically if you have a 1.5" diameter will one ind down to .750.

chuck up on the round part and set a 2" tool setter like you use in a mill and touch off the same way. I kept several sizes under the bench so I wasn't swapping jaw sizes all the time. Works pretty good. set your comp a few thou high and walk it in.

Thanks g-coder05 I ordered a 2" tool setter. I think that'll be a pretty good method.

wmpy The offsets I'm measuring are perhaps not super significant out at the OD of the stock, perhaps you're right. However, it's not nothing... the Y axis bore measurements so far are -4.9 thou, -7.9 thou, -12.4 thou (sub bore), -25.1 tho (sub live). Actually, I should redo the sub side and verify they're that large. I won't measure Y for every tool change... just the really common ones that don't get changed often. (OD rough, OD finish, etc) The coaxial holders also could just be measured once and copied in from a "master" copy in a higher tool offset range.

Those numbers definitely are significant and more than I would expect in a well-aligned machine. I guess you could compensate for them in the Y, but you might be doing yourself a disservice by covering up some bigger alignment issues with your machine. Has the spindle been checked for straightness? What about the turret? Is the sub lined up with the main spindle?

Before doing anything, though, I'd double check those numbers to make sure your checking method is accurate. It's easy to get indicator droop if you're not careful. Maybe verify by putting a .500" pin gage in a holder and another in the spindle to see if they line up when you think you have the holder zeroed in.

What kind of numbers should I be seeing?

It's a well used machine that had an in-place spindle rebuild last year. I had a tech level it before I started using it a couple weeks ago. He took off two static BMT60 toolholders to level looking at the top face of the turret. I meant to watch him put the toolholders back on, but I missed it (are they highly repeatable by design, or do you need to indicate them in?)

Before I bought the coaxial indicator, I had brought the sub up to the main with a 1/2" end on some stock and a 1/2" collet in the sub. I brought them right up against eachother and checked with a piece of paper all around as I brought the sub up over the stock. The back & bottom sides got tighter slightly before the front & top, but otherwise it seemed "reasonably" lined up for a 12-15" 303 stainless bar. It was a 1 3/16" bar with the last inch or so turned down to 0.5". By reasonably I mean to me with my very limited experience.

I'll recheck and measure the sub from the main with the coaxial indicator tomorrow. Actually, that may be a good bit of it right there... the higher numbers were measured with the coaxial indicator in the sub.

Edit: I do recall the CNC manager of the previous owner company said not too much about the machine other than "don't hit the sub with the turret, it's a bitch to get the sub realigned again". Maybe the sub was hit and they didn't work as hard to fix it that time.

Use a coax indicator to sweep the sub from the main, the main from the sub, and a boring bar holder (the same one) from both sides as well.

If it isn't lined up (I'm talking no movement on a ten thousandths indicator) you have a machine alignment problem. Y zero should be Y zero, IMHO.

Rick Finsta said:

Use a coax indicator to sweep the sub from the main, the main from the sub, and a boring bar holder (the same one) from both sides as well.

If it isn't lined up (I'm talking no movement on a ten thousandths indicator) you have a machine alignment problem. Y zero should be Y zero, IMHO.

Click to expand...

I agree with the method but not so much the outcome, because when you then index the turret to a turning tool, it assumes that all your turning tool stack up tolerances (insert, seat, holder, turret interface, curvic etc, before you even get to your actual encoders/scales or thermal growth) are also zero. There are so many interfaces there that the stack up means even one micron on each of them puts your tolerance at a minimum of 5 microns. If they're 5 microns each, now you're at 25um or roughly 0.001. Sub spindles also have manufacturer tolerances for alignment both in parallelism and actual concentricity. That is never perfect, the ones I've worked with are adjusted in 2 degrees of freedom and while you can certainly get it pretty close, you have a constant battle between parallelism and concentricity at a point in order to achieve proper coaxiality. If your indicator shows no motion when you test that, your indicator simply ran out of resolution.

Regardless of that though, there isn't anywhere near the same requirement for Y zero to be exact for turning tools as there is for other tools. Being a few microns out in Y for an OD or ID turning tool is in most cases not a huge problem, it doesn't significantly affect X values or rake angles until it's a fair way out. Drills and reamers are another matter, but hit them with the coax and you should be fine.