Turning 1" axle between centers

[Glenn Brooks]

Here is sort of a newbie question.

What causes shafting turned between centers to be oversized in the middle and undersized on both ends??

Here's the details:

I've been turning some 1" silica Bronze shafting (15" long) between centers to make a new shaft for my Dalton back gear drive assembly - basically a 9" South Bend three step, flat belt pully arrangement with attached motor turning a 9" V belt pully.

My Turning method: 3/4" HSS bit, 12x48 1950 Standard Modern lathe, turning 150 RPM, couple of .030 Rough cuts, then finished the shaft down with two .008 in feeds at .0035 IPM. No following or steady rest - don't have one...

After much aggravation, I was able to turn the shafting to .875 (7/8) OD- more or less- for the length of the casting (9 1/4" ) plus 3" on the left side to accommodate the drive pulley. My biggest issue is that both ends of the shaft - approx 1-2" each side - turned out undersized (.869) by .oo6, while the middle of the shaft ended up after the rough cut at oversized by .008.

I don't have a following rest, or steady rest available, so Leading into the middle of the shaft, about every 2"-3" on the finish cuts, I would stop the cut and measure the OD, then turn in .003 on the cross feed to keep the OD at .875, plus 1- 2 thou or so.

When finishing the cut, on the left end about 4" from the dead center in the headstock,( last 3" of which was more rigid, unturned 1" stock), the tooling cut rapidly into the work, going from .875 OD to about .866 OD one inch of travel.

I was very surprised by this as I had stopped turning and measured the shaft every two inches or so, all along the work, adjusting the infeed to hold the OD.

So, 1) I am guessing this variance on the shafting OD is partly due to tool pressure in the middle, causing the stock to push away from the cutter? Causing a larger OD in the middle?? And,

2) the smaller OD at both ends was due to me cranking in several thou to compensate for the center oversize OD, and as the work became more supported at the ends, the cutter took a deeper bite???

Or would a worn bed (.030 wear near the headstock) also cause this to happen??

Can anyone comment on likely causes for this little 'learning excercise'? Also, what could I do next time to improve my method and produce a cleaner overall shaft?

Thanks much for any advice you may be able to offer.
Glenn

[GlennW]

So, 1) I am guessing this variance on the shafting OD is partly due to tool pressure in the middle, causing the stock to push away from the cutter? Causing a larger OD in the middle?? And,

2) the smaller OD at both ends was due to me cranking in several thou to compensate for the center oversize OD, and as the work became more supported at the ends, the cutter took a deeper bite???

I'd say yes on 1, and definitely a contributing factor on 2 depending on technique.

Bronze needs seriously sharp tooling to cut properly with minimum deflection. Rake helps a lot when turning, but be careful if machine rigidity and lead screw wear is questionable, as the cutter can be drawn into the cut.

[tommy1010]

Having an older lathe myself I found shafts cut to be smaller on one end. I blamed it on cross feed screw wear and backlash. It seemed that when cutting the tool was pulled into the cut. When I tightened the gib screws to the point of locking the cross slide problem solved. This may help in your case???

[SteveM]

Not familiar with the lathe, so I can't say how flexible it is.

If you were doing that on an Atlas, I'd say that deflection is definitely the culprit. On a Monarch 10ee, then I'd say no way Jose. Anything else is somewhere in between.

Bronze is definitely strange to cut. Sharp tooling, as Glenn pointed out, helped when cutting bronze on my atlas. You don't say if you are using carbide or HSS, nor what the rake is.

I think your RPM is way too slow. It may be climbing on the tool and pushing the tool away, rather than cutting.

Per LMS
http://littlemachineshop.com/reference/ ... speeds.php
Bronze with HSS is 200-250 sfpm (715 for carbide), which at 1"

SFPM/RPM calculator at:
http://www.carbidedepot.com/formulas-turning.htm
shows 764 rpm for HSS (2,700 for carbide!).

Steve

[Glenn Brooks]

Thanks for the comments. The machine is an old heavy iron lathe and plenty rigid, although worn a lot on the ways... I ground the tooling just before starting my finish cut, so it was sharp and had I think pretty good geometry. My finish was excellent, almost mirror smooth, after I slowed down the machine from 240 to 150'rpm because of chatter.

I will try running fast on another piece of stock I have left over and see what happens. I use HSS tooling so will try 760 RPM or thereabouts and report back.

[SteveM]

Another question I would have is why use bronze rather than steel for the shaft?

If it runs in bronze bearings, steel on bronze should be fine. The backgear shaft is never going to spin very fast.

Steve

[epanzella]

I ran into the same problem when turning gun barrels. I solved it by letting most of the barrel go thru the headstock. I let 4 inches stick out the 4 jaw and put the end on a live center. Turn 3 inches and then stick it out another 3 inches and turn that. Keep going 3 inches at a time (always turning near the chuck) until you get to the last 3 and then reverse it, putting the last unturned 3 inches onto the live center. Then turn that last 3 inches. On my lathe (Grizzly G4003G) this will put the whole shaft within .001". This method not only prevents the part from flexing, it minimizes and taper generated by your lathe because you're using the same 3 inches of the bed over and over again.
PS; you can also do this with a 3 jaw but you'll lose a bit of accuracy depending on how good your three jaw is.

[Glenn Brooks]

Well I thought I had this thing figured out. Tried making a few experimental cuts at 600 RPM - nearest Imhave available to th recommended 760, and was pleasantly surprised with a good finish - except when I moved up against to the headstock, got a bunch of,chatter, which I couldn't resolve at any speed. And now when finishing the last cuts for the 9" pully ID on the end up against the headstock, chattering problems have manifested themselves big time. I've got a section of stock on one end that Imuse to make trial cuts, maybe 5" long with horrible wavy cuts that almost look the stock has been knurled. And to make things worse, it shows up at every speed I have available, from 800RPM down to 100 rpm. Even with a feed of .0035/inch.

I need to take .004 finishing cut off the center portion of stock to achieve a slip fit through the back plate, but don't want to screw up the actual part due to chatter.

Iam wondering if there is a critical not-to-exceed diameter , that I may have dropped below , causing the chattermarks? Right now the long part of the shaft is right at .879". Where I experiments with feeds, the shaft OD is about .740. This part will be cut off and discarded when Iam done. But don't want to loose the work now on this final cut because of a rough surface. Previously the cuts were mirror smooth. Aggravating!


I do have some round steel stock I could use to make another shaft, but don't really want to waste this perfectly nice piece of bronze - which I had laying around from when I rebuilt my rudder out of a 30' cruising sailboat a few years ago.

Glenn

[f350ca]

You could try a Shear tool Glen.
http://conradhoffman.com/shop_images/sheartool.jpg
Don't think I've ever used one on bronze but it should work.
They're best at only taking maybe a thou or even 1/2 thou cuts , but put very little force on the material so it won't spring it, and leave a great finish.

Greg

[BadDog]

It's getting late and I didn't read too carefully, so may have missed something, but long lengths between centers always tend to be larger in the middle because of material flex. How much depends on aspect ratio dia to unsupported length. Tools and/or materials that cut with more pressure exaggerate the effect. It sometimes helps to mentally exaggerate the ratio so your mind can easily grasp the effect. For instance, imagine the difficulty of single pointing a 1/4-20 thread on a 20" unsupported shaft. It wouldn't surprise anyone when the center deflected and remained largely untouched because the bar flexes with fingertip pressure and threading is a high pressure operation. With that in mind and, understanding the rigidity is just an illusion of perfection that can never quite be achieved (everything moves, everything flexes), the rest is pretty easy to predict. Long flexible beds (like my first Griz G4000) certainly add to the problem, just from the other side.

Follow rests of various types are generally used to help prevent that situation by restraining cuter and work in relation to each other.

Wear unless excessive generally doesn't manifest in what you saw, at least not on prismatic way beds. Wear usually just lets the near side of the bed nestle further down on the ways. As you move end to end, the tool may rise and fall sever thou, but if you trig that effect on diameter you see that for most practical purposes it can be ignored if not working to VERY close tolerances.

You also have to be careful taking very light cuts. Some tooling actually goes up in cutting pressure if you go below a certain depth of cut. So minimal depth of cut depend on tooling and material. There is also the related problem of different results depending on depth of cut. You may crank in 0.003 and get 0.001 or 0.005, and that may change depending on the diameter you are currently cutting at (not drastically, but some). So if you are shooting for close tolerances on parallelism, and you also need close tolerances on diameter, it's generally better to make the last several cuts at the same depth so you can predict exactly what the final cut will produce. I have missed a final diameter by a few thou over, where it had been cutting very close on size for each in feed, and the final in feed that should have produced desired size took me several thou under size. I was expecting there to be some of that because lower forces don't "pull up the stack up" like heavier cuts do, so allowed for it over feeding a bit, but didn't allow enough and scrapped the part.

Oh, and the shear tool can produce some nice finishes in "mild steel", but it's not a low cutting pressure tool, so while I like the tool for some things, that's not what I would turn to for fighting deflection.

Heh, didn't plan on typing much, but here I am rambling on anyway...

[Harold_V]

Rule of thumb for reducing, or even eliminating chatter, is to decrease spindle speed and increase feed rate. The lighter the feed, the more chatter you can expect, and once it's established, unless you can break the harmonic, it will repeat and repeat, getting worse with each pass.

One way of controlling chatter is to ever change the velocity of the cut. With some lathes, that's not impossible, but most of them won't allow that luxury. A VFD can be quite useful in this instance.

Chatter can be the result of many things. One of them is how well the material is supported in the holding device. Older chucks are often sprung, so while the piece may be held within reasonable limits, the actual support may be only at the very rear portion of the jaws. Check your chuck for jaw contact at the end---using a very thin feeler. If you can get a thin feeler to go when the chuck is tightened on the work, you are gripping somewhere beyond the tips. That, in this case, may not make much difference.

If you are supporting with the tailstock, how well the quill fits the tailstock can be a source of chatter. Try locking and unlocking the quill to see if that makes a difference. If the quill is quite loose, it may even make a change in taper and the resulting diameter.

One more thing of interest. How much pressure you apply with the tailstock (assuming a live center) can make a HUGE difference. Too much pressure encourages chatter.

I fully expect that, even with all conditions being good, you are expecting more from a lathe than it can provide. Long cuts chatter, and long cuts cut larger in the center, due to cutting pressure (and the resulting deflection). You can control that by various means, but to eliminate it is a hard call unless you can machine with a follower. Even they can be troublesome, however, so that may or may not be a solution for you.

Considering the value of bronze as compared to steel, I would have never made the choice to use bronze simply because I had it. If the day comes when you need a piece of material like that, you'll kick yourself a dozen times over for having wasted in where it wasn't needed, and you find it's going to cost you more than $5/lb to buy your needs.

Just sayin!

Harold

[spro]

You said it. Imagine keying the bronze shaft for a steel key. A steel shaft would be the original. These days with cheap pillow block bearings, there's no need for bronze into iron trunions. The bearings have a cam lock onto the variations of the shaft and alignment.