What's new
What's new

Working between centers question- big cuts?

Long Tom

Stainless
Joined
Aug 21, 2011
Location
Fiddlefart, Oregon
Haven't worked between centers much but I'm bidding a job for (500) bronze castings that have a spigot that needs turned down... at that quantity cycle time will be key, and my lathe is stout, so I'd like to take the material in fairly big cuts, roughly .125" off diameter at a pass. The center/drive dog I made for the spindle side has a shoulder so it can't push back into the 5c collet under tool pressure... so I can get the part nice and tight between the centers... but I was a bit skeered <grin> to really push it on the test pieces I had on hand. I will of course push the envelope if I get the job, but since this is new territory for me I'm hoping for any advice RE: what goes wrong in this scenario.

I know how things can crash when taking big cuts with work held in chucks, cause I've done it, but I haven't pushed work between centers to the crash point. :)

So the nut of my question is I guess "how secure is work between centers in terms of taking big cuts".

Thanks guys!!
 
Haven't worked between centers much but I'm bidding a job for (500) bronze castings that have a spigot that needs turned down... at that quantity cycle time will be key, and my lathe is stout, so I'd like to take the material in fairly big cuts, roughly .125" off diameter at a pass. The center/drive dog I made for the spindle side has a shoulder so it can't push back into the 5c collet under tool pressure... so I can get the part nice and tight between the centers... but I was a bit skeered <grin> to really push it on the test pieces I had on hand. I will of course push the envelope if I get the job, but since this is new territory for me I'm hoping for any advice RE: what goes wrong in this scenario.

I know how things can crash when taking big cuts with work held in chucks, cause I've done it, but I haven't pushed work between centers to the crash point. :)

So the nut of my question is I guess "how secure is work between centers in terms of taking big cuts".

Thanks guys!!

.
many a lathe i have had to tighten the gibs on the compound rest or go all the way to the end so tight and tighten the cross slide gibs and carriage gibs and have a short low stickout tool. and have to watch tool post pivoting if pushed too hard deeper into the cut. as well as worrying about enough horsepower and well as watching tail stock staying tight against part.
.
that said even if everything can take it the part can vibrate from cutting forces and long chips can wrap around part causing big problems. or worse hot chips flying at you while taking heavy cuts
.
many a job i have had to stop to cut the long chips away from part, and a hot part will measure bigger and be smaller when cooled off. usually you just try different things and see what works best for you trying to not mess up the part
 
"how secure is work between centers in terms of taking big cuts".

Thanks guys!!

Depends on the size of the center holes, if you use a #8 bigger center drill I think it will hold fine, I would worry about the center/drive dog slipping in the collet more than anything else. Most lathes with 5C collets are not what would I call stout. Put a center in the spindle and use a dog drive plate.

CarlBoyd
 
0.0625" DOC in bronze wouldn't scare me if it had a reasonable starting diameter, say 3/4" or more and stickout was limited to maybe 5D and it wasn't paper thin (ID > ~50% OD).

I guess the real question is- how much material remains after you take this pass?
 
I second what Carl said. Put a center in the spindle and drive it with a dog. The other thing to watch out for is your tailstock center. I assume you're using a live center in the tailstock but maybe not. Regardless with that heavy a cut the part is going to grow on you. Make sure your center in the tailstock is not too tight or too loose. Other then that the biggest issue with a heavy cut in bronze are the chips. DMF mentioned something about chips wrapping things up. I know there are a lot of different types of bronze but the kind I have turned comes off in a shower of chips. I usually make a chip guard when I am turning bronze to keep from getting a face full.
 
1/8" on diameter doesn't sound like too heavy a cut, it sounds about normal to me.

I prefer to use a finer feed and more depth of cut when machining bronze in order to reduce the divergence of the 'chip spray' a little bit (like only a 5 foot radius instead of 15 :D). Use a neutral rake flat top tool. I've even machined bronze with Top Notch grooving inserts and use a quite healthy feed rate for the finish pass and still get a very smooth surface that needs no other finishing (filing or sanding). Maybe a very fine abrasive cloth could be used to impart a uniform sheen on a pretty part, but you may want to avoid any sort of hand work on a part with knobs sticking out nearby.
 
A description / sketch etc of the part would help.

Most cast bronzes I've come across have been short chipping, so with luck birds nests shouldn't be a problem.

Using the right insert is a must, ..sharp and high rake, .......which greatly reduce the cutting forces - which I'd say you need, I like the Korloy H01 inserts for non ferrous and use the CC** & DC** etc from this list Turning Inserts for Aluminium & Non-Ferrous.

Hint, - Allow for plenty of inserts - bronze can be very abrasive, and when the edge goes off the insert the cutting forces go up through the roof.
 
Can you clamp the part in another way? I mean, do you have an interior cylindrical surface or could you give the part one temporarily? Then you could clamp with an expanding mandrel on the spindle side and give it a hot go. An eigth inch depth of cut is fine, I personally cut shallower but with a more aggressive feed. Cutting speed up to 900 sfm, slower with alloys containing more elements than only copper and tin.
 
1915 at ATW. Showing lathe with center in spindle - so possibly that is where this was done - between centers. HSS of course at the time.
 

Attachments

  • 1915 Ad.jpg
    1915 Ad.jpg
    95 KB · Views: 210
When I want to take some big cuts on a between centers job I usually rough it out in a three jaw first then do final turn between centers to get everything concentric and true. Between centers is usually only necessary for shaft work where you want all your diameters to be concentric.
 
Thanks guys. No way to hold it in a chuck; this is a pure between-centers operation. Final OD of the (solid) spigot is either 3/4" or 5/8" depending on the version. Length is 2"-4" also depending. I've got +/- .002" tolerance to work with on the OD which shouldn't be a problem.

I'm using the CCMT sharp inserts that I use all the time on aluminum. For cosmetic reasons I'm keeping the center dimples small at this time.

These seem like kind of a pain but I've been looking for some regular, production-type work to supplement the lower-volume and prototyping stuff that are my preferred niche. This customer supposedly needs a batch of at least 500 of these every month, so, along with some bigger aluminum castings I'm also now doing for these guys this could fill up the empty time I'm wanting to fill. But at qty 500, shaving seconds will add up, hence my question.
 
By that description alone, (meaning, without seeing a print,) that wouldn't scare me at all. What WOULD worry me most, is keeping all those small, hot, flying brass chips from getting all over me. Beyond that? Run it man...

There's little chance you'll push the part out of the centers. The greater danger is either going to be chatter, or slipping of the drive-dog...

This is apples & oranges, but this part is being held between centers. "Big" centers - maybe a 5/16" pilot diameter, and around 1/2" to "5/8" at the largest part of the chamfer. Pre-hardened 4140, around .015"/rev, around 1/8" deep per side...

Trochoidal Turning - YouTube
 
IMHO it all comes down to center size, whats safe for a 1/4" depth of cut is massive over kill for 1/8" of cut.

The only real way of finding limits is to spit one out, go hard enough, you can break the tip off the centre, far more likely to skid the tail-stock back on the bed.

Other key thing to remember its not just depth of cut, but also often feed were the real forces come into play, personally i much prefer deep cuts and lighter feeds than the other way around. Uses more of the insert that way.

Alu spec inserts are a bit over kill in bronzes, i much prefer the coated super alloy - stainless ones. Still have nice sharp edges but the coating really helps with tool life. I like and use Sami's HA01 koroly inserts a lot, but i often use the negative style holders with them and often with a coated grade, there sharp and still very much a positive cutting geometry but nothing like a polished alu insert edge or rake. They work really well in anything that wants to be cut not ploughed and the coatings really helps reduce abrasive wear.
 
Thanks guys. No way to hold it in a chuck; this is a pure between-centers operation.
Dunno.. Part isn't all that long...
Final OD of the (solid) spigot is either 3/4" or 5/8" depending on the version. Length is 2"-4" also depending. I've got +/- .002" tolerance to work with on the OD which shouldn't be a problem.

A TWO Jaw chuck, bespoke top-jaws or plate with pins & such fixturing can hold a LOT of stuff that one would not think was "chuckable", and cycle it swiftly.

Part of why I have one.

If I had to "shave seconds" it would be power-operated, too, rather than manual, as mine is.
 
Swiss type lathe would be nice, would allow to turn from bars. No centers needed

What? And tell the customer to JF scrap the castings?

They are usually cheaper.

2-J chucks have been at this game - castings, even ignorant pipe nipples - since forever-ago lineshaft days.
 








 
Back
Top