Lathe material unsupported how much?

[3DM]

I'm not a lathe guy at all. How far out unsupported can I run a 3" bar of 6061 cutting simple features? The part is 3" OD x 0.75" thick, with a .075" boss on the back with the front having a radiused OD edge with a chamfered center hole. Simple less than an inch thick part.

Asking as I run 700 of these parts at a time. The vendor that's been cutting them just upped the price, and it's time I just put a lathe on the shop floor and run them in-house and bring the rest of my round work in-house as it should be. There is not a lot of open space on the shop floor, so a smaller well, used machine for now. So not bar feeding 3"!

Could I hold a 3" 6061 bar, 2" deep in jaws, then have, say, 6" unsupported, and then cut six parts per load? Cut face features, pre-chamfer (groove) the back, drill/chamfer, then groove/part off cut in to create the boss on the back, step over, and part off? Then do this down the material? Maybe lighter cuts/lower RPM at first, then more aggressive closer to the chuck? Just trying not to have to hand load 700 blanks, let alone cut 700 on the saw each run.



This is the back of the part. The front has a large radius, which you can see, and then a countersunk chamfer on the center hole. Simple part.

 

[camhead420]

Get a lathe with a sub-chuck so you can pull and face and chamfer in one cycle,
Drop it in the parts catcher as well.

As to your question 6" is as much as I let er hang out.

 

[3DM]

Get a lathe with a sub-chuck so you can pull and face and chamfer in one cycle,
Drop it in the parts catcher as well.

As to your question 6" is as much as I let er hang out.

I would love to get a dual spindle Y-axis lathe. But in our current economy, I need to keep the acquisition cost as cash upfront, so it limits me to $30k ish tops. I need to make whatever I get work for a while and let our economy come back some before I take on another machine tool payment. I just paid off my mill last week! I'm looking at smaller, well-used lathes. I just don't want to be leashed to it, feeling these pucks in.

Ok, so vote for no more than 6" unsupported. Thank you!

 

[Tungsten Carbide]

When you part them off, that aluminum is going to fling around and get dented. I agree with the sub/parts catcher idea. If you don't like having to do the saw cutting, a machine with a 10" chuck on the main and an LNS S2 barfeeder can run 4 foot long bars of 3" stock for you. I bet you could find that size machine with S2 barfeed for the 30 grand neighborhood. If the machine does not have a sub spindle, then make sure the parts catcher is well padded.

 

[Ox]

All depends on:

A) How well centered the bar is. (liner)
B) How fast you want to spin it
C) can you keep others away from the spinning / open end of the bar so that they don't git caught up into it?

Depending on your answer to these, you could easily stick it out 3', or as little as NONE!


I don't see this bar being a bend hazzard, as the lathe will likely be walkin' the floor before the bar bends?


----------------

I am Ox and I approve this here post!

 

[Orange Vise]

Could I hold a 3" 6061 bar, 2" deep in jaws, then have, say, 6" unsupported, and then cut six parts per load?

Yes, easily.

That's only 2xD. I'd go as far as 3.5xD in aluminum with adequate workholding, 2" in the jaws is more than adequate.

 

[3DM]

When you part them off, that aluminum is going to fling around and get dented. I agree with the sub/parts catcher idea. If you don't like having to do the saw cutting, a machine with a 10" chuck on the main and an LNS S2 barfeeder can run 4 foot long bars of 3" stock for you. I bet you could find that size machine with S2 barfeed for the 30 grand neighborhood. If the machine does not have a sub spindle, then make sure the parts catcher is well padded.

Good point the 7.8oz finished part would knock about a bit. Padding makes sense.

 

[Vancbiker]

Yes, easily.

That's only 2xD. I'd go as far as 3.5xD in aluminum with adequate workholding, 2" in the jaws is more than adequate.

How good the chuck is, chuck pressure, and whether hard jaws or soft jaws are the real determining factors in the workholding question.

 

[Tungsten Carbide]

That gives you a 2" remnant for every 10 or so parts. The LNS barfeeder gets you 45" worth of parts for every 3" remnant. I have seen lots of used package deals with barfeeder plus 3" bar capacity lathe. You can load up the magazine with like 12 bars, and all you have to do is keep emptying out your parts catcher bin. You can even cut this step out by getting one of those part collector systems to attach to the parts bin.

 

[3DM]

Yes, easily.

That's only 2xD. I'd go as far as 3.5xD in aluminum with adequate workholding, 2" in the jaws is more than adequate.

That's good to hear. It seems like it would work, but my material is usually not the part spinning in all the milling I have done.

All depends on:

A) How well centered the bar is. (liner)
B) How fast you want to spin it
C) can you keep others away from the spinning / open end of the bar so that they don't git caught up into it?

Depending on your answer to these, you could easily stick it out 3', or as little as NONE!


I don't see this bar being a bend hazzard, as the lathe will likely be walkin' the floor before the bar bends?


----------------

I am Ox and I approve this here post!

Ox, I would not run the material out the back of the lathe but inside the work envelope. Hold 2" deep with the jaws, then have 6" into the work envelope to machine the features, then salami slice off each 1" part.

Yeah, no thanks for spinning material out of the backend of the spindle! Thirty years ago, as a button pusher in the first shop I worked in, I saw firsthand what an unsupported material (brass, in this case) outside the spindle does. An "experienced" programmer wiped the backside sheet metal, and then the bar broke and launched through a cinder block wall. No one was hurt but the guy's employment.

 

[3DM]

That gives you a 2" remnant for every 10 or so parts. The LNS barfeeder gets you 45" worth of parts for every 3" remnant. I have seen lots of used package deals with barfeeder plus 3" bar capacity lathe. You can load up the magazine with like 12 bars, and all you have to do is keep emptying out your parts catcher bin. You can even cut this step out by getting one of those part collector systems to attach to the parts bin.

My non-lathe brain was thinking I would accumulate the 2" spuds, then hand load them holding .75" in dedicated soft jaws, cut one face feature, hand flip cut the other face feature, then run a wide grove in the middle to make the boss, then part off. = two parts.

I agree. If I can find an affordable use 3" bore, though, I am down to bar feed full 48" bars. Way less saw time!

 

[Tungsten Carbide]

With a spindle liner, you only go as deep as the back end of the spindle, so 3-4' long. This machine would give you plenty of bar capacity, with room in the budget to get the barfeeder:

DAEWOO PUMA 12LC CNC Lathes Used - Good #595407 - MachineTools.com

DAEWOO PUMA 12LC CNC Lathes for sale by Industrial Machinery Company - Used - Good - Texas, United States - #595407

www.machinetools.com

 

[Ox]

That's good to hear. It seems like it would work, but my material is usually not the part spinning in all the milling I have done.



Ox, I would not run the material out the back of the lathe but inside the work envelope. Hold 2" deep with the jaws, then have 6" into the work envelope to machine the features, then salami slice off each 1" part.

Yeah, no thanks for spinning material out of the backend of the spindle! Thirty years ago, as a button pusher in the first shop I worked in, I saw firsthand what an unsupported material (brass, in this case) outside the spindle does. An "experienced" programmer wiped the backside sheet metal, and then the bar broke and launched through a cinder block wall. No one was hurt but the guy's employment.

I have one job that I can think of that I run (ran ... not seen that come through in several years now?) that I run steel that I turn an 8" length of 1" diameter - unsupported.

I know, and have seen what you speak of above.


-------------------------

I am Ox and I approve this here post!

 

[guythatbrews]

Barfeed it without a bar feeder. Get a bar puller. Royal makes a coolant operated style, and spring finger styles are available. Surely you have enough room for 3 extra feet clearance at the headstock. A good spindle liner is still a must.

 

[Pete Deal]

Aren’t you still going to have to finish the back side in a separate later operation? If so you’re going to have 700 partially finished parts floating around. i wonder if it would be possible to make some jaws with mitee byte versa grips for first operation and same jaws also bored out for the back side operation. I know you’d need to precut the 700 blanks.

I never used versa grips, maybe not possible.

 

[3DM]

Aren’t you still going to have to finish the back side in a separate operation? If so i wonder if it would be possible to make some jaws with mitee byte versa grips and same jaws also bored out for the back side operation. I know you’d need to precut the 700 blanks.

I was thinking I could get away with one op.

Prior to the part off, I would v grove the area the part off tool would go into so that it creates the chamfer on that backside OD edge. Then run a .200" wide part off/groove tool (no idea if they make them, but I think they would) down to the outside OD edge of the boss. (.4375" R for the boss) Then come in with a .120" wide part-off tool (I know it exists) stepped over, creating a .080" wide boss on that backside. (Currently .075" but it's our part so I can change the depth if it fits, and .080" will) The part falls, and we make the next one. I then will have to manually deburr the backside center through the hole from the part off op. But if this would work, it's a one op part.

One of the first vendors making them for us definitely was using a part off tool on the backside. All along, I have assumed they were making the way I described above. But the current vendor is cleaning up the back and putting a nice radus at the base of the boss and a clean little chamfer on the center hole on that backside. I think they have a duel spindle lathe or some poor button pusher chained to the machine tool.

@Ox @Tungsten Carbide : with parting off "heavy" in this case, half lbs each aluminum part. How do you keep them from getting beat up? Tungsten Carbide, you made a great point earlier on padding a parts catcher. If a lathe does not have one, what is the best practice? Stick your hand in and manually catch it? Slow the part off RPM down so the part mostly drops vrs getting slung? (big burr I would imagine)

I don't remember from 30 years ago if we ever had "heavy" parts parted off in production. Certainly, remember me as the lowest guy in the shop's job of fishing through chips to find the small parts parted off. It was always fun, gloves in a machine shop??!... nope, just cuts flushed out with old stanky coolent. Bandaids were free. Good'ol days.

 

[Ox]

Well, I'm not seeing why you need more than your normal cut-off blade?

Recess with a threading tool. Line up your point to the end of the part...

Cut-off:

Run it down to your boss D at .. say Z-.02 (long for safety's sake))
Come back up and back chamfer the OD with the cut-off tool and work your way back down in at +.100.

Then move back .080 (should have some Clarence yet) and back chamfer (or rad) the boss OD, and then finish the cut.

If you can't recess for whatever reason, then you can cut-off all but a smidge.
If a solid bar - then twist it off by hand. If you are using a 15* insert, then it should break off relatively clean.
If a hole through, then leave as little as possible, and break off with a rubber hammer.


These are how I run low qty parts that don't make it on the 8x machines.

---------------------

Think Snow Eh!
Ox

 

[eKretz]

Out to 3xD is generally as good as 1xD for all but the most demanding work. (Like very large form tools).

 

[Triaged]

... how do you keep them from getting beat up?

This might be a bit big but a coat hanger through the ID bent around to be able to stack a few up.

 

[EmGo]

I'm not going to argue that you can't do this, but ... I would not choose to do it this way.

Parting 1" stuff is okay, a little bit pain in the ass because parting tools aren't that great and revving the spindle to 2,000 rpm to try to get a decent surface speed down low and the finish is always a pita and then the part flying off or you figure some way to catch it and and and ... but 3" bar ? No thanks.

Many materials suppliers are equipped to cut the bars into slugs for pretty cheap right when you buy it..

If not, there are places that do nothing but saw and considering the partoff blade width you'll need to go that deep, might save material as well.

If not that, a halfway decent band saw is a beautiful, useful thing to have in the shop. A power hack for five or ten but 700 is worth some kind of bandsaw. And you'll use it all the time for other stuff.

Soft jaws, two programs, do the back side with program one then flip and do the front side with program two all in one sequence and you have a steady stream of completed parts going to wash and clean and anodize or whatever. Pretty finishes, big bubbles no troubles, the end result will probably be, it's a lot easier to just do it "the hard way" than try this salami-slices method.

I think all of us who do lathe work have tried this. It sounds attractive but for most guys we gave up and accepted that the quickest, easiest, cheapest method was usually just give up and do it what seemed like "the hard way". Not always but mostly. The parts you show, for sure.

A few are still out there promoting this method but if you quantify the results, well ... hard heads don't change easy