Chip extraction from tubular parts on CNC lathe

"Robin S." wrote in news:205ff240-a541-4ff1- snipped-for-privacy@p32g2000vbi.googlegroups.com:

The groove/thread is at the chuck end of the bore??? Or the entrance end????

Possibilities:

Do the grooving/threading last.

Off the wall: see if you can use a peck cycle to groove. Should help chip length.

Use a smaller dia. bar to finish bore.

Different tool geometry to break chips better. And leave a little more material for finish pass.

Like Cliff asked, what is material??

Snip

Hi Robin, Any chance of leaving the bore finish cut for last, and doing it as a "drag out" pass? You might even try this in two steps, first sending the bar in deeper with a movement profile that tries to hook the nest onto the cutting edge, but doesn't move in X enough to cut material during the Z+ move. Set up a coolant jet to knock off the chip nest, then drop the bar back into the bore for the final pass.

With the tube stock, as long as you can reliably push the nest down the tube, it might work out, but it could foul the bar feeder if you're using one.

One other possibility is trying to change the cutting profile of the groove to produce short, heavier chips, perhaps by changing the chipbreaker profile and programming short move/pause feeds. Then aim a coolant jet down the bore to wash them out with the spindle off.

HTH, GPN

Chuck end (the tough end).

The problem is that I have to finish the 1" ID of the tube after the groove and thread is finished because the boring/threading chips mar the finished surface if they are done last.

Using Fanuc 18T. I have not seen such a cycle (turn pecking). This _would_ very likely help, but I'm loath to hard code this. Perhaps I'm not being cunning enough with the G71 canned turning cycle? Ach. Perhaps I should just run a couple of G71 cycles as the Z feed length is reasonably short (about 0.3)

3/4" solid carbide bars extending 4-1/4" from holder =3D 5.7:1. I don't think we can drop a size (that would be $1500 to replace the three bars too)

The groove tool currently has no chip control. I think there is that possibility, but I'm not entirely confident that inserts with chip control will even do anything (from prior experience). I'll have to look in the Kennemetal book.

Doh! 6061 T6.

Regards,

Robin

There is some possibility of using the groove tool to grab the chip nest. I haven't really tried this as the bar and the insert are carbide. Seems like a busted insert in the making.

The 1" ID bore finishing tool is 55=BA DCMT (or similar - I forget exactly which insert we're using). It can't even access the chips due to the bore's geometry. We are pull finishing the 1" bore to prevent chips getting between the bar's shank and the tube.

Not currently, but we will be soon(ish). We put a plastic plug with an o-ring in each tube previously (we're trying to switch to solid stock now, but things aren't looking good).

Yeah. I could try a couple of G72 cycles with heavier feeds to create smaller chunkier chips that won't turn in to continuous streams of chips (i.e. nest building material).

I guess I'd just prefer to reliably pull the chips out every time, hence the grabber idea....?

Regards,

Robin

How about some high pressure coolant?

I'm sure it could be quite a mess, done wrong.

Later,

Charlie

Looks spendy BUT we're now doing three variations of this part (three different products) so it may be worth the investment.

Any idea how much for one of those boxes? Perhaps will call Monday am.

Regards,

Robin

I don't have a clue about the cost. The only reason I know anything about it is the first shop I worked in had just bought one and we got to see some demo video of this thing clearing chips like nothing you've ever seen before. I never did see it run in real life. The problems were solved in a completely different way, so the thing just kind of sat behind a lathe during my 15 months there. I was surprised I didn't find any video clips of it in action on their web site. I went looking on YouTube, and I found these guys.

have some nice videos. There might be even more companies out there with this kind of product, so if you get a few to bid against each other the price might be better than expected.

Later,

Charlie

Try using a smaller, dampened boring bar. They will work up to 10 x shank diameter.

www2.coromant.sandvik.com/coromant/pdf/Silent_tools/Silent_tools.pdf

Robin, I wonder if a boring bar with thru coolant blasting away would help?

Best, Steve

The grooving bar and the 55=BA bar have through coolant. Not high pressure though. Our coolant pressure does nothing against this chip nest. Totally useless.

I'm wondering about forcing the coolant through a small nozzle to increase pressure. We just installed a fine stainless steel mesh filter after the pump as the tool holders were showing up with chips in them after several hours of production. If a chip ever made it through, it would plug a smaller nozzle. Would not result in a crash, but rather scrapped parts. Not sure if our pump can keep up with this, though I should really just try and see.

Regards,

Robin

It continues to astonish me how bad indexable cutter companies are at selling their products. I didn't know those bars existed.

I'll look into them. Would be worthwhile to have a 55=BA bar with a 1/2" shank for the final finish. This would pretty much eliminate the need to remove that nest.

Thanks for the heads-up!

Regards,

Robin

Robin, I also had to put a fine mesh filter on both lathes and mills. I was surprised at how large a chip could get run through the coolant system.

On a general coolant note these guys have a huge selection of coolant nozzles:

I use these a lot on my lathe: Best, Steve

"Robin S." wrote in news:ab422604-2990-43b1-8488- snipped-for-privacy@p8g2000yqb.googlegroups.com:

I've had good results with these -

"Robin S." wrote in news:ab422604-2990-43b1-

Why can't you turn the part around and do the groove on th "short end?

Think about this:

1. Start with stock close to chuck.

1. Drill just deep enough to do the groove.

2. Do the groove. Stop spindle while tool is in hole. Use the tool to drag out the chips.

1. Thread. Stop spindle in hole, use it to drag out chips.

2. Bar pull part out to length you want.

1. Drill and bore rest of ID. Why not use an inserted drill to drill AND bore? Kennametal has a 4X drill. (I've been doing this for 15 + years on a part that I make: drill 1.125 hole, bore to 1.182 +/-.0005. X 3.265 deep.)

You know, I've been looking at this problem for too long. The machine has a subspindle.

We've run out of Z with the part hanging out (main chuck + part + indexable drills + turret + subspindle chuck =3D crash), but with the part in the chuck and two sets of boring tools (both ends of the part require the use of internal grooving and threading tools), this is actually a possibility.

It would increase our cycle time because the subspindle moves kinda slowly and it would require an extra tool change BUT the reliability would be far greater. It would also eliminate the special cutoff tool we use to reduce the cutoff burr, and the part would require no deburring after it comes off the machine. Still only one bar pull too.

We have an extra set of steel boring bars which use the same inserts so I could do this next time one of these parts gets up on the machine.

Fudgesicle.

Thanks for the suggestion. Will run it through the boss.

Regards,

Robin

We have some jobs where we take a bag filter to cover the coolant pump inlet to stop fines and small chips from getting where they cause grief.

Wes