Chatter. Could go for some creative programming or...?

Hardened · Jan 30, 2018

So we Turn, chucking on to a (304ss) 4ft long, 5in diameter part with a 1.25" diameter shaft 8" long, centered, in a CNC with tailstock.

Trouble is, when turning the small shaft for a bearing fit, there is a LOT of chatter. I suppose the solution for the past umpteen years has been to have the operator toggle the speed/feed override continuously, which works "well enough" ...

Lathe is a 1998 Yang, Fanuc, turret type with tailstock, no accommodation for a steady or follower.

Is there a way to simulate the toggling from a programming perspective, akin to having it ride some sine wave perhaps? I'm running it now and would love to fix this age old problem while sparing my hands.

jeffm8622 · Jan 30, 2018

What is your G50 value? Your G96 value? Also, what is your insert geometry for the rougher? I'm assuming the chatter is during the roughing cycle?

Gobo · Jan 30, 2018

Is your turning tool optimized for the application? Give some specifics. Your length to diameter ratio is pretty nuts with no follow or steady rest.

Hardened · Jan 30, 2018

Likely capped at 450rpm, wouldn't surprise me if they programmed it straight rpm and not sfm. I'll check tomorrow, I'd venture to say it's pretty basic.

55deg .032R GP chipbreaker AlTin coating

Same tool roughing/finishing (I KNOW!)

I'm tempted to rewrite it all together to get roughers and finishers in there.

There's a lot to be done from a technical standpoint but I doubt I could get them on board with revamping what's "worked" for 20 years, but I'mma try.

Triaged · Jan 31, 2018

Hardened said:
...55deg .032R GP chipbreaker AlTin coating

Same tool roughing/finishing (I KNOW!)

Iscar insert? Try a -TF.

Guest · Jan 31, 2018

My go to default on getting rid of turning chatter is to lower the RPMs then bump the feed up.

precisionmetal · Jan 31, 2018

Possibly...

Rough with the tool you have at a high enough feed rate to avoid chatter (reduce depth of cut if necessary).

Finish with .016" radius insert (or even sharper), at higher speed and lower feed rate.

Jashley73 · Jan 31, 2018

You need a positive/single sided insert for sure. Something with a thin PVD coating, and probably intended to finish stailess or super-alloys. These will have a sharper cutting edge, and will cause less deflection & cutting pressure - which is what upsets the part & creates chatter in the first place.

I'd recommend a smaller nose-radius too.

Tungsten Carbide · Jan 31, 2018

This won't help the current situation, but if you look at new machines (or even used up to about a decade old), some of them have that harmonic spindle speed control feature built in so you don't have to play with the speed over-ride. My Okuma and my Hardinge have it and it works great. Just set the amplitude and period of the spindle speed oscillation and the finish is beautiful. Turn it on and off with an M code. My Haas has it too, but the machine is not as rigid so it can't achieve the same finish on the same parts.

With your current machine, I agree with sharp and small radius -- I use .008 nose radius for finishing.

gorrilla · Jan 31, 2018

I was gonna say, before TC beat me to the punch, this problem has been approached by Okuma I know, and I figure likely many others, with a harmonic speed variation program, which does the same thing as you standing there floating the spindle speed up and down.
Why in the hammer headed hell you are seeing resistance to writing a program with separate rough and finish tools I'll never understand. That's SOP around here. We run hundreds of shafts about every 90 days. Bearing fits typically in the +/-.0001 range. The smaller tool nose radius could likely solve your problem, as could the much more positive geometry. But any of these is gonna force you to re-write the program to include a separate finish tool. Which I think you need anyway.
Just because "it's the way we used to do it" has probably cost more in lost production than any phrase in history.
Since you are not likely to get a new machine with the fancy software to vary the speed automatically, I'd say look into the separate finish tool, and play with geometry. Good luck convincing somebody above you to spend the money, which is exactly why they are resisting.

Hardened · Feb 1, 2018

Figured I'd chime back in with some more info and pics, small shaft chatter throughout, wider portion chatters 1st 10 inches.
G50 1000
No G96, S500 for shaft (slow IMO) S350 body (Eh) feeds are in IPM and God Knows WHy
Machine is 1996 vintage so likely no okuma-esque anti-chatter, nothing in the programming manual.
I agree with finish tools, would help us keep things tighter too, I'm going to get a copy of the program and modify it.

Is there a way I guess to go G96=A
A= a number between lets say 400 and 500 where once it gets to 500 it goes down to 400, and this shift takes X amount of seconds.

https://i.imgur.com/tmdAD59.jpg

https://i.imgur.com/Ai0XOG7.jpg

litlerob1 · Feb 1, 2018

Hardened said:
Is there a way to simulate the toggling from a programming perspective, akin to having it ride some sine wave perhaps? I'm running it now and would love to fix this age old problem while sparing my hands.

Okuma does that, it's not great result, I wouldn't use it to finish. But to answer your question YES of course you could long hand the code in segments that changes the RPM thus the frequency. But I don't thing that is the best solution.

In post #4 you said you are running it, but use words like "likely" and "wouldn't be surprised" what is it? If your use 450 RPM at 5" diameter in 304 :eek:

thats 588 SFM a wee bit fast. At 1.25" it's 150 SFM, a little slow for Turning but hey?

Are you using CSS or CRPM?

Ox · Feb 1, 2018

I have a face grooving job that likes to chatter if I allow it to. So I go a little bit and then change the RPM, and go some more, and then change back. Not a nice canned cycle, but git's the job done.

If you told me that you was having issues with chatter on the 5" portion - I would understand (BTDT) but I haven't had issues on the stub ends like you are.

???

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

Think Snow Eh!
Ox

mikiemus · Feb 2, 2018

Doing a cut with right angle of cutting... 87, 83, 75, 63 degree angle of cuttingtool is one thing. do the right cuttingspeed is one thing. Make variable cuttingspeed to avoid shatter is a pain in the butt, but doable in a machine that has not that option. G1 some or part of inch and change speed during that distance, change it on the next distance.. etc. (yes programming pain in the butt) Everything pends on how many parts you want to do, in what of machine. If you can not do scrap parts for test, your in the cloud and grey zone. Use your scrap parts to learn from it, and do small steps at the time. Smaller dia and your ok, works on the greater. Have patience sacrifice some time and try it out. Smaller cutting dia speed and cutdepth.. use to be the treat. Milling or Turning.
Cheers

litlerob1 · Feb 2, 2018

mikiemus said:
Doing a cut with right angle of cutting... 87, 83, 75, 63 degree angle of cuttingtool is one thing.

What do you mean by that? (This is a Turning)

mikiemus · Feb 3, 2018

litlerob1 said:
What do you mean by that? (This is a Turning)

The angle the edge is positioned towards the cutting. A 87 is 3° rake (I think its called)
Usually a standard VBMT, DNMG has 3-5°, but there is those others aswell.
Why different angles? If you can get 100% of the cutting load axial then the radial force is minimal, and shatter minimal.

Long bars use to climb up on the cutting edge and get out of Y pos, = shatter.
If nothing works at all, and your workpiece is a straight bar, try a piece of plastic or similar
above the cuttingtool, pressing slightly downwards on the bar preventing the bar from climbing.

BSCustoms · Feb 3, 2018

Sometimes when working on shaft work near the center end it is helpful to cut towards the center so it is loading positively instead of towards the chuck possibly bowing and unloading your center support.

Ox · Feb 3, 2018

mikiemus said:
If nothing works at all, and your workpiece is a straight bar, try a piece of plastic or similar
above the cuttingtool, pressing slightly downwards on the bar preventing the bar from climbing.

Could be a mounting challenge, but that is a simple follow rest eh? :cool:

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

Think Snow Eh!
Ox

Chatter. Could go for some creative programming or...?

Aluminum

Aluminum

Titanium

Aluminum

Aluminum

Guest

Guest

Stainless

Titanium

Aluminum

Stainless

Aluminum

Diamond

Diamond

Aluminum

Diamond

Aluminum

Cast Iron

Diamond

Similar threads