What's new
What's new
By:
Advanced search…

eliminating chatter

S

smp4616

Plastic
Joined
May 9, 2015
Hi, this might be a stupid question but I'm trying to take on a job that might just be too big for my lathe, I already removed the tool changer and am running a tool holder I made for an 1/2" insert, I have .1" clearance between the part and the max X travel on the lathe, so I'm a bit limited on strategies. I need to cut the center section but am running into chatter so bad it's moving the part around, or breaking inserts, is there a feed/speed recommendation for this? I am also running into stopping the spindle if I enter the part or feed too aggressively... would really like to be able to make these parts, but I need to know if I should call it and move on. I am also considering using a smaller 6mm round insert, but I feel like having such a skinny tool holder would make the chatter worse....

lathe_zpsar1fkrwe.jpg
 
Way too big of a tool. You need to use the smallest full-radius tool you can get even if you have to buy a new holder.

On the finish pass you'll need to run real slow RPMs.
 
Plunge some material out with a much narrower parting blade or grooving tool before trying to plunge with the full radius tool. Try to engage as little of the full radius tool as you can. The further away the tip of that tool is from the tool post the more rigid the holder needs to be, and it looks small to be hung out that far.
 
thanks, that's kinda what I thought, I've got some 6mm inserts coming in tomorrow, I will build a new holder today, also, will adding a jack screw to the bottom of the tool holder help or is that a bad idea?
 
CNC I assume? Even 6 mm may be too big. I'd grind a much smaller radius left and right hand tool from HSS. As above, remove as much as possible with a parting tool or similar first. Watch out for SFPM on larger diameters- it can sneak up on you.
 
What about doing with 2 different tools, a pair of opposite 35 degree profiling tools comes to mind.

I just picked up a Kennametal SVABL-082D, I think a SVABR-082D would be the opposite. The "L" tool is about 6 inches long and by the screw marks I have extended it at least 2 inches. It is a 1/2 square tool I use on the gang tool machines. I am sure they have other tool heights.
 
FredC said:
What about doing with 2 different tools, a pair of opposite 35 degree profiling tools comes to mind.

I just picked up a Kennametal SVABL-082D, I think a SVABR-082D would be the opposite. The "L" tool is about 6 inches long and by the screw marks I have extended it at least 2 inches. It is a 1/2 square tool I use on the gang tool machines. I am sure they have other tool heights.
Click to expand...

That's how I've done it in the past, and how I would attack this part also.

I've tried those big round bastards before, and they seem to fail far more often than not.
Just far too much contact area.
 
The work shouldn't be moving around, because of the tail center pushing against a plug on the outboard end. It's not shown in your pic, but it must be there ;) :D

I'm in the two (or even three) tool camp. A cnc lathe certainly doesn't require a radius tool except maybe to blend across the center line for appearance/accuracy's sake. Somebody mentioned Sandvik Prime turning, that's some new technology toolholder and insert that can apparently cut in the unexpected direction!
 
yup, tailstock supported, it just chattered and made the whole machine shake... the 35 degree cutters unfortunately won't reach that far in without running into the tailstock side, also I am trying to avoid swapping tools since I didn't build a quick change tool holder, so changing a tool in this configuration requires turning something to reset the diameter... ugh. I'm putting hope on the small insert
 
Button inserts are nice to get all around, but you have to push them pretty good OR you tickle it to death to avoid chatter.

I'd go for using cutoff like tools plunging to center, MDT's to plunge or back and forth. I have had good success VNMG's, One turning right to left, the other left to right...long small sharp insert can really get in there and amazingly it can make quite the chip.

As you into a Too Small machine for the job...avoid thinking big honking tools and think small cutting tips, small cutting area, smaller, faster lighter cuts. Its CNC, make tight chips and let machine do its thing.
 
I can say my experience with the round button tool inserts are not a great roughing insert. They do lend themselves better to small depth of cuts steady say right to left or vise versa. Basically you would be peeling that metal off at least .02 depth of cut per pass.


Taking more depth of cut will cause more chatter. I would try not to use a jack screw as that likely will come loose and if that happens then just trust me you do not want to find out. Most of your chatter problem is geometry of tool depth of cut, feed rate and speed combo. It is better not to go too fast. Allow your tools to have enough time to round out. Leave a fair amount of material on your first complete roughing process and that way if you have chatter on the finish you allow material on to find your best settings for finishing.
 
smp4616 said:
yup, tailstock supported, it just chattered and made the whole machine shake... the 35 degree cutters unfortunately won't reach that far in without running into the tailstock side, also I am trying to avoid swapping tools since I didn't build a quick change tool holder, so changing a tool in this configuration requires turning something to reset the diameter... ugh. I'm putting hope on the small insert
Click to expand...

Maybe time to get a Multi-fix toolpost on there. For a situation like yours, you need to be able to change tools, going from beefy, to light duty. No question.
 
smp4616 said:
thanks, that's kinda what I thought, I've got some 6mm inserts coming in tomorrow, I will build a new holder today, also, will adding a jack screw to the bottom of the tool holder help or is that a bad idea?
Click to expand...

Something along this line would be my first try.
I was thinking more along the lines of a pc of 1/2 x 2 standing on edge under your skinny tool, but you may need a bigger (deeper?) holder to make something like that happen?


That shank needs to be narrow, but it doesn't need to be square!



Another thing to help is to vary the spindle rpm's.
I'm guessing that you are running an incr smaller D on a subroutine, so if you can put some RPM changes in the sub - possibly frequently - this can help a bunch. (Depending on how long it takes to start ringing)



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

Think Snow Eh!
Ox
 
Ox said:
Something along this line would be my first try.
I was thinking more along the lines of a pc of 1/2 x 2 standing on edge under your skinny tool, but you may need a bigger (deeper?) holder to make something like that happen?
Click to expand...

The ones I have made by Kenny,Carbo, Seco all have full depth shanks,
don't understand why the OP would make it shallow in depth.

I would braze a piece under it (to thicken it up), I would not play around with a simple screw.

EDIT: thinking on this more.

Seeing how its a homemade tool holder, how about tilting it slightly so it has
some positive rake, a "helical sheer" ramp to it ?

Yes, the radius will be slightly compromised (not a true circle).
 
Last edited:
I skimmed the posts in this thread and never saw anything about speed or feed. While it may not be the greatest for production try cranking the rpm down. I always figured that 40 rpm on an engine lathe was for the benefit of large radius tools when cutting something like a flywheel. Lower rpm = less chatter. As for feed/rev it should be more or less the same it would be at higher sfm IMO.
 
Just plunge the Tool you are using in about .025" and Feed across on the Z Axis, then go in another .025, and feed back...so on, until it's Roughed out. The Chatter and Load are coming from straight Plunging on the X Axis.

R
 
litlerob1 said:
Just plunge the Tool you are using in about .025" and Feed across on the Z Axis, then go in another .025, and feed back...so on, until it's Roughed out. The Chatter and Load are coming from straight Plunging on the X Axis.

R
Click to expand...

that stopped the spindle... when I manually tried plunge feed at very low rates, the tool started to chatter massively once it got enough contact area. I think it's the lack of pressure on the cutting edge that's doing it really, with such a large cutting area, it's not really possible for the setup I have to make that tool work, I'd need a very rigid tool holder and a ton of horsepower to keep the pressure where it would be for an insert with a .031 radius. I am going to look into a quick change toolpost for this setup, I think this job is going to need a couple different tools to make work, I'm also trying the 6mm insert today, I have a better feeling about it
 
smp4616 said:
that stopped the spindle... when I manually tried plunge feed at very low rates, the tool started to chatter massively once it got enough contact area. I think it's the lack of pressure on the cutting edge that's doing it really, with such a large cutting area, it's not really possible for the setup I have to make that tool work, I'd need a very rigid tool holder and a ton of horsepower to keep the pressure where it would be for an insert with a .031 radius. I am going to look into a quick change toolpost for this setup, I think this job is going to need a couple different tools to make work, I'm also trying the 6mm insert today, I have a better feeling about it
Click to expand...


That makes no cents to me.


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

Think Snow Eh!
Ox
 
You must log in or register to reply here.

Similar threads

1
Help chatter while machining a shaft (CNC lathe).
2 3
Replies
41
Views
2K
Sandy171
S
Bendak
Purposely Introducing Chatter into a workpiece
Replies
5
Views
552
rons
rons
Q
Cutting 316L with long tools
Replies
10
Views
393
Turntech
T
G
Parting off 400 series custom age S.S.
Replies
9
Views
281
Ox
Ox
M
2A thread pitch undersized
Replies
11
Views
503
camhead420
camhead420








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top