Boring bar

[Joels]

I am using a 1 inch dia boring bar with a neg 5 deg rake and a diamond shape carbide chipbreaking insert. I am going approx 3.2 inches into the part. The problem is that it chatters like crazy. If i slow the rpm down to about 200 rpm it works ok. but the cycletime is way too long. I am cutting 6061 aluminum i will put the program in the lathe folder on the FTP site. I would appreciate any information. the file will be called watermaker.mc9

[Brendan P]

Are you saying that you are getting chatter on the finish path,or it is chattering on the ruffing passes and the girls are complaining?

You are only taking .100 per side which IMO,is nothing.

 

If it is the finish pass that you cannot get a good finish,ruff it out with the 1.0" bar and finish with a more meatier bar 1.5 dia.

Also if you do use this method,you may want to leave a little more for finish pass if it is chattering on the ruffing,because with only .010 for finish,even with a bigger bar,it may still chatter.

Leaving more for finish pass with a bigger bar will allow you to 'get under' the chtter.

 

HTH's

Also,a solid carbide bar works great but pricey....

[chris m]

I just looked at your file and here are my thoughts:

 

1) 3 X D is a relatively long overhang for a steel bar but not ridiculous especially when cutting aluminum.

 

2) Your surface speed is WAY low for aluminum and carbide isn't going to like that too much. If I was running this job I'd be roughing it at 1000-1200 SFM [around 2730 RPM on the first pass]. Is there a reason that you're running G97 instead of G96? Constant spindle speed in a lathe, in my opinion, sucks.

 

3) Your DOC and feedrate seem pretty reasonable for a bar hanging out that far.

 

My ideas on this:

 

1) Make sure that your bar is on center, nothing chatters worse than a boring bar that is low.

 

2) Choke the bar up as far as you can without running the turret into the face of the part; the overhang required to machine the part is big enough without another 1" hanging out for 'clearance'.

 

3) Make sure you have an insert with very positive cutting geometry [sandvik's CNMP is what we use for a negative insert in aluminum] to keep the radial cutting forces down. I'm not sure what insert you're using now but a steel or cast iron geometry will present a FAR too negative edge to the part and definitely cause vibration with that bar hanging out that far.

 

4) Assuming that you have a pretty good grip on the part and that your machine has the capability I would defintely run a lot more RPM and use CSS instead of G97. I'd start at about 800SFM and move up from there; sacrifice a little DOC if you have to but keep the RPMs up or you'll have a very unhappy insert.

 

 

Let us know how you make out

 

C

[Joels]

Thanks for the information. I am using a CNMG 432 insert now. I did put CSS in the program on the machine but i had to use G96s150 to get the chatter to stop. I also have a feeling that the negitive 5 degree angle on the boring bar is not good should i be using a zero degree rake angle? I have also tried a PCD diamond insert and it chattered to so thats why i am thinking the rake angle is bad.

[unknown]

Are you sure that the turret isn't out of line or that maybe the boring bar isn't bent or otherwise not properly oriented to the piece? THere is no way that you should have to choke the RPM back that far; I'm surprised that the insert doesn't chip going that slow.

 

As far as the positive / negative argument goes, the insert geometry is at least as important as the actual boring bar geometry. CNM inserts designed for aluminum are in the boring bar negative [for security and durability] but are ground or molded strongly positive for a good free cutting action. If you are using a CNM insert designed for aluminum now, going positive is unlikely to make a HUGE difference in cutting forces, nor are you likely to be able to run the DOC or feedrate that you want for very long without edge failure.

 

If you choke the boring bar up and only bore about 1" deep with the same setup and parameters what does it do? If it is still loud or shows vibration I'd say you definitely have a cutting tool or machine tool prob...

 

C

[chris m]

Weird; how the heck did I post as 'unknown' ?

 

C

[Joels]

i was reading other posts on boring bar and someone suggested i use a positive rake instead of a negative rake so i will try that. I have the bar sticking out about 4 inches and i cant put it in any more. I didnt think sticking out 4 inches on a one inche dia bar would do this but it does. I am thinking of ordering a one inche carbide bar with a zero rake angle how does that sound? the biggest problem is i am using a old Hass lathe and the turret tooling is very limited.

[Harryman]

I'd cut off the steel bar before buying a carbide one, but if this job will run a while or be back often, go carbide.

 

Is the insert pocket screwed up? It doesn't take much deformation from a previous crash to eliminate insert support. This will cause chatter in cases where there should be none. If the pocket is deformed, some careful peening of the pocket edge can help till you replace the bar.

[Hardmill]

quote:

---

Weird; how the heck did I post as 'unknown'

---

puff, puff pass Chris

No bogarting

 

Never saw that one before

 

Even got a member #

---unknown

---New Member

---Member # 8535--

 

 

PEACE

[Hardmill]

How old is your lathe?

I had this prob. before and it was fixed as simply as

tightening the gibbs (old lathe of course)

Sounds like a machine prob to me.

All other variables don't look out of range for

what your trying to do.

 

 

 

PEACE

[Joels]

well i was thinking of buying a carbide bbar and using a zero degree angle. How does that sound?

[Brendan P]

Carbide boring bar is always better for less chatter,but I think you should try as suggested to 'stub' up the tool a couple of inches and see if it still chatters.

[Bunny McRabbit]

What is your insert corner radius ,watermaker ?

[Joels]

i have a .031 radius on the insert and the bbar is in the turret as far as possible i have about a .5 clearance from the turret to the part at the deppest part.

[PE @ IHS]

Try a CCMT instead of a CNMG insert. Also, the .5 clearance is still longer than necessary, unless you have no other way of getting coolant in the hole.

 

Are you sure the tip is on center? Do you know how to check?

[McRae]

Are you sure the tip is on center? Do you know how to check?

 

Peter, What method do you use to check, I have seen the Turning-Tool-Chuck-Jaw-Scribe-Then-Check-The-Boring-Bar trick in the past but I hope that you have something more elegant.

[Hardmill]

quote:

---

but I hope that you have something more elegant.

---

Is'nt any more simple than putting an indicator in

the jaws and sweeping the turret.

I honestly believe its a machine issue.

Has any one crashed that lathe lately??

Even the slightest bump could throw it out.

 

PEACE

[Fralex_francois]

does it chatter only at final pass, cause at final pass with .010'' it's not enough and you need to cut at least the radius of the corner of the insert.

With this you can repeat very tight tolerance and have nice finish.

I did'nt check your part, but if you finish it with a different tool it would maybe be better...

HTH

[Philcott]

Watermaker,

 

I was just wondering if you might be having clamping problems. Is the chuck pressure high enough and is the paty being firmly held? A 1" bar out 3.2" shouldn't give you much trouble. Others here have made good sugestions regarding the center height of the bar (there could be an incorrect shim in the bar), pocket damaged. I don't think your problem is with bar overhang It doesn't seem excessive to me. Also, Chris's feed and speed recomendations are right on.

 

Another thing I am curious about is the direction of the cutting force. In other words when the part is running, are the cutting forces pushing the turret down onto the ways or is it cutting in a manner that lifts the turret away the ways? I ask this because we had problems with our Hardinge Conquest when the trucks and rails were worn. If your cutting forces are lifting the turret (even minimally this could be the problem.

 

Phil

[Müřlıń®]

quote:

---

the biggest problem is i am using a old Hass lathe and the turret tooling

---

Rigidity on a turrent is weak.

 

I would definatly go with a highspeed boaring bar on this application.

 

Something very positive and sharp.

 

Slow down the speeds and feeds but take more of a cut so the cycletimes dont get out of control.

 

Your part is probably off the chuck a bit also which adds to the ridigity problem and with any slack in the gibbs, once the chatter starts, it keeps going.

 

my 02

[Brendan P]

I'm starting to believe it's a machine issue.

I use cnmg 432 series bars like this with no problems at all.

Providing you are not clamping your part by .100

[McRae]

Is'nt any more simple than putting an indicator in

the jaws and sweeping the turret.

 

That will tell you if the bar is on centre, what about the rotational orientation of the insert pocket? That is what really matters, the bar could be out .100" and I wouldn't care if and only if the insert was on centre...

[Hardmill]

Well unless the machines been crashed and maybe the

boring bar is bent or the turret moved and the

pot is hi or lo @ X0.

Turrets are pretty weak it don't take much to move

them.

 

 

PEACE

[Philcott]

Brendan,

 

quote:

---

I'm starting to believe it's a machine issue.

---

I agree.

 

Phil

[Joels]

The machine is a Hass SL-1. It was one of the first machines Haas made. The turret tool holders are mounted through holes in the turret and screwed in from the back to hold them in place. I am running a CSS of 200 and a depth of cut of .100 a side. I changed the feedrate to .011 yesterday and the chatter went way down. The cycle time is about 30 minutes to machine this side of the part. I work in a small 3 machine shop and the lathe is 10 years old I keep informing them about the capabilities of a new lathe so someday they might buy one. I tried to use a 1 inch bbar with a PCD diamond insert to finish the part but it chattered too and i was only taking off .01 a side. right now i have the chuck jaws set at a low pressure so i will try to raise it up today and see what happens. I doo all the machining towards the spindle except the face off. The jaws are aluminum and i cut the to a depth of one inch so i am holding the part well. We could have a machine issue but i use a stick tool with the same insert to face (.05 depth of cut) and turn the OD and it works perfectno chatter or anything so thats why i thought the bbar had the wrong rake angle.