Newbie- Deep boring

[jacers]

Hello
I am new to this so bear with me.
I am running a sl30 Haas lathe and am having trouble boring 5" in deep
on 304 ss. Part is 7" long. 3.6 out from chuck and is just chattering.Material is hollow bar with 1.5 ID boring a 1.650 ID. Rough and finish.
I think it has to do with the vdi turret.
Any help would be app.
Thanks
Jacers

[Superman]

Hi, welcome to the forum

many things could give the effects you describe,
from chuck pressure, jaw shape
to turret condition
even tool & tip seletion and overhang

If this is not occuring on OD as well as ID, then first look at the tool,
recheck speeds and feeds, DOC, tip and holder

We had an issue with a certain repeat job that ran OK, a bar from a different Co was used ( same specs, even used the same tip ), found the the bar was sh*t, replaced the bar and problem was solved.

[jacers]

This is a brand new machine and have only ran a few jobs on it.
I have checked tool center and tried all kinds of feeds and speeds.
chuck prs 275 pds and still bore just sings. You can hold the bar and it stops.
It is also a 1" carbide but the rough is a 1.25 steel they both sing.
Machine works well if bars are not handing out that far.
Thanks Jacers

[Technical Ted]

Are both the rough & finish bar chattering?
What size & type of boring bars are you using?
What speed, feed & depth of cut are you using?

Make sure the bars are on center.

In general - leaving more stock for the finisher & running slower rpm & higher feed rates help with chatter. Have you tried SSV (spindle speed variation)?

Is there any possibility of boring just half way on the 1st op & finishing the other half on a second op?

This could be a good time to invest in an anti-vibration boring bar.

[Mr.Xtreme]

Jacers,

bars are usually 7-8 times dia before you have major problems with chatter, solid carbide is better rigidity wise.
A few questions might help us help you.
1 What are your depth of cuts (per side)?
2 what type of insert (insert shape,grade, rake etc.)?
3 What type of bar(s) are they?
4 What are your feed rates?
5 what SFM?
Other things that come to mind are..............
Are the ID of jaws bored .001- .002 smaller than the part od?
Is the OD of part your holding on round and true, if not you can take a skin cut to true up, then flip in jaws holding on the true dia will stiffen things up.

Paul

[swain]

Having done a fair bit of deep boring...I tend to disagree on the 7-8 times depth on boring bars.

Most steel bars are good for 3x diameter in best condition. Carbide bars are
5x diameter. I have a specially tuned bar that can go 10x diameter with no chatter...

One other tip to keep in mind, do not take a cut lighter than the nose radius of your tool tip.

Any stretching of these guidelines can be compensated to an extent with slower feeds and speeds...lighter depths of cut....but you are just giving it the oppertunity to chatter if you go outside the box.

If worse comes to worse...try the 1970's cure....wrap a spring around your part like we used to do with brake shoes to stop the chatter...<ha>

I would dare guess you are using a 1.25 boring bar...that is most of your problem. Best situation on it is a 3.75 deep bore depth.

I can't say on the vdi turret as I run an older haas lathe with the other turret...where boring bars install in holders that go through turret. It works
almost every times with what I said above.

Let me know if any of this helps...

[gepperta]

Long jaws around the part, so the much less sticks out. We used 6 inch jaws, it worked great.

Lead tape around the boring bar, like they use on golf clubs.

Sharper tool nose radius.