[weihmue]

I have a question about Bore Bars...Carbide vs. Steel.

In my shop we usually run a lot of Ø.750 bore bars.

Material : 17.4 Stainless HT
Bore Bar: Ø.750 ...stickout 2.5-3.5 inches
Insert: CCMT 3-2-UM sandvik
SFM: 400
Rough Feed: .007
Finish Feed: .005

I used to run a lot of carbide bore bars and we were able to push them pretty hard. In my new show they use 99% steel bars.
We are looking to improve runtime...and I thinking by using a carbide bar I can get my SFM up a little rough feed around .010-.012 and finish at a about .007.

we are looking for a 125 finish or better.

everytime I start pushing a steel bar....i get chatter.


any ideas?


Thanks a lot

[Geof]

What do you need ideas for, you already know the answer.

I used to run a lot of carbide bore bars and we were able to push them pretty hard.

Carbide is stiffer and denser than steel so a carbide boring bar deflects less the a steel boring bar under the same conditions and is much less prone to chatter.

I will admit sometimes it is difficult to convince the people signing the purchase orders that it is worth paying twice as much (or more) for a carbide boring bar because they often cannot comprehend that the cost difference is recouped in reduced run time. You need to crunch a few numbers based on your current feed rates compared to your expected feed rates so you can predict how long it will take to recover the cost difference between the different bars.

[weihmue]

True....
I do know the answer. The problem im having is people not wanting to run it fast. Its sad to see how many people dont know and wont even try.

Cost for us is not to much of a problem. But faster runtime is huge for us.
What kind of feeds and speeds would you run in 17-4 ss using a .750 bar.
Also whats a good depth of cut for carbide bars.


Thanks

[txcncman]

SFM will be about the same. That is based on your insert, not the bar. 0.010-0.012 feed sounds good. Where you will gain additional time is upping your DOC.

[fizzissist]

I've used both Sandvik's steel bars and one of their carbide bars... and the carbide bar would run rings around the steel.
At 3" out, you're already at 4x diameters...... assuming you couldn't run up to a 7/8" bar.... That extra 1/8 can make all the difference..

[DareBee]

More dia always helps.
Sandvik (and others) also have specially engineered "heavy metal" bars that are supposed to work very well.
I have no first hand experience

[txcncman]

More dia always helps.
Sandvik (and others) also have specially engineered "heavy metal" bars that are supposed to work very well.
I have no first hand experience

I have loved the heavy metal bars when I have used them. No idea what the prices for them are now. 15 years ago they were close to the same as carbide. The advantage was they were sightly more forgiving in an "accident" and less likely to just snap off. Most just opted to pay for the carbide for whatever reason.

[Leonelix]

I would recommend to use an indexable boring bar with carbide insert. I rough 4140 and 4130 at .012/rev. at 250 rpm. The chatter problem come in great part to deflection. The diameter/lenght ratio is crucial in boring bars. Deflection of a boring bar is inversely proportional to the lenght of the bar to the 4th power. If the depth of cut is too shallow (say less than 1/2 tool nose radius) the tool tend to rubb and bounce, thus causing chatter.

[Delw]

I have a question about Bore Bars...Carbide vs. Steel.

In my shop we usually run a lot of Ø.750 bore bars.

Material : 17.4 Stainless HT
Bore Bar: Ø.750 ...stickout 2.5-3.5 inches
Insert: CCMT 3-2-UM sandvik
SFM: 400
Rough Feed: .007
Finish Feed: .005

I used to run a lot of carbide bore bars and we were able to push them pretty hard. In my new show they use 99% steel bars.
We are looking to improve runtime...and I thinking by using a carbide bar I can get my SFM up a little rough feed around .010-.012 and finish at a about .007.

we are looking for a 125 finish or better.

everytime I start pushing a steel bar....i get chatter.


any ideas?


Thanks a lot

with out seeing your part and your setup I would say your insert is the problem. use a .015 or a .008 rad. .032 may just put too much pressure on it. always on finsh passes I use a .015 rad on 3/4" bars with a bore like that.
the difference between using a .032 rad and a .015 is like using steel vs carbide.
also with small bores you need to make sure your turret is allinged and not off center. I try to have my bar just a tad above center this way when pressures hit the bar its moving away from the parts and not digging into the part causing chatter.

[dak1]

"I try to have my bar just a tad above center this way when pressures hit the bar its moving away from the parts and not digging into the part causing chatter."

Makes sense. How much is a "tad"? 0.001, 0.005, % of ID?

[Delw]

I been running lathes for 30 years so I just use a tad LMAO I eyeball it
try .005

[Shane1234]

I been running lathes for 30 years so I just use a tad LMAO I eyeball it
try .005

same here lol.