[Fred Ashley]

I need to machine a face groove with an 8.5" O.D. and 4." I.D. that is 4.81" deep. Any suggestions on tooling that might be available for purchase. I will be doing this on a Romi C.N.C. lathe(with tool post). I realize I will have to probably alternate 2 tools and cut the depth in steps. I would like to be able to get an inch depth at a time. About the widest insert I will be able to use is.25" with a full radius.
Thank you

[star-turn]

thats not a face groove its a canyon!

have you looked at the iscar range ?

they do blades for face grooving which are around 6 inches in length, so you could go in a couple of inches, pull the blade out further and go in deeper.




ST

[Geof]

Have you considered doing it on a VMC? There is plenty of width for a large diameter mill that would have the rigidity to go that deep.

If it has to be on a lathe yes look at Iscar tooling.

And I thought I did a deep face groove once when I did something about an inch wide, 1-1/2" deep with on OD of 6". Clearly that was chicken feed. At that time I hand ground a piece 1" square HSS and did it in a single cut on a big turret lathe.

[HuFlungDung]

Wow, this is a deep one

I'd consider trying it with two 1" boring bars, using a CNMG insert, with one bar right hand, the other bar being left hand. You could also try a DNMG insert for more penetration per ramp.

With 5 degrees of side clearance, and having a maximum range of tool movement within the groove of 1.25", you could still ramp in almost .1" across that 1.25".

Take the cuts alternately with the two bars, each bar dedicated to one direction. You'll need a toolchange between each pass.

You can likely get decent chip control, which is a big headache with normal face grooving tools. However, you can likely be fairly aggressive with the feedrate on the boring bar. Coolant entry will be good too, because you can keep the groove open full width all the way down.

[Mike Phung]

vbmt insert would probably work bit better. It will give more plunging options.

[ctate2000]

Ditto Iscar if money is no issue. I would expect to spend a few hundred dollars but it will be worth the money. I think the tools are call heli-face or heli-groove. I have used them and they are the best.

[Fred Ashley]

thanks for all the input, yes I have to use a lathe because our vmc's are all loaded with too much work allready, my cnc lathe doesn't have a turret, it has a tool post and tools have to be changed manually after a process is completed so swaping b.bars back and forth may be too time consuming, I have looked at iscar catalog but could not find 6" long face grooving blade, I did do one of these parts with a homemade tool holder(1 1/4" dia.) with a .26"wide HSS toolbit hanging out the front 1" and useing a bore bar on each side going 1" segments all the way down,it came out pretty good but took a lot of time and I have 19 more to do.
Thanks again
Fred A.

[Andre' B]

You can to the two boring bar method with a single bar if you can reverse the spindle direction, and get the bar on both sides of the centerline.
Work on the large diameter of the groove for a bit.
Pul the bar out and reverse directions.
Move the bar to the other side of the centerline and work on the small diameter for a bit.

Edit:
Rereading your last message maybe that is what you were doing.