What's new
What's new

1018 steel face grooving tips and speeds etc

zschary

Aluminum
Joined
Oct 5, 2012
Location
Dallas TX
have to hog out steel with a face grooving tool capable of 1.2 inch depth .. The lathe is 25 hp and the groove is around 5 inch to 3 inch from center on a 6.5 inch part diameter..

I do machine some stainless from time to time but have not done too much steel on this lathe and am looking for some tips on what folks do to for tool paths and feeds speeds as well as a good tool brand tips for this sort of thing.. Will have to make a bunch of these and have some money for tooling on this job..

any recommends on this type of thing i would really appreciate..
thank you
 
Wouldn't it be quicker and cheaper to rough out the slugs on a mill?
 
This is Iscars HFHR/L I like the square shank, the double ended inserts, the positive screw down clamp, and the variety of insert grades and chipbreakers.

HELIFACE_medium-diameter1a_2a.jpg
 
It would be nice to have a live tool on A or B axis. You could mill-turn the face groove, a matter of two minutes. Else buy a sturdy tool (holder), plunge in at about 100 m/min and gentle feed. You want steel to become warm enough to almost burn the chips in order to keep them breaking into small pieces. Nothing’s worse than strings in a face groove!
 
I'm a Sandvik guy, but when it comes to grooving, it's hard to be better at it than Iscar.
That being said, any top brand will have capable tooling.
Ideally you'd be running approximately 800sfpm, .004ipr minimum depending on width of insert.
Peck or not is your choice, but I would at least chip break the first cut on a groove that deep. Then you could treat it like a boring bar or a turning tool depending on if you start at the inner or outer portion of the groove.

Some people like to take the first cut to depth, others like to take the whole groove profile to depth at the same time, meaning a depth cut of the entire groove profile until final depth is reached.

If you have a good, stable setup and holders get a 5/16 wide insert or so.
The wider the insert the quicker the job will go.

1018 is gravy, especially compared to stainless. I've been cutting it for over 30 years. :)
 
For big ass face grooves, I don't use conventional wisdom. "Straight in-feed". I start at the top of the groove with the Tool I posted(or variation of) and an R style insert. feed in .05" then feed down, R style inserts handle this very, very well. This way, I'm not fighting a deep groove and chips. It's clearing away as I go. Transverse as opposed to Longitudinal, exact same thinking, Rough passes the Finish pass.

R
 
And who now owns Widia which was part of Krupp and one of the first carbide suppliers?
AFAIK Manchester did the first inverted vee which was big in stability over the other options.
Iscar would grow exponentially playing on this concept.

History or other is of no matter. What runs best today as I need to peel of steel is the only concern.
Bob
 
For big ass face grooves, I don't use conventional wisdom. "Straight in-feed". I start at the top of the groove with the Tool I posted(or variation of) and an R style insert. feed in .05" then feed down, R style inserts handle this very, very well. This way, I'm not fighting a deep groove and chips. It's clearing away as I go. Transverse as opposed to Longitudinal, exact same thinking, Rough passes the Finish pass.

R

I agree with the round insert. If you have Mastercam, you can use the Dynamic Grooving toolpath which is supposed to keep the cutting load constant throughout the path. It generates a lot of lines of code, but it lets you feed the hell out of it to try to break chips. I think they have a video of it on their website.

-Gene
 
Litlerob1 suggested the HFHL holder which is what my ISCAR rep is saying on this.. Iscar is calling for a ic808 grade.. I would like to do this on the lathe if poss, not have to transfer to the mill to hog out first.. I will look at the tool paths that BOBCAD Has, i am running their software with this lathe, and i will try to run a 5/16 width or better insert as some one said above.. so off to speed and feed for this and whether to dive to the bottom or take it in passes, and whether to go across or straight down into part..
any other feeds input or tooling methods you guys have i would appreciate hearing about.. Have a feeling there will be some trial and error here..

thank you Zach
 
For big ass face grooves, I don't use conventional wisdom. "Straight in-feed". I start at the top of the groove with the Tool I posted(or variation of) and an R style insert. feed in .05" then feed down, R style inserts handle this very, very well. This way, I'm not fighting a deep groove and chips. It's clearing away as I go. Transverse as opposed to Longitudinal, exact same thinking, Rough passes the Finish pass.

R

so go to .05 depth, then feed down towards me across part toward center right? and take .05 pass across the part? Interesting.. it does need a square non radius to the bottom, i am guessing that would be a different tool in this scenerio for the finish pass right? Is this much harder using the same tool with an insert that is not round? i like the idea very much..
 
so go to .05 depth, then feed down towards me across part toward center right? and take .05 pass across the part? Interesting.. it does need a square non radius to the bottom, i am guessing that would be a different tool in this scenerio for the finish pass right? Is this much harder using the same tool with an insert that is not round? i like the idea very much..

So your groove is a basic [ shape?
What littlerob1 is suggesting and what I've done also is to basically groove it in the style of a facing toolpath.
G01 Z-.05
X down to your diameter
Z.1
Repeat.
With a round style insert you can feed it pretty good. It's also less risky of busting tools by not having to take the tool to depth on the first pass.

Another thing we do on large grooves is to use the groover to remove some stock, then swap to a boring bar and bore it out.
Or use a reverse DNMG,VNMG tool to turn/face it out.
 
I agree with the HFHR recommendation from Iscar. If there is something else that even comes close I would be interested in hearing it but it sure isn't Manchester. That being said I have had to use Manchester on a few jobs where Iscar didn't have the right blade depth/diameter/width combination and Manchester did. There is no comparison.
 
so go to .05 depth, then feed down towards me across part toward center right? and take .05 pass across the part? Interesting.. it does need a square non radius to the bottom, i am guessing that would be a different tool in this scenerio for the finish pass right? Is this much harder using the same tool with an insert that is not round? i like the idea very much..

Correct. And you don't need software to generate the code, it's very basic. The benefit of the holder that I posted up there, is that itll take lots of different insert styles and shapes, including Round. With a Square cutting edge you'll need to slow down the feed, but with Round .025" per rev is not too much.

R
 








 
Back
Top