What's the rule for determining SFPM for finishing vs roughing? (Lathe)

TLDR:
Basically, the roughing inserts would usually break after 1-3 facing+turning operations until I unintentionally turned the SFPM down to 250 from 550, but the finishing insert lasted for all 144 operations (72 parts, 2 sides) at 650 SFPM. Why would such a drastic difference in velocity still produce desirable results, especially since the finish speed is even faster than the roughing speed that was breaking inserts?

More info:
I hope this isn't too much exposition for a simple question.

I just started my first machinist job. I'm running the oldest lathe in the shop right now (Daewoo Puma 10S). The blanks are heat treated 4140, ~282 BHN (and I got 32 HRC near the edge and 26 HRC at the center). The part is turned down to 3.95" OD from 4.3" and faced to 2.492" long from 3".

Originally the part I was running was programmed for Roughing with [CNMG 432, .010 Feed facing and .015 Feed turning, 550 SFPM, .050 DOC on Z and .180 DOC on X] and for Finishing with [VNMG 432, .005 Feed, 650 SFPM, .005 DOC on Z (but 2 passes to double check the critical 2.492 dimension), and .005 DOC on X.] Supposedly the program had been proved out, but the people running this part before are no longer at the company. I think the inserts are carbide, but I'm just pulling lightly used inserts from around the shop of random/unknown brands and specs. I had 1 new insert that I never used because I didn't want to break it after 1 operation.

The second most recent hire (also inexperienced) ran 38 of these parts before I took over. He said he was getting 2-3 parts per insert. The guy who set the job up for him thought .180 DOC on X was too much and reduced it to .100 and tried turning the feed/speed overrides up and down as it cut to see how it responded, but nothing came of it. They just gathered a bunch of lightly worn inserts from around the shop to run through.

I started checking the insert condition after the rough facing op and before the rough turning op to see it was broken. I would turn the spindle down to 50% to reduce the speed of the chuck while I open the door and look. I forgot to turn the spindle back up one time and noticed it was at 260 RPM mid cut (at 3.96 OD = ~250 SFPM), but it sounded fine. I then set the SFPM to 280 and was able to run the final 6 parts on the same insert without it wearing out or breaking.

I also turned the DOC back up to .180 from .100. After noticing the chatter from that, I overrode the Feed + and - 10%, mid-cut, to see which sounded better and ended up turning the feed up to .0165. Spindle load increased to 70% from <20% for this. I ran it at 70%, but I've been told by 3 other guys on 3 different occasions/jobs that I ran to watch the Spindle load (and x, y, z loads on mill) for indication of an issue and that it shouldn't be above 50-55%.

Another thing I noticed: the finish pass leaves a poor surface finish on the face from 1.07" diameter down. The lathe was ran in low gear and tops out at 840 RPM. When facing it dropped below the programmed 550 SFPM and 650 SFPM at 2.501" and 2.956" respectively because it can't go faster than 840 RPM. Before I accidentally adjusted the rough speed down to 250, I had already thought that 235.3 SFPM was where it's too slow based on the poor surface finish at that speed and lower ((840RPM × 1.07"Ø × π) ÷ 12") = 235.3 SFPM.

So I wanted to ask if there's a rule of thumb for speed choices for roughing vs finishing. I get how feedrate, tool geometry, rigidity, etc. are important for a good finish, but I don't see the connection to increasing the speed.

And, concerns that came up as I wrote all this out:
Would the difference in hardness from edge (32 HRC) to center (26 HRC) of the part be a possible reason for the poor surface finish as the cut approaches center?
Was it risky of me to run the final parts at 70% spindle load during the rough pass? (and while roughing the face, spindle load briefly rose just above 100% as the RPMs increased to it's max of 840)

Sorry, for going off topic on my first post. Appreciate any comments.

Because your depth of cut is different on the finish cut.

when roughing tool length sticking out, basically tool and part vibration are higher
.
when tool length is 2x longer flexing increases 2x2x2 or 8x more. make sure tool not sticking out more than it has too

When having insert life / finish issues and trying to sort out what is going wrong :-

Rule 1 :- Start with manufacturers speeds and feed recommendations for that insert with the material you are using

Rule 2 :- Use a new insert thats been kept in its proper packing so you can be sure it is sharp and in good order. Carbide Bob can look at an insert and say whether still its OK or not. Us mere mortals usually can't.

Rule 3 :- Remember insert lifetime. At factory speeds many types of insert don't last very long in cut, often seriously less than an hour. (But they make a metric boatload of chips in that time.) Random part worns are almost certainly worn out.

Rule 4 :- Grossly oversimplifying carbides can be considered as being designed so they need to put a certain amount of energy into the cut to leave a clean finish. Lighter cuts on finishing are easier to make than heavier roughing cuts so finishers run faster for the same amount of energy (work)..

Moving OT judging by what you are saying its time to look for another job. Good shop is organised to make money by making parts quickly and accurately. Part of being a good shop is having a good system to sort out problems. Leaving the new guy to fumble around is not only a bad system but also hugely expensive. That sort of thing that drives a shop to the wall.

Clive

many a job operator finds things go better when not at 100% rpm and 100% feed.
.
sometimes its as simple as last guy was not running at 100%/100%. if you have less problems and things are actually going faster by going slower why wouldnt you run with less problems. previous operator might not say anything

Can't believe the shop allows a newbie so much freedom to screw around with so many parameters
Sink or swim attitude it sounds like
I am with Tom on this one
Your the newbie,previous runners of that job could very well be stretching the truth

My guess is you're killing the inserts on the facing pass. If you're pulling 100% load you're probably going deep enough to be breaking off a considerable tit and chipping the edge.

Any rules for SFM go out the window if you're grabbing literally any halfway decent insert in the shop.

If I was buying a box I would probably go with Seco Duratomics in a suitable flavour.

running a carbide drill at over 30 ipm feed is a classic case.
.
if drill breaks 2% of the time and by the end of the year you figure you lost $5000. in time and tooling, then you calculate if going slower takes $1000./year more in labor but saves $5000/year in time and tooling dealing with broken tooling then its cheaper to go slower. and drilling a hole even if it takes 5 seconds longer per 100 holes that 500 seconds or 8.3 minutes. dealing with broken drills or even just changing drills faster and increased sharpening costs its often costing more trying to go faster

So I found some useful info related to this here and here. Still not quite what I'm looking for.

Thanks for the tips. Having the insert manufacturer's recommendations would have been enlightening. I had no idea the cutting speed could vary so much for the same material.


I'm adding this just so it's here for anyone searching about this in the future. The Machinery's Handbook had the answers I needed. It's a lot to go through, but it's quite useful if you can find what you need.

"Tool life is influenced most by cutting speed, then by feed rate, and least by depth of cut... The depth of cut will be limited by the amount of metal to be machined from the workpiece, by the power available on the machine tool, by the rigidity of the workpiece and cutting tool, and by the rigidity of the setup. Depth of cut has the least effect upon tool life, so the heaviest possible depth of cut should always be used."

This is reflected in my recent experience. I went from spending 1 roughing insert per part to only 1 corner of an insert for 40+ parts by taking everything off in one deep, high feedrate, low cutting speed pass as opposed to multiple shallow, medium feedrate, high cutting speed passes. The overall time per part ended up about the same, but I'm not having to interrupt and reset a cut to change a shattered insert and I haven't wasted $400 on inserts in one day as I would have if I had ran it as is.
From what I can tell, you want to cut as fast as you can as long as your part comes out nice and your tool life is acceptable. Based on the speed/feed tables in the Machinery's Handbook, I'm now almost certain those inserts were breaking because they must be uncoated and no one took that into consideration.

As for determining what the finish speed should be, the book also has a data-driven table that provides surface speed scalars based on chosen feed and depth of cut. From that table you can infer that you want faster cutting speeds when using slower feeds or shallower cuts and vice versa. As finish cuts are usually slow of feed and shallow of cut, they get double stacked with modifiers that can skyrocket the suggested cutting speed.

Azoth

I'm glad you are pretty much sorted.

Its easy to assume that running fast and light is the only way to go with carbide because so many inserts are made top work that way. But, as you have found, some like the old school HSS / brazed negative rake tip approach of slow (relatively) and heavy cut. Familiar stuff for old penguins like me who remember how carbide used to be exploited but probably little novel for new guys.

+1 for the wide variation of speed, feed and cut depth recommendations between apparently similar inserts. These things are engineered metal cutting systems and you have to drive them right.

Clive

Young man - you're going to go far in this trade. What a mature approach! You took what you could from this thread and went to the "go to" book for help and you processed the info and made an informed decision. My hat's off to you.

For 4140 pre-hard (which is what it's usually called that you're cutting) I would be exactly where you ended up for my roughing - 250 sfpm. For finishing my starting parameter would be 300-350 sfpm. Your results surprise me in that you got good insert life at 650 sfpm. I will keep that in mind for the future.

Typically you want about 30-40 minutes of cutting time off an insert for a good payback on insert cost in a production environment.

Best wishes on your new job and your new career.

Azoth said:

So I found some useful info related to this here and here. Still not quite what I'm looking for.

Thanks for the tips. Having the insert manufacturer's recommendations would have been enlightening. I had no idea the cutting speed could vary so much for the same material.


I'm adding this just so it's here for anyone searching about this in the future. The Machinery's Handbook had the answers I needed. It's a lot to go through, but it's quite useful if you can find what you need.

"Tool life is influenced most by cutting speed, then by feed rate, and least by depth of cut... The depth of cut will be limited by the amount of metal to be machined from the workpiece, by the power available on the machine tool, by the rigidity of the workpiece and cutting tool, and by the rigidity of the setup. Depth of cut has the least effect upon tool life, so the heaviest possible depth of cut should always be used."

This is reflected in my recent experience. I went from spending 1 roughing insert per part to only 1 corner of an insert for 40+ parts by taking everything off in one deep, high feedrate, low cutting speed pass as opposed to multiple shallow, medium feedrate, high cutting speed passes. The overall time per part ended up about the same, but I'm not having to interrupt and reset a cut to change a shattered insert and I haven't wasted $400 on inserts in one day as I would have if I had ran it as is.
From what I can tell, you want to cut as fast as you can as long as your part comes out nice and your tool life is acceptable. Based on the speed/feed tables in the Machinery's Handbook, I'm now almost certain those inserts were breaking because they must be uncoated and no one took that into consideration.

As for determining what the finish speed should be, the book also has a data-driven table that provides surface speed scalars based on chosen feed and depth of cut. From that table you can infer that you want faster cutting speeds when using slower feeds or shallower cuts and vice versa. As finish cuts are usually slow of feed and shallow of cut, they get double stacked with modifiers that can skyrocket the suggested cutting speed.

Click to expand...