speeds and feeds advice for 4140 annealed ID bore

What would you recommend for speeds, feeds, and DOC to get a smooth surface finish on a ID im doing(currently have a vinyl record finish). after the drill I have .027 inches to bore. I need a 32 micro surface finish
Im using a 1.2inch boring bar with ISCAR WNMG 431 Grade IC8250(.015 nose radius). I cant use a bigger nose radius due to the small chamfer at the end of the ID.
Using a kia turn 15
15 hp spindle

You're looking at .004" IPR or a little less. 350-400 sfm is where I usually start on 4140 and 4340 with GP grades- that may be a little slow for your finishing pass.

You might have trouble breaking a chip on a light cut like that, so preventing it from wrapping around the bar and chewing up the finish may be necessary.

I usually prefer positive rake inserts for boring, but I have had good results with CNMG bars on larger bores in 4340/4150/EN30B

what exactly are the advantages and disadvantages of a positive rake? I have some positive rake wnmgs that I could try

fettersp said:

What would you recommend for speeds, feeds, and DOC to get a smooth surface finish on a ID im doing(currently have a vinyl record finish). after the drill I have .027 inches to bore. I need a 32 micro surface finish
Im using a 1.2inch boring bar with ISCAR WNMG 431 Grade IC8250(.015 nose radius). I cant use a bigger nose radius due to the small chamfer at the end of the ID.
Using a kia turn 15
15 hp spindle

Click to expand...

Surface finish is determined by the measured height and width of the surfaces peaks and valleys, similar to measuring a thread. Tool nose radius determines the maximum feedrate allowable to maintain the desired surface finish.
There has been much discussion here recently in other threads on the finer points of a shiny finish vs. measured roughness.
Do you have a Profilometer to check the finish?

32 is roughly equivalent to a 180 grit sandpaper finish.
With a .015" nose radius, you want to be in the .002-.004 FPR range.
A few points for success finishing steels at low DOC.
You need spindle speed to be as high as allowable, I run 1100-1500 SFM for finishing.
DOC wants to be at least the Tool nose radius if possible.
Use Coolant for the least amount of smearing and chip evacuation.
Use a positive finishing chipbreaker.

Here is my go to for steel, it has all of the best characteristics for low DOC passes.
Other manufacturers likely have a good insert as well, just try to find something close to this.
CNMG 431-PF 4325

Here is a demo video of it in action, the video begins with a normal DOC finish pass.
Finishing Steel on a Lathe - YouTube
A .004" DOC pass is then made to bring the mock part to size. (I know this DOC is not recommended for finishing, but it just may save you some grief polishing if you need to sneak up on a tolerance). 1100+ SFM and .017" per side DOC are the recommended minimums, but lower is possible if necessary.

fettersp said:

what exactly are the advantages and disadvantages of a positive rake? I have some positive rake wnmgs that I could try

Click to expand...

Sorry, I didn't mean the top rake. Your WNMG is a negative insert geometry, but it should be fine.

Positive rake, CCMT or equivalent. Or TPG. But I'm doing smaller bores these days.

1/2" IC WNMG or CNMG I assume that's a decent size bore and you have plenty of room. The relief is set by the bar, so as long as you're above the DMin you're good.

That other insert might give you better chip control, that's what's going to make or break you if you want to keep your 32 finish. If you have the rigidity, don't be afraid to run it fast and dry with that light cut. If you can make it break a blue chip at .004" IPR, life will be a lot easier.

If you're having chip control issues it can help to cut from the inside out. Other than that I have nothing to add to what was already said.

annealed steel is gummy, is there a possibility to machinability hardening to 27-36 HRc?
it is a easier to get a 32 micro , not that is not possible in the annealed condition.
is there any subsequent heat treating required?

you guys are the pro's I don't know much, but it has been my experience that a final DOC ,010-015 is gold,
smaller than that it start to rub and not cut, if try to sneak up on a bore it starts to work harden,
starts to go out of round and tapered. being what I experience in the past, old school machining.
correct me if I am not correct. or out of date.