Need Help!- speed for turning mild steel

[noshoesnoshirt]

hello everybody i made this turning program but since i havent run this kind of steel, for a very long time i was wandering if some one can help with the amount of material to leave for finish and rpm for the spindle to turn .5 OD in order to get an aceptable finish and dimension . right now i am leaving .012 thousend per side and runnig at 1400 rpm and .006 per revolution, and worst thing is the upper edges of a small grove .4 OD and .050 wide they have big burs, but the tool looks sharp and i am just plunging the grooving tool at
0.0015 per revolution ant 700 rpm leaving .005 thou per side for the finish plunge , the first too parts came out ok but the third have the big burs this is soft steel , i am also using .0156 thou tnr. for the finishing, thankyou for your help and if some one have a reliable surface speed chart for turning that would be great but any help is greatly appreciated thanks alot

[PixMan]

First of all, what machine do you have and what is it's top speed? Manual or CNC? You should be calculating your cutting speed in "surface feet per minute" rather than rotations per minute.

The groove's burrs are usually caused by the tool being off center. In this case, I'd guess a touch too high because it seems to be pushing the material rather than cutting it. If your groove tool is also carbide (and the correct C5-C6 grades for steel), there is no reason to be running any slower than your turning speed. That said, if the "first too (sp) parts came out OK", then the tool is failing and is probably dull now. With carbide tooling, the most common mode of failure is dulling the tool from running too slow rather than too fast.

There really is no standard chart for speeds and feeds with carbide lathe tooling, as there are so many variables. The choice of the insert's shape, grade, and chipbreaker (top form geometry) all depend upon your machine's speed and feed capability, and rigidity of the workpiece. Add into that the desired surface finish, dimensional tolerance and geometry of features in the workpiece.

For mild steels, I've been having the best luck (assuming CNC machines) with Valenite's VP5615 and VP5625 grades. I cut 1018 steel in a roughing operation with a CNMG432M8 VP5625 at 1200 sfm, .014" inches per rev, .150" depth of cut. I finish with a DMNG431F3 grade VP5615 at 1400 sfm, .006 ipr feed, and .015 doc. You're running at 183 sfm. If you have the right grade of a coated insert...speed it up!

For grooving I use a Top Notch style insert. What are you using for turning and grooving, and what is the spec for the steel? What shape, grade, and chipbreaker are the inserts you're using for both operations?