recommended rpm for finishing cut.

[scrapper400]

Hi all,

I have an 80mm dia flycutter with 10 inserts. The recommended Vc for the insert is 80-200m/min for roughing and 350 for finishing. I am taking 0.1mm finishing cut but it seems really slow and the finish is only okay on the steel. I speeded it up to 500 m/min and hiked the speed from 825 rpm to 1650 rpm but now the chips are coming off red hot which doesn't sound great.

Can any one suggest a good speed and feed combo for this. I always decided on a cutter rpm by the usual equation but am wondering can I ramp up both speed and feed for tiny finishing cuts or am I only damaging the tips.

All comments welcome.

Cheer,
Scrap.

[Boots]

Usually for finishing passes I have to caluculate the Surface Footage then figure out your speed and feed based on the dia of the cutter and number of teeth. One trick I have always used is to shim one instert lower than the rest and it becomes a wiper. The other inserts will do the bulk of the work on a 1mm depth of cut. Don't use the same tool for roughing as finish. It will come out better.
Regards,
Chuck.

[kling8]

Sometimes your depth of cut can be the problem, you may be taking to light, or heavy of a cut, inserts have different rake angles that can affect your finish, are you flooding it with coolant? If your burning up the tips of your inserts I think spindle is going to fast. Another idea is call the rep. that you bought the tool from and ask him for recommended speeds feeds and inserts.
Hope this helps
Good Luck
kling

[scrapper400]

Thanks for that. I think I was travelling twice as fast as I should have (Zn instead of Zc in the feed calculation). Anyway the SF now is okay but I ordered a couple of wipers from the rep so they should hopefully improve it. While there are no major problems with the finish you can still feel the difference between the passes with your finger nail. They are probably less than 50um but I want to use this plate as a semi permenant fixture on the machine so I'd like to take the time to get it right. Thanks for the suggestions. The shim idea is interesting Chuck but I'll wait for the wiper.

Cheers.

Scrap.

[BobWarfield]

Not sure exactly what steel you are cutting, but if I run it through G-Wizard, I get 300 rpm spindle and 388 M/min feedrate at the low end of your surface speed range for your inserts.

Since it says you can go to 350 for finishing, that would get you all the way to 1400 rpm, but your 1650 is too fast for that surface speed. Also, to maintain the chipload, you should be feeding much faster at the higher rpm, about 3x faster. By travelling that much more slowly, you're really making the cutter rub.

Chips are probably red hot both because of the 1650, but just as much because they're too small to carry away the heat very well from the cut and because the slow feed is rubbing. I agree you're taking too fine a cut. Try more like 0.25mm depth of cut, 1400 rpm, and at least half the desired feedrate or maybe 800 M/min.

Try G-Wizard for these kinds of calculations. Saves on those transposition problems of Zc vs Zn.

Cheers,

BW

[scrapper400]

Thanks BW. I went with 1400rpm and 1080 mm/min when I fitted the wiper and I got a good mirror finish off it with a 0.2mm cut.
Thanks for all the replys and the links.

[BobWarfield]

Outstanding!

Don't you love it when a plan comes together. Parts cut so sweetly when you get all the parameters right.

Cheers,

BW