feeds and speeds

[Paul_S]

A quick check on the internet, suggest 50% faster than for P20 mold steel. I assume the cutting angle is less than 30 degrees on the outer edge of the mold. On that basis I would use 20000 RPM and a feed of .0006 per flute with a max step over cut of .0057. Assuming taking .008 depth of cut with .500 cutter stickout. If the major dia of the cutter is used I would limit the RPM to about 19360 with a max feed of .0002 per flute. Max width of cut .008 per side. If this doesn't snap off the cutter it should work great. If you break your cutter, reduce feed by 50% until the cutter doesn't break. I am assuming a max step over of no more than .0057

If the cutter wears too fast, reduce the RPM to 80% of what you were using, until you get an acceptable tool life.

Anyway, your max feed should not exceed .0057 x the RPM. And do not use a step over greater than .0057. The theoretical finish should be about that of 19 Ra finish. I believe that finish should serve well toward polishing without being too slow for machining.

On the conservative side, I would limit my RPM to 180 SFPM. Which would be 11000 RPM at 30 degree angle or less at .008 depth, or 5500 RPM at the cutter major dia (.125 Carbide Ball EM). Max step over would still be limited to .0057. Feed rate not to exceed the .0057 x RPM. The removel of .008 stock and cutter stickout of .500 I would limit the feed to about .0007 max per flute.

I am guessing NAK 80 40 HRc will cut like P20 mold steel. (I have never cut P20, but I have cut H13, A2, O1. The steels I currently program for cutting are 303, [304,] 17-4PH.)

[rollie]

Thanks I will be cutting it sometime next week.Will let you know the outcome.I am going to high speed machining now so all the info I get is great.I cut alot of P-20 and some QC-7 aluminum.Cores and Cavities for injection molds.Have a Happy New Year and any other advice will be greatly appreciated

[Paul_S]

Rollie,
Just a side note. If your Z axis resolution is only .0001 you may have .0001 steps to polish out. .0057 step over using a .125 ball EM will leave .000065 theoretical scalops. Any .0001 steps will be greater than the machining finish. Also make sure you only cut in one direction. Cutting in two directions is just like using double the step over when it comes to finish cutting. (Not that you would.)