[Paul_S]

Estimating feeds and speeds is always of great interest to me. Since typically I am on my own trying to decide what is best. Currently I have to machine some D2 air harding tool steel. The program has not been ran as of yet.

From a starting point for surface speed I use the recommened SFPM from the 19th edition of the Machinery Handbook. At home here, I only have my 26th edition. And it does not provided the tradtional SFPM for carbide, only HSS. But has so-called tool life tables which does include for carbide end milling.

So from the HSS table for 420 gives SFPM 95 for 135-175 Brinell which would be the annealed condition.

Since I typically use SFPM 70 for 303. And the book recommends 100 SFPM. I would use 60 to 66 SFPM for 420 to start.
And since I use 225 for Carbide using 303 I would choose 150-180 for 420. Now just guessing. and estimating.

I would use .003 per flute index value for the cutter feed. (I use .004 index for 303.)

So if I was to calculate the feed for 1/4 carbide ball em 4 flute.
.003 x .250 x 4 x RPM.

My max RPM using 180 SFPM. Calculates out to 2750 RPM.
The roughing feed would be 8.25 IPM. If I am side cutting with a step over of lets say .008 per pass I would up my next and remaining feeds to 46.11 IPM (IPM = ref IPM * sqr(.25/.008).) But I would check this against another program that I have written depending the flute length of the cutter and depth of cut given the dia of the cutter. I don't want to break the cutter. That program recommened 17.62 IPM using a chip load of .0003. And my starting feed would be more like 3.3 IPM.

(giving the flute length of about .85, z axial depth of .5 roughing with a side cut of .008 step per pass.)

My finish feeds though can be much faster for spring cut finish clean up. Using a .008 finish step over the feed would be typically .008 * RPM > 22. IPM.

Summery. My first estimate might work. But I do not want to break my cutter. So I go with the more conservative estimate. (Using an experimetal algorithm which I have been using with generally good results for the past few years.)

Checking another earler (now modified) program that I have suggests a reduced RPM of 1790 (a reduced 117 SFPM) with a feed rate of 18.49 IPM with the .008 step over during rough out. I would be inclined to use these values because the feed is higher here. 18.49 IPM. The index chip load being .00046. The lower RPM giving better tool life (even though it is more of a HSS SFPM range.)

The programs are written in TI-BASIC on a TI-86 programmable calculator.

Then kick up the RPM to 2750 for finishing at the 22. IPM.

Anyway I would also be inclined also to use a HSS/Cobalt roughing cutter to take out most of the material first before roughing and finishing with a 1/4 ball.

But only if it looked like it would give me shorter maching time over all. It depends on how mach material must be roughed out.