machining steel

what do you guys use for spindle speeds, feed rate, and max depth per cut on a mild steel with a 1/2 bit

First, let me caution you that I am completely self-taught in these matters, and I immediately defer to an actual machinist like rjw if they disagree. Also, it is worth your time learn how all this fits together, but I'm not gonna go into that right now. (Maybe another post some other day)

I will double check this from my charts when I get to school today, but my conservative calculations are as follows:

Assume 4 flute High Speed Steel endmill. Also I'm just gonna recommend mist lube/coolant, even though I do not know if the online charts I got my info from make that assumption. If you've got flood coolant or are using carbide endmills, I'm pretty sure you could go much faster. If you are using 2 flute, then the table speed should be half what appears below.

.250inch depth of cut

750rpm spindle, with table moving at 4.5 inches per minute.

If you decide to go faster, first increase the spindle speed, then increase the table feed. Faster spindle speeds create heat, and higher table feeds increase forces on the tool, part, and machine.

The numbers from above come from a surface speed of 100 feet per minute and a chip thickness of .0015, both of which are pretty low estimates.

It is my understanding that, except for materials that either heat-harden or catch fire (s7 or Titanium, for example), your limiting factors on speed and feed are really the horsepower of your machine and the tool life. You can mill (spin and table) lots faster usually, but the tool will wear out really quickly.

Well, the spreadsheet I use at school has a chip thickness of only .001 inch for 1/2 HSS endmill in mild steel. I don't recall where I got that from, but it seems too small. Anyway, what that would mean is for the settings/assumptions from my previous post is

Table speed is only 3.1 inches per minute, NOT the 4.5 I calculated before. Also, the spreadsheet was a touch more precise on the spindle speed, increasing it to 764 rpm.

I am of the opinion that the prior settings, with lubrication, would work just fine.

Well, since I've got an extra hour this morning (Yay daylight savings?), I'm gonna 'splain how speeds and feeds work on a mill (to my knowledge). This stuff is much easier if you are familiar with dimensional analysis (we teach this in chemistry class). All calculations and recommendations are based on using High Speed Steel (HSS) endmills, and I always recommend using coolant/lubricant.

First, about Depth of cut:
For depth of cut (from what I can tell), it doesn't matter what the material is, what the cutting tool is made of, or the number of flutes, just use the following recommendations:

For a tool diameter of 1/4 in., cut .05 inches deep per pass.
For 1/2, you can go as deep as .25 inches.
Larger tools go .25 inches deep per pass.
I don't have recommendations for smaller tools, or the in-between sizes but I just figure you can prorate/interpolate it (1/8 inch tool would cut at half the depth of a 1/4 inch tool, etc.)

Now about 'speeds':
(You must calculate spindle rpm before calculating table feed) Every material has a recommended rate that a cutting tooth can pass through it. This is the "speed" of "speeds and feeds." The values we use in our shop (expressed in surface feet per minute) are:

Al-300, Mild Steel-100, Titanium & Tool & Stainless steel-50

These will determine how fast your spindle can turn, because the faster you spin the tool, the faster the tooth passes through the metal. But the diameter of the tool also matters. A larger diameter tool will move the tooth faster at the same rpm of the spindle (think about it). Mathematically, to find the rpm you have to divide the tooth speed (from above) by the circumference of the tool, making sure to use the right units. For example, cutting mild steel with a 1/2inch diameter bit:

Tool circumference is 0.5*pi, which gives us about 1.57 inches per revolution (abbbreviated in. /rev.)
Tooth speed is 100 feet per minute, which is 1200 in./min.
Dividing 1200 in./min. by 1.57 in./rev. gives us. . .
764 rev./min.--our spindle speed should be 764rpm

Now about 'feeds':
Each tooth will cut a certain thickness of material each revolution, depending on how fast the table is moving (obviously). This chip thickness is the 'feed' of 'speeds and feeds.' For each material there are recommended chip thicknesses. But the tool size matters again, because a small diameter tool will break off or clog up if the chips are too thick. In our shop, we use the following chip thicknesses:

Aluminum: 1/4 inch dia mill - .002, 1/2 inch tool - .003, 3/4 - .004
Titanium: 1/4 - .0015, 1/2 - .002, 3/4 - .003
Steel (Mild through s7 and stainless): all diameters up to 1/2 cut a .001 chip, 3/4 tool can cut .002

Also, a 2 flute tool passes two teeth per revolution, and a 4 flute eats twice that much per revolution (duh), so the number of flutes affects the table speed too. Figure it this way, if each tooth cuts a thickness 'f,' and there are 'n' flutes then for each revolution of the tool, the table should move n times f inches. Since the tool turns 's' revolutions each minute (which you calculated above), then the table needs to move n times f times s inches per minute. For example:

spindle speed is 764 rpm (from above, with mild steel and a 1/2 inch bit)
chip thickness is .001
using a 4 flute mill, this gives us .004 inches per revolution.
764 rev/min * .004 in./rev gives us approximately 3.1 in./min.
Our table speed is 3.1 ipm

Work some problems, and the math becomes easier. Again, dimensional analysis is fundamental to really getting this.