jario_
Back to overview

CNC Basics · Chapter 9

Cutting values and short paths

When you drive a car you choose the gear to suit the road: a low one uphill, a high one on the motorway. Too fast and the engine stalls, too slow and it takes forever. On a CNC machine, spindle speed and feed are your gear. They depend on the tool and the material. Time matters too: the shorter the paths and the fewer the tool changes, the sooner the part is finished.

The spindle speed

The manufacturer gives the cutting speed vc: the distance the cutting edge travels along the material in one minute, in m/min. From it you calculate the spindle speed n (revolutions per minute):

n = vc × 1000 / (π × d)

d is the diameter of the tool in mm. As a rule of thumb you calculate with 1000 / π ≈ 318. A thick drill needs a lower speed than a thin one. You write the speed as S in the program.

; Drill d = 12 mm in aluminium, vc = 30 m/min; n = vc x 1000 / (pi x d) = 30000 / (3.14 x 12) = about 796G90 G21 G17T2 M6S800 M3G81 X30 Y30 Z-10 R2 F80G80M5M30

The feed

A catalogue often gives the feed per revolution f in mm per revolution. The machine wants mm per minute, though. You multiply by the spindle speed:

vf = f × n

You write this value after F. So always calculate n first, then vf. For tapping the feed is already fixed: F = S × pitch.

; Drill d = 12 mm, f = 0.1 mm per revolution; n = 800, so vf = f x n = 0.1 x 800 = 80 mm/minG90 G21 G17T2 M6S800 M3G81 X30 Y30 Z-10 R2 F80G80M5M30

The shortest path

Between two holes the machine moves in rapid traverse. Nothing is machined while it does. In the top view you see these moves as lines. Visit the holes so that you never have to jump back: one row forwards, the next one backwards, like a snake path.

You decide the order of the positions yourself. With a cycle it is enough to write them down differently, the holes stay the same.

; Four holes in a square, snake path without jumping backG90 G21 G17T2 M6S1590 M3G81 X20 Y20 Z-8 R2 F159X60               ; rightY40               ; upX20               ; leftG80M5M30

Few tool changes

A change takes a few seconds and the tool has to get up to speed again. So drill all holes with one tool first, then with the next one. If a part has holes for two drills, two changes are enough, no matter in which order the holes are on the drawing.

At the end of a block you are at a corner. Start the next block there and visit the holes in reverse order, then you save the way back.

; Holes 1 and 3 need tool 2, holes 2 and 4 need tool 3; Sorted by tool: two changes instead of fourG90 G21 G17T2 M6S1590 M3G81 X20 Y20 Z-8 R2 F159X60G80M5T3 M6S1120 M3G81 X40 Y20 Z-8 R2 F112X80G80M5M30

Common mistakes

  • Spindle speed and feed swapped

    S is the spindle speed in revolutions per minute, F the feed in mm per minute. The two numbers usually differ by a factor of about 10. If you swap them, you drill far too fast or not at all.

  • The same values for all tools

    Every tool has its own diameter, so its own values. If you take S and F over from the previous tool, you cut wrongly. Calculate again after every change.

  • Diameter instead of radius

    The formula uses the diameter d, not the radius. With the radius you get twice the speed.

  • Jumping back at the end of a block

    If every block starts again at the first hole, you travel the whole way back. Reverse the order in the next block.