G01 - Linear Motion at Feed Rate

Details:
(a) For linear motion at feed rate (for cutting or not), program: G01 X~ Y~ Z~ A~, where all the axis words are optional, except that at least one must be used. The G01 is optional if the current motion mode is G01. This will produce coordinated linear motion to the destination point at the current feed rate (or slower if the machine will not go that fast).

Example:

• G01 Example

Last Updated Mar 2, 2011

` (Sample Program G01EX2:) (Workpiece Size: X4, Y3, Z1) (Tool: Tool #3, 3/8" Slot Drill) (Tool Start Position: X0, Y0, Z1)`

` N2 G90 G80 G40 G54 G20 G17 G50 G94 G64 (safety block) N5 G90 G20 (Block #5, absolute in inches) N10 M06 T3 G43 H3 (Tool change to Tool #3) N15 M03 S1250 (Spindle on CW at 1250 rpm) N20 G00 X1.0 Y1.0 (Rapid over to X1,Y1) N25 Z0.1 (Rapid down to Z0.1) N30 G01 Z-0.125 F5 (Feed down to Z–0.125 at 5 ipm) N35 X3 Y2 F10 (Feed diagonally to X3,Y2 at 10 ipm) N40 G00 Z1.0 (Rapid up to Z1) N45 X0.0 Y0.0 (Rapid over to X0,Y0) N50 M05 (Spindle off) N55 M30 (Program end) `

In the sample program, several different examples of the G01 command are shown:

1. The first G01 command (in N30) instructs the machine to plunge feed the tool below the surface of the part by 0.125 in. at a feedrate of 5 in./min.
2. N35 is a two-axis (X and Y) diagonal feed move, and the linear feedrate is increased to 10 ipm.

Note: Because there is contact between the cutting tool and the workpiece, it is imperative that the proper spindle speeds and feedrates be used. It is the programmer's responsibility to ensure acceptable cutter speeds and feeds.

• All Machine Code Reference Examples

Last Updated Sep 16, 2016