Helical Milling in the Z Axis

Sat, Jun 5, 2010

FAQs, G-Code, Programming

Dear Answer Man,

How do I program helical milling in the Z axis? Do I have to loop circular interpolation with a Z value added for each revolution (G02 X__, Y__, I__, J__, Z__)? Or is there a G code for helical milling or interpolation in the Haas control?

Chuck Wong

Dear Chuck:

The simplest way to achieve helical motion is by X and Y circular interpolation (G02 or G03) with a Z value added per revolution. Use an I command to specify the distance in X from the starting point to the center of the arc. To cut a complete circle of 360 degrees, do not specify an ending point for X or Y. If you use incremental positioning (G91), you can loop the cycle to achieve your depth using an L command. Here’s a sample program:



(Helical Milling Example);

T1 M06;

G00 G90 G54 X0. Y0. S3000 M3;

G43 H01 Z0.1;

G00 X0.5;

G91; (incremental positioning)

G02 I-0.5 Z-0.25 F20. L4; (helical motion, 1 in. dia. x 1 in. deep)

G00 G90 X0;

G0 Z0.1 M09;

G53 Z0.;

G53 Y0.;



Sincerely, Answer Man

|| More
, ,