Not sure exactly what you are doing, but something like this.
M3 S4000
G90 G21
G0 Z0.500
G0 X5.900 Z-1.000
G1 Y-0.70 F50
G18 G03 X4.100 Z-1.0 I-0.900 K1.2 F50
G0 Z0.500 M2
Hi!
I am having trouble with G02/G03 with IJK method.
This is the arc i am trying to define:
This is my attempt at the gcode
It results in a tangetal arc like this:Code:M3 S4000 ; G90 G21 ; G0 Z0.500 ; G0 X5.900 Y0.000 ; G1 Z-0.700 F50 ; G18 G03 X4.100 Y0.000 Z-0.700 I-0.900 J+1.2 F50 ; G0 Z0.500 M2 ;
My mill does not accept M90.1 so I have to work with I and K as relative coordinates.
I don't think i can use the R method since i sometimes need to move in Y as well.
How can i alter my program to move in the arc shown in my first image?
Not sure exactly what you are doing, but something like this.
M3 S4000
G90 G21
G0 Z0.500
G0 X5.900 Z-1.000
G1 Y-0.70 F50
G18 G03 X4.100 Z-1.0 I-0.900 K1.2 F50
G0 Z0.500 M2
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Mills use G17 for standard arcs where the centre point is on the same plane as each point on the arc...
so G17 XY & IJ
G18 XZ & IK
the 3rd axis is sometimes used for creating a helical move
so to correct your program... get rid of G18... or change to G17
G2 is for clockwise movement.... G3 for CCW
plus the M2 should be on the last line, by itself
Try this for G17 .. using IJ
Try this for G17 .. using RCode:G21 ; ( inch programming... by itself ) G17 G90 ; ( safety lines.... XY plane, absolute ) M3 S4000 ; G0 Z0.5 ; G0 X5.9 Y-0.7 ; G1 Z-0.7 F50 ; G02 X4.1 Y-0.7 I-0.9 J1.2 F50 ; G0 Z0.5 ; M2 ;
I also stripped trailing zeros, as they are not necessaryCode:G21 ; ( inch programming... by itself ) G17 G90 ; ( safety lines.... XY plane, absolute ) M3 S4000 ; G0 Z0.5 ; G0 X5.9 Y-0.7 ; G1 Z-0.7 F50 ; G02 X4.1 Y-0.7 R1.5 F50 ; G0 Z0.5 ; M2 ;
Last edited by Superman; 06-12-2019 at 08:27 AM.
Removing feedrate from the G03 instruction seem to work in the simulator at least. I am writing a python program that generates this code thus the trailing zeroes. I will use it to engrave text in a groove. That is why i use G18 (XZ plane) and the additional Y coordinate.
This code works in the simulator:
Does it look OK?Code:G21 ; M3 S4000 ; G90 ; G0 Z0.500 ; G0 X5.900 Y0.000 ; G1 Z-0.200 F50 ; G18 G03 X4.100 Y0.000 Z-0.200 I-0.900 K1.200 ; G0 Z0.500 ; M2