[SCULLYISAFOX]

HELLO!
I'm a newbie to this site. It seems to be helpful. So here goes. I just started to machine on an Okuma Lathe with an OSP 5020L Control. I do not know how to use G2's or G3's. I was told by some one I can use the "L" word as well. Is there anyone out there that can give me an example. I'm trying to make a .531 radius on an I.D. Also.....does anyone know where I can get manuals for Okuma Lathes? Thanks!

[dcoupar]

Feed the tool to the start of the arc.
Program the arc using L for the radius, or I and K for the X and Z distance from startpoint to center of arc.


G01 X2.062 Z0 F0.01
G02 X1.000 Z-0.531 L0.531 (OR I0 K-0.531 INSTEAD OF L)
G01 Z-2.0

[SCULLYISAFOX]

Thanks dude!

[jitendrabagal]

he,dude how can i get the valu of I,J,K, in radius G02,G03,programing please give me formule,and some examples for same

[neilw20]

It becomes much clearer once you understand the terms.
This is for the XY plane. G17 selects this plane.
The start point for the arc is current XY location
G2 x y i j
where x and y are the end point. (same and not needed for a full circle)
i is the x offset to the center and j the y offset to the centre.
This doesn't require radius R, so all the incomplete circle problems vanish.
I J and K is the X Y Z location of the center.
You need to make sure you use the correct distance mode.
See G90/G91 below.

I prefer absolute mode (G90)
Straight out of the Mach3 manual:

10.7.3 Arc at Feed Rate - G2 and G3
A circular or helical arc is specified using either G2 (clockwise arc) or G3
(counterclockwise arc). The axis of the circle or helix must be parallel to the X, Y, or Z-axis
of the machine coordinate system. The axis (or, equivalently, the plane perpendicular to the
axis) is selected with G17 (Z-axis, XY-plane), G18 (Y-axis, XZ-plane), or G19 (X-axis,
YZ-plane). If the arc is circular, it lies in a plane parallel to the selected plane.
If a line of code makes an arc and includes rotational axis motion, the rotational axes turn at
a constant rate so that the rotational motion starts and finishes when the XYZ motion starts
and finishes. Lines of this sort are hardly ever programmed.
If cutter radius compensation is active, the motion will differ from the above; see Cutter
Compensation.
Two formats are allowed for specifying an arc. We will call these the center format and the
radius format. In both formats the G2 or G3 is optional if it is the current motion mode.

10.7.25 Set Distance Mode - G90 and G91
Interpretation of Mach3 code can be in one of two distance modes: absolute or incremental.
To go into absolute distance mode, program G90. In absolute distance mode, axis numbers
(X, Y, Z, A, B, C) usually represent positions in terms of the currently active coordinate
system. Any exceptions to that rule are described explicitly in this section describing G-
codes.
To go into incremental distance mode, program G91. In incremental distance mode, axis
numbers (X, Y, Z, A, B, C) usually represent increments from the current values of the
numbers.
I and J numbers always represent increments, regardless of the distance mode setting. K
numbers represent increments in all but one usage (the G87 boring cycle), where the
meaning changes with distance mode.

10.7.26 Set IJ Mode - G90.1 and G91.1
Interpretation of the IJK values in G02 and G03 codes can be in one of two distance modes:
absolute or incremental.
To go into absolute IJ mode, program G90.1. In absolute distance mode, IJK numbers
represent absolute positions in terms of the currently active coordinate system.
To go into incremental IJ mode, program G91.1. In incremental distance mode, IJK
numbers usually represent increments from the current controlled point.
Incorrect settings of this mode will generally result in large incorrectly oriented arcs in the
toolpath display.

Nice way to check out your code is with NCPlot, and make sure you select absolute or incremental mode according to your programming habits.

http://www.ncplot.com/