Programming manual.
CNC 8070
8.
PATH CONTROL.
Linear interpolation (G01).
·140·
(REF: 1709)
• For polar coordinates, define the radius (R) and the angle (Q) of the end point relative
to the polar origin. The "R" radius will be the distance between the polar origin and the
point. The "Q" angle will be formed by the abscissa axis and the line joining the polar origin
with the point. If the angle or the radius is not programmed, it keeps the value
programmed for the last move.
Feedrate.
The programmed feedrate "F" stays active until a new value is programmed, thus not being
necessary to program it in every block.
Considerations for the feedrate.
• When several axes are involved, the CNC calculates the feedrate for each axis so the
resulting path is executed at the programmed feedrate "F" .
• The programmed feedrate "F" may be varied between 0% and 200% using the selector
switch on the CNC's operator panel or it may be selected by the program or by the PLC.
However, the maximum override is limited by the OEM (parameter MAXOVR).
• The behavior of the auxiliary axes is determined by general machine parameter
FEEDND.
Properties of the function and Influence of the reset, turning the
CNC off and of the M30 function.
• Function G01 may also be programmed as G1.
• Function G01 is modal and incompatible with G00, G02, G03, G33 and G63.
• On power-up, after an M02 or M30 and after an emergency or a reset, the CNC assumes
function G00 or G01 as set by the OEM (parameter IMOVE). If the CNC assumes the
function G00, and this function is defined as non-modal (parameter G0MODAL), after
programming G1, G2 or G3, the CNC assumes G1 as a modal function.
Parameter.
FEEDND
Meaning.
Yes The programmed feedrate will be the result of composing the movements onto
all the axes of the channel. (main and auxiliary). No axis will surpass the
programmed feedrate.
No If a movement has been programmed on any of the main axes, the programmed
feedrate will be the result of composing the movement only onto these axes. The
rest of the axes move at their corresponding feedrate to end the movement of
them all at the same time. Auxiliary axes can exceed the programmed feedrate,
but they may not exceed their maximum working feed rate (parameter
MAXFEED). If an axis were to exceed the MAXFEED, the programmed feedrate
of the main axes would be limited by the CNC.
If none of the main axes are programmed, the programmed feedrate will be
reached on the axis moving the farthest so they can all reach their destination
at the same time.
G00 G90 X20 Y0
G01 R20 Q72 F350
G01 Q144
G01 Q216
G01 Q288
G01 Q360
M30
To Next Page
Loading...
