Programming manual.
CNC 8070
8.
PATH CONTROL.
Rapid traverse (G00).
·138·
(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.
Considerations.
Feedrate behavior.
• A movement in G00 temporarily cancels the programmed "F" feedrate and the CNC
executes the movement based according to the rapid traverse specified by the OEM
(parameter G00FEED). The CNC recovers the "F" feedrate when programming a
movement function G01, G02, G03, etc.
• When several axes are involved, the resulting feedrate is calculated so at least one of
the axis moves at its maximum speed.
• When defining an "F" value and G00 in the same block, the CNC will store the value
assigned to "F" and it will apply it next time a G01, G02 or G03 type function is
programmed.
Feedrate override.
The override percentage is set at 100% or it may be varied between 0% and 100% using
the switch on the operator panel, depending on how it was set by the OEM (parameter
RAPIDOVR).
Canned cycles.
Within the range of influence of a canned cycle or modal subroute (#MCALL), the last
programmed G will be maintain active, G0 or G1, meaning G0 remains as modal.
Properties of the function and Influence of the reset, turning the
CNC off and of the M30 function.
Function G00 may be programmed as G0.
The G00 function can be modal or non-modal, depending on how it has been configured by
the OEM (parameter G0MODAL). Function G00 is modal and incompatible with G01, G02,
G03, G33 and G63. For the following program block, if there is no programmed movement
function in a non-modal G00 function (G0, G1, G2, G3, G33 or G63), the CNC uses G1.
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.
To Next Page
Loading...
