Fagor 8025 GP, Руководство по эксплуатации

Страница: 197 / 423

8025/8030 CNC PROGRAMMING MANUAL 77
C Indicates the type of movement between the machining positions. If not
programmed, a value of C=0 will be assumed.
C=0 Movement in rapid (G00).
C=1 Linear interpolation (G01).
C=2 Clockwise circular interpolation (G02).
C=3 Counter-clockwise circular interpolation (G03).
When setting C=0 or C=1, the sign of parameters "B, I and K" indicate the
direction of the movement: "+" counter-clockwise, "-" clockwise.
When defining "B I" the moving direction is set by the sign of "I".
When defining "B K" the moving direction is set by the sign of "B".
When defining "K I" the moving direction is set by the sign of "I".
F Defines the moving feedrate from point to point. Obviously, it will only be
relevant for "C" values other than "0". If not programmed, a value of F0 will be
assumed which is set by machine parameters "P110" and "P210".
Q, U These parameters are optional and are used to indicate which points or between
which points the machining operation is not to be performed.
Thus, when programming Q7, it indicates that point 7 is not to be machined and
when programming Q10.013, it indicates that points 10 thru 13 are not be
machined (that is, points 10, 11, 12 and 13).
When defining a group of points (Q10.013) it must be borne in mind that the
last point has to be indicated with three digits since programming "Q10.13"
will be interpreted as points 10 thru 130. (Q10.130).
The programming order for these parameters is Q U and the numbering order
assigned to them must also be kept. That is, the numbering of the points assigned
to Q must be smaller that the ones assigned to U.
Example: Correct programming Q12.015 U20.022
Incorrect programming Q20.022 U12.015
If these parameters are not programmed, the CNC interprets that the machining
operations must take place on all points of the programmed path.
Basic operation:
1.- This cycle calculates the next programmed point to be machined.
2.- Movement to that point at the feedrate programmed by "C" (G00, G01, G02 or
G03).
3.- Once at this new point, it will execute the selected canned cycle.
4.- The CNC will repeat steps 1, 2 and 3 until the end of the programmed path. Once
the multiple machining cycle is completed, the tool will be positioned at the last
machined point of the programmed path.