CNC 8055 - Operating manual (MC option) - Fagor Automation

6.
EXECUTION AND SIMULATION
Graphic representation
CNC 8055
CNC 8055i
·MC· OPTION
SOFT: V01.3X
·156·
ISO
Operating manual
In the conversational mode of the CNC, it is possible to generate an ISO-coded program with some
basic G functions as well as M and T functions from an operation (cycle) or on a part-program.
To enable this feature, set general machine parameter ISOSIMUL (P183) with a value other than
zero. This parameter identifies the number of the ISO program generated in user RAM memory.
The program generated from the conversational program is an ISO-coded program created in RAM
memory. This program may be later edited, copied or executed at the CNC itself.
To generate the ISO program, use the simulation in conversational mode through the "GRAPHICS"
key. This can be done in a whole program on the PPROG screen or in any of the particular TC or
MC cycles.
Once inside the graphic simulation screen, the ISO generation maybe selected using the
softkey. Then, pressing [CYCLE START] will generate the program defined by machine parameter
ISOSIMUL (that will only contain ISO instructions) while it simulates it graphically.
When generating that program, parametric programming, rounding (G36), tangential entry (G37),
tangential output (G38), chamfer (G39) and path tangent to previous path (G8) are resolved and
generated only using G1, G2 and G3 blocks.
If the program already exists, it will be deleted without requesting confirmation. If the generated
program exceeds the available user memory, the CNC will issue the corresponding error message,
but it will keep in memory the portion of the ISO program generated so far.
Description of the functions used to generate an ISO-coded program:
The ISO-coded program is mainly generated to control axes. It provides information of the moving
conditions and indications on feedrate using the following set of functions
G functions: Motion preparatory functions to determe the geometry and work conditions.
Function Meaning
G2 (G3) G6 X Y I J In the circular interpolation, the center will be programmed with respect to
the origin, not referred to the starting point of the circle.
Rigid tapping cycles G84 (mill) and G86 (lathe) only generate the equivalent ISO block.
"F" and "S" functions: Functions to control the feedrate of the axes and the spindle turning
speed.
T and D functions: Tool control functions.
If the T function has an associated subroutine, the blocks of this subroutine are ignored when
generating the program set by g.m.p. ISOSIMUL (P183).
M function: Complementary or auxiliary functions.
If the M functions have an associated subroutine, the blocks of this subroutine are ignored when
generating the program set by g.m.p ISOSIMUL (P183).