Optimum Optimill F3 - Page 143

OPTIMUM
MASCHINEN - GERMANY
808D
Page 143
ISO Mode
Brief instruction 808D Milling
Operating and Programming — Milling
Basic Theory
Frequently used letter meanings of typical fixed cycle codes in ISO mode.
P. Descriptions Unit Applied range and note
X/Y Cutting end point X/Z absolute
coordinate values
G73 / G74 / G76 G81 ~
G87 / G89
Z
The distance incremental value
between R point and the bottom of the
hole, or the absolute coordinate value
of the bottom of the hole
G73 / G74 / G76 G81 ~
G87 / G89
R
The distance incremental value
between the start point plane and R
point or the absolute coordinate value
of R point
G73 / G74 / G76 G81 ~
G87 / G89
Q
The depth of every cut
（incremental value）
G73 / G83
Offset value
（incremental value）
G76 / G87
P The delay time at the bottom of the
hole
ms G74 / G76 / G89 G81 ~
G87
F The feedrate of the cutting mm/min G73 / G74 / G76 G81 ~
G87 / G89
K The repeat times of the fixed cycle G73 / G74 / G76 G81 ~
G87 / G89
In 808D, the default ISO program feed distance unit is mm!
(X100→100mm)
Note: change the parameter 10884 = 0, to make X100 → 100 um / X100. → 100 mm
Brief introduction of typical fixed cycle codes in ISO mode.
G73 fast-speed deep hole drilling
Common programming structures:
G73 X—Y—Z—R—Q—F—K
Motion process:
① Drilling motion (-Z) → intermediate
feed
② Motion at the bottom of the hole →
none
③ Retraction motion (+Z) → fast feed
G73 application example program:
M3 S1500 ;spindle rotation
G90 G99 G73 X0 Y0 Z-15 R-10 Q5 F120
;after orientation drill 1st hole, back to R point
Y-50 ;after orientation drill 2nd hole, back to R point
Y-80 ;after orientation drill 3rd hole, back to R point
X10 ;after orientation drill 4th hole, back to R point
Y10 ;after orientation drill 5th hole, back to R point
G98 Y75 ;after orientation drill 6th hole, back to R point
G80 ;cancel fixed cycle
G28 G91 X0 Y0 Z0 ;back to reference point
M5 ;spindle rotation stop
M30
For the meaning of letters when programming typical fixed cycles,
please refer the figure on the left!
G74 reverse tapping cycle
Common programming structures:
G74 X—Y—Z—R—P—F—K
Motion process:
① Drilling motion(-Z) → cutting feed
② Motion at the bottom of the hole →
spindle rotation in positive direction
③ Retraction motion(+Z) → cutting feed
G74 application example program:
M4 S100 ;spindle rotation
G90 G99
G74 X300 Y-250 Z-150 R-120 P300 F120
;after orientation drill 1st hole, back to R point
Y-550 ;after orientation drill 2nd hole, back to R point
Y-750 ;after orientation drill 3rd hole, back to R point
X1000 ;after orientation drill 4th hole, back to R point Y-
550 ;after orientation drill 5th hole, back to R point G98
Y750 ;after orientation drill 6th hole, back to R point G80
;cancel fixed cycle
G28 G91 X0 Y0 Z0 ;back to reference point
M5 ;spindle rotation stop
M30