Programme D'usinage En Code G - Siemens SINUMERIK 828D Manuel D'utilisation

10.18.4

Programme d'usinage en code G

G17 G54 G71
PIECE(,,"","BOX",112,1,-20,-100,-2.5,-2.5,182.5,182.5)
;****************Changement d'outil****************
T="SURFACAGE" D1 M6
G95 FZ=0.1 S3000 M3 M8
CYCLE61(50,1,1,0,-2.5,-2.5,185,185,2,80,0,0.1,31,0,1,10)
G0 Z200 M9
;****************Changement d'outil****************
T="FRAISE20" D1 M6
G95 FZ=0.14 S3900 M3 M8
CYCLE76(50,0,1,,20,180,180,10,0,0,0,5,0,0,0.14,0.14,0,1,185,185,1,2,2100,1,101)
;CYCLE62(,2,"MA1","MA0")
CYCLE62(,2,"E_LAB_A_PARTIE_4_POCHE","E_LAB_E_PARTIE_4_POCHE")
CYCLE62(,2,"E_LAB_A_PARTIE_4_ILOT","E_LAB_E_PARTIE_4_ILOT")
CYCLE63("TEIL_4_GEN_01",11,50,0,1,10,0.1,0.3,40,3.5,0,0,0,0,0,2,1,15,1,2,,,,0,101,111)
G0 Z200 M9
;****************Changement d'outil****************
T="FRAISE10" D1 M6
G95 FZ=0.04 S8500 M3 M8
POCHE3(50,0,1,4,70,40,10,90,60,15,4,0,0,0.04,0.2,0,21,40,8,3,15,2,1,0,1,2,11100,11,111)
POCHE3(50,-4,1,2,35,20,6,90,60,15,2,0,0,0.04,0.2,0,31,40,8,3,15,10,2,0,1,2,11100,11,111)
G0 Z200 M9
;****************Changement d'outil****************
T="FRAISE8" D1 M6
G95 FZ=0.018 S9000 M3 M8
SLOT2(50,0,1,,3,1,180,10,85,135,40,180,90,0.01,0.018,3,0,0,2001,0,0,0,,0,1,2,100,1001,101)
G0 Z200 M9
;****************Changement d'outil****************
T="FORET_A_CENTRER10" D1 M6
G94 F1000 S12000 M3 M8
MCALL CYCLE81(50,-10,1,5,,0,10,1,11)
POS_1: CYCLE802(111111111,111111111,15,15,165,15,165,165,15,165,,,,,,,,,,,0,0,1)
MCALL
G0 Z200 M9
;****************Changement d'outil****************
T="FORET10" D1 M6
G94 F500 S1600 M3 M8
MCALL CYCLE82(50,-10,1,-25,,0,0,1,12)
REPEATB POS_1 ;#SM
MCALL
G0 Z200 M9
;****************Changement d'outil****************
T="FRAISE8" D1 M06
Fraisage
Manuel d'utilisation, 07/2021, 6FC5398-7CP41-0DA1
Créer un programme ShopMill
10.18 Exemple d'usinage standard
391