post g54 and g54

[hoa75nguyen]

Hi everyone,

 

Thank you for all your help and support! i just wonder is there a way i can post my fisrt tool running g54 then g55 and so on to the next tool rather then running complete operation on g54 then g55.

 

thank you

[Tim Johnson]

Yes with macro;

 

(Fadal snippet)

 

N970(NO. 2 CENTER DRILL)
N980T2M06S7868
N990G90M03
N1000#V40=V42+1
N1010#:2
N1020#V40=V40-1
N1030#R9=V40
N1040G00X-.8Y-.5E+R9
N1050H2Z2.5
N1060G99G81Z1.302R01.6F78.
N1070G98X-.2
N1080G00G80Z2.5
N1090#IF V40>V41+1 THEN GOTO :2
N1100G91G28Z0
N1110M01

 

N1120(1/8" .125 DIA. DRILL)
N1130T3M06S10000
N1140G90M03
N1150#V40=V41
N1160#:3
N1170#V40=V40+1
N1180#R9=V40
N1190G00X-.2Y-.5E+R9
N1200H3Z2.5
N1210G99G83Z.9924R01.6Q.0625F72.P.02
N1220G98X-.8
N1230G00G80Z2.5
N1240#IF V40<V42 THEN GOTO :3
N1250G91G28Z0
N1260M01
 

[jlw™]

I'm curious, why? Would this not cause a greater chance for a booboo at the machine? Are you G10ing every offset?

 

Totally just curious.

[hoa75nguyen]

Thank for your input! yes, would be a big booboo at the machine if someone doesn't do the setup right.

[Tim Johnson]

They are standard work offsets loaded just like G54, G55, etc. The macro just tells the program to rerun a program segment on a different offset until it the last part, then go back (in the instance I posted). We've been running this style of macro since the early nineties even though we are currently phasing out the vertical machines for production work.

[jlw™]

Well, I get that then. I misunderstood the first post. I thought he was wanting to run T1 on G54 T2 on G55 T3 on G56 and so on. My bad, I was over complicating it.