Originally Posted by
whiteboy
Harry,
Maybe I can help you out. First, lets dissect your program and see what you have ....
G20 --- Default command. Okay to have here but not absolutely needed.
(TOOL - 7 OFFSET - 0) --- Okay. Tool# and Offset # description
(7/32 DRILL) --- Okay. Tool description
G28 U0. W0. --- Don't need U0. W0. with G28
G50 X10. Z10. --- Bad line. G50 is Spindle Speed MAX RPM Limit ie; G50 S3100
G0 T0700 --- Bad Line.
M23 --- bad Line. M23 is Angle Out on threading "ON"
G0 X9.5 Z-2.3 --- Okay. Rapid move in X and Z to your start point ?
C90. --- Bad line. Can't run C- Axis without first engaging C-Axis with M154
G97 S1222 M51 --- BAD line. 1) DO NOT turn spindle (G97 S1222) when cross drilling & 2) M51 is Optional User M Code Set
G81 X.4 R4.5 F4.11 --- I don't believe you can use a G81 drill cycle with the live tool
C30. --- Okay. Rotate to 30 degrees...
C-30. --- ??? Rotate to -30 degrees
C-90. --- ??? Rotate to -90 degrees
C-150. --- ??? Rotate to -150 degrees
C-210. --- ??? Rotate to -210 degrees
G80 --- Not sure. If G81 is usable with live tool, then okay.
G28 U0. W0. H0. M55 --- Bad line. Don't need H0. and M55 is another Optional User M Code Set
T0700 --- Potentially bad line. "00" after T07 cancel tool 7's offset. This can get you in BAD trouble if you're not careful.
M30 --- Okay. Reset program and return to beginning.
So..... we need to know a few things.
1) What kind of material are you working with ?
2) What is diameter of area being drilled ?
3) How deep are you drilling ?
4) Is hole blind or thru ?
5) Are the holes in specific relation to any other part features ? ie; Does hole #1 start xxx degrees off from a flat that is on the part ? Or are there simply 5 (?) holes equally spaced around the part ?
I'll keep an eye on this post for your reply or you can email me.
Best Regards,
Steve