[harry smith]

Hello to everyone.
Just started with new company, they manually programmed some c-axis drilling etc. Also new to mastercamx. Not much experience with lathes.
Should this program be close to working (don't want it on machine yet.)
Any input would be appriciated.
thanks-harry.


G20
(TOOL - 7 OFFSET - 0)
(7/32 DRILL)
G28 U0. W0.
G50 X10. Z10.
G0 T0700
M23
G0 X9.5 Z-2.3
C90.
G97 S1222 M51
G81 X.4 R4.5 F4.11
C30.
C-30.
C-90.
C-150.
C-210.
G80
G28 U0. W0. H0. M55
T0700
M30

[APP]

No.

[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

[Haas_Apps]

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

G50 is also a command to set your coordinates

I would recommend looking at the examples in the manual.

[whiteboy]

Haas_Apps,

I stand corrected.... My only defense is that 1) I have never had need to use G50 for anything other than spindle speed clamping 2) When I was replying to the original post, I referred to my copy of Haas' Machinists CNC Reference Guide for G50 and M23 and it says only that G50 is Spindle Speed Maximum Rpm Limit, and nothing about work coordinate setting...

At any rate, thanks for the info. Will download latest Operators Manual from your site and read up on G50.