Need Help!- Bridgeport CNC G-Code Program Question

[minton]

Please review and edit this sample program. It will be used on a Bridgeport with a DX-32 control.
Regards,
Bob Adams
989 798 6581

G90 M6
G0 X-6.5 Y5.0 T1 S1000 M3
G0 X3.75 Y0.0 Z.1
G81 X3.75 Y0.0 Z.42 F1.0
G90 M6
G0 Z-6.5 Y5.0 T2 S400 M3
G0 X3.75 Y0.0 Z.1
G81 X3.75 Y0.0 Z.85 F4.0
G90 M6
G0 X-6.5 Y5.0 T3 S150 M3
G0 X3.75 Y0.0 Z.1
G84 X3.75 Y0.0 Z1.0 F9
M22

[gdwood3rd]

Go to Odin, Ltd.'s website (odinltd.net) and fill in the contact form and they will contact you. If anybody has manuals or can teach you about your machine, it's these guys.

[minton]

I added the tool and number to the G90 line and the program worked. Is this the format that you use? If not, please advise. Regards,

G90 T1 M6 ; (Center Drill)
G0 X-6.5 Y5.0 S1000 M3
G0 X3.75 Y0.0 Z.1
G81 X3.75 Y0.0 Z.42 F1.0
G90 T2 M6 ; (Drill Q .332 dia.)
G0 Z-6.5 Y5.0 S400 M3
G0 X3.75 Y0.0 Z.1
G81 X3.75 Y0.0 Z.85 F4.0
G90 T3 M6 ; (Tap 10mm X 1.5)
G0 X-6.5 Y5.0 S150 M3
G0 X3.75 Y0.0 Z.1
G84 X3.75 Y0.0 Z1.0 F9
M22

[John Bennett]

Gcodes that are in effect when machine powers on G0, G17, G30, G40, G70, G72, G75, G90 (that applies to the Boss 8-9 control but should also apply to yours)

Although first G0 is not required, it is easier to read with it. G30 at end will end program, rewind program go to clear point, G22 just ends program,goes to clear point,,,,to run program again you would have to reset with G22.


%
:1234;Simple Drill and Tap Program
T1 ; (Center Drill)
S1000 M3
G0 X3.75 Y0.0 Z.1
G81 X3.75 Y0.0 Z.42 F1.0
T2 M26 ; (Drill Q .332 dia.)
S400 M3
G0 X3.75 Y0.0 Z.1
G81 X3.75 Y0.0 Z.85 F4.0
T3 M26 ; (Tap 10mm X 1.5)
S150 M3
G0 X3.75 Y0.0 Z.1
G84 X3.75 Y0.0 Z1.0 F9
M30
%

Additionally, ":1234" could be put at beginning to note program number

On the Boss 8-9, all programs, have to have, the first and last line as character "%"

The programs to look for are EZLINK or EZUTIL, these will allow REM and DNC input. (I have copies if required)

CNCSIMULATOR.COM has a free simulator that works for moves but not canned cycles or drill cycles due to the z

[gdwood3rd]

There is an old saying,"If it works don't fix it", but in this case there are a couple of things I would ask you to try(cautiously). I am curious as to why you have to re-initialize absolute positioning after every tool change (G90). Typically the tool change macro begins with a G91 code and proceeds to position, index, change tools as prescribed by the M6 Macro Call, but should end with a G90 ergo no need to re-initialize. If you can access the macro, see if it has been omitted and if so put it back in as the very last line of code. Then omit the G90 from your part program and that should save you some typing in the future. The other thing I noticed was repeating X & Y locations in your canned cycle lines (G81), although it has no negative impact other than taking up memory space, once you call a canned cycle, it will perform as programmed on that line at whatever point it is at in X & Y first.
Hope this helps, also try John Gale at Solvers Techline - Home , or look up Gale Force Technologies, Cool Dude with lots of "Old Iron" information. I don't know his fee structure but tell him George Wood sent you.

Good Luck !