[Darth Yoda]

Hi guys. Got a bit of a problem. I have a HwaCheon ECO31A with a 18T controller. I use BobCam for code (I know, please don't laugh).
The first problem was the machine went backwards. Got a different postprocessor and now I'm getting a "Improper code in G71-73" error.
Here is part of the code.
%
O80 (QL80 E)
( PROGRAM START - TURNING CYCLES )
( PROGRAM NAME: QL80 )
( POST: FANUC 18T )
( DATE: TUE. 02/19/2013)
( TIME: 08:30AM)
N01 G99 G90 G80 G40 G20
N02 G00 G28 U0. W0.
( )
( )
N03 G54 G97 S763 T0505 M04
N04 G50 S3000
N05 G97 S500
N06 G00 X-1.25 Z.1369 M08
N07 G71 U.1 R.1
N08 G71 P09 Q38 U.01 W.01 F6.
N09 G00 X-1.1102 Z.1269
N10 G41 G01 X-1.0102 Z.0269
N11 X-1.0575 Z-.0186
What am Idoing wrong to cause the improper code?
Also, in another post I read the G50 is no longer used. If so why does BobCam continue to use it? How would you properly code it?

I really appreciate your help guys. Responses are quick and helpful.

[underthetire]

G50's are always used on lathes to limit the max spindle speed. Last thing you want is some massive piece of material spooling up with CSS on and flying out of the chuck. G50 for WORK SHIFT is rarely used anymore. Can't help on the rest.

[txcncman]

Your machine might be set up for single line G71 (canned cycles).

[txcncman]

One should always know how to manually write G-code for the machines they are programming before using CAM software in order to be able to identify bad code and make needed corrections.

[angelw]

Hi guys. Got a bit of a problem. I have a HwaCheon ECO31A with a 18T controller. I use BobCam for code (I know, please don't laugh).
The first problem was the machine went backwards. Got a different postprocessor and now I'm getting a "Improper code in G71-73" error.
Here is part of the code.
%
O80 (QL80 E)
( PROGRAM START - TURNING CYCLES )
( PROGRAM NAME: QL80 )
( POST: FANUC 18T )
( DATE: TUE. 02/19/2013)
( TIME: 08:30AM)
N01 G99 G90 G80 G40 G20
N02 G00 G28 U0. W0.
( )
( )
N03 G54 G97 S763 T0505 M04
N04 G50 S3000
N05 G97 S500
N06 G00 X-1.25 Z.1369 M08
N07 G71 U.1 R.1
N08 G71 P09 Q38 U.01 W.01 F6.
N09 G00 X-1.1102 Z.1269
N10 G41 G01 X-1.0102 Z.0269
N11 X-1.0575 Z-.0186
What am Idoing wrong to cause the improper code?
Also, in another post I read the G50 is no longer used. If so why does BobCam continue to use it? How would you properly code it?

I really appreciate your help guys. Responses are quick and helpful.

Check the status of parameter bit 0001.1 (FCV). If set to "1", the single block G71 - G73 will apply. If set to "0", the format in your example code applies.

Regards,

Bill

[Tnichols]

I have similar problems as this. But one thing that I have figured out is that you can not have a G41/G42 within the canned cycle. It has to be before the first G71 line. An the G40 after the last line of the cycle. And also can not have a G00 move whle G41/G42 is still active if they are used when not running a G71/G72 cycle.

[Tnichols]

Another problem that I see is that you have G99 active and you have a G01 feedrate of F6. That would be 6 ipr. With that feedrate rate you will need a G98 instead of G99.

[Darth Yoda]

Thanks for the responses guys. I thought since "BobCAD-CAM is the World Leader in Powerful & Affordable CAD/CAM Software" that they would do it right. But apparently not.
Will check my machine settings and recompile code. Thanks again.
My machine parameter is "0".

Trinichols, I saw the speed setting was wrong but I was just trying to get the machine to move in the correct direction, so the actual speed didn't matter in this case. When I run it's usually .006 rough cut.

[Darth Yoda]

Angelw Here is a picture of my parameters. If I understand correctly this program should run, correct?
Just for my own understanding, what observations did you make to reach this conclusion? (That sounds harsh but is NOT meant to be.)
As it is the machine doesn't accept a G54 command at all. I know G54 is mainly mill code but in this instance what would set up part home?