Need Help!- Getting Bobcad to not use G00 rapid.

[joefox]

For some reason one of my CNC routers with a Allen Bradley 9 series controller is acting stupid. If the G-code has 2 lines in a row that are G00 rapid motions it stops and won't go any farther than the first rapid motion. It will run fine with just one rapid command but two or more make it stop
I'm running V20 and would like to have it eliminate rapid motions all together and just have it change the feed rate to 1200ipm.
Do I need a new custom post or is there a setting I can change?

[tobyaxis]

Use all solid lines in your geometry. Dashed lines will translate into rapid movements.

[Sowen]

If you are using V19-V21, in the nc window click on setup conversion in the left hand side of the conversion window type in G00 directly to the right type in G01 this will convert all the G00 moves to G01.

If the duplicate codes are causing an error try turning on the gcodes modal setting your code would be as follows...

MODAL GCODES
G00 X10.0 Y10.
X0.0 Y0.
G01 X5.0 Y5.0
X10.0 Y10.0


NON-MODAL GCODES
G00 X10.0 Y10.
G00 X0.0 Y0.
G01 X5.0 Y5.0
G01 X10.0 Y10.0

If the above modal issue solves the problem you can change bobcad by just checking or unchecking the Gcodes Modal box. Click on Setup Driver then the ISO tab Check or uncheck the Modal Box.

You can also convert the ipm in the conversion box




I'm running V20 and would like to have it eliminate rapid motions all together and just have it change the feed rate to 1200ipm. ------
Here is the conversion..

LEFT SIDE OF CONVERSION
G00@ {X-*[0-9]*.[0-9]*}@ {Y-*[0-9]*.[0-9]*}@ {Z-*[0-9]*.[0-9]*}
G00@ {X-*[0-9]*.[0-9]*}@ {Y-*[0-9]*.[0-9]*}

RIGHT SIDE OF CONVERSION
G01 @1 @2 @3 F1200
G01 @1 @2 F1200

SEE ATTACHED PIC