need help with drill cycles, G81 etc.

[cabledude]

Hey all. I'm running my Bridgeport BOSS5 under Mach3 now, but transitioning from the simple Gcode of BOSS to Mach is sometimes a bit daunting. My question is, when using G81 or G83, the Z axis pops down to Z zero (top of the work surface) as the cycle begins even though I start the drill cycle at Z.050 (.050 above the work surface). With each repeat move within the cycle, the drill comes back up to .050, the X/Y moves, then the drill rapids to Z0 instead of starting at Z.050. What am I missing?

Thanks for any help here!

Rob

[mcarvey]

Can you post the exact code you are using? The X/Y moving is a red flag, but let's check to see that the code is correct before debugging any other areas of your machine.

-Matt

[G0G90]

"typical" G-Code machines use an "initial height" paramater on canned cycles that tells the control where to go after each X-Y position.
G98 = Initial Height return
G99 = Reference Height return
If you are using the G99 function, make certain you are using a positive clearance value for your "R" address.
You can also verify this by going to a larger value before you start your canned cycle (G81, G83) This becomes your "Initial Height".
Example;
G43Z1.0
G98G81Z-1.0R.05F5.0
X.. Y..
.... G80
This will move to Z1.0, rapid down to Z.05, drill down to Z-1. and return to Z1.0 and move to the next hole location
G43Z1.0
G99G81Z-1.0R.05F5.0
X.. Y..
.... G80

This will move to Z1.0, rapid down to Z.05, drill down to Z-1. and return to Z.05 and move to next hole location.


As I'm not familiar with your type of machine, the code may be different however, the function will be the same.

[cabledude]

Thanks for the responses guys. Here is an excerpt from one of my programs:

G20
G49
G53
G90
G17
G0Z0
(T2 1/4 CENTERDRILL)
G0X-4.0Y4.0T2M6S1800
G43H2
M3
G0X.219Y-.250
G0Z.050
G81Z-.180F2.5
X.427
X1.000
X1.574
X1.781
Y-.750
X1.574
X1.000
X.427
X.219
M5
G49
G0Z0
(.125 DRILL)
G0X-2.0Y-2.0T3M6S2000

I'm rapiding to my X and Y points, then rapid Z down to where I want to start my drilling cycle. I then invoke the G81. I am not specifying an R or a G98/99. Is this my problem? Do I always need to use an R value? Is the drill popping down to Z0 each time because the G81 is assuming R0? It rapids back up to .050 each cycle for the XY move, but rapids down to Z0 before it starts to drill the next hole.

Thanks.

Rob