How do I set Parameter 592 for G 83 Cycle

[Farmer]

Fanuc 0TD control on a Turning Center.
I am using the G 83 Cycle to peck drill in Z. Tool feeds to set depth, retracts to remove chips and returns into hole for another drilling feed distance. Problem I am having is when drill rapids back to depth that it retracted from for another feed, there is no clearance from the bottom of the hole to the drill point. It goes right to the depth it came from then changes to feed. Manual indicated that this clearance distance can be specified by setting "Parameter # 592" but then does not tell one how to do that, or at least not that I have found yet. I have found a parameter screen but am not sure which data to change. Anyone familiar with this ???

[wms]

Farmer,

"Changing or altering a parameter can cause a machine tool to do strange and unexpected thing that can lead to serious damage to operator, the machine and the parts. Do so only at your own risk. And with a full understanding of what you are about to do and it's consequences."

That said here you go, a blow by blow:

Place the "mode select" in MDI.

Press the DGNOS/PARM button twice to get to the Parameter screen. The one that says "Parameter > (setting 1).

Next press the page down key to get to the second parameter page. It will say (setting 2) and PWE=0

Now place the cursor on the PWE line and press "1" on the key board and then the "input" key. The control will go into a 100 alarm..no worry.

Now press and hold the "CAN" button and then while still holding down the "CAN" button press the "RESET" button. This will clear the alarm.

After clearing the alarm, press the "PARM" button to get back to the parameter page .

Now use the page down button to get to the screen that has the #592 parameter on it and use the "cursor " buttons to get the cursor on that line.

Now type the value you want for that parameter from the key pad. And press the "input" button to enter it. It will show up as soon as you press input.

Now back track to the second parameter page the one with the PWE line and re-enter a "0" in place of the "1" you input earlier at the PWE line.

Now power down and re-power the machine.

All set.

By the way in inches it is .0001 units. So 100 = .010 as far as the parameter is concerned

[AdvanTech]

Originally Posted by wms By the way in inches it is .0001 units. So 100 = .010 as far as the parameter is concerned

Every machine that I've seen is in metric for paramters even if the machine runs in inches. So 100 = .100 mm

[wms]

Well not true for a Fanuc 0T series...it as I have stated if you are using Inch as your input values..Says so right in the manual.

[AdvanTech]

Originally Posted by wms Well not true for a Fanuc 0T series...it as I have stated if you are using Inch as your input values..Says so right in the manual.

This is just my experience even on OT's. Doesn't mean it the same on all machines. He might want to check it.