Changing Parameters in the Program

[danrudolph]

I have one program that uses the G83 "high speed peck" where it only retracts a small amount then continues feeding. All my other programs use the "full retract where the drill exits the hole to clear the chip.

According to the Fanuc books, this appears to be something that is possible, but I have not attempted it. I would like to set the parameter (5101 bit 2) to a 0 at the start of the program and to a 1 at the end, so the parameter always remains with a 1 for use with the other programs. I will need to do this in both $1 and $2. Machine is a citizen a20 type 7.

Do any of you regularly change parameters in programs? What about the R plane distances for the G83 cycle, can that be changed at the start of a program?

Thanks.

[jimiscnc]

But, if it's a mitsubishi control, then it probably has a letter address assigned to load G83 parameters right in the G code program. In other words, a G83.1 or G83.2 or G73 or some other variant of the basic G83 can now accept new program words to control R plane, peck amount, and whether to have a quick peck or full withdrawal. Or a combination of both.

This is probably covered in detail in the EIA program manual, if it's available.

jim

[cogsman1]

G83-(option) Peck drilling cycle. There are (3) parameters related to G83.
Param #5101 bit2 "High speed" if "0" then the pecks do NOT come out of
the hole, they only back up the amount of Param #5114 "G83 Retract",
to break the chip and then start feeding again. Remember there are
2 systems $1 -$2 so there are two of each of these parameters.

Param #5114 "G83 Retract -.02" is the amount to rapid back into the
hole from the last peck for clearance. If #5101 bit2 =0

Param #5115 "G83 Retract -.02" is the amount to rapid back into the
hole from the last peck for clearance. If #5101 bit2 =1

I suggest...
Param #5101 bit2 = "1" -Rapid out of hole every peck.
Param #5114 "G83 High speed Retract" = "-.02" from last peck.
Param #5115 "G83 Retract" = "-.02" from last peck.


Example-
G0 Z-.05 T22
G83 Z1. F.001 R.03 Q04000 P0

Z1. =Z position of the bottom of the hole

F.001 =Feed in IPR or IPM

R.03 =Rapid from current Z position the R amount incrementally.
If starting at Z-.05 and R=.03 then the Z axis rapidly
positions to "Z-.02" and after every peck Z retracts to
the same position "Z-.02". If you use "R-.03" it is the same
as "R.03".

Q04000 =Peck amount -same as .04 but not allowed a decimal point
(Q04000 for sub inch / Q0400 for non sub inch)

P0 =Dwell amount at the bottom of the hole. You can just leave
P off the command line if you want.

[dookie2022]

It is most possible to change parameters on a Fanuc control inside a program.
This function is usually an option as most machines come with advance features these days it is most likely available but the machine tool company does not document that fact that you have the feature.
You can access most paramters but I would not reckonmend it is like opening up pandora's box and if you make a mistake or do not close correcly you can cause a lot damage. The most common problem is poorly written programs that allow access and if you stop in the middle of the process that the door is still open for access to the parameters and damage occurs at this point.

[Ovrclck350]

Best thing to do would be just write a macro for that program and leave the parameters alone since everything else you run is the same.

Does your control support Macros?