G10 L? for setting G54.4 (Mazak)

[rsbeadle]

I have a macro made up to calculate G54.2P1 from G54 and G54.1P1. We have a new VCU machine that uses the new G54.4 for dynamic fixture offset. Is there an L number for G54.4 that I can use in the G10 data setting? I have searched the internet for a couple of days and can't find anything. I can work around it by using the G10 to set another work offset and use macro variables to copy it to G54.4 but having the L number would be much cleaner.

 

L2 P(1-6) is for G54-G59

L20 P(1-300) is for G54.1 P(1-300)

L21 P (1-7) is for G54.2 P (1-7)

 

L?? P(1-8) for G54.4 P(1-8)

 

Thanks in advance for any help. 

 

[crazy^millman]

Look it up in the PDF's that come with the machine. Mazak is very good on the Variable definitions.

 

HTH

[rsbeadle]

I checked in the eia programming and operating manuals and could not find it. would it be in a different manual?

[Colin Gilchrist]

I can't find anything for setting the G54.4 WSEC values. This would be the amount of error you are trying to compensate for. What work offset are your picking up before calling WSEC? In the e-1850 manual that I've got, it mentions that only G54-G59, and G54.1 P1-P300 are valid.

 

I did see some information for setting G54.2 P1-P8:

 

G10 L21 Pn Xx Yy ..... Aa (A=angle)

 

But, it looks like you aren't able to run both WSEC and Dynamic Work Offsets at the same time. (I could be wrong about that, I seem to remember someone saying that do that...)

 

Is your fixturing setup to be repeatable so that your WSEC values are the same when loading a fixure back into the machine? Or is this something that you want to be able to set with a Probe for example?

 

The variable values for WSEC are as follows:

 

 

 

 

[Colin Gilchrist]

So technically, I think you could input your values into the WSEC registers using variables instead of a G10 line...

#5811=.0021
#5812=0.0
#5813=-0.0013
#5814=0.023
#5815=0.0
#5816=-2.248

[GPC_CNC]

Chapter 26 in our variaxis manual covers G54.4. There doesn't seem to be a G10 line for it as the settings are more comprehensive than X,Y,Z,A,C. You can however set them with variables in the program, which is what I do.

[steadyfred]

I store the machine center point of rotation in G59 and also in G54.1 P300

 

I then set up my job in G54 and run a program (mine is saved as prog #1 on the machine)

 

O1()
(CALCULATE WORKPIECE SETUP ERROR CORRECTION VCU4005X)

(G54 - G54.1 P300 = G54.4 P1)
(G54 B & C TO G54.4 P1)

#5811=#5221-#75981
#5812=#5222-#75982
#5813=#5223-#75983
#5815=#5224
#5816=#5225
#5817=#5224
#5818=#5225
M30

 

This sets up your G54.4 P1

 

You could also change the M30 to an M99 and call the program from your posted program with a simple post mod (or just add the # lines to the post)

[Guest]

Try G10 L23 P...

 

That's what it is on FANUC.