Mazak Work offset macro variables

[Jcncprogrammer]

Im doing some work with a shop that has a few mazak vertical mills. A Nexus 700D/40 II, and a VCN-530C. Does anyone have a list of the variables that are assigned to the work offsets? Do both these machines utilize the same designated macro variables? thanks

[JParis]

#5021 = G54 X

#5022 = G54 Y

#5023 = G54 Z

Add 20 to each register for the next G55, G56, etc

Extended are #7021, #7022, #7023.....again, add 20 to each for the next offset value

Not sure if the Nexus is the same....older control of which we have none 

[JParis]

Just got into the office, Mazak starts at

#5201 = X

#5202= Y

#5203 = Z

Same +20 to shift to the next offset

Extended offsets start at 

#7001 = X

#7002 = Y

#7003 = Z

Again, same +20 to shift to the next work offset

That's what I get for working from memory

[Jcncprogrammer]

Thanks alot!  So I would assume G54 A  axis would be #5204?

[JParis]

It'll be the 4th axis...

Could be A or B address depending on the machine setup

 

[Jcncprogrammer]

Looks like Haas starts just 20 after.

Haas G54 X is #5221

[Wargo]

I just came across this while searching for this list to program a Mazak HMC. Looking at existing programs that were done by previous programmers I noticed they were using #5223 for G54 Z

Essentially, if I'm reading this correctly, our current programs are changing variables for one offset greater than intended. Is this correct? If so, this company has been doing this for every probe routine on our Mazak.

[JParis]

49 minutes ago, Wargo said:

I just came across this while searching for this list to program a Mazak HMC. Looking at existing programs that were done by previous programmers I noticed they were using #5223 for G54 Z

Essentially, if I'm reading this correctly, our current programs are changing variables for one offset greater than intended. Is this correct? If so, this company has been doing this for every probe routine on our Mazak.

This was for a Matrix Control, however, the newer Smooth Control also utilizes the same variables...

 

On the new Smooth, up to P48

If you have the extended to P300

[navsENG]

6 hours ago, Wargo said:

I just came across this while searching for this list to program a Mazak HMC. Looking at existing programs that were done by previous programmers I noticed they were using #5223 for G54 Z

Essentially, if I'm reading this correctly, our current programs are changing variables for one offset greater than intended. Is this correct? If so, this company has been doing this for every probe routine on our Mazak.

They could be using g10 to write to 54. And then probing and updating g55. 

All that matters is what offset is being used for actual machining? 

[Wargo]

19 hours ago, navsENG said:

They could be using g10 to write to 54. And then probing and updating g55. 

All that matters is what offset is being used for actual machining? 

I found our manual and it matches what JParis posted. It's being done correctly.