HAAS offset from FANUC

[mikechvz]

howdy

for the past 8 years ive only worked on DAEWOO and DOOSAN machines with FANUC controls of course. I recently took a new job, and they have all HAAS. When I used the FANUC there was G54, G55, G56 etc.

 

Above my G54 setting was a "shift offset 000" where if I wanted to offset my Y +.010 all I had to do was put .010 into the y coordinate instead of adding +.010 into the G54 and changing my TRUE origin. On the HAAS I see there are G54 G55 and so on, but also a G52. do I have to change my actual G54? is there a world coordinate offset that I can make incremental offsets instead?

[Guest MTB Technical Services]

You can run it just like a FANUC.

[Clarence L Cook]

It depends on setting 33.

 

Do you have probing on the machines?

 

If yes, the G52 will not be a global offset to the other work offsets because setting 33 is Fanuc.  When the reset or cycle start buttons are pressed, all the values ins G52 will go to 0.

 

If no, change setting 33 to Haas and G52 will hold the values and apply the values to all of you other work offset.

 

Setting 33 can also be Yasnac, and G52 will be another work offset like G54, G55, etc.

 

The inspection plus macros supplied by Renishaw require that setting 33 be in Fanuc mode.

 

Kind regards.

Clarence

[mikechvz]

It depends on setting 33.

 

Do you have probing on the machines?

 

If yes, the G52 will not be a global offset to the other work offsets because setting 33 is Fanuc.  When the reset or cycle start buttons are pressed, all the values ins G52 will go to 0.

 

If no, change setting 33 to Haas and G52 will hold the values and apply the values to all of you other work offset.

 

Setting 33 can also be Yasnac, and G52 will be another work offset like G54, G55, etc.

 

The inspection plus macros supplied by Renishaw require that setting 33 be in Fanuc mode.

 

Kind regards.

Clarence

 

no sir we do not have the probing on this machine, and I do not want the Yasnac settings.

 

is the difference between HAAS and Facuc setting in 33 just that the fanuc setting goes back to ZERO in the offsets?

[Machineguy]

Haas mode has some extras built in on the g- code side.

Probing saves a lot of time in setup. Worth adding on if the software can allow it. It WILL pay for itself in time saved very quickly.

 

Machineguy

[Clarence L Cook]

Yes, the only difference that I have read about and experienced between the Haas and Fanuc setting is what happens to G52.  

 

I personally like it in Haas mode because it allows global shifting.  I typically use the G52 as the machine specific distance between the gage line and the reference I have established on my table because of our Zoller presetter.  I then use the part Z offset to contain the parallels and material height if any.  For myself and my team, the numbers have more meaning and it is a little easier to trouble shoot when I did something wrong during programming.

 

Kind regards.

Clarence 

[Clarence L Cook]

Machineguy,

 

I agree with you.  I am in the process of adding the probing to the last of my Haas verticals.  I will be making some modifications to the probing macros to allow setting 33 to stay in Haas mode.  I realize that this is a little risky, but as I envision my process, I will be removing a number of macros from the control and this should reduce the risks involved.

 

Kind regards.

Clarence

[Machineguy]

The probe macros take half your memory away. You'll be down to about 500 k on a 1 meg machine. I have a VM3 so I have all the bells a whistles installed.. On big programs I put them on the Hard drive and run from there. That's 40 gig.

I have no issues running on the fanuc side. G52 and G92 run differently in the 3 modes to chose from. Look at the book under settings,  #33.

Also Look at the macros in the book. Some Fanuc macro codes are not allowed in the Haas control. Its a short list.

 

Machineguy

[mikechvz]

 

Yes, the only difference that I have read about and experienced between the Haas and Fanuc setting is what happens to G52.  

 

I personally like it in Haas mode because it allows global shifting.  I typically use the G52 as the machine specific distance between the gage line and the reference I have established on my table because of our Zoller presetter.  I then use the part Z offset to contain the parallels and material height if any.  For myself and my team, the numbers have more meaning and it is a little easier to trouble shoot when I did something wrong during programming.

 

Kind regards.

Clarence 

 

this is exactly what im talkin about.  thanks everyone, great help