Help needed on FAGOR controller

[CNC_Geek]

Hi Everybody !


Does anyone know which G code disables the axes stop at the end of each G-code line on FAGOR 8040 NC ? I would like the axes' speed to be constant all along the toolpath.


Thanks in advance for your help
Luis

[Kiwi]

I use a Fagor 8055M and I put G51 E0.0001 at the beginning of my code.
This is Look-Ahead with error of .0001mm and the tool dosen't hesitate.

[g-codeguy]

Not sure if this is what you are looking for, but on an 8025 control G05 is corner rounding, G07 is square corner. In G05 the movements programed in the next block are executed before the machine has reached the exact position programed in the previous block. The faser the feedrate, the greater the differance between the theoretical and actual profiles.

In G07 the CNC does not execute the next block of the program until the exact position programmed in the previous block has been reached. The theoretic and actual profiles coincide.

Some controls use an M-code for positive cornering. I didn't see one in the 8025 manual.

[CNC_Geek]

Thanks to both of you !


As a matter of fact, what I was looking for was the G51 function given by Kiwi. I wanted the tool speed to be constant all along the toolpath. It works just fine.

Regards
Luis

[Tapper]

I got the same problem whit Fagor 8055M "Lagging"
When i put G51 E0.0001, i get this Error
CNC: 0174 Cirkular interpolation not possible.

[Kiwi]

Originally Posted by Tapper ...When i put G51 E0.0001, i get this Error CNC: 0174 Cirkular interpolation not possible....

Helical interpolations are not possible while the Look-Ahead (G51) function is active.