Printable View
Trying to use a G1 with z moves for a bar puller. When this line is reached it stops and shows the correct distance to go but will not move. If I turn it on DRY RUN it will move and do the cycle fine. I'm using the same program for 3 other machines with Fanuc controls. I even tried MDI ( G1 z-.1 F50. ) and it would not move with out DRY RUN either. Is this a parameter that is turn off ?
Thanks
Stab in the dark here but it sounds like your machine is not going into mm/min (G98) but if your machine uses special G code this would be
G95 (mm/min)
G94 (mm/rev)
Hope this helps
At the beginning of the bar puller I use G0 G40 G98. All programming is in inch. Should I try G95 in place of G98?Quote:
Originally Posted by Ant29018
Thanks for your time.
Yes that is where i would start
Heres a link to a list of special G codes
http://www.memex.ca/wp-content/uploads/Memex-Standard-Lathe-G-Code-Chart.pdf
Still no luck. It says no feed rate specified when using G94 and illegal G code with G95. When I put it back to where all the other machine are and press dry run to get z to move then immediately release it will do the feed rate i want but after m69 to unclamp I have to press dry run again to get moving then release to get proper feed rate. I even photoed the active G codes on another Fanuc 0i machine while bar pulling and they match. Any other ideas ?Quote:
Originally Posted by Ant29018
Thanks for your time.
Did you give it a feed rate after the G1 command ?
What machine is it?
Yes I did.Quote:
Originally Posted by gabedrummin
G0G40G98
x0.z0.
G1Z-1.F50.
Once it reaches the G1 Line it stop. Will start axis movement with DRY RUN and if I take it off it will finish its stroke in the specified feedrate.
Hwacheon HI-Tech 200A Fanuc 0i-tbQuote:
Originally Posted by Ant29018
There could be an M code that allows the machine to move whilst the spindle is not rotating like on a doosan
There could be a keep relay that could affect the same
I have done a little digging and found this, does it sound familiar?
http://www.cnczone.com/forums/fanuc/108494-bar-puller-hwacheon-oi-tb.html
I changed bit 0 on parameter 3708 from 1 to 0 and it worked !!! The other guy chimed in and said that it will cause problems with thread cutting if bit 2 of parameter 3708 is also 1 but I will check parameters on other Hwacheon 0i tomorrow cause it threads fine while doing feed rates with spindle off. I will let you know.Quote:
Originally Posted by Ant29018
Thanks again !!!
Doing ID threading using G76 code with no problem Changing Parameter 3708 bit 0 to 0.
Thanks for all your help Ant29018 !!!