Results 1 to 10 of 10
Thread: bar puller ?
09-13-2007, 08:24 PM #1
I'm trying to write a bar puller program and having some problems. my machine will not feed in g98 ipm mode unless i give it a g97 s0 m3 comand. if i don't put that in it will rapid to the x z pos in the program and just sit there.
is there something in the parameters i need to change? the control is a fanuc 18t.
09-13-2007, 08:40 PM #2
You should probably post your code so everyone can take a look and see what it is you have programmed. Will be a lot quicker to diagnos rather than everyone trying to guess what you may have.
09-13-2007, 08:41 PM #3
move to part...
G1 Z?.??? F20.
just make sure to put a G99 at the start of the program to put it back into ipr mode...
I do bar puller jobs all the time...
One machine used the older friction type bar puller... and the other is hydrolic...
very simple and easy
09-13-2007, 08:52 PM #4
Solar has it. Ran pullers for 'bout 7 years on the 18-T. Bar feeders one servo the other bar stop after that.
GO X0. Z.1
G1 G98 Zxxxx F75.
G0 Xxxxx Zxxxx
09-13-2007, 08:54 PM #5
even if i just put an m3 in there it will work. then i have to put an m5(spindle stop) then an m11(open spindle) then i put in a g1 feed rate to pull the bar out but it just sits there because i had to stop the spindle in order to open the chuck. and i am putting in a g98 at the beginning and a g99 with my first cutting tool. i will try to post some code tomorrow.
this machine had a barfeeder on it before i got it. i even tried turning the barfeed interface on and off from the front panel to no avail.
09-13-2007, 09:51 PM #6
If it had a barfeeder on it before you got the machine it will probably need a parameter changed if it has not already been done.If you turn the barfeed on and the param is set for a barfeed it will be looking for signals from a barfeed that does not exist so will still not work.If you have the param list check and see what options have been turned on.
09-13-2007, 09:58 PM #7
bar feeder on off ( or somethings like that)
you probably miss some G code or using wrong one
09-13-2007, 10:38 PM #8
This is how I use a bar puller on a Fanuc OTC
G0X2.Z-.35(APPROACH BAR IN RAPID)
G98G01X0.0F140.0M31(FEED ON THE BAR)
G01Z1.055F140.0M31(M31 interlock bypass chuck&tailstock)
G01X2.0F140.0M31(FEED OFF THE BAR)
G99(INCHES PER REVOLUTION = G99)
G28U0.W0.(RAPID FROM BAR TO HOME POSITON)
This control needs M31 for a interlock bypass, yours may as well.
Mike Roy in Canada
09-14-2007, 09:37 AM #9
on my control m34 is the bypass. i put that where you have your m31's and bingo!! well almost. it went through one cycle and stopped.
here is my barpuller prog:
O0016(bar puller program)
M98 P1237 L16;
so i did a search and found a post by boris, so i gave it a try and re-wrote my bar puller program like this:
O0016(bar puller program)
M98 P161237; (call prog 1237 16 times)
looped 16 times and stopped.
THANKS EVERYONE FOR THE HELP!!!!
If it was'nt for this site i'd still be scratchin my head.
09-14-2007, 03:14 PM #10
Glad to be some help