PDA

View Full Version : SR20 STAR Lathe



jrob69
09-10-2008, 01:11 AM
Im trying to use the 6-station toolholder position which i need to command
with a m900 code after selecting t500. Which then it should go to 6 tool position. It gives me an alarm. Number not found. anybody knows what im doing wrong or is there a parameter i need to adjust

kasey435
09-12-2008, 06:42 PM
Hey jrob69,

On our star screw machines, you just have to call up T600. Is there a reason you are going T500, then M900?? Just curious.

Are you using a special tool holder or something???


kasey

jrob69
09-22-2008, 10:23 PM
Hi, Yes this machine is a 1998 model and t600 is a drill station. the holder position 6 is not in the system so they added a diffrent way to use it.

PixMan
12-07-2008, 10:44 PM
The M900 means someone wrote a custom M code to pull up a sub-program (O9000 range) that would move the Y axis cross slide over another increment. The error you're getting means the macro program (or sub program, as you prefer), is probably missing.

There are parameters to look at to see what M code designation is associated with a given O90xx program.

You should have Fanuc manuals. Look in the 6071-6089 range and see which is set to "900". Parameters 6050-6059 are custom G codes. The book will tell you which 90xx program is associated with whatever digits have been entered for that parameter. Then you can look for those O9000 programs to see if the one the M900 is looking for has been deleted. You would need to enable the NE9 parameter (3202.4, I *think*) to see those programs. DO NOT edit any of them unless you know what you're doing!

On those SR20's, the missing program would go deep and temporarily override the soft limits of the travel to get to that position, look for interference with the sub-spindle slide, perform the operation programmed, then return and reset the soft limits. If you don't have hardcopy printouts of all the protected O9000-series programs that were in the machine as shipped, you should call Star to see if they can help. They should have the custom O90xx programs on file, based upon your machine's serial number. I don't think I want to give too much info for fear of getting blamed for a hard crash. ;)

Good luck!

ZOSOSWISS
02-14-2009, 11:24 PM
M900 on my old SR20 calls up tool position six on the main gang. Older Stars only had 5 o.d turning stations. The addition of the sixth tool came before the Fanuc control was updated, thus the need for the M900 to call the tool up and M901 to call off the tool.

chet470
03-12-2009, 09:19 PM
1)Go into your custom graph page
2)select the keep relay option
3)select yes for using overhang tool for T600