[jslater20]

I just started working with this machine its a citizen A-20 and everytime i load a new bar or towards the end of one it alarms out in the program check that the Z-axis is going to overtravel my Z push is 4.065 and my overall length in the machine data is 4.375 help please!

[micky316]

check your cancelling all ofsets in Z axis ,I had it once where it kept adding a small ofset on one tool that wasnt canceled and then eventually overtravelled

[gizmo_454]

Also, check your bar loader portion of the program where you back the old bar out, loader inserts a new bar, and then the spindle pushes forward again to cut off the end. Make sure that the location you are sending Z to is the same as the G50 call out at the beginning of the program.

If that is not your problem, check to make sure any coordinate shifts are being un-shifted the correct amount. This gets me every time.

Good luck!

Mike

[danrudolph]

Another way to diagnose the problem: turn on program pre-analysis. It will run through your program and make sure you start and end the program in the same position, in every axis. It will find your error.

Only drawback is that not every program can work with pre-analysis and may throw errors if that is the case, see the manual.

[cogsman1]

"Pre-analysis" could tell you OR you could just do "Start Position" and run one part. When it stops look at the top of the screen for the "Position" in the "MCH POS" side. Write down ALL the values. Run a second part (DO NOT DO START POSITION BEFORE SECOND PART!) compare the same numbers. Any differences will show you have a program problem. Shift or offset not canceled corectly. Usually the "G50 Z##" and the "G0 X## Z## T0" is not correct. The "Z" MUST be the same.

[z369]

I just started working with this machine its a citizen A-20 and everytime i load a new bar or towards the end of one it alarms out in the program check that the Z-axis is going to overtravel my Z push is 4.065 and my overall length in the machine data is 4.375 help please!

Not sure if this will help but your bar-feeder should "push" out as much as your Z axis stroke requires, i always try and add more in the bar-feed program (a half inch), also check to make sure your cut-off shift if you require one is calculated into the bar-feed data. Also make sure your G04 codes are in the program in the right spot at the beginning and end of the program most especially on bigger stock.
My bar-feeder is still set in Metric and I just round it all up.

[K-Bear]

Hi guys,

Running a Citizen L12, and my programs include a G50Z shift at the beginning, and a corresponding G0T0Z shift at the end. As a result, the Z1 axis returns to the same absolute position after every part. This absolute position seems to be determined by wherever I make the initial cutoff. I was curious which variable or parameter this was stored in, but I can't seem to find it. When I change the Machining Length value (#818) in the MC-Data page, it has no effect on the absolute position that the headstock returns to. I found a parameter labeled #25119 that says Mach Length+Cutoff Tool Width, but when I changed that, it also had zero affect. Can anyone tell me definitively--not just speculation or guessing--what the Mitsubishi control is using as it's stroke length? Is it memorizing the absolute position at initial cutoff and returning to that position, or is it moving back a specific amount that's stored in a variable? Thanks.

[gizmo_454]

If the L works like the E and M machines, then the Machining Length Value in the MC-Data page will tell the spindle where to move the main spindle. However, this is only moved there, and utilized when in preparation mode, after making the machine cutoff the bar, and then sending the machine to "start position." The G50Z at the beginning of the program tells the machine, "You are here." Then the G0T0Z after the cutoff says, "Go back where you started from." If these values are not the same, the main spindle will creep one way or the other, part after part, until it over travels. The long and short of it is, if you want the main spindle to change its starting location for longer or shorter parts, you change the machining length value in MC-Data, go to prep mode, run the cutoff cycle, and then open the main collet and run start position cycle. Then close the collet. Your spindle will be in its new location.