My Okuma lathe uses the EP-P300L-R controller. Can I use the program to on / off parameter 29 bit 1 with VOPRB code? (Image in attachment). Please help me. Thank for all
Printable View
My Okuma lathe uses the EP-P300L-R controller. Can I use the program to on / off parameter 29 bit 1 with VOPRB code? (Image in attachment). Please help me. Thank for all
try
VOPRB[29] = [VOPRB[29] OR 2]
please, what is VOPRB ? kindly :)
I tried and encountered this error (please see attached image). Please help.Quote:
Originally Posted by kurmay
Hi deadlykitten, I don't really understand.Quote:
Originally Posted by deadlykitten
hey duongcave, why do you wish to change #29.1 ?
Parameter 29 bit 1 on my machine is used to on / off the "Cycles time check over" function. I have tried on / off manually. I think the VOPRB code can replace me doing thatQuote:
Originally Posted by deadlykitten
please, what is doing this " cycles time check over function " ? inside manuals is nothing about it; only in the machine catalogue i find that "An alarm occurs after the completion of a set cycle " ... i have no clue what this function is doing ...
it seems like the controller does not support the voprb system variable :)Quote:
I tried and encountered this error (please see attached image). Please help.
Right. UnfortunatelyQuote:
Originally Posted by deadlykitten
I think you can do this via m code on your machine. Don’t remember it off the top of my head, check your list in the machine or I’ll dig it out when I get to the office.
I checked and only M code to on / off "STM check over". I'm not sure how it works. But it is not what I need now.Quote:
Originally Posted by OkumaWiz
please, what is voprb ? and how to use it ?
oh, i just discovered what is the " cycles time over check function " : it verifies the duration of the cycle ... hmmm :) so far i could not find a thing, because i was looking for " check over " instead of " over check "
however, i am not sure if this function delivers nice results; it's estimations should be similar to the "cycle time calculation function" ( or maybe these 2 functions are one and the same ? ), and i have seen differences between real time and estimated time; of course, maybe there are a few parameters that can be adjusted, but with so many ctr & motions stuff, i really doubt that the controller can estimate it's self
to control such things, i don't relly on special functions, but on a real baseline; do you wanna know what was the machine doing in 2015, at 10.35am, 1st monday of july ? i can tell that, with <1 second accuracy; do you wanna know the spindle time on 2016 april? again, my methods are not designed to verify or check wrong operator behaviour, thus their output can be messed up, but this can be prevented, only if needed; i said this, because i suppose that you are still hunting your operator :)
about ' cycle time over chek ', i also found these :
... #29.0 STM time over check ON (R-side)
... #29.1 Cycle time over check ON (R-side)
... #44.0 STM time over check ON (L side of parallel two-spindle machine)
... #45.0 STM time over check ON (L side of parallel two-spindle machine)
... #45.1 Cycle time over check ON (L side of parallel two-spindle machine)
* it seems like there is no bit to control the L-side of a normal lathe ( 1 spindle, 1 turret ); of course, manuals translation from japanese is not accurate, especially in such wild areas like the bits, so i would test them :)
and these optional M's:
... M124 STM time over check ON
... M125 STM time over check OFF
... M677 Time over check ON
... M678 Time over check OFF
... M725 Loader time over check start
... M726 Loader time over check stop
kindly :)
I think M677 and M678 are the ones I was thinking of. Please test.Quote:
Originally Posted by OkumaWiz
by the way - are you getting into trouble with this by using a GOTO command for looping rather than the recommended Schedule program (SDF file)?
The control cues off of the M02 or M30 for many things such as tool life, alarm C, work counters, cycle time, MAC MAN,etc,, and GOTO's should NOT be used to loop a program endlessly. You'll get yourself into trouble easily by doing a GOTO. Use it only to skip sections of code but never to loop a program.
Best regards,
I tried M677 and M678, it does not exist on the controller. As you said, using GOTO to loop the program will be a problem. I only use SDF. Best regards.Quote:
Originally Posted by OkumaWiz
hello :) i use goto's to loop programs all the time :
... tool life : i manage tool life in my own way, being able to estimate time left before begining a cut, counting cutting time also during restarted programs that are being reseted after a few operations, and there are other things as well
... work counters, cycle time, mac man : i have an alternative for all these, and i really don't relly on cnc counter, because it does not know if a program was re-started, or simply started again; even when the cycle time is short, like <30seconds eq, i may use a different method to count parts; cycle time, again, is relative, i don't wanna know the cycle time, but the randament of the process
is not a must to avoid looping a program by using goto's; if sdf is used, then will be needed to create the sdf file ( which means an extra file with extra content ) : this means downtime; also, it will be needed to pay attention to "program select" interface, or " schedule select ", thus one has to be carefull to avoid the wrong selection mode
if a program is looped by using a sdf, and the process is restarted, then the counter will reset to 0; if the program is looped by goto's, and the process is restarted, then the counter value is saved if common variables are used
so far, i have not seen a case where i would really need a *sdf file instead of *min file; kindly :)
What are you trying to accomplish by turning this off and on in the program? Perhaps a better explanation may bring up another way to accomplish what you want.
Most either want to monitor the cycle time or the stm time to make sure their machine hasn’t stalled. Turning it off in the cycle defeats the purpose.
Are your guys turning it off when you don’t want them to?
I’m assuming you get unusable m code when you tried M677/8?
We produce a lot of details, you will understand how important the Cycle time is. However, operators regularly adjust Feedrate override and Rapid override on panels to control even edit Feedrate on my program. They want to increase Cycle time with bad intentions. I'm still struggling to try to stop that. I only manage the program and do not advise me to lock the control panel or program, or find and handle him. That is impossible for me. Best regards.Quote:
Originally Posted by OkumaWiz
hy duongcave, M's listed below should allow to ignore overrides during auto-mode; if M160/161 works only for feed, and not also for rapids, then replace rapids with feeds inside the programQuote:
However, operators regularly adjust Feedrate override and Rapid override on panels
M48, M49 (spindle speed override ignore)
When the spindle speed override ignore function is valid, the spindle speed override rate is
fixed at 100% regardless of the setting of the spindle override switch. The spindle speed
override ignore function is canceled by specifying the cancel M code, resetting the CNC, or
changing the operation mode.
< M codes >
Spindle speed override ignore••••••••••••••� �••••••••••••••M49
Spindle speed override ignore cancel••••••••••••••� �•••••M48
M160, M161 (feed rate override fixed at 100% OFF, ON)
These M codes are used to specify whether or not the setting of the feed rate override dial,
when other than 100%, is valid; in the M161 mode, if the setting of the feed rate override dial on
the machine operation panel is in other than 100%, the setting is ignored and the feed rate
commands are executed assuming a setting of 100%, and in the M160 mode, the setting of the
feed rate override dial is valid.
M162, M163 (rotary tool spindle override fixed at 100% OFF, ON)
These M codes are used to specify whether or not the setting of the rotary tool spindle speed
override dial, when other than 100%, is valid; in the M163 mode, if the setting of the rotary tool
spindle speed override dial on the machine operation panel is in other than 100%, the setting is
ignored and the rotary tool spindle speed commands are executed assuming the setting of
100%, and in the M162 mode, the setting of the rotary tool spindle speed override dial is valid.
so far, i can't help you with simple methods for protecting the file ... this was allready discussed in another thread / kindly :)Quote:
even edit Feedrate
ps : another method to ignore feed override, is to replace G01 with a threding code ...
i just had an idea : in that thread, we discussed possible protection methods while the file is in MD1, but what if the file is not in MD1 ? for example, put the file on an usb with edit protection, and use sdf to select the file from the usbQuote:
even edit Feedrate
i don't know how to create such an edit-lock usb, and i am not sure if sdf can select from usb, but i would try this / kindly :)
Another idea is that all of your switches on the control panel can be checked out from within the program. This means that you can check the feed rate override and generate an alarm if you’d like. Let me know if you want me to send you the codes to do this.
Best regards,