Kitamura Mycenter H400 - Spindle stops at M00/M01, parameter?

We just got a '98 Kitamura H400 with 15m control. We are still getting it set up (took sheet metal off, new air and lube lines, etc). Still doing some minor work on it but I am almost ready to put it to work.

Anyway, we have a '93 Mycenter 3 already that has a problem for us: when you have a M0 in the program (or M1 with optional stop on) the spindle shuts off and doesn't turn back on afterward. we never did find a diagnostic parameter to change on the mycenter 3.


Anyway, I just tried it on the new H400, and it does the same thing. The spindle turns off when the machine stops, and it doesn't turn back on.

I can work around that if necessary, but I hate it. None of the other machines behave like that (Leadwell, Makino, robodrill), only the kitamura does.

So the question is, does this thing have a parameter or keep relay that changes this? I have the ladder and manual, I did browse through it and did not see anything of the sort. I really hope it has a setting I can change for that. Seems like a popular machine for the era, there's a bunch of them out there, so somebody ought to know if I can fix this?

Thanks

I believe this is something I found on the settings page. Peck around in there and see if you see something spindle off at M1. I'm pretty sure that is where I saw something like this on the newer i control. Give me a few and when I get in I'll see if I can find it?

Brent

OK well I lied to you! Look down through your keep relay list. My K3.4 = 0 because I turn on the spindle manually in the program each time after the M1 & M0's.

It most likely would be a different keep relay on your machine that is if even your MTB handled this in this way. My builder handled this with a keep relay it may not be the same on your machine but this may give you a place to start looking? Thats all the help I have.

Good luck!

Brent

Thanks. I don't think it is in the keep relays (I at least don't have a really clear listing like your machine has). But I do notice that the machine is a '98, the keep relay list is from 1995, and there were a few things penciled in (by kitamura?) adding keep relays related to the pallet changer. I wonder if it is possible that some of the unlisted bits might be related to spindle stopping?



on the image I just posted, if you right click -> view image, then click on it, it should show up full size (readable)

Yeah Dan I'm not seeing anything on your list. That's where I found this setting, in the keep relays. Curious if when looking at the relay screen at the control does it appear that more relays are being used then what you have on your list?

I suppose this could be something you won't be able to change? Or possibly a setting or keep that not listed? Could be information just a service tech would have. If you can't find a up to date list that your sure is for this machine that has any more information on it then I'd try calling the company and see if they can point you in the right direction? My gut tells me this could be changed but you may just have to deal with it.

Maybe someone will show up and be more helpful then me? Sorry!

Brent

I don't think that I have ever had a machine keep the spindle turning under M1/ M0 command.

What odd application would you have that you want it this way?


The rest of y'all have spindles that keep turning under M1/M0?

the spindle shuts off and doesn't turn back on afterward

Click to expand...

Is it simply that you are having troubles with it restarting, rather than you wanting it to keep turning?

If you program an M3 S after the M0/M1 it still won't start?
Preferably - I would add in your header info at that spot anyway as that is a logical place to restart anyway....

I habitually program like this in all apps. Most need it, some don't. With the code in place - they all werk.



edit:

I ass_u_me this to be a ladder issue.
Not likely easilly edited.




-----------------------

Think Snow Eh!
Ox

The spindle does stop at M1 & M0. But resumes rotation instantly with the next push the green button without having to call the S×××× M?

At least that is what mine did before I changed it, assuming that's what he looking to do?

Brent

Ox said:

I don't think that I have ever had a machine keep the spindle turning under M1/ M0 command.

What odd application would you have that you want it this way?


The rest of y'all have spindles that keep turning under M1/M0?




Is it simply that you are having troubles with it restarting, rather than you wanting it to keep turning?

If you program an M3 S after the M0/M1 it still won't start?
Preferably - I would add in your header info at that spot anyway as that is a logical place to restart anyway....

I habitually program like this in all apps. Most need it, some don't. With the code in place - they all werk.



edit:

I ass_u_me this to be a ladder issue.
Not likely easilly edited.




-----------------------

Think Snow Eh!
Ox

Click to expand...

To clarify, I want the spindle to resume after M0/M1. I don't care if it stays on or turns off, as long as it turns on afterward. We have half a dozen leadwells (mid 90's with 0m controls), a Makino a88 (2000, 16i), and a '97 robodrill with 16i that all resume spindle after M0/M1 (Actually the leadwells do not turn the spindle off, only the coolant)

But both Kitamuras turn the spindle off and don't resume.


This isn't a horrible situation when gibbscam spits out an M1 at the end of every operation, then it throws in an M3 when it goes to the next operation. However, when I, or one of my guys, decide we want to add M0 somewhere to check something before the program continues, and forget that this machine behaves different than the machines we are used to and doesn't turn the spindle on, crashes happen.

I am afraid it is a ladder issue. I struggled with this on the mycenter 3 and thats the conclusion I came to, although not 100% certain.

dandrummerman21 said:

.....I am afraid it is a ladder issue. I struggled with this on the mycenter 3 and thats the conclusion I came to, although not 100% certain.

Click to expand...

You are correct. What happens in regards to spindle operation, coolant, positioning, etc., at M0 or M1 is totally dictated by the the machine builders ladder, or in the case of Makino (they don't use ladder) the PMC program.

i added a M0 once between a group of holes and i wanted it to stop to put tap back in tap holder as i already tapped previous holes and wanted to restart after where i broke a tap, got it out and hand tapped
.
long story but cycle start, spindle not turning it goes into hole tapping cycle with no spindle rotation. obvious dont work too good that way. i just put M3 S200 M8 after M0 and it works ok
.
some use M0 or M1 on purpose to shut spindle off and coolant off

DMF_TomB said:

long story but cycle start, spindle not turning it goes into hole tapping cycle with no spindle rotation. obvious dont work too good that way. i just put M3 S200 M8 after M0 and it works ok

Click to expand...

That was a long story indeed.

Vancbiker said:

...or in the case of Makino (they don't use ladder) the PMC program.

Click to expand...

Say whaaaaa?



What's wrong with...


gcode gcode gcode
M01
M3 <--- You don't need to re-state an "S" word here, as it will be modal.

Jashley73 said:

What's wrong with...


gcode gcode gcode
M01
M3 <--- You don't need to re-state an "S" word here, as it will be modal.

Click to expand...

Nothin'

... Except when you are used to a certain lot of machines that behave a certain way, running them for years without this being an issue, then walk up to the new machine and do it without giving it a second thought.

I say to my self, "well at least I am aware of it, so I won't possibly make that mistake", and on the mycenter 3, that's true... except for a broken endmill a few months ago because I was in a hurry and did possibly make that mistake. On the Leadwell sitting next to it, I wouldn't have had that broken tool. Whoops.

Code generated by CAM will always have an M3 after M1, its those pesky M0's I fat finger at the control that screw me up.

Anyway, not a big deal. Was hoping for that golden parameter to make all my CNC woes disappear.


Edit: before I go, I had a magical and possibly impossible idea: Can I set M0 and M1 to a 9000 program, which has M0/M1 embedded in it with a spindle command afterward? I know I've seen M06 macro programs that have M06 in them. Something like:

09000(M0 PROGRAM)
M0
M3
M99
O9001(M1 PROGRAM)
M1
M3
M99


Something to that effect?

dandrummerman21 said:

Nothin'

... Except when you are used to a certain lot of machines that behave a certain way, running them for years without this being an issue, then walk up to the new machine and do it without giving it a second thought.

I say to my self, "well at least I am aware of it, so I won't possibly make that mistake", and on the mycenter 3, that's true... except for a broken endmill a few months ago because I was in a hurry and did possibly make that mistake. On the Leadwell sitting next to it, I wouldn't have had that broken tool. Whoops.

Code generated by CAM will always have an M3 after M1, its those pesky M0's I fat finger at the control that screw me up.

Anyway, not a big deal. Was hoping for that golden parameter to make all my CNC woes disappear.


Edit: before I go, I had a magical and possibly impossible idea: Can I set M0 and M1 to a 9000 program, which has M0/M1 embedded in it with a spindle command afterward? I know I've seen M06 macro programs that have M06 in them. Something like:

09000(M0 PROGRAM)
M0
M3
M99
O9001(M1 PROGRAM)
M1
M3
M99


Something to that effect?

Click to expand...

SHHhhhhhhh. Don't let everyone know that I use M codes in my main programs so I don't have to put in the damn start and end safety lines of every program. It is even a zero return program in some instances and a turn spindle/coolant etc etc off and M0 in others. On my machines my warm up programs are also called by M15 so that the operator can run the warmup in MDI and not screw up the parts counter on the control.

Your program numbers are assigned to certain M codes. If your control is similar to mine then ( and this is off the top of my head here without a manual in front of me so please check for errors)

Parameters #6071 - #6079 are the parameters that you input the M code that you want to call programs O9001 to O9009. So if 6071 is set to 15 then a M15 in your program will call up program O9001. Make sure that there are not any digits in those parameters already because M codes could be used by the machine to call up certain programs. I chose M15 but also use M100 M10 M55 and so on that are not generic M codes. I think you have to have macro unlocked on your control to do this.

So in your program you would just put a M15 (or whatever you assign) and it will call program O9001 if parameter 6071 is set to 15. You need editing of 9000 programs also to be unlocked in your parameters for you to input your program.

I also know that you can call more 9000 programs further down the parameters (6080 jumps to O9021 or something like that??). I am sure others will correct me or chime in here, I usually have the manual in front of me when I set an M code to call a program.

On edit: I did a bit of thinking on it and I think that 6071-6079 call sub programs and that is why I stuck with them because of the loop back to your main program. Not sure if the others (6080 and so on) call subs or main programs that don't loop back.