[varrtrix]

Hello

I have a fanuc robodrill alpha T21 with control fanuc 31i-A5. I want the control to be able to read 2 M-codes (M03 M08) in the same line. I have followed the instructions shown in the manual, but it doesn´t work. Any suggestion will be accepted.

[txcncman]

Won't work. Can't put 2 M-codes on a line in Fanuc. Look up M13 instead. Might work on a lathe. Works on mills.

[fordav11]

there's really no need to do that anyway. Put M8 first if you want the coolant on a bit earlier then M3 after on the next line.
One of the hard rules of programming on Fanuc controls is only 1 M-code is allowed per line. No exceptions.

[sinha_nsit]

From 0i parameter manual

Parameter 3404#7 (M3B) = 0 : only one M-code in a block is permitted
=1 : up to three permitted

[gwiz]

Newer controls can handle more than 1 M code at a time. BUT the machine tool manufacture's ladder must also handle it. M-codes are generally operated by the PMC(ladder) and designed by the MTB. Contact the manufacture to see if it is available. My guess if it was not turned on then it is not supported and you should leave it off to head of any other issues with it.
Regards,

[varrtrix]

Hi, sure that´s what manual say. I have tried several times, but it doesn´t work. The tool just hold in that line. Maybe other parameter may be related.

From 0i parameter manual

Parameter 3404#7 (M3B) = 0 : only one M-code in a block is permitted
=1 : up to three permitted

[stevo1]

It sounds like it is a MTB issue that is not going to allow these 2 particular M-codes to be in the same line. You are programming the S() along with the M3 in the same line correct?

Sinha is correct there are parameter settings to allow more then 1 M-code in the same line. It is really only some of the older Fanuc models that may have some limitations on this. I program many M-codes in the same line all the time so you should not have any issues especially on a 31i control unless the ladder does not allow it.

Have you tried switching the order of the M-codes in the block.
M3S()M8
M8M3S()

I guess on the other hand I never really tried any other M-codes with the M3.....just G-codes. You may just be SOL and have to program the M8 after or before.

Stevo

[varrtrix]

hi, the postprocessor i want to use has those settings: m03 m08 Sxxxx. Weird thing is that i have coleagues in romania, they use same control and have no trouble using those settings. For know i use a modified postprocessor, but will be out of date soon. So i need to find a solution. Sorry but i don't know what is mtb? Motherboard? Thanks for your help.

It sounds like it is a MTB issue that is not going to allow these 2 particular M-codes to be in the same line. You are programming the S() along with the M3 in the same line correct?

Sinha is correct there are parameter settings to allow more then 1 M-code in the same line. It is really only some of the older Fanuc models that may have some limitations on this. I program many M-codes in the same line all the time so you should not have any issues especially on a 31i control unless the ladder does not allow it.

Have you tried switching the order of the M-codes in the block.
M3S()M8
M8M3S()

I guess on the other hand I never really tried any other M-codes with the M3.....just G-codes. You may just be SOL and have to program the M8 after or before.

Stevo

[hanzlaser]

read, than you!

If any requirements about laser equipment, please feel free to contact me!

[stevo1]

MTB stands for Machine Tool Builder. Just because you have the same model control does not mean that the ladder written by the MTB processes the M-codes in the same manner. Did you try different orders of the M-codes in the same block as I suggested?

Stevo

[drdos]

In accordance with the 31i CONNECTION MANUAL (FUNCTION) you must "FIN" out the three M-Codes separately within the PMC (Ladder logic). Standard M-Codes use MF to FIN the M-Code. When using multiple M Codes you also must FIN out MF2 and MF3 in case of 2 or 3 M-Codes in the same block. Bottom line, you need to contact the machine manufacturer and ask if your machine can handle the multiple M-Codes. If not,what can be done to make that happen.

[varrtrix]

hello

I tried with different order M3 S() M8= the tool just gets in stand by
M8 S() M3= The coolant turns on and the tool gets in stand by

I tried to simulate the nc code in graphic mode with the order M3 M8 S() and the simulatation goes fine. No message of error showed up

MTB stands for Machine Tool Builder. Just because you have the same model control does not mean that the ladder written by the MTB processes the M-codes in the same manner. Did you try different orders of the M-codes in the same block as I suggested?

Stevo

[stevo1]

My best guess would be then that the ladder does not support these 2 codes in the same line.

Stevo

[barbter]

Yep, Stevo - bang on.
It is 100% a ladder issue with the robi. Ours is the same.
And as said earlier, if you have 2 (or 3) M Codes in a row, the robi will process the 1st only.
You have to have your Sxxx and then on the next line the M8.
Mod your post and all will be well.
HTH

[varrtrix]

Hello

Our fanuc dealer found the solution to this issue. The problem was the settings of keep relay #5, I changed it to 0 and finally it worked. That keep relay means "coolant trought tool" or something like that. I don´t undestand the relation between reading 2 Mcodes in the same line and that keep relay. But it was the solution

Thanks for your advices, Best regards