M198 on Fanuc 18i-MA

[Milling man]

Hello! Sorry for my English. I am writing through a translator.
We have a Mazak FF-660 machine with CNC Fanuc 18i-MA. The machine was made in 2001. The CNC has 64kB of built-in memory ..... I cannot convey in words how it saddens me, especially after 10 years of working on a Delta-Tau machine with a hard drive of at least a terabyte.
But we need to work, not be sad, so I decided to do everything to make it convenient for my technologists to work - a DNS terminal, increase the rack memory and run programs from a memory card. The DNS terminal is now coming to us, there are certain problems with the memory and I am trying to run the program from a 256MB Compact Flash memory card via the M198 code. I must say right away that I managed to send programs from the CNC to this memory card without any problems, as well as make backups of parameters and everything like that. Also, programs are sent from the memory card to the CNC, absolutely no problem.
I created a program in the memory of the machine:
O0002
M198 P0001
M30

I have verified that there is no program named O0001 in the machine memory.

And I put one program on the memory stick. I removed the extension from the file. The file is named O0001.
%
O0001;
G01 X10. F100.;
M99;
%

I checked all the related parameters, tried changing them one by one.
“I/O Channel” to “4”
0.0 = 0
138.7 = 1
3404.2 = 1 or 0
6030 = 0 or 198
The option "Macro B" is on for me, the option "Macro A" is off.

When this program is executed, nothing happens! I have tried all the options for recording the command:
M198 P0001 L0001
M198 P00010001
At the same time, I see on the screen that the system has read the argument L0001. If I write simply M198, the program is also executed in a split second, without any errors. If you remove the memory card from the CNC, everything will be the same, no errors.
I’m already in utter despair, I don’t know what to try

 

[dandrummerman21]

And I put one program on the memory stick. I removed the extension from the file. The file is named O0001.
%
O0001
G01 X10. Form 100.
M99%

Make sure there is an end of block ( ";" ) character after M99 (in your text editor, start a new line, so the % is on the next line after m99)

Also What does "form 100" refer to? I've never seen that.

Also just to make sure it isn't something dumb, such as the machine being in absolute mode and already being at X10., change your program to something like this and run it in single block:


%
O0001

G91G1X10.F100.

M0

M99
%

The reason for G91 is to make sure it moves incrementally, JUST IN CASE you're already sitting pretty at x10. ALSO make sure you have your feedrate not set to 0% override lol



Also since you've messed with those parameters, make sure they are set back to what they should be. From another post, I see it should be:

138 bit 7 is 1
I/O channel is 4
3404 Bit 2 is 1
3030 equals 3
6030 set to 198

I use M198 often on a 16ima control.

 

[Milling man]

dandrummerman21
Looks like I was in a hurry and just wrote the program wrong.. Corrected the first message.
Of course, the program looks like this:

%
O0001;
G01 X10. F100.;
M99;
%

The machine is not exactly located in these coordinates, I checked. In addition, I have previously used our part work program as a program. The parameters were in the same meaning as you wrote. 6030 = 198 is the same as 6030 = 0, according to the documentation. But I tried both 198 and 0.
I already have a suspicion that my CNC has old software, or something like that. And I can't run this damn routine, no matter what I do. And I have to wrap with a PC-232 cable and drip programs into the CNC from an old laptop.

 

[Milling man]

I use M198 often on a 16ima control.

I have a question, the answer to which seems to be obvious. When you start the program with the M198 code, in which position is the mode switch - MEM or TAPE?
I run the program only in MEM mode, in TAPE mode I cannot run the program from the CNC memory.

 

[Ox]

[tangent]

A late model Yamazaki with a Fanuc?

I had to look that up!

Several hits for that machine, and all seem to have a Fanuc controller.

Also interesting that it has a 3 pallet system.
Only time I seen one like that was one Mori.
Never seen another, and that one wasn't near this big.
That was prolly a 300 machine?

I wonder why they put Fanuc on that machine?
Did they sell that model State Side?
All hits that I noticed were not in the America's.


[/tangent]



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

http://[/B Rose in Paradise
Ox

 

[Milling man]

[tangent]

A late model Yamazaki with a Fanuc?
Ox

Yes, as far as I know. I thank the Universe that they no longer use Fanuc in their machines.
A colleague of mine told me that Fanuc has come in with a series of super fast (FF-550 and FF-660 have a rapid speed of 90 meters per minute, or 288 feet per minute) drives with an optical task. And these drives worked, of course, only with Fanuc CNC's. That is why Mazak installed them on this top series of machines (FF-550 and FF-660).
But I must say that I have only seen 2 pallets on these machines.
I am very pleased with this purchase so far, we bought it for a very low price. Even if I cannot run the program from the memory card in any way, I will still be satisfied.

 

[memoryman]

The control needs BDF2 software to dnc from the memorycard, and also to expand the memory to 2Mbytes. We can supply both: tulipmemory.com

 

[Milling man]

The control needs BDF2 software to dnc from the memorycard, and also to expand the memory to 2Mbytes. We can supply both: tulipmemory.com

Do I also need additional software for the M198 to work?

 

[memoryman]

I can't be sure of that, but it seems to be a standard OPTION.
Send me a PM and I'll tell you which option bit.

 

[Milling man]

I will write my adventures here in case someone has the same problem.
The problem has not been resolved yet. Software version on my CNC - BDFA.

 

[Milling man]

I continue the story of my adventures.
Yesterday we tried to carry out a drip feed of the program to the rack through the RC-232. Everything worked out without any problems. This will allow us to somehow work for now. Several very helpful people gave me a hint about the process of replacing CNC software. It turned out to be not difficult. Now I am in search of this software, BDF2. A small bonus - now I can make a really FULL backup of the system in case of some big incident.

 

[memoryman]

If you are A.Cherkasov, my emails are rejected by your email server.
We do not charge for the software or instructions; to make a complete backup you need to have a pcmcia sram card (minimum 512k, but 4 Mbyte is best). Do you have the maintenance manual GFZ-63005? Its in appendix C.

 

[Milling man]

Hello. Thanks so much for writing here. I thought that you were just busy with work and I was waiting for an answer
I was able to load all files from the boot menu from the machine. I wrote to you from google mail, I think there should be no problems with it.

 

[Milling man]

Hello everyone. Thanks to the help of one kind person who gave me new software, my problem was solved! Now the program is started both with the M198 code and in the TAPE mode.

 

[Milling man]

Glad it is sorted and sorry for being late.

For reference, my notes for this era control (16/18/21 is:-

Parameter Settings: #138.7 = 1

DNC operation with memory card is:
0 = disabled
1 = enabled
#3404.2 = 1

Address P in M98 block of subprogram call function is:
0 = indicating a file number
1 = indicating a program number
#6300.4 = 1

External program number search
0 = disabled
1 = enabled
#6080 = 0

I/O Settings:
Channel = 4

ATA Card:
File name on card must match program number, DO NOT use filename extension. (.txt)
Example:
card filename - O0001
program number - O0001

Use % at beginning and end of program file.

Program Call:
Create program in NC memory:

%
O0001
M198P2 (calls O0002 on ATA card)
M30
%

I have tried, probably, all of these points. All parameters, command options and the like. For more than a week I stood and poked at the keyboard of the machine an infinite number of times ...