Mazak fusion control error 228

[mcpgmr]

I'm getting an error code 228 Ilegal M Code. There is no M code anywhere near the line of code where the machine stops. All m codes being used are the standard coolant, spindle and optional stop. Any ideas?

[Rick Henrickson The Boeing Co.]

What machine is this on, you may need to look several lines ahead or run it in single block to get the exact line.

[mcpgmr]

Mazak pc fusion 640 control on a VTC 20 mill. I looked ahead and no m codes. I ran it in single block and it stops on a g01 line where it's roughing an open pocket. The very next m is in a comment way down 50 or 60 lines of code. This does not make sense at all.

[Rick Henrickson The Boeing Co.]

can you email me the code? are you running a sub? is this a brand new machine to you?

[mcpgmr]

Brand new machine to me. The guys on the floor know the machine well but this is the first time they are running my code. I'll send it to you. Thanks!

[mcpgmr]

Well we got it fixed. Seems Mazak didn't like where the M05's were. We stripped them all out and problem solved. Now to change the post. Thanks for taking a look Rick!

[Ocean Lacky™]

Where were they?

[Rick Henrickson The Boeing Co.]

at the end of path

 

G00 Z2.0

M09

M05

G91G28Z0.

M01

 

I think it was because machine was still moving but it shouldn't matter spindle can be off during rapid unless they have a parameter set.

 

Another you do not need and H value after the G43 line the control assumes tool in spindle is the active length offset

[Joe788]

Rick, depending on how his parameters are set, that H can still be important. I have all of mine setup to use the actual tool length stored in the Mazatrol Tool Data, and then the wear lengths from the EIA Tool Offset page. In my opinion, it's the best all around setup because you use different H codes for different features if you've got some really touchy parts.

 

So if I'm using tool 86, and I call H295, it will use the correct length for tool 86, but then it will add whatever wear value is in 295 in the EIA Tool Data page.

 

I'm surprised he was getting that error with the M05 on it's own line like that. Usually that only happens if you've got conflicting M codes on the same line, like M05 and M19, or M03 and M05. I know my Fusion and Matrix controls don't like having two coolant calls on the same line.

[Psychomill]

M5 right before the move may not work but this will:

 

G91G28Z0.M5

or

G91G28Z0.

M5

 

Be careful about removing or not using the H after G43... it depends on how the machine parameters are set and where the offsets are being read from. If not set right, you can crash it like you would on a FANUC with no H. Check to be sure the machine is set OK to run without an H.

 

quote:

---

I know my Fusion and Matrix controls don't like having two coolant calls on the same line.

---

Why not? I do it all the time... even 3 of them...

[Ocean Lacky™]

Rick,

Mine are at the end of the path, exactly as you posted.....no issues here. Mazak VTC300C/640m Fusion control

[Rick Henrickson The Boeing Co.]

Lacky I am sure it is a parameter setting I just don't have the books here.

 

Concerning parameters

 

Joe788 you are correct many people like to use multiple offsets for one tool so it wouldn't be best to use sctive tool length only.

 

Another death parameter is the return through home position and I can't remember the other one but when you cancel length comp the Z axis moves to the location without comp and crashes

[Joe788]

quote:

---

I know my Fusion and Matrix controls don't like having two coolant calls on the same line.

 

Why not? I do it all the time... even 3 of them...

---

Really? Mine poop when there's and M131 on the same line as an M8. Although, now that I think about it, it could be angry because the M131 is on the same line as the G43, and the M131 calls a macro to start the 1000psi coolant. I'll have to try putting them on a line together without the G43.

[Psychomill]

M131 is a PLC macro so it should have no bearing. You should be able to do this:

 

G43H...Z...M8M131M130

[Joe788]

Just went out and tried it, and it's definitely the macro that's tripping things up. M131 takes me to 9900 to start the Superflow.

 

It works fine with M130 and M8 on the G43 line, but it trips up with M131, gets alarm: 043 DESIGNATED SNo. NOT FOUND

[Psychomill]

You're right, if your machine is set up like that, it will do that. You'll have to have the M131 on a different line. If you wired the M131 as a M code, you can get around that. Or, if you did not get the pressure switch option, it would be wired only. It's looking at a couple of "R" outputs.

 

I remember now too, I have a couple switches my eMachines are looking at so I had to split off the M131 as well...

 

The DEATH parameter Rick is talking about... F114.1

[mcpgmr]

Turns out the M05 had to be just M5. I changed the post to out put M5 and left it come out in the code where it was and it works just fine now. Thanks!

[Psychomill]

What?? Getting stranger by the minute there... Should be no difference between M05 and M5 for the machine. Sure the code wasn't maybe MO5 by chance? (as in the letter O and not a zero)?

 

Glad you're fixed up though....

[iowajim62]

Rob,

quote:

---

Sure the code wasn't maybe MO5 by chance?

---

Shouldn't be posting MO5 to start with. Definitely a strange occurence tho.....

[mcpgmr]

No, It was the number 0 not the letter O. Must be a parameter setting.