MPMASTER and Haas

[motor-vater]

So I am doing war with a VF2 SS a few years old, not nextgen. Anyway when transferring the file onto the control get an alarm, Invalid Code! I have ran the program piece by piece and it works but as a whole no go. I verified the program on the control and it faults out saying I have a different tool and tool height somewhere. I'm thinking that is the precalls cause it is all corect when manually verifying the code. So I'm sure that is not the invalid code. How in the heck do I locate where this is going bad. Why cant the control give you a dam line number. WTF. I ask because I know I am not the first to deal with these issues. If I had to guess I would think its in the optirough program cause I cant get past that in the verify, but if I post the optirough by itself it runs perfect.... I already weeded out the M29 in the tap cycle by isolating programs and just running them but that was the only thing that stopped the machine. Everything runs fine alone but again when combined bam INVALID CODE.... Could it be in all the notes at the top?

 

[Robert Ouellette]

do a manual search for all your "H" values. one of them is not the same as your "T" number. might be at the beginning right after tools change. or some where in middle if there are multiple ops with same tool. Sometimes when you post out 1 op at a time it post the correct tool "H". but when you do it all together no go. Out pops an "H" not equal to your tool "T" number. When you verify in control, it will alarm out before it gets to the problem. That's because of the look ahead. So where it stops usually look after that and you will find the problem. But somewhere in your posted program you have an "H" not equal to your "T" that's supposed to be in spindle. Precalling tool will not alarm out if you have the double arm tool changer.

 

[motor-vater]

Thank you for the suggestion, I will check it again just to make sure, but I have been through it line by line. Everywhere there is a T# shortly after is a G43H(same #)... But it wouldnt be the first time I found something hiding in plain sight... lol

[gcode]

Is the post staging the next tool

That might cause this problem

 

And

It's been 17 years since  ran a Haas, but the ones I ran had a parameter to control

this safety feature. 

Flip through the parameter section of your manual

I'm sure there is a setting to turn this off

 

[motor-vater]

So went back through it, and all T values Match their H Values. I also went a head and removed the precalls for now. I Have a section in the middle of the program that optiroughs, rest roughs and has 2 contours, they all use the same tool, and in between programs it has a the comment from the tool selection page in parenthesis but never has a tool or height call out after the first one which makes seance, its all the same tool. So I Will try to feed it back into the machine tomorrow and see what I am up against. Also after doing some searching online seems a double parenthesis has been known to trigger the invalid code alarm. Low and behold I found one of them (See Pic) so Ill remove that too... Still open for suggestions, but I'll give this a go and see where it takes me next.

 

[nickbe10]

8 hours ago, motor-vater said:

Also after doing some searching online seems a double parenthesis has been known to trigger the invalid code alarm.

Been caught by this one a few times. my money is here.....

[geirsj]

3 hours ago, nickbe10 said:

Been caught by this one a few times. my money is here.....

Mine too, Fanuc control does not like double pharentesis either!

[motor-vater]

yup double parenthesis it was.. Even the bad tool height was because of the same double parenthesis lower in the code... Amazing how the most simple things can drive you insane... I love machining...

[Colin Gilchrist]

Which Post are you using Motor-vater? It would be pretty easy to "scan" each comment string, and look for extra parenthesis characters, and either warn you, or remove/change the characters automatically.

The "Generic Haas 4X Mill Post" from CNC Software, already has some special "comment processing" logic, that can be used to limit the length of each Comment String to 80 characters or less. It does this by passing every single comment string to a "common comment variable", for processing. It would be really easy to use the 'strstr' function to scan the string, and fire off a warning, or just replace the characters (perhaps with a "$")?

[Thongphamckm1978]

On 3/29/2018 at 10:29 AM, motor-vater said:

So went back through it, and all T values Match their H Values. I also went a head and removed the precalls for now. I Have a section in the middle of the program that optiroughs, rest roughs and has 2 contours, they all use the same tool, and in between programs it has a the comment from the tool selection page in parenthesis but never has a tool or height call out after the first one which makes seance, its all the same tool. So I Will try to feed it back into the machine tomorrow and see what I am up against. Also after doing some searching online seems a double parenthesis has been known to trigger the invalid code alarm. Low and behold I found one of them (See Pic) so Ill remove that too... Still open for suggestions, but I'll give this a go and see where it takes me next.

 

My machine had Moriseiki MV40 Fanuc OMC control , I need edit post with mcode line : T.... ; M06 . Can we help me edit post ( i use mpmaster.pst) . Thanks all .

Sample tool change using T + M06

N10 T12 ( Select Tool #12 )

N20 M06 ( Change to selected tool )