Tool length comp missing

[Greg_J]

I have a new machine and use tool length compensation, when I post it's not there. Where would I look to enable it in MC or in the post?

 

# Post Name           : MPMASTER
# Product             : MILL
# Machine Name        : MACHINE
# Control Name        : xxxxOR 8050/8055 M CNC
# Description         : IHS MASTER GENERIC MILL G-CODE POST
# 4-axis/Axis subs.   : YES
# 5-axis              : NO
# Subprograms         : YES
# Executable          : MP v11.0
# Post Revision       : 11.0.06347 (MC_FULL.MC_MINOR.YYDDD)

 

 

I would dig into the post and look for it I just don't have the time if one of you guys could send me in the right direction it would be a big help.

TIA,

 

Greg

[Greg_J]

What part of a post generates tool length, it must be missing from my post.

[Zoober]

That is usually in the ptlchg or ptlchg_common (I think, not at pc) Post blocks. Search for *speed or m6. That will get you near the tool change blocks.

[DavidB]

If your using MPMASTER down load it again.

 

Maybe your post has been editted for controllers 8050/8055 M CNC ?

 

The standard MPMASTER will output a G43

 

# Post Name    : MPMASTER
# Product             : MILL
# Machine Name        : MACHINE
# Control Name        : CONTROL
# Description         : IHS MASTER GENERIC MILL G-CODE POST
# 4-axis/Axis subs.   : YES
# 5-axis              : NO
# Subprograms         : YES
# Executable          : MP v11.0
# Post Revision       : 11.2.07337 (MC_FULL.MC_MINOR.YYDDD

 

phsm1_on #must remain before G43

pbld, n$, "G43", *tlngno$, pfzout, scoolant, next_tool$, e$

[Greg_J]

Another question I had is if I want to change notes in the program from having brackets to semi colon how where would I look.

 

I've been using the generic fanuc 4 axis post to get around the issue with the tool length.

[DavidB]

slbracket : "("
srbracket : ")"
sslash    : "/"
ssemicolon : ";"

[gcode]

are you getting G43 H0 ??

 

or is the whole line not being output

 

You might what to check the Tools page on the control def

There are settings there that affect tool length output

[Greg_J]

Here’s a bit of code from the post.

 

;OVERALL MAX - Z8.

;OVERALL MIN - Z6.05

N100 G00 G17 G70 G40 G80 G90

N110 T22 M06 ;.203 CARBIDE DRILLchange this line

N120 ;MAX - Z8.

N130 ;MIN - Z6.05

N220 M07

N230 G00 G90 X2.9375 Y0. A90. S4700 M03

N240 G43 D22 Z8 take this out

 

And this is what I need it to look like.

 

N116 ;OVERALL MAX - Z8.

N118 ;OVERALL MIN - Z6.05

N120 G00 G17 G70 G40 G80 G90

N122 T22 D22

N124 M06 ;.203 CARBIDE DRILL

N126 ;MAX - Z8.

N128 ;MIN - Z6.05

 

From what I can tell this machine doesn’t use G43 in the way we use it on a fanuc, when the tool is called there is a D(tool number) after it and that turns on the tool length offset.

 

So I need the D right after the tool call and M06 on the next line and I need G43 line removed.

[MIL-TFP-41]

Is it a Siemens control?

[Greg_J]

xxxxOR 8855 Mill <----rofl fail

 

F.A.G.O.R 8855 Mill

[gcode]

I'm going to move this to the post forum..

You might have better luck there

[Chris McIntosh]

Look in the ptlchg_com post block.

 

Should be a section of code that looks like this:

 

     if stagetool >= zero,
       [
       if omitseq$ = 1 & tseqno > 0,
         [
         if tseqno = 2, n$ = t$
         pbld, *n$, *t$, "M06", ptoolcomm, e$
         ]
       else, pbld, n$, *t$, "M06", ptoolcomm, e$
       ]

 

change to read this:

 

     if stagetool >= zero,
       [
       if omitseq$ = 1 & tseqno > 0,
         [
         if tseqno = 2, n$ = t$
         pbld, *n$, *t$, *tlngno$, e$
         ]
       else, pbld, n$, *t$, *tlngno$, e$
       pbld, n$, "M06", ptoolcomm, e$
       ]

 

 

then we need to remove the tool length call later in the post. Here's the original line:

 

     pbld, n$, "G43", *tlngno$, pfzout, scoolant, next_tool$, e$

 

Should be this:

 

     pbld, n$, pfzout, scoolant, next_tool$, e$

 

Depending on the version of mpmaster you have, the tool length may cancel after retracting, so look for "G49" of sg49 in the retract and retract0 post blocks and remove them if unwanted.

 

There is also a G43 Dxxx call in the ptlchg0$ post block. If you need to recall the tool length here, position the tlngno$ where you would like the output, otherwise delete the G43, *tlngno$ from this post block

[Rodent]

I originally posted this on Mastercams facebook page, and another user suggested I try it here:

 

If I call up say, an endmill with a D value, then a drill, then the same endmill again, I notice the D value is not posted the second time. Worse is if I use the "force tool change" checkbox. For instance if I want to go to a safe position, (the tool change location) move some clamps out of the way and go back to milling, both the H and the D are then missing. We have one machine with a 8" ring in the table about a half inch deep from a missing H value on a 8" facemill. Is there any way to fix this issue?

[Chris McIntosh]

Is this on the same post? I thought the 8055 only took a D value, no H. If you don't mind some redundancy in your code you can search for any tloffno$ or tlngno$ variable and put a * in front of it to force it out every time. Make sure the variables are in lines that aren't commented out in the ptlchg_com post block and you shouldn't have these issues. if you are using H for length and D for diameter offset, then the tloffno$ should be located in the pccdia post block. Stuff a * in front of the tloffno$ to force the D value to output every time cutter comp is applied.

[Rodent]

I kind of hijacked this thread I guess. Greg J had the same type of problem, so I figured it would be a good place to look for an answer.

I do have a post that generates a D every time theres a G41. The generic Haas post, its ok when you program the correct tool number, but if you need to make a change at the machine then its a whole "change all "D5" to "D7" or whatener. Not hard, but kind of annoying. At least now I know how to stop that post from doing that. Ideally I would like my Kuraki post to just posted a D and H everytime it picks up a tool, new or previously used in the program.