OKK Fanuc10M help

[killall-9]

Hello i have the MPMASTER post file for X4. Code is good but there are minor changes i need to make.

 

1. T6M06 will not work, the M06 needs to be on a separate line

 

2. I need to orient the spindle before a tool change (M19)

 

I dont see an option to do this in machinetool definitions.

 

Can someone guide me ?

 

Current sample:

 

N70 G00 Z2.

N75 M05

N80 G91 G28 Z0.

N85 M01

N90 T2 M06 (NO.3 CENTER DRILL)

N95 (MAX - Z2.)

N100 (MIN - Z.13)

N105 G00 G17 G90 G54.1 P49 X.1601 Y.1788 S1200 M03

[Ron Branch @ 5th Axis]

Need to put up certain parts of the post and can be a task if you have never worked with posts before. I would suggest you contact your dealer they are a great asset to lean on for things of this nature.

 

Welcome to the forum.

[Chris McIntosh]

Open up the pst file (mpmaster.pst) in notepad or another text editor. Your tool change code should look like this (search for M06 in the file):

 

     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$
       ]

 

Should be changed to this (also adding in the M19):

 

     if stagetool >= zero,
       [
       pbld, n$, "M19", e$
       if omitseq$ = 1 & tseqno > 0,
         [
         if tseqno = 2, n$ = t$
         pbld, *n$, *t$, ptoolcomm, e$
         ]
       else, pbld, n$, *t$, ptoolcomm, e$
       pbld, n$, "M06", e$
       ]

[killall-9]

This worked perfect.

 

The only other problem i'm having is the post writes my G54 line incorrectly :

 

N125 G00 G17 G90 G54.1 P49 X.1601 Y.1788 S1200 M03

 

simply needs to be

 

N125 G00 G17 G90 G54 X.1601 Y.1788 S1200 M03

[crazy^millman]

No you have 54 for the offset number and not zero. The logic does not follow 54 is 54 it is zero is 54, 1 is 55 then goes from there. A lot of people changed their post to support 54 is G54. That can be done easily.

 

Look in this part of the post in MPMaster:

 

pwcs        	#G54+ coordinate setting at toolchange
 	if wcstype = two | wcstype > three,
   	[
   	sav_frc_wcs = force_wcs
   	if sub_level$ > zero, force_wcs = zero
   	if sav_mi9 = 1, workofs$ = sav_workofs
   	if workofs$ < 0, workofs$ = 0
   	if workofs$ <> prv_workofs$ | (force_wcs & toolchng) | sof,
     	[
     	if workofs$ < 6,
       	[
       	g_wcs = workofs$ + 54
       	*g_wcs
       	]
     	else,
       	[
       	if haas,
         	[
         	p_wcs = workofs$ - five    	#G154 P1 to P99
         	"G154", *p_wcs
         	#g_wcs = workofs$ + 104    	#G110 to G129
         	#*g_wcs  
         	]
       	else,
         	[
         	p_wcs = workofs$ - five
         	"G54.1", *p_wcs
         	]
       	]
     	]
   	force_wcs = sav_frc_wcs
   	!workofs$
   	]

[killall-9]

pwcs #G54

if wcstype = two | wcstype > three,

[

sav_frc_wcs = force_wcs

if sub_level$ > zero, force_wcs = zero

if sav_mi9 = 1, workofs$ = sav_workofs

if workofs$ < 0, workofs$ = 0

if workofs$ <> prv_workofs$ | (force_wcs & toolchng) | sof,

[

if workofs$ < 6,

[

g_wcs = workofs$ + 54

*g_wcs

]

else,

[

if haas,

[

p_wcs = workofs$ - five #G154 P1 to P99

"G154", *p_wcs

#g_wcs = workofs$ + 104 #G110 to G129

#*g_wcs

]

else,

[

p_wcs = workofs$ - five

"G54", *p_wcs

]

 

 

This is what i have modified. i Need to get rid of the P code as well. Where can i find this ?

[CJep]

This is what i have modified. i Need to get rid of the P code as well. Where can i find this ?

 

What Ron trying to tell you is that you have activated the auxiliary work offsets by having a value other than -1 or 0-5 associated with the toolplane in your toolpath.

 

If you activate the work offset value in the planes page of the toolpath parameters and set it to zero the work offset will be G54, 1 = G55, 2 = G56, 3 = G57, 4 = G58, 5 = G59 when you start using numbers 6 and up the post will switch to the auxiliary work offsets, that's where the P value is coming from.