Okuma MC-4VB tool change variable for active tool

[Darin]

Hello,

 

I am working on a post for a Okuma MC-4VB vertical 50 taper mill. I started with a MPmaster post. I need it to have the following code before every tool change. How do I do this in the post..

 

 

Needs to look like this..

 

(prog)

...

N2 IF [VATOL EQ 10] N4 <---------------- I need the [VATOL EQ (the current tool nuber)] N4 --------------- to post before every tool change...

N3 T10 M6

N4 S---- M3

.......

........

 

In my MC-4Vb, VATOL is the system variable for active tool. Line N2 is a conditional that will jump to N4 if the tool 10 is already there, if not, it will proceed to N3 and change the tool

 

Thanks

[Peter - Avivi CNC Solutions]

I'm not tested this, but should work.

 

Very first thing: Make a backup of your post!

 

Define a variable (in start of post) to hold actual T number for VATOL

 

# Set variable for VATOL
oku_VATOL : 0 #VATOL

 

 

Find this section in ptlchg_com postblock.

 

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 it:

("N4" will be an empty line)

 

if stagetool >= zero,
 [
    oku_VATOL = t$
 if omitseq$ = 1 & tseqno > 0,
	 [
	 if tseqno = 2, n$ = t$
        "N2 IF [VATOL EQ ", *oku_VATOL, "] N4", e$
	 pbld, *n$, *t$, "M06", ptoolcomm, e$
        "N4", e$
	 ]
 else,
        [
        "N2 IF [VATOL EQ ", *oku_VATOL, "] N4", e$
        pbld, n$, *t$, "M06", ptoolcomm, e$
        "N4", e$
        ]
 ]

 

If you need to follow the different "N" line numbers at toolchanges, thats a bit different story, but not impossible.

Let me think.... Hmm... Yes, I think you have to, beacuse it's an OKUMA... :S

...but give a try for this first.

HTH

 

Is it an older controll? OSP5000?

[systemtek]

This is what I did, I'm sure there is a better way. I would like to know what it is. I only use line numbers on the first few lines of a toolchange.

 

I created this Variable here,

 

# --------------------------------------------------------------------------

# Toolchange / NC output Variable Formats

# --------------------------------------------------------------------------

fmt 4 okuma_skip_toolnumber

 

 

I added / modified the code under this part of the post

 

#Start of file for non-zero tool number

 

spaces$=0

okuma_skip_toolnumber = t$

pbld, n$, " IF [VATOL EQ ", *okuma_skip_toolnumber,"] ",

n$ = n$ + seqinc$,

n$ = n$ + seqinc$,

*n$, " (SPINDLE TOOL CHECK)", e$

spaces$=sav_spc

n$ = n$ - seqinc$

n$ = n$ - seqinc$

pbld, n$, *t$, "M6", e$

pbld, *n$,[if nextdc$ <> 7, *speed, *spindle], pgear, strcantext, "(SPINDLE TOOL JUMP)", e$

 

 

output looks like this..

 

N1 IF [VATOL EQ 104] N3 (SPINDLE TOOL CHECK)

N2 T104 M6

N3 S1055 M3 (SPINDLE TOOL JUMP)

[Greg Williams]

There are a few ways to do this

 

spaces$=0

pbld, n$, "IF [VTLCN EQ ", *t$,"] ", *n$, " (SPINDLE TOOL CHECK)", e$

spaces$=sav_spc

n$ = n$ - seqinc$

pbld, n$, "T", *t$, ptoolcomm, e$

pbld, n$, "M6", e$

t_nt = t$

pbld, *n$, "(SPINDLE TOOL JUMP)", e$

 

or

 

http://www.emastercam.com/board/index.php?showtopic=24828&hl=g116

[Darin]

This is great guys.. Thanks

[Darin]

This is what I did, I'm sure there is a better way. I would like to know what it is. I only use line numbers on the first few lines of a toolchange.

 

I created this Variable here,

 

# --------------------------------------------------------------------------

# Toolchange / NC output Variable Formats

# --------------------------------------------------------------------------

fmt 4 okuma_skip_toolnumber

 

 

I added / modified the code under this part of the post

 

#Start of file for non-zero tool number

 

spaces$=0

okuma_skip_toolnumber = t$

pbld, n$, " IF [VATOL EQ ", *okuma_skip_toolnumber,"] ",

n$ = n$ + seqinc$,

n$ = n$ + seqinc$,

*n$, " (SPINDLE TOOL CHECK)", e$

spaces$=sav_spc

n$ = n$ - seqinc$

n$ = n$ - seqinc$

pbld, n$, *t$, "M6", e$

pbld, *n$,[if nextdc$ <> 7, *speed, *spindle], pgear, strcantext, "(SPINDLE TOOL JUMP)", e$

 

 

output looks like this..

 

N1 IF [VATOL EQ 104] N3 (SPINDLE TOOL CHECK)

N2 T104 M6

N3 S1055 M3 (SPINDLE TOOL JUMP)

 

Ok I think I might be changing it in th wrong place.. It posted out fine for the first tool but the next tool there is no M6 or anything.. Below is where I put the changes in the mpmaster post

 

 

N100 G00 G17 G20 G40 G80 G53 G90

N110 G91 G30 P2.0 Z0.

N120 IF [VATOL EQ 1] N140 (SPINDLE TOOL CHECK) <------------------- this looks great --------------->

N130 T1 M6

N140 S2800 M03 (SPINDLE TOOL JUMP)

N150 (MAX - Z4.)

N160 (MIN - Z-1.025)

N170 M08

N180 G00 G17 G90 G54 X8.665 Y.5 S2800 M03

N190 G56 H4 Z4. T12

N200 Z.2

N210 G94 G01 Z-1.025 F120.

N220 G41 D4 Y0. F80.

N230 Y-2.4375

N240 G02 X8.25 Y-2.8525 I-.415 J0.

N250 G03 X2.8525 Y-8.25 I0. J-5.3975

N260 G02 X2.4375 Y-8.665 I-.415 J0.

N270 G01 X0.

N280 G40 X-.5

N290 G00 Z2.975

N300 X8.635 Y.5

N310 Z.2

N320 G01 Z-1.025 F120.

N330 G41 D4 Y0. F80.

N340 Y-2.4375

N350 G02 X8.25 Y-2.8225 I-.385 J0.

N360 G03 X2.8225 Y-8.25 I0. J-5.4275

N370 G02 X2.4375 Y-8.635 I-.385 J0.

N380 G01 X0.

N390 G40 X-.5

N400 G00 Z4.

N410 (FINISH MILLS OUTSIDE PROFILE WITH 3/4 ENDMILL)

N420 X8.625 Y.5

N430 Z.2

N440 G01 Z-1.025 F120.

N450 G41 D4 Y0. F40.

N460 Y-2.4375

N470 G02 X8.25 Y-2.8125 I-.375 J0.

N480 G03 X2.8125 Y-8.25 I0. J-5.4375

N490 G02 X2.4375 Y-8.625 I-.375 J0.

N500 G01 X0.

N510 G40 X-.5

N520 G00 Z4.

N530 M09

N540 M05

N550 G91 G30 P2.0 Z0.

N560 M01 <------------------------ not tool change after this line --------------------------->

N570 (MAX - Z4.)

N580 (MIN - Z-1.025)

N590 M08

N600 G00 G17 G90 G54 X8.75 Y-2.5925 S550 M03

N610 G56 H12 Z4. T1 <-------------------------- There is a height offset for t12 ------------------>

N620 (ROUGH AND FINISH MILLS WITH 15 DEG TAPER E.M.)

N630 Z.2

N640 G94 G01 Z-1.025 F125.

N650 G41 D12 X8.25 F5.

N660 G03 X2.5925 Y-8.25 I0. J-5.6575

N670 G01 G40 Y-8.75

N680 G00 Z2.975

N690 X8.75 Y-2.5625

N700 Z.2

N710 G01 Z-1.025 F125.

N720 G41 D12 X8.25 F5.

N730 G03 X2.5625 Y-8.25 I0. J-5.6875

N740 G01 G40 Y-8.75

N750 G00 Z4.

 

 

This is where i changed the mpmaster post

 

ptlchg_com #Tool change common blocks

if force_output | sof,

[

result = force(ipr_type,ipr_type)

result = force(absinc$,absinc$)

result = force(plane$,plane$)

]

pcom_moveb

pcheckaxis #Check for valid rotary axis

c_mmlt$ #Multiple tool subprogram call

#ptoolcomment

if sof & scomm_sav <> snull,

[

spaces$=0 <------------------------------------------------------------ From here to ------------------------------------->

okuma_skip_toolnumber = t$

pbld, n$, " IF [VATOL EQ ", *okuma_skip_toolnumber,"] ",

n$ = n$ + seqinc$,

n$ = n$ + seqinc$,

*n$, " (SPINDLE TOOL CHECK)", e$

spaces$=sav_spc

n$ = n$ - seqinc$

n$ = n$ - seqinc$

pbld, n$, *t$, "M6", e$

pbld, *n$,[if nextdc$ <> 7, *speed, *spindle], pgear, strcantext, "(SPINDLE TOOL JUMP)", e$ <------------------------------------ Here ------------------------------>

]

spaces$=0

if output_z = yes$,

[

preadbuf5

if (opcode$ > 0 & opcode$ < 16) | opcode$ = 19,

[

n$, pspc, scomm_str, "MAX - ", *max_depth, scomm_end, e$

n$, pspc, scomm_str, "MIN - ", *min_depth, scomm_end, e$

]

]

spaces$=sav_spc

pstock

if plane$ < 0 | opcode$ = 3 | opcode$ = 16, plane$ = 0

sav_absinc = absinc$

if wcstype > one, absinc$ = zero

pindex

if safe_index,

 

 

And here

 

 

# --------------------------------------------------------------------------

# Toolchange / NC output Variable Formats

# --------------------------------------------------------------------------

fmt "T" 4 t$ #Tool No

fmt "T" 4 first_tool$ #First Tool Used

fmt "T" 4 next_tool$ #Next Tool Used

fmt "D" 4 tloffno$ #Diameter Offset No

fmt "H" 4 tlngno$ #Length Offset No

fmt "G" 4 g_wcs #WCS G address

fmt "P" 4 p_wcs #WCS P address

fmt "S" 4 speed #Spindle Speed

fmt "M" 4 gear #Gear range

fmt 4 okuma_skip_toolnumber <----------------------added this line here --------------------------->

[Bjorn Petersson AME AB]

" if sof & scomm_sav <> snull"

 

I guess sof isn't true except for the first tool.

(Start Of File)

 

Try and remove that line.