V9 post edit help

[Roger]

Can someone help me with editing the generic fanuc post for V9 Mastercam? The machine is a Mori-Seiki MV-45 mill with a Fanuc 6m control.

 

I've alredy changed it to stage the tools, what I need now is to output T5001 for tool 1, T5002 for tool 2 etc., and just M6 for the tool change. Since the tool is already in position.

 

Here is a sample program that was in the control that shows what is needed.

 

%

O1618

(1618)

(STAND PART VERTICAL HOLDING ON .840/.850 DIA WITH EAR TO RIGHT )

(2397-1T MILL .1 05/28/09 REV-ORIG)

(1/2 DIA STOP PIN ROTATE PART TO PIN FOR ALIGNMENT)

N1G90G49G94G57G40

G0T5010M5

G0X0.78Y0.4135

G43Z2.0H9

G1Z-.5F100.0

M0

G0Z2.0

G0G91G28Z0M19

G28X0Y0

M01

M06

(1/2 DIA ROUGHING ENDMILL ROUGH PROFILE )

N2G90G49G94G55G40

G0S3000M3T5011

G0X0.78Y-0.6385

G43Z2.0H10M8

G0Z0.6

G1Z-1.2F200.0

G41G1Y-0.1885D26F18.0

G1X0.4059

G2X0.0Y-0.4475I-0.4059J0.1885F22.5

G2X-0.4475Y0.0I0.0J0.4475

G2X0.0Y0.4475I0.4475J0.0

G2X0.4059Y0.1885I0.0J-0.4475

G1X0.78F18.0

G40G1Y0.6385

G0Z2.0

M9

G0G91G28Z0M19

G28X0Y0

M01

M06

(3/8 DIA ENDMILL FINISH .840/.850 DIA)

N3G90G49G94G55G40

G0S2400M3T5001

G0X0.7675Y-0.551

G43Z2.0H11M8

G0Z0.6

G1Z-1.2F200.0

G41G1X0.955D27F20.0

G3X0.5675Y-0.1635I-0.3875J0.0F15.0

G1X0.3896F20.0

G2X0.0Y-0.4225I-0.3896J0.1635F25.0

G2X-0.4225Y0.0I0.0J0.4225

G2X0.0Y0.4225I0.4225J0.0

G2X0.3896Y0.1635I0.0J-0.4225

G1X0.5675F20.0

G3X0.955Y0.551I0.0J0.3875F15.0

G40G1X0.7675F20.0

G0Z2.0

G0Y-0.551

G0Z0.6

G1Z-1.2F200.0

G41G1X0.955D27F20.0

G3X0.5675Y-0.1635I-0.3875J0.0F15.0

G1X0.3896F20.0

G2X0.0Y-0.4225I-0.3896J0.1635F25.0

G2X-0.4225Y0.0I0.0J0.4225

G2X0.0Y0.4225I0.4225J0.0

G2X0.3896Y0.1635I0.0J-0.4225

G1X0.5675F20.0

G3X0.955Y0.551I0.0J0.3875F15.0

G40G1X0.7675F20.0

G0Z2.0

M9

G0G91G28Z0M19

G28X0Y0

M1

M6

M30

%

 

A big thank you to those that are willing to help.

[Roger]

I also need to know with V9 Mastercam where you add 20 to your tool diameter offset. T1 post out D21 for cutter comp.

 

Thanks.

[K2csq7]

Wish I could help with adding the 20, the last time I looked at a V9 screen was 2003 (i think).

 

 

But for the post, I see you already have the "T5001" being posted... just not in the right spot.

If you can find the ltlchg postblock, post a screen shot of it.... (not sure if the variables are the same as they are now, need to see it).

BTW, this is a pretty simple thing to modify, a call to your reseller & they can probably do it for you pretty quick. And it will be done correctly (no guessing)

[Roger]

Keith A-1,

 

The program I showed was in the control of the machine, not one I posted. The guy I'm helping with this, just bought this machine used, and they had 3 programs already in the control.

[K2csq7]

Sorry, I don't have V9 so I cant help much.

If you want to, send me the post he is using, I could try and at least get you on the right track. But It will be a trial & error type deal.

 

 

 

[Roger]

Bump....

 

Please help....

[Roger]

175 views, but only one person replied.........That's sad.....I was working for this guy today, and answer part of my question on adding values to your tool number in the job set-up field before you do any toolpaths.

 

I started programing back with version 7 MC, so going back to V9 it's hard to remember how to do things.

 

I guess I'm going to have to install V9 on my computer, and mess with the post myself. Anyone want to point me in the right direction?

[gcode]

175 views, but only one person replied.........That's sad

 

v9 is a dead release.. not one person in 20 on the forum still has it installed

 

most win 7 computers can't even run V9 anymore there's not much we can do to help

[Colin Gilchrist]

Roger,

 

Try contacting your Mastercam Reseller:

 

Steve Kidd

Cimtech Inc.

253-333-0126

[Tinhman]

Well, the best way is to call your reseller. But if you want to give it a try, here is a couple thing you can do.

I dont have V9 any more in my computer, so i will try my best.

First of, BACK UP you post then try to locate this section in your post

 

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

# FORMULAS - global formulas

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

toolcountn = toolcount + 1 # Index!

toolcountp = toolcount - 1 # Index!

tloffno_roger1 = tloffno + 5000

tloffno_roger2 = tloffno + 20

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

 

then find this section:

 

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

# 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 D 4 tloffno_roger2 #Diameter Offset No + 20

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

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

 

then find this section:

 

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

# Tool Comment / Manual Entry Section

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

ptoolcomment #Comment for tool

tnote = t

toffnote = tloffno_roger1

toffnote = tloffno_roger2

tlngnote = tlngno

tldianote = tldia

"(", pstrtool, *tnote, *toffnote, *tlngnote, *tldianote, ")", e

 

 

pstrtool #Comment for tool

if strtool <> sblank,

.

.

.

 

then find this section:

 

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

# Motion output components

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

pbld #Canned text - block delete

if bld, '/'

 

pfbld #Force - block delete

"/"

 

pccdia #Cutter Compensation

#Force Dxx#

if prv_cc_pos <> cc_pos & cc_pos, prv_tloffno_roger2 = c9k

sccomp

if cc_pos, tloffno_roger2

 

pfxout #Force X axis output

if absinc = zero, *xabs, !xinc

else, *xinc, !xabs

 

.

.

.

 

 

You should get it going somewhere.

Good Luck.