How to stop WCS on every B axis move?

[Darin]

Hi,

 

We have a Niigata horizontal mill.. When we use transform translate or even on any B move it will post a new WCS (G54).. I though this was controlled in the transform translate page.. But not matter what I change to it still posts a new WSC for each B move... Where can I change this? is this control def or post controlled?

 

 

 

 

G90 G10 L2 P1 X0 Y0 Z0 B0 (G54)

G90 G10 L2 P2 X0 Y0 Z0 B0 (G55)

G90 G10 L2 P3 X0 Y0 Z0 B0 (G56)

G90 G10 L2 P4 X0 Y0 Z0 B0 (G57)

G90 G10 L2 P5 X0 Y0 Z0 B0 (G58)

G90 G10 L2 P6 X0 Y0 Z0 B0 (G59)

N100 G20

N110 G91 G28 Z0.

N120 G91 G28 X0. Y0. B0.

N130 G00 G17 G40 G49 G80 G90

N5 M01 ( 1/8 FLAT ENDMILL )

( MILLS FIRST .984 HOLE TOP AT 10 DEGS )

N140 T05 M06

N150 G00 G90 G54 X0. Y9.8425 B10. S6500 M03

N160 G43 H05 Z9.93

N170 M08

N180 X-.2946

N190 Z9.78

N200 G01 Z9.55 F25.

N210 G41 D05 X-.4196

N220 G03 X0. Y9.4229 I.4196 J0.

N230 X.4196 Y9.8425 I0. J.4196

N240 X0. Y10.2621 I-.4196 J0.

N250 X-.4196 Y9.8425 I0. J-.4196

N260 G01 G40 X-.2946

N270 X-.3046

N280 G41 D05 X-.4296

N290 G03 X0. Y9.4129 I.4296 J0.

N300 X.4296 Y9.8425 I0. J.4296

N310 X0. Y10.2721 I-.4296 J0.

N320 X-.4296 Y9.8425 I0. J-.4296

N330 G01 G40 X-.3046

N340 G00 Z9.93

( TRANSFORM MILLS SEVENTEEN .984 HOLES TOP 20 DEGS APART )

( MILLS FIRST .984 HOLE TOP AT 10 DEGS )

N350 G00 G90 G55 B30. <---------------------------------------------------------- Need to all be G54 ------------------------->

N360 X0. Y9.8425

N370 Z9.93

N380 X-.2946

N390 Z9.78

N400 G01 Z9.55

N410 G41 D05 X-.4196

N420 G03 X0. Y9.4229 I.4196 J0.

N430 X.4196 Y9.8425 I0. J.4196

N440 X0. Y10.2621 I-.4196 J0.

N450 X-.4196 Y9.8425 I0. J-.4196

N460 G01 G40 X-.2946

N470 X-.3046

N480 G41 D05 X-.4296

N490 G03 X0. Y9.4129 I.4296 J0.

N500 X.4296 Y9.8425 I0. J.4296

N510 X0. Y10.2721 I-.4296 J0.

N520 X-.4296 Y9.8425 I0. J-.4296

N530 G01 G40 X-.3046

N540 G00 Z9.93

( MILLS FIRST .984 HOLE TOP AT 10 DEGS )

N550 G00 G90 G56 B50.

N560 X0. Y9.8425

N570 Z9.93

N580 X-.2946

[gcode]

what post are you using

[Darin]

what post are you using

 

 

It is a post that came with machine I guess... I just started here.. It looks like this on top... We use X6

 

 

[post_VERSION] #DO NOT MOVE OR ALTER THIS LINE# V15.00 P0 E1 W15.00 T1337895754 M15.00 I0 O0

# Post Name : Fanuc 4X Mill.pst

# Product : Mill

# Machine Name : NIIGATA

# Control Name : Fanuc

# Description : Generic 4 Axis Mill Post

# 4-axis/Axis subs. : Yes

# 5-axis : No

# Subprograms : Yes

# Executable : MP 14.0

#

# WARNING: THIS POST IS GENERIC AND IS INTENDED FOR MODIFICATION TO

# THE MACHINE TOOL REQUIREMENTS AND PERSONAL PREFERENCE.

#

# THIS POST REQUIRES A VALID 3 OR 4 AXIS MACHINE DEFINITION.

# YOU WILL RECEIVE AN ERROR MESSAGE IF MORE THAN ONE ROTARY AXIS IS DETECTED IN

# THE ACTIVE AXIS COMBINATION WITH READ_MD SET TO YES.

#

# Associated File List$

#

# GENERIC FANUC 4X MILL.control-5

#

# Associated File List$

#

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

# Revision log:

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

# CNC 06/09/05 - Initial post setup for Mastercam X

# CNC 10/06/05 - Changed parameter read for min_speed, modified pspindle, pprep$ and pset_mach

# - Modified pset_rot_label to use srot_y for horizontal machines

# - Added call to pset_mach in pq$ to set rotaxtyp$

# CNC 11/18/05 - Added psynclath with call to pset_mach to set rotaxtyp$, removed call from pq$

# CNC 02/03/06 - Added logic for high-speed toolpath tool inspection (see prapidout & plinout)

# CNC 06/26/06 - Initial post setup for Mastercam X2

# CNC 12/15/06 - Modified pset_mach for horizontal rotation when rotating about world Z axis.

# CNC 02/26/07 - Modified pwcs

# CNC 11/02/07 - Added prv_shftdrl$ = zero

# CNC 04/08/08 - X3 release - Removed check for write_ops

# CNC 01/26/09 - Initial post update for Mastercam X4

# CNC 04/15/09 - Added read_md switch to enable or disable setting rotary axis from Machine Definition

# CNC 05/06/09 - Modified pindxcalc to omit ctable check when rotary is not indexer

# CNC 06/09/09 - Updated MD parameters

# CNC 08/31/09 - Added check for read_md in pset_mach

# CNC 02/03/10 - Initial post update for Mastercam X5

# CNC 04/21/10 - Added Toolpath Transform Enhancements

# CNC 08/17/10 - Added fix for canned drill cycle incremental mode code output and Z output in incremental mode

# - Added fix for X coolant output

# - Added fix for MP line break pattern

# - Added fix for stock to leave output in tool table

# - Removed CD_VAR variables

# - Added axis sub direction logic

# CNC 08/23/10 - Added logic to handle axis sub with signed or shortest direction and rotation >= 360 degrees

[gcode]

I thought I knew how to lock the WCS on that post.. but they've stripped a bunch of things out of it.

[Darin]

I thought I knew how to lock the WCS on that post.. but they've stripped a bunch of things out of it.

 

Ok thanks.. I am finding out from other sources that these older MPfan posts are a lot harder to fix this issue then the MPmaster... I might start over and use MPmaster...

[Darin]

I thought I knew how to lock the WCS on that post.. but they've stripped a bunch of things out of it.

 

You know how to fix this with the MPmaster post?

[gcode]

Yes.. set misc 9 to 1

It only has to be set in the first op, but I set it in every op for safety

If I'm doing a patch months later, and I post something in the middle of the tree, I'll get bad workoffsets output

and a really pissed off operator.

So I set it in every op and forget about it.

[Darin]

Yes.. set misc 9 to 1

It only has to be set in the first op, but I set it in every op for safety

If I'm doing a patch months later, and I post something in the middle of the tree, I'll get bad workoffsets output

and a really pissed off operator.

So I set it in every op and forget about it.

 

Thanks.. In the misc values great.. How hard would it be to add this to a old post? Probably be better just to make my MPmaster post work with my Niigata's..