Okuma Lathe Post Troubles

[gcode]

I've got an old V9 Okuma Post (OSP-7000)

It worked great in V9 and X.

I don't use it much , but now, in X2, it

won't output G41 and G42 (toolnose radius comp)

all the numbers are good, just no G41 or G42

does anyone have any ideas.. they don't ship X2

with an Okuma post

[Greg Williams]

Gcode,

 

This post

 

[post_VERSION] #DO NOT MOVE OR ALTER THIS LINE# V11.00 E1 P4 T1163637166 M11.00 I0

# Post Name : MPLOSP7

# Product : LATHE

# Machine Name : GENERIC OKUMA LATHE

# Control Name : OSP5000/7000

# Description : GENERIC OKUMA LATHE C-AXIS POST

# Associated Post : MPLFAN

# Mill/Turn : YES

# 4-axis/Axis subs. : YES

# 5-axis : NO

# Subprograms : YES

# Canned Cycles : YES

# Executable : MP 8.00

 

 

Gives me this output

 

$ 158504 .MIN %

VCHKL=0

VCHKD=0

VCHKX=0

VCHKZ=0

CLEAR

DEF WORK

PS LC,[-1160,0],[850,750]

END

DRAW

VZSHZ=0

( TOOL - 1 OFFSET - 1 )

( LFINISH OD ROUGH RIGHT - 80 DEG. INSERT - WNMG 08 04 08 )

( FINISH FORM )

NAT1

G50 S3800

G0 G97 X500. Y0. Z500. T0101 S1210 M03 M8

G42 G0 X-39. Z-82.486

G50 S3600

G96 S3800

G18 Z-98.149

G95 G1 X-37. F.3

Z-91.738

X-36.902 Z-91.62

X-32.417 Z-90.8

X-17.

G18 G2 X-16. Z-89.8 K1.

G1 Z-85.

X-15. Z-84.

X-12.463

Z-68.

X-12.413

Z-66.65

Z-.95

X-11.463 Z0.

X-9.5

X3.

G40 Z2.

G0 X500. Y0. Z500. M05 M9

[gcode]

quote:

---

# Post Name : MPLOKUMA

# Product : LATHE

# Machine Name : OKUMA

# Control Name : OSP7000 (OSP-U100L)

# Description : GENERIC 2 AXIS OKUMA /W LAP3 CYCLES

# Mill/Turn : NO

# 4-axis/Axis subs. : NO

# 5-axis : NO

# Subprograms : NO

# Canned Cycles : YES

# Executable : MPL v9.13

---

This is the post I have..I think I got it off

an old V9 install disc.

I don't get any of the header stuff, but the gcode would be pretty much the same except teh G42 would be dropped.

I don't program for Okuma's very often , but it used to work.

[gcode]

I dug out my old V9.1MR0105 dics

It has 2 Okuma posts

MPLOKUMA.PST

and

MPLOSP7C.PST

 

The first is what I was using (updated to X2)

I just tried the 2nd and got this

 

$14470.MIN%

NAT02

( TOOL - 2 OFFSET - 2 )

( LFINISH OD FINISH RIGHT - 35 DEG. INSERT - VNMG-431 )

( OD FINISH PASS_CONTROL COMP_ 0R )

N10 G13

N20 G50 X20. Z0.

N30 G97 T20202 S1528 M41 M3 M87 M8

N40 G42 G0 X.5 Z0.

N50 G50 S3600

N60 G96 S200

N70 X.2

N80 G95 G1 X0. F.003

N90 G3 X-.01 R.005

N100 G1 X-.7724

N110 G2 X-.8732 R.06

N120 G3 X-.8816 R.005

N130 G1 X-1.564

N140 X-1.5757

N150 X-2.06

N160 G40

N170 G0

N180 X.5

N190 M9

N200 T0200

N210 M01

 

For some reason, all my toolplanes are Right

and the output is totally jacked up, but I'm getting the G43 output now

[Greg Williams]

quote:

---

For some reason, all my toolplanes are Right

and the output is totally jacked up, but I'm getting the G43 output now

---

I hope that is a typo? G43 would give you a BAD result

[DavidB]

They have not shipped an Okuma post since V9

X Posts

[Paul Decelles]

Do me a favor. Open the .pst file and look for the following section:

code:

---

pe_inc_calc     #Incremental calculations, end

!x$, !y$, !z$, !xa, !ya, !za

!xia, !yia, !zia, !cc_pos$

---

if it is there, modify it by either deleting the !cc_pos$ or commenting it out like so:

code:

---

pe_inc_calc     #Incremental calculations, end

!x$, !y$, !z$, !xa, !ya, !za

!xia, !yia, !zia #, !cc_pos$

---

By the way, the MPLOkuma post for X or X2 is still available, it has simply been renamed to OKUMA OSP7000 2X LATHE.PST and updated to support new X functionality:

code:

---

## NEW FEATURES FOR X

# - Machine definition, control definition and toolpath group parameter read sections added.

# - Variable initialization with CD_VAR are read directly from CD. Changing these initial values

# in the post will not effect output. These values are only processed during the update post routine.

# - Variable initialization with SET_BY_MD or SET_BY_CD are overwritten in this post by parameter or

# variable settings from MD or CD.

# - Enhanced tool information - Added switch for tool comments (see tool_info)

# - Supports X comments including machine name, group name and group comment output (see pcomment2)

# - Additional date, time and data path output options (see pheader)

# - Support for 10 additional canned text options for X

# - Decimal support for sequence number output (set "Increment sequence number" in CD to a decimal value

# for output. I.E. "Increment sequence number" = .5, "Start sequence number" = 10 : N10, N10.5, N11, N11.5, etc...)

# - Switch for output of M00 or M01 at tool change (3 position switch, off, M00, M01 - see prog_stop)

# - Support for seperate XY, XZ and YZ plane/arc variables (see Arc page in CD)

# - Support for X style coolant. Allows up to 10 different coolants to be turned on/off before, with, or after like

# canned text. Coolant output is handled by "coolant" variable and string selector for V9 style coolant,

# "coolantx" variable and string selector for X style coolant.

---

I believe that !cc_pos was erroneously added somewhere in the V9 cycle and should not be there. The issue is that pe_inc_calc is called prior to the cutter comp output at the beginning of the program and since the value has been updated it is not output (modality).