converting from Haas to Okuma control. Program differences?

[honeybunches]

I finally have a post working just as I like it but it is for a Haas.  I was looking to run programs on an Okuma OSP control and curious if these will be small changes if any, or a complete start over?  These are both VMCs.  the Haas's are carousel changers and Okuma is side mount but I want to say I simply disabled the tool prestaging in the post.  

[RaiderX]

Been a very long time but

work offsets are different not g54 etc

tool length offset code is different? not g48?

some canned cycle codes are different, g98 g99 is a different code?

macro programming is way different but very powerfull

that's just from memory there may be a bit more

your going to love it once you get used to it. Okuma rocks.

[honeybunches]

Thanks.  I have been looking at this and would like to get some general ideas which way might be easiest to fix this issue.  I am not all that concerned about directly converting any Haas  programs, and I would just repost.  

 

However, regarding the post, I am not yet sure if it would be easier to edit my existing post for the Okuma or maybe edit a generic Okuma post and work it up?  

Here are the things I have modded in the fanuc post.  

1.  Work offsets with subroutines. I define a variable in MCX as the amount of offsets I want to repeat the work.  The program then generates with internal subroutines, repeated as many times as I indicated in the variable table.  Example, I want to repeat the same work at 4 offsets, I enter variable = 4, I will get subs of G54,55,56,57.  If the variable stays as 1, no subroutine would be generated.  I simply LOVE subroutines!!!  Typically if something needs changed, it would be on all parts.  Obviously there are drawbacks to.  

 

2. The work offsets, count up, then down, then up, etc.  So on T1, it would run G54,55,56,57, then change tool, and run G57,56,55,54.  

 

Now some of this was done to optimize for older machines with slower rapids and apparently machines don't want to reposition the table while doing a tool change.  This became more of an issue on a longer travel VMC.  LOTS of waiting.  

 

Other simple adjustments were to move the coolant turn on to ensure it was flowing before making chips.  I also added a work coordinate at the end of every program, usually G110, X0, Y0.  I would then simply jog the machine to where the best place is to change out work depending on parts, and set the offset there.  

 

 

Can I can some ideas which will be an  easier way to go here?  

 

 

 

 

[gcode]

I would contact my dealer.

Back in the day my dealer had a pretty good Okuma VMC post they gave away for free

All I had to do was ask

 

[honeybunches]

Another guy has already checked and we already have an Okuma post that works just perfect.  I just got so used to subroutines and such that I would like to have the option.  If I need to change a drill depth, I change it in one spot.  

[Brad Lisle]

Here is a brief rundown of OSP vs FANUC

The G116 tool change call is a custom macro in a .LIB file format that is assigned to a macro G-code. If you do not have this you can use T# M6

(Traditional Oxxxx program number not necessary)
(The CNC machine will recognize the Windows file name as the program name)
(the file extension MUST be .MIN for a main program and .SUB or .SSB for a sub program)

N2 G116 T2 (Tool call. T# M6 is also valid for calling tools)
G15 H01 (this indicates work offset #1, or G54 in Fanuc) 
G0 G90 X-13.535 Y8.0
S8000 M3 T9
G56 H2 Z.25 M8 (G56 is command to read tool length offset. Fanuc G43)
Z0.02
G1 Z0 F100.
X-11.135 F90.
Y0
X11.8
G1 Y8.0
G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0)
M1


N66 G116 T9  (Drill)
G15 H01 (Work offset)
G0 G90 X10.593 Y33.7878
S7000 M3 T1
G56 H9 Z15. M8 (TLO read)
Z.25
G71 Z2.5 (optional- set a clamp clearance point)
G83 M53(special retract- Fanuc G98) X0 Y0 Z-.5 R.1 F38. (all codes same as Fanuc)
CALL O1234 (Cal sub for modal hole drilling- Fanuc M98) 
G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0)
M1


N66 G116 T1  (spot Drill)
G15 H01 (Work offset)
G0 G90 X10.593 Y33.7878
S7000 M3 T10
G56 H1 Z15. M8 (TLO read)
Z.25
G71 Z2.5 (optional- set a clamp clearance point)
G81 M53(special retract- Fanuc G98) X0 Y0 Z-.15 R.1 P1. F38. (all codes same as Fanuc- P=Dwell)
CALL O1234 (Cal sub for modal hole drilling) 
G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0)
M1

N66 G116 T10  (bore)
G15 H01 (Work offset)
G0 G90 X10.593 Y33.7878
S7000 M3 T15
G56 H10 Z15. M8 (TLO read)
Z.25
G71 Z2.5 (optional- set a clamp clearance point)
G85 X10.322 Y31.8297 Z-1. R.1 F20. M53  (Same as Fanuc)
CALL O1234 (Cal sub for modal hole drilling) 
G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0)
M1

N66 G116 T15  (rigid tap)
G15 H01 (Work offset)
G0 G90 X10.593 Y33.7878
S3000 M3 T16
G56 H15 Z15. M8 (TLO read)
Z.25
G84 X10.322 Y31.8297 Z-1. R.1 F166.66 M54  (Same as Fanuc-M54 means return to R plane. Fanuc G99)
CALL O1234 (Cal sub for modal hole drilling) 
G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0)
M1

N66 G116 T16  (rigid peck tap)
G15 H01 (Work offset)
G0 G90 X10.593 Y33.7878
S3000 M3 T2
G56 H15 Z15. M8 (TLO read)
Z.25
G283 X0 Y0 Z-.5 I.075 R.1 Q.1 F166.66(G283 is a peck tap. I=retract amount, Q=depth of peck)
CALL O1234 (Cal sub for modal hole drilling) 
G0 Z50. M5 (Move Z axis to travel limit. Fanuc G91 G28 Z0)
M1

M2 (Or M30)

O1234(Sub)    (Subs can be either in a separate file or attached to the main program)
X1.
X2.
X3.
X4.
RTS(Return to system. Fanuc M99)