541,109 active members*
3,634 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Okuma > Okuma lathe grooving program
Results 1 to 1 of 1
  1. #1
    Member
    Join Date
    Apr 2021
    Posts
    1

    Okuma lathe grooving program

    I need help programming a groove for okuma lathe to 3.0" Dia .325 in Z direction sarting @ 4.0 " DIA stock.
    Anyone please?

  2. #2
    Registered
    Join Date
    Apr 2009
    Posts
    1126

    Re: Okuma lathe grooving program

    G00 X4.1 Z2.325 S500M3 T010101
    G73 X3 Z2 K.1 F.003 D.1L.1
    G00 X20Z20
    Experience is what you get just after you needed it.

  3. #3
    Registered
    Join Date
    Mar 2009
    Posts
    1454

    Re: Okuma lathe grooving program

    there is also possibility to change the tool offset number in the grooving cycle in order to get both edges accuratelly. Sure, the grooving tool must have two offsets set up in the tool description.

  4. #4
    Member
    Join Date
    Jun 2015
    Posts
    3286

    Re: Okuma lathe grooving program

    hy dsandovalm check this out :

    Code:
    
    
        NOEX LINK = 8 V1 = 123 V2 = 0.075 V3 = 0.5 ( tvf chamfer)
    
    
      ( * )
    
    
        G00 X500       Z300                      ( home )
        T+LINK*101 G97 S+V1*320/55 M03 M08 M42   ( index rpm coolant )
            X100       Z-10                      ( rapid way above part, at target z )
            X60+2*2.5                            ( rapid at clearance )
        G01 X60-2*V3-1             F+V2 G95      ( cut a bit under chamfer end point )
        G00 X60+2*2.5                            ( x+ )
                       Z-10+2.5+V3               ( z+ )
        G01 X60-2*V3   Z-10        F+V2*1.25     ( 45*, feed a bit faster )
            X55                    F+V2          ( restore feed ) 
            X55.5                                ( break chip )
            X50
        G04                        F+60/V1*0.75  ( dwell for smooth finish )
            X50.3                                ( disengage cutting edge )
        G00 X60+2*2.5                            ( rapid at clearance )
            X500        Z300 T+LINK*100          ( home )
    included so far :
    ... increased clearance approach ( good to avoid chips that are arround the part, and/or when rapids are not interpolated )
    ... mapped feeds ( go home sooner ? )
    ... parameterized chamfer ( for fine tuning )
    ... modulated ccs ( don't wave the spindle for short x travels )

    future develop directions :
    ... rad comp
    ... 2nd offset & 2nd chamfer
    ... chamfering angle <> 45*
    ... chamfer or fillet
    ... ctr & custom parameters, linked to tool offset page or variables
    ... custom roughing and finishing toolpath
    ... monitoring available from above 4mm width
    ... custom shape
    ... etc etc etc / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •