• Milling in lathe, siemens sinumerik 840D

    If you got driven tools in your lathe, try this

    Mill in lathe, on the edge of the workpiece.

    milling in lathe

    f you can't see the moving gif, check my youtube

    Raw code with comments:

    N10 G54

    N20 WORKPIECE(,,,"CYLINDER",0,0,-100,-80,200)

    N30 G0 G53 X400 Z600 D0 (safe position, tool change)

    N40 T="FRÄS10"

    N50 M6

    N60 G94 F100

    N70 SPOS[1]=0 (set chuck (workpiece) to 0 degrees, need to be before SETMS(1) )

    N80 SETMS(1) (set work spindle, driven tool)

    N90 S1000 M3

    N100 TRANSMIT (start G17, end plane milling)

    N110 G0 X70 Y35 Z3

    N120 Z-3

    N130 G1 Y-35

    N140 G1 X-70 (value X2 without DIAMOF, program in dia)

    N150 G1 Y35

    N160 G1 X70

    N170 G0 Z5

    N180 G0 G53 X400 Z600 D0

    N 85 TRAFOOF (return to turning, G18)

    N190 M30

    How do you do that?

    The programming make you able to do a mill program on the edge, see the pictures below.

    If you does'nt use DIAMOF (and don't) the X-coordinate will be programmed in the double value, the machine (lathe) use diameter measurment on X.. If you use DIAMOF do'nt forget to DIAMON after the milling, otherwise everything will be interesting when you try to do your ordinary turning afterwards

    And don't forget to shut off the milling with TRAFOOF (yep, correct spelling)

    Programming, the blue square is the milling in the exemple, Zero on X and Y is in the middle, Z- is down into the picture




    Email: webmaster@tomasw.com