SINUMERIK CNC PROGRAMMING FOR COMBINE CYCLE 95 & 97 (taper threading cycle)

MAIN PROGRAM

HARSH .MPF

N01  G90 G71 G94 F100 ;

N02  G28 X0 Z0  ;

N03  M06 T06 D01 ;

N04  M03 S1000 ;

N05  M07 ;

N06  G00 X50 Z 2 ;

N07  Cycle 95 [ RAM , 0.2 ,0.1 ,0.1 , 0.1 , 200 , 300 , 200 , 9 ,_ ,_,_]

N08  G28 X0 Z0 ;

N09  M05 ;

N10  G94 F50 ;

N11  M06  T02  D01 ;

N12  M03  S600 ;

N13  G00   X50  Z2 ;

N14  CYCLE 97 [ 2 , 0 , -5, -45 ,20 , 50, 0 ,0 , 1.226 , 0.05 , 30 , 0 , 12 , 2 ,

3, 1 , _]                                              

N15  G28  X0  Z0 ;

N16  M05 ;

N17  M09 ;

N17  M30 ;

SUB  PROGRAM FOR CYCLE 95

RAM.SPF

N01  G01 X16 Z0 ;

N02  G01 X16 Z-5 ;

N03  G01 X20 Z-5 ;

N04  G01 X50 Z-45 ;

N05  G01 X30 Z-45 ;

N06  G01 X30 Z-55;

N07  G01 X50 Z-55 ;

N07  M17 ;                                                        More examples..........!!!!

DISCRIPTION OF PROGRAM

MAIN PROGRAM

N01-   Program in absolute co-ordinate system,  all dimension in mm (G21 used infanuc) , feed in               mm per min , feed rate 100 .

N02 -  Referance point command where tool at X0 Z0 .

N03 – Tool change command , select tool no 6 and offset diameter 01 .

N04 – Spindle onclockwise at speed 1000 rpm.

N05 – Coolant ON .

N06 – Rapidcommand to near to the job and ready for machining , where X50  & Z2 .

N07 – For understanding these  block we have to need knowledge about “stock removal  cycle data “

           Refer this link – STOCK REMOVAL CYCLE DATA

          The following data directly put value in computer

       NPP – RAJ

       MID – 0.2

       FALZ – 0.1

       FALX – 0.1

       FAL -    0.1

       FF1 -   200

       FF2 –  300

       FF3 -   200

       VARI -  EXT=9(Operation perform externally therefore we take  9, if internally we take 11)

       DT -   ___ (skip it)

       DAM -  ____(skip it)

       VRT -   ____(skip it)

N08 -  Referance point command where tool at X0 Z0 .

N09 – Spindle stop .

N10-  Feed rate in mm per min , feed 50 .

N11 - Tool change command , select tool no 2 and offset diameter 01 .( threading tool)

N12-  Spindle on clockwise at speed 600 rpm.

N13 – Rapid command to near to the job and ready for machining , where  X50 & Z2 .

N14 – For better understanding refer this link –  THREADING CYCLE 97.

          This  parameter value directly put into computer .Fig shows threading pitch 2 and tapered                    threading starting and ending diameter is different .  

      PIT -    PIT means pitch of threads is 2 mm .

      MPIT -  It is also pitch of thread but it takes whenever if not given ,it is standards threads pitch                     from 3.5  to 60 . To produce metric cylindrical threads . But in these program we don’t                            need MPIT ,  we take zero  .
      SPL –  Starting point of thread along  Z – axis , we take -5 .

      FPL -  End point of thread along Z – axis , we take - 45 .

      DM1 – Diameter of thread at starting point is 20 .

      DM2 – Diameter of thread at end point is also 50 .

      APP – How much tool away from when start operation , in these program no clearance is provide

                 hence we take zero .                 

      ROP -  After threading  ideal run path for Z axis , we take zero .

      TDEP – Thread depth , there is calculation  0.6134 x pitch ,

                        0.6134 X 2 = 1.226

      FAL – Finishing allowance for finish cut , we take 0.05 .

      IANG – Thread angle , if angle is 60 we take always half of the angle 30.

      NSP – Used for offset at starting  1⁰  , 2⁰  , but we naver take offset in these program hence we                       used 0 .     

      NRC – No. of rough cut , its deped on depth of cut . We take 12 .

      NID – Finishing cut at last . we take 2 .

      VARY – In computer panel there is four option for thread , generally we select for external                              threadin No. 3.    

                 

      NUMTH – No of thread cut this is depend upon single start and multi-start . We take 1 .

      VRT   ___ (skip it )

                                         

N15 -  Referance point command where tool at X0 Z0 .

N16 – Spindle OFF

N17-  Coolent OFF .

N18 – Main program end .

SUB PROGRAM FOR CYCLE-95

RAM.SPF – Sub program name .

N01-  Tool at linearly where X16 and Z0 .(Position A)

N02 – Tool start cutting  linearly , where X16 & Z-5 (Position A to B)  .

N03 – Tool moves linearly X20 and Z -5 ( Position B to C).

N04 - Tool moves linearly X50 and Z -45 .(Positione C to D)

N05-  Tool moves linearly X30 and Z -45 ( Position D to E ).

N06-  Tool moves linearly X30 and Z -55.(Position E to F)

N07-  Tool moves linearly X50 and Z -55.(Position F to G)

N06-  Sub program end .