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



MAIN PROGRAM

HARSH .MPF
N01  G90 G71 G94 F100 ;
N02  G75 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  G75 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  G75  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
N02Referance 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  1, 2, 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 .
SINUMERIK CNC PROGRAMMING FOR COMBINE CYCLE 95 & 97 (taper threading cycle) SINUMERIK CNC PROGRAMMING FOR COMBINE CYCLE 95 & 97 (taper threading cycle) Reviewed by HARSHAL DHAWAS on March 01, 2018 Rating: 5
Powered by Blogger.