SINUMERIK CNC PROGRAM FOR COMBINE CYCLE 95 & 97

SINUMERIK CNC PROGRAM FOR COMBINE CYCLE 95 & 97 
In this programming we performed turning , chamfering , radius cutting , taper turning and threading in single program



MAIN PROGRAM

HARSH .MPF
N01  G90 G71 G94 F100 ;
N02  G75 X0 Z0  ;
N03  M06 T06 D01 ;
N04  M03 S1000 ;
N05  M07 ;
N06  G00 X26 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   X30  Z1 ;
N14  CYCLE 97 [ 1.5 , 0 , -16, -55 ,32 , 32, 0 ,0 , 0.9201 , 0.05 , 30 , 0 , 12 , 2 ,
3, 1 , _]
N15   G75  X0  Z0 ;
N16   M05 ;
N17   M09 ;
N17   M30 ;

SUB  PROGRAM FOR CYCLE 95SS

RAM.SPF
N01  G01  X0 Z0 ;
N02  G03  X30 Z-15  CR=15 ;
N03  G01  X32 Z-16 ;
N04  G01  X32 Z-55 ;
N05  G01  X48 Z-65 ;
N06  M17 ;                                                   More examples..........!!!!

DISCRIPTSION OF PROGRAM

MAIN PROGRAM

N01-   Program in absolute co-ordinate system ,  all dimension in mm , feed in mm permin , feed rate 100 .
N02Referance point command where tool at X0 Z0 .
N03 – Tool change command , select tool no 6 and offset diameter 01 .
N04 – Spindle on clockwise at speed 1000 rpm.
N05 – Coolant ON .
N06 Rapid command to near to the job and ready for machining .
N07 – For understanding these  block we have to need knowledge about “stock removal  cycle data “
Refer this link – STOCK REMOVAL CYCLE DATA
In these cycle we performed radis cutting , turning , chamfering and taper operation .
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 .
N12 – Spindle on clockwise at speed 600 rpm.
N13 – Rapid command to near to the job and ready for machining .

N14 – For better understanding refer this link – THREADING CYCLE-97
          This  parameter value directly put into computer .Fig shows 32M X 1.5 , it means given is 20mm
      PIT -    PIT means pitch of threads is 1.5 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 -16 .
      FPL -  End point of thread along Z – axis , we take -55 .
      DM1 – Diameter of thread at starting point is 32 .
      DM2 – Diameter of thread at end point is also 32 .
      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 1.5  = 0.9201
      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                               threading  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 X0 and Z0 .
N02 – Outer radius 15 , where X30 and  Z-15 (Radius cutting ) .
N03 – Tool moves linearly X30 and Z -16 ( Chamfering).
N04 - Tool moves linearly X32 and Z -55 ( Turning).
N05-  Tool moves linearly X48 and Z -65 (Taper turning ).
N06 - Sub program end .


SINUMERIK CNC PROGRAM FOR COMBINE CYCLE 95 & 97 SINUMERIK CNC PROGRAM FOR COMBINE CYCLE 95 & 97 Reviewed by HARSHAL DHAWAS on February 26, 2018 Rating: 5

No comments:

Popular Posts

Powered by Blogger.