Can we run CNC lathe with combine program # Combine program for sinumerik cycle 95 & 97

YES SURE !!!

In this programming we performed turning, chamfering, radius cutting, taper turning and threading in a single program

MAIN PROGRAM

HARSH .MPF

N01  G90 G71 G94 F100 ;

N02  G28 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  G00 X50 Z20 ;

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   G28  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 .

N02 -  Referance 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 -  tool stop at safe position where x50 & z20 .

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  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                               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 .