CYCLE/TURN automatically generates the g-code necessary to remove excess stock during outside and inside rough turning.  It requires a closed profile path defined by standard APT part programming that defines the start and end points of the path and the profile of the part being turned.  "Closed" means that the profile path begins and ends at the same cutter location.  A full example of the command's usage is shown later on this page.  The syntax of the command is:

CYCLE/TURN, index number, cutter diameter, radial depth of cut, axial feedrate, radial feedrate.

Index number defines the index number that encompasses the closed profile path.  For example:
    INDEX/1
        APT command
        APT command
        .
        .
        .
    INDEX/1,NOMORE

Cutter diameter is (no surprise) the actual diameter of the cutter used in rough turning the part.  In usage the part programmer defines an oversized cutter when defining the profile path so that material is left for a finishing pass.  For lathes the cutter diameter is the tool nose radius of the cutter multiplied by 2.  Example:
    CUTTER/.084                                             $$ (.032 tool nose radius + .010) * 2 will leave .010 on all surfaces for the finish pass
    CYCLE/TURN,1,.064,.050,.010,.003      $$ .032 tool nose radius * 2 = the actual diameter
    .
    .
    .

Radial depth of cut specifies the X-axis depth of cut to take for each roughing pass.  For example, a value of .050 will take .100 off of the diameter during each roughing pass.

Axial feedrate specifies the feedrate generated for Z-axis only or combined X- and Z-axis  moves.  The value specified is used literally so be aware when using feedrates in units per revolution versus units per minute.  For example, specifying .010 causes F0.01 to be generated and specifying 10.0 causes F10.0 to be generated.

Radial feedrate specifies the feedrate generated for X-axis only moves, i.e. plunge cuts in X+ or X-.

DO NOT transform the cutter locations when defining the profile path.  The CYCLE/TURN command requires the actual cutter center point locations when calculating intersections.  CYCLE/TURN will automatically apply tool nose radius compensation (i.e. TRACUT) in the generated g-code using the specified cutter diameter.  For finish passes it is fine to use the standard TRACUT command to compensate for the tool nose radius.

A final pass to remove any left-over stock is done when all of the roughing passes are completed.  This final pass follows the profile path defined by the part programmer.

Following is a sample profile of a part to be turned.  Note the start/end point which both opens and closes the profile path.  This also defines a point at which the cutter will clear the rough stock dimensions for both length and radius.  The red arrows show the direction of the tool path.




In this image the closed profile path defined by the APT source is shown in red.  In the APT source (shown later on this page) the path is defined by all of the statements between the INDEX/1 and INDEX/1,NOMORE statements.




Following is a screen shot of the final tool paths in the NC plotter, plotted directly from the generated NC tape file.  All of the horizontal turning cuts plotted in dark blue were automatically generated by the postprocessor using the CYCLE/TURN command.  More sample plots are shown below.




Following is the APT source for the entire part.

MACHIN/ACORNL
PARTNO CYCLE/TURN 1
SEQNO/1000,INCR,10,1
PRINT/ON    $$ This controls the printing of canon data after each geometric definition
CLPRNT        $$ This controls the printing of postprocessor data. Options are "ON", "OFF", AND "OPTION".

SYN/ AA,ATANGL, CA,CANON,  CE,CENTER, CI,CIRCLE, CY,CYLNDR, DC,DNTCUT, $
     FR,FEDRAT, GB,GOBACK, GD,GODLTA, GF,GOFWD,  GL,GOLFT,  GR,GORGT,  $
     GT,GOTO,   IP,INDIRP, IV,INDIRV, IT,INTOF,  LF,LEFT,   LI,LINE,   $
     MX,MATRIX, OB,OBTAIN, PA,PARLEL, PD,PENDWN, PU,PENUP,  PP,PERPTO, $
     PL,PLANE,  PT,POINT,  RA,RADIUS, RT,RIGHT,  TT,TANTO,  TH,THICK,  $
     TA,TLAXIS, TL,TLLFT,  TN,TLON,   TR,TLRGT,  VE,VECTOR, XL,XLARGE, $
     XS,XSMALL, YL,YLARGE, YS,YSMALL, ZL,ZLARGE, ZS,ZSMALL, RP,RAPID

HOME=PT/5,5,5
LX=LI/XAXIS
LY=LI/YAXIS
L1=LI/(PT/0,(.86/2)),AA,30,YAXIS
L2=LI/PA,LX,YL,(1.0/2)
L3=LI/PA,LY,XS,(1.0-.062)
L4=LI/PA,LX,YL,(.88/2)
L5=LI/PA,LY,XS,1.0
L6=LI/(PT/-1.0,(1.0/2)),AA,-45,XAXIS
L8=LI/PA,LX,YL,(2.0/2)
L9=LI/PA,LY,XS,(2.0-.188)
L10=LI/PA,LX,YL,(1.75/2)
L11=LI/PA,LY,XS,2.0
L12=LI/PA,LX,YL,(3.0/2)
L13=LI/PA,LY,XS,3.0
L14=LI/PA,LX,YL,(4.0/2)
L15=LI/PA,LY,XS,3.5
L16=LI/PA,LY,XL,.1
L17=LI/PA,L14,YL,.1
C1=CI/YS,L6,YS,L8,RA,.25
C2=CI/YS,L2,XL,L3,RA,.010
C3=CI/YS,L6,XS,L5,RA,.010
C4=CI/YS,L8,XL,L9,RA,.010
PL0=PL/0,0,1,0

$$************* ROUGH TURN, .032 RADIUS TOOL **************************

PPRINT
PPRINT ROUGH TURN, .032 RADIUS TOOL

$$ This macro defines the bulk of the profile path
$$ along with the additional statements enclosed by the
$$ INDEX statements.  This macro is also called when
$$ the finish passes are defined.  Using a macro is not
$$ required.  It just simplifies part programming and
$$ saves a bit of typing.
RTURN=MACRO
  GL/L2
  GR/L6
  GF/C1
  GF/L8
  GR/L11
  GF/(CI/XS,L11,YS,L12,RA,.010)
  GF/L12
  GR/L13
  GF/(CI/XS,L13,YS,L14,RA,.010)
  GF/L14,PAST,L15
  GO/PAST,L17
  RP,GO/PAST,L16
TERMAC

RESET
TURRET/1,1
ORIGIN/54
SPINDL/500,SFM,CLW,MAXRPM,10000
COOLNT/ON
FROM/HOME

CUTTER/.084 $$ declare oversized cutter diameter for rough turning
FEDRAT/.008 $$ declare a default feedrate just to be safe

$$ In the following CYCLE/TURN command:
$$ 1 = The index number that defines the closed profile path
$$ .064 = The actual cutter diameter.  Note that an oversized cutter is declared above which will leave .010 on all surfaces for clean up.
$$ .060 = The radial depth of cut.
$$ .008 = The axial feedrate.
$$ .003 = The radial (i.e. plunge) feedrate.
$$ Note that the tool path for the CYCLE/TURN is not (and must not) be transformed in any manner.
$$ The finish operation coded later uses TRACUT per standard lathe programming.
CYCLE/TURN,1,.064,.060,.008,.003
INDEX/1
  RP,GO/L16,PL0,L17   $$ this is the start/end point and matches the ending location in the macro
  RP,GO/L16,PL0,L1
  TR,GR/L1
  CALL/RTURN
INDEX/1,NOMORE

COOLNT/OFF
SPINDL/OFF
RP,GOHOME
OPSTOP


$$************* FINISH FACE AND TURN, .032 RADIUS TOOL ****************

PPRINT
PPRINT FINISH FACE AND TURN, .032 RADIUS TOOL

RESET
TURRET/2,2
ORIGIN/54
SPINDL/500,SFM,CLW,MAXRPM,10000
COOLNT/ON
FROM/HOME

CUTTER/.064
FEDRAT/.008
TRACUT/(M1=MATRIX/TRANSL,-.032,-.032,0)   $$ TRACUT by the actual tool nose radius.

$$ FINISH FACE
CUTCOM/LEFT
RP,GO/(LI/PA,LY,XL,.05),PL0,(LI/PA,L2,YL,.05)
GO/LY
GO/PAST,LX
CUTCOM/OFF
GO/PAST,(LI/PA,LY,XL,.05)

$$ FINISH TURNING
CUTCOM/RIGHT
RP,GO/(LI/PA,LY,XL,.05),PL0,PAST,L1
TR,GL/L1
CALL/RTURN
CUTCOM/OFF
TRACUT/NOMORE
COOLNT/OFF
SPINDL/OFF
RP,GOHOME
OPSTOP

$$ *************** 1/16 (.062) GROOVING, .010 RADIUS ******************

PPRINT
PPRINT 1/16 (.062) GROOVING, .010 RADIUS
RESET
TURRET/3,3
ORIGIN/55
SPINDL/500,SFM,CLW,MAXRPM,3000
COOLNT/ON
FROM/HOME
CUTTER/.020
TRACUT/(M2=MATRIX/TRANSL,-.010,-.010,0)
RP,GO/L5,ON,PL0,(LI/PA,L2,YL,.050)
FEDRAT/.002
GO/L4
RP,GO/PAST,(LI/PA,L2,YL,.050)
GO/L6
TL,GL/L6
GF/C3,TT,L5
RP,GO/PAST,(LI/PA,L2,YL,.050)
TRACUT/NOMORE
TRACUT/(M3=MATRIX/TRANSL,-.052,-.01,0) $$ X VALUE = -(TOOL WIDTH - TOOL RADIUS)
RP,GO/ON,(LI/(PT/CE,C2),PP,LX)
GO/C2
TR,GR/C2,TT,L3
RP,GO/PAST,(LI/PA,L2,YL,.050)
TRACUT/NOMORE
COOLNT/OFF
SPINDL/OFF
RP,GOHOME
OPSTOP

$$ *************** 1/8 (.125) GROOVING, .010 RADIUS *******************

PPRINT
PPRINT 1/8 (.125) GROOVING, .010 RADIUS
RESET
TURRET/4,4
ORIGIN/55
SPINDL/500,SFM,CLW,MAXRPM,3000
COOLNT/ON
FROM/HOME
CUTTER/.020
TRACUT/M2
RP,GO/L11,ON,PL0,(LI/PA,L12,YL,.050)
FEDRAT/.002
GO/L10
RP,GO/PAST,(LI/PA,L8,YL,.050)

TRACUT/(M4=MATRIX/TRANSL,-.115,-.01,0) $$ X VALUE = -(TOOL WIDTH - TOOL RADIUS)
RP,GO/L9
GO/L10
TRACUT/NOMORE
TRACUT/M2
GO/L11
RP,GO/PAST,(LI/PA,L8,YL,.050)
TRACUT/NOMORE
TRACUT/M4
RP,GO/ON,(LI/(PT/CE,C4),PP,LX)
GO/C4
TR,GR/C4,TT,L9
RP,GO/PAST,(LI/PA,L8,YL,.050)
TRACUT/NOMORE
COOLNT/OFF
SPINDL/OFF
RP,GOHOME
OPSTOP

$$********** 90 DEGREE SPOT DRILL TO .460 DIAMETER ********************

PPRINT
PPRINT 90 DEGREE SPOT DRILL TO .460 DIAMETER
RESET
TURRET/5,5
REVS=(500*3.82)/.5     $$ RPM = (SFM * 3.82) / dia
SPINDL/REVS,RPM,CLW
COOLNT/ON
FROM/HOME
RP,GOTO/1,0,0
CYCLE/DRILL,(-.460/2),.1,.002
CYCLE/OFF
COOLNT/OFF
SPINDL/OFF
RP,GOHOME
OPSTOP

$$******************* 7/16 (.438) DRILL THRU **************************

PPRINT
PPRINT 7/16 (.438) DRILL THRU
RESET
TURRET/6,6
REVS=(500*3.82)/.438     $$ RPM = (SFM * 3.82) / dia
SPINDL/REVS,RPM,CLW
COOLNT/ON
FROM/HOME
RP,GOTO/1,0,0

DPTH=3.5+(TANF(31)*(.438/2))+.01
CYCLE/DEEP,-DPTH,.1,.004,(.438/2)

CYCLE/OFF
COOLNT/OFF
SPINDL/OFF
RP,GOHOME
OPSTOP

$$*********************** 1/4-18 NPT TAP ******************************

PPRINT
PPRINT 1/4-18 NPT TAP, DEPTH IS ONLY A GUESS
RESET
TURRET/7,7
SPINDL/300,RPM,CLW
COOLNT/ON
FROM/HOME
RP,GOTO/1,0,0
CYCLE/TAP,RIGHT,-.5,.1,(1/18)   $$ Depth is only a guess.
CYCLE/OFF
COOLNT/OFF
SPINDL/OFF
RP,GOHOME
OPSTOP

$$ *************** 1"-12 EXTERNAL THREAD ******************************

PPRINT
PPRINT 1"-12 EXTERNAL THREAD
RESET
TURRET/8,8
SPINDL/300,RPM,CLW
COOLNT/ON
FROM/HOME
RP,GOTO/.1,.55,0
$$         pitch, major diameter,    z, depth of first cut, min depth of cut, depth of last pass, pull out, taper, infeed angle, spring passes
THREAD/(1/12),(1-2*(1/12)*.61343),(-1.0+.031),.01,.001,.001,0,0,60,3
COOLNT/OFF
SPINDL/OFF
RP,GOHOME

REWIND
FINI


Here is another plot showing OD roughing and finishing with an undercut:



Here is an example path and plot showing roughing out a bore:






And here is a chess pawn being roughed and finished turned and parted off: