马上注册，结交更多同行朋友，交流，分享，学习。
您需要 登录 才可以下载或查看，没有帐号？注册
x
$----------------------------- HEADER ---------------------------------------
Customer : LICOM STANDARD MILL POST
Machine :
Control : Based on Fanuc 6MB
Database Name:
Units : MM
Axes Used : XYZ
Coord System : Absolute
Z-Axis : Vertical
Contact :
Tel :
Fax :
Dealer Name :
Post Author :
Ver 1 Date :
Notes :
Last Edit : 30 Jan 95 - User Cycle $1208 for MAHO circles with G43 Lead-In
15 AUG 95 - Tool Array data inserted at $10
17 FEB 97 - Helical Arcs allowed. See $50, $60 and
new number $527 and new options for $530
$---------------------------- INTRODUCTION ----------------------------------
For help in configuring a post processor, open a second (horizontal) window
and load POST HELP FILE into it so that you can look at the notes as you go.
Remember to select Machine Type (Mill or Lathe) from F4-Format before saving
the completed Post - to be sure, check top right of screen NOW !
Also, set the default Post from F4-Format. Make the default the one you most
often want to use - your NC code will be produced to suit the default auto-
matically - but you can choose another Post when you program a part in APS.
Remarks:
That are to appear in the NC code (but NOT be sent to the machine)
should be preceded by ' (a single apostrophe)
That are local to the Post for your information only should be
preceded by '' (TWO single apostrophes)
$------------------------- PROGRAM LEADING/TRAILING LINES -------------------
$5 $STORE, $RUN and $RECALL - See manual Appendix A for details
$10 File LEADING lines
$LET DATE = DAT ''NOTE: In $1000, DATE is set to first 9 chars only
$12 Main Program LEADING lines
O[PROGNUM];
N[N]G54X[0.0]Y[0.0]Z[SAFE_Z];
$15 Main Program TRAILING lines
N[N] G0 Z[SAFE_Z];
N[N] G0 X[0.0]Y[0.0];
N[N] M05;
N[N] M02;
$17 File TRAILING Lines
'[TNT]
$----------------------- RAPID MOVES ----------------------------------------
$20 Rapid Move in XY (MILL/ROUTER/FLAME/LASER) or XZ (LATHE) only
N[N]G00X[AX]Y[AY];
$----------------------------------------------------------------------------
$21 3D Rapid Move in XYZ (MILL/ROUTER ONLY)
N[N]G00X[AX]Y[AY]Z[AZ];
$----------------------------------------------------------------------------
$25 Rapid Move in Z only (MILL etc)
N[N]G00Z[AZ];
$----------------------------------------------------------------------------
$30 Lines BEFORE a rapid move if Z levels are not used eg Laser or Geometry
UP
$----------------------------------------------------------------------------
$35 Lines AFTER a rapid move if Z levels are not used eg Laser or Geometry
DN
$----------------------- MACHINING FEED MOVES -------------------------------
$40 Machining FEED lines
$IF MC + IN = 2 ''M/C comp applies, and this is LEAD-IN Line
N[N]G01[TC]D[T+10]X[AX]Y[AY]Z[AZ]F[F]S[S];
$ELSEIF MC + OUT = 2 '' M/C comp applies, and this is LEAD-OUT Line
N[N]G01[TC]X[AX]Y[AY]Z[AZ]F[F];
$ELSE '' Applies to all other lines (with APS or M/C comp).
N[N]G01X[AX]Y[AY]Z[AZ]F[F];
$ENDIF
$----------------------------------------------------------------------------
$50 Feed CW arc (APS will automatically limit arcs to 180 degrees maximum)
$IF II*II+IJ*IJ>0.004
N[N]G02X[AX]Y[AY]I[II]J[IJ]F[F];
$ELSEIF IJ*IJ+II*II>0.004
N[N]G02X[AX]Y[AY]I[II]J[IJ]F[F];
$ELSE
N[N]G01X[AX]Y[AY];
$ENDIF
$----------------------------------------------------------------------------
$60 Feed CCW arc
$IF II*II+IJ*IJ>0.004
N[N]G03X[AX]Y[AY]I[II]J[IJ]F[F];
$ELSEIF IJ*IJ+II*II>0.004
N[N]G03X[AX]Y[AY]I[II]J[IJ]F[F];
$ELSE
N[N]G01X[AX]Y[AY];
$ENDIF
$------------------------ TOOL CHANGES --------------------------------------
$70 Cancel current tool. Use [T] for current tool number if required.
$75 Code for CLOCKWISE spindle rotation - entered into variable ROT (or RT)
M03
$76 Code for COUNTER-CLOCKWISE spindle rotation - entered into variable ROT
M04
$80 Select new tool. Use [T] for new tool number, [S] for spindle speed.
N[N]M03S[S]; 'Next tool is [NT], Next XY is [NX], [NY]
$-------------------------- SUBROUTINES ------------------------------------
$90 CALL subroutine. Use [SN] for subroutine number.
N[N]M98P[SN]; 'CALL SUB [SN]
$----------------------------------------------------------------------------
$100 BEGIN subroutine. Use [SN] for subroutine number.
:[SN] 'BEGIN SUB [SN]
$----------------------------------------------------------------------------
$110 END subroutine
N[N]M99; 'END SUB [SN]
$------------------- REFERENCE ZERO or ORIGIN SHIFT -------------------------
$120 Origin shift. Use [OX] and [OY] for values to shift by)
N[N]G52X[OX]Y[OY]; 'ORIGIN SHIFT
$----------------------------------------------------------------------------
$130 Cancel Origin shift. [OX] and [OY] are values by which origin was shifted)
N[N]G52X0.0Y0.0; 'CANCEL ORIGIN SHIFT
$----------------------- MACHINE TOOL COMPENSATION --------------------------
NOTE: Codes given in $140 to $142 are assigned to TC as required for each path
$140 Code to CANCEL Machine Tool Compensation
G40
$141 Code for LEFT Machine Tool Compensation
G41
$142 Code for RIGHT Machine Tool Compensation
G42
$145 Percentage increase in blend radius for sharp internal corners
0
$146 Adjust G41/42 code at internal corners for tool radius (1 = Yes 0 = No)
1
$----------------------- COOLANT OFF/MIST/FLOOD/TOOL CODES ------------------
Codes in $150 to $153 are assigned to CLT as required for each path
$150 Code to Turn Coolant OFF
M09
$151 Code to apply MIST Coolant
M07
$152 Code to apply FLOOD Coolant
M08
$153 Code to apply THROUGH TOOL Coolant
M10
$------------------------ DRILLING/TAPPING CYCLES ---------------------------
[ZR] = Retract level, the Z level to rapid down to before feed down begins.
[ZB] = Z value of the bottom of the hole, [ZP] = peck DISTANCE.
[ZS] = Safe Rapid level, [ZM] = Material top. All values are ABSOLUTE.
For LINEAR code use $210/211, $214/215 etc. For SUBROUTINES use $205/206 for
X/Y values and $212/216 etc to set Z levels etc before calling the subroutine.
$200 CANCEL drill/tapping cycle
N[N]M09; ''Turn coolant OFF
N[N]G80;
$----------------------------------------------------------------------------
$205 First Hole in SUBROUTINE. NOTE $205/206 apply to ALL drill/peck etc cycles
N[N]X[AX]Y[AY];
$206 Next holes in Subroutine
N[N]X[AX]Y[AY];
$----------------------------------------------------------------------------
DRILL cycle - traverse to next hole at SAFE RAPID level [ZS]
$210 First Hole
N[N]G98G81X[AX]Y[AY]Z[ZB]R[ZR]F[F][CLT]; ''CLT = Coolant Code
$211 Next holes
N[N]X[AX]Y[AY];
$212 Set PARAMETERS before Subroutine call (APS will insert Subroutine call)
N[N]G98G81Z[ZB]R[ZR]F[F][CLT];
$----------------------------------------------------------------------------
DRILL cycle - traverse to next hole at RETRACT level [ZR]
$214 First Hole
N[N]G99G81X[AX]Y[AY]Z[ZB]R[ZR]F[F][CLT]; ''CLT = Coolant Code
$215 Next holes
N[N]X[AX]Y[AY];
$216 Set PARAMETERS before Subroutine call (APS will insert Subroutine call)
N[N]G99G81Z[ZB]R[ZR]F[F][CLT];
$----------------------------------------------------------------------------
PECKING cycle - traverse to next hole at SAFE RAPID level [ZS]
$220 First hole
N[N]G98G83X[AX]Y[AY]Z[ZB]R[ZR]Q[ZP]F[F][CLT]; ''CLT = Coolant Code
$221 Next holes
N[N]X[AX]Y[AY];
$222 Set PARAMETERS before Subroutine call (APS will insert Subroutine call)
N[N]G98G83Z[ZB]R[ZR]Q[ZP]F[F][CLT];
$----------------------------------------------------------------------------
PECKING cycle - traverse to next hole at RETRACT level [ZR]
$224 First hole
N[N]G99G83X[AX]Y[AY]Z[ZB]R[ZR]Q[ZP]F[F][CLT]; ''CLT = Coolant Code
$225 Next holes
N[N]X[AX]Y[AY];
$226 Set PARAMETERS before Subroutine call (APS will insert Subroutine call)
N[N]G99G83Z[ZB]R[ZR]Q[ZP]F[F][CLT];
$----------------------------------------------------------------------------
TAPPING cycle - traverse to next hole at SAFE RAPID level [ZS]
$230 First hole
N[N]G98G84X[AX]Y[AY]Z[ZB]R[ZR]F[F][CLT]; ''CLT = Coolant Code
$231 Next holes
N[N]X[AX]Y[AY];
$232 Set PARAMETERS before Subroutine call (APS will insert Subroutine call)
N[N]G98G84Z[ZB]R[ZR]F[F][CLT];
$----------------------------------------------------------------------------
TAPPING cycle - traverse to next hole at RETRACT level [ZR]
$234 First hole
N[N]G99G84X[AX]Y[AY]Z[ZB]R[ZR]F[F][CLT]; ''CLT = Coolant Code
$235 Next holes
N[N]X[AX]Y[AY];
$236 Set PARAMETERS before Subroutine call (APS will insert Subroutine call)
N[N]G99G84Z[ZB]R[ZR]F[F][CLT];
$----------------------------------------------------------------------------
BORING/REAMING/SPOT FACE etc - traverse to next hole at SAFE RAPID level [ZS]
$240 First Hole
N[N]G98G82X[AX]Y[AY]Z[ZB]R[ZR]P[DW]F[F][CLT]; ''CLT = Coolant Code
$241 Next holes
N[N]X[AX]Y[AY];
$242 Set PARAMETERS before Subroutine call (APS will insert Subroutine call)
N[N]G98G82Z[ZB]R[ZR]P[DW]F[F][CLT];
$----------------------------------------------------------------------------
BORING/REAMING/SPOT FACE etc - traverse to next hole at RETRACT level [ZS]
$244 First Hole
N[N]G99G82X[AX]Y[AY]Z[ZB]R[ZR]P[DW]F[F][CLT]; ''CLT = Coolant Code
$245 Next holes
N[N]X[AX]Y[AY];
$246 Set PARAMETERS before Subroutine call (APS will insert Subroutine call)
N[N]G99G82Z[ZB]R[ZR]P[DW]F[F][CLT];
$-------------------------- GENERAL FORMATS ---------------------------------
Separate modal values with spaces. More than one letter is OK eg X VX VY
$500 Modal Text (Will not be repeated in following lines)
G00 G01 G02 G03
$502 Modal ABSOLUTE Values (Will not be repeated if the VALUE is the same)
X Y Z F
$504 Modal INCREMENTAL Values (Will not be put into NC code if VALUE is ZERO)
I J
$510 X Y Z I J K values must have + as well as - signs (1 = Yes, 0 = no)
0
$515 Use point <.> as decimal separator (1 = Yes, 0 = use comma <,>)
1
$520 Put sub-routines at end of main program (1 = Yes, 0 = put at start)
1
$525 Quadrant Limit arcs (1 = Yes, 0 = Standard APS 180 degree limit)
0
$526 Output arcs as one move (1 = Yes, 0 = No - split arcs >= 180)
0
$527 Output HELICAL (XYZ) arcs as straight line segments (1 = Yes, 0 = No)
0
' 530 Determines which PLANAR arcs are output as straight line segments.
$530 0=None, 1=All, 2=All Except Horizontal (XY), 3=Except Horizontal and Vertical (YZ or XZ)
0
$531 Maximum Arc Radius - arcs will be output as straight lines if radius >
0
$532 If arcs are straight line segments, give chord error (mm or inches)
.1
$540 Suppress Operations List, START and Comments in NC code (1 = Yes, 0 = No)
1
'Set $560 - $580 all to 0 if machine is 3-axis.
$560 4/5 axis Programming point: (1 = pivot, 0 = tool tip)
0
$562 4/5 axis Tool C/L offset from pivot point in X
0
$563 4/5 axis Tool C/L offset from pivot point in Y
0
$565 4/5 axis Tool holder length
0
$570 4/5 axis Max angle (degrees). Set to 0 to indicate 3 - axis machine.
0
$580 Is this a horizontal machining centre (1 = Yes, 0 = No)
0
$582 Horizontal M/C. Select Work Plane BEFORE Tool Change (1 = yes, 0 = no)
0
$-------------------------- NUMBER FORMATS ----------------------------------
$700 SUBROUTINE Number format
6
$701 Leading figures
0
$702 Figures after point
0
$705 Subroutine start number
1
$----------------------------------------------------------------------------
$710 LINE NUMBER format
6
$711 Leading figures
0
$712 Figures after point
0
$715 Line start number
1
$716 Line number increment
1
$----------------------------------------------------------------------------
$720 X Y Z values format
2
$721 Leading figures
0
$722 Figures after point
3
$----------------------------------------------------------------------------
$730 ARC centre/radius format
2
$731 Leading figures
0
$732 Figures after point
3
$----------------------------------------------------------------------------
$740 SPINDLE SPEED format
6
$741 Leading figures
0
$742 Figures after point
0
$743 Maximum Spindle Speed
15000
$744 Fixed Speeds (eg 100, 200, 1000, 2000 ... 0 = speed is variable)
0
$NOTE: Fixed speeds can use more than one line. 80 chars per line maximum
APS will select the nearest lower value to the calculated value.
$745 below only applies if $744 is 0 - ie variable speed range.
$745 Round Speed Up/Down to Nearest: (.1 or 1 or 10 ... 0 = don't round)
100
$----------------------------------------------------------------------------
$750 MACHINING FEED format
6
$751 Leading figures
0
$752 Figures after point
0
$753 Maximum Feed Rate (Use mm/min or in/min. APS will convert)
3000 mm/min
$755 Round Feed Up/Down to Nearest: (.1 or 1 or 10 ... 0 = don't round)
10
$----------------------------------------------------------------------------
$760 TOOL NUMBER format
10
$761 Leading figures
2
$762 Figures after point
0
$------------------------ RAPIDS and TOOL CHANGE TIMES ----------------------
Put mm/min or in/min. AlphaCAM will convert
$900 XY Rapid Speed
1500 mm/min
$901 Z Rapid Speed
1500 mm/min
$902 Time to change tool (seconds)
10
$--------------------------- USER VARIABLES ---------------------------------
ALL user variables must be declared. Variable names can be up to 20 chars.
Prompts can be up to 50 chars max and can include a default inside < >.
Put (" ") as format for a text variable. Put ( ) as the format of any numeric
variable which is to have the same format as X Y (Z) moves. If a different
format is required, put (Format, Lead figs, Trail figs) eg (6,0,0) = Integer.
$1000 VARIABLE (format) " rompt <default>" '' Remark for your info.
PROGNUM (7,4,0) "程序号码" ''Integer with up to 4 lead zeros
MY_NAME (" ") "rogrammer <J Smith>" ''Text - free format
DATE ("9") ''DATE only (not Time) required
SAFE_Z ( ) "Safe Z Level <40>" ''Output with same format as X Y moves
HEAD (6,0,0) "New Head Number" ''Normal Integer
WEIGHT ( ) ''No prompt - only used in calculations
DENSITY ( ) "Density Kg/cu M <7800>"
THICKNESS ( ) "Material Thickness"
OPMSG (" ") "Operator Message <this is a msg>"
INDEX (" ") = "M57 'Index Pallet" '' = means initial value (not prompt)
HOLE_DEPTH ( ) "Hole DEPTH"
DWELL (6,0,0) "DWELL Time (sec) <1>" ''Default value 1 will be in dialog box
DRILL_FEED (6,0,0) "Drill FEED" ''Normal Integer
DRILL_DIAM ( ) "Drill Diameter" ''Free format - any number accepted
DRILL_SPEED (6,0,0) ''Normal Integer
TOOL_NUM (7,2,0) "Tool Number T" ''Integer with up to 2 leading zeros
TOOL_DIAM ( ) "Tool DIAM" ''Free format - any number accepted
END_DEPTH ( ) "End Depth for Ramp"
SAFE_Z_RAPID ( ) "Safe Z Rapid Height <50>"
RAP_DOWN ( ) "Rapid Down To <5>"
FEED_DOWN ( ) "Feed Down To <-10>"
PITCH ( ) "itch <2>"
CUT_FEED (6,0,0) "Cut FEED" ''Normal Integer
XSTART ()
YSTART ()
ARC_XCEN ()
ARC_YCEN ()
XDIFF ()
YDIFF ()
COSINE ()
SINE ()
FRACTION ()
ANGLE ()
TOOL (8,4,0)
$-------------------------- USER PRE-DEFINED CODE -------------------------------
This section applies only to TOOLPATHS (not geometries). Any $number in the
range $1100 - $1149 can be used for each definition. First line after $number
appears in the first dialog box. Next lines up to $ line are variables with
prompts (which must be declared in $1000) which are to appear in second dialog
box. Lines up to next $ line will be added or inserted on any toolpath.
$1100
Operator Message
OPMSG
$ ------------------------- NC lines to be entered into program follow
N[N]([OPMSG]);
$ ------------------------- ends $1100 user defined code
$1101
Index Pallet
$ ------------------------- NC lines to be entered into program follow
N[N]M05;
N[N][INDEX];
$ ------------------------- ends $1101 user defined code
$1102 Calculate Parts Weight
Weight of Parts
DENSITY
THICKNESS
$ ------------------------- NC lines to be entered into program follow
$LET WEIGHT = THICKNESS * AR * DENSITY / 1e9
N[N]( Parts Weight is [WEIGHT] kg)
$ ------------------------- ends $1102 user defined code
$-------------------------- USER DEFINED CYCLES -------------------------------
This section applies only to GEOMETRIES (not toolpaths). Use for machine or
work specific NC code (eg canned cycles) which require geometry coordinates.
Any $number in the range $1200 - $1249 can be used for each definition. First
line after $number appears in the first dialog box. Next lines up to first $
are variables with prompts (which must be declared in $1000) which are to
appear in second dialog box. Lines up to next $ line will be added at the end
of NC program so far created.
$1200 This asks for one hole only ''This is a Post remark only
Single Hole Drill + Dwell
SAFE_Z '') These variables will be asked
HOLE_DEPTH '') for in the second dialog box.
DWELL '') All must be declared in $1000.
$ ------------------------- NC lines to be entered into program follow
$SELECT_TOOL
'' Tool dialog box provides Tool Number T, Tool Diam TD, Tool Length TL,
'' Offset OFS, Feed Down FD, Feed Cut FC and Spindle Speed S
T=[T] TD=[TD] TL=[TL] OFS=[OFS] FD=[FD] FC=[FC] S=[S]
$PICK_CIRCLE Pick One Circle '' Pick One Circle will appear on bottom line
N[N](DRILL WITH DWELL: DRILL DIAM = [TD]; ''[TD] is extracted from tool dialog box
N[N]S[S]; ''[S] is extracted from tool dialog box
N[N]G01Z[SAFE_Z];
N[N]X[XC]Y[YC];
N[N]G01Z[HOLE_DEPTH]F[FD]; ''[FD] is extracted from tool dialog box
N[N]G04X[DWELL];
N[N]G00Z[SAFE_Z];
$ ------------------------- ends $1200 user defined cycle
$1201 This uses $GOTO and LABELS
Multiple Drill + Dwell
SAFE_Z
HOLE_DEPTH
DWELL
$ ------------------------- NC lines to be entered into program follow
$SELECT_TOOL
N[N](MULTI DRILL WITH DWELL: DRILL DIAM = [TD]; DWELL = [dwell])
'' Any lines which are above the $PICK line will be added
'' to the NC code one time only for the complete section
$PICK_CIRCLES Drill + Dwell ''Drill + Dwell appears on bottom line
$IF RAD >= TD/2 GOTO 1 ''13 Mar 94: Cannot use $IF or $LET with APS variables yet
$MSG Drill is too big for hole
$GOTO 99
$LL 1
N[N]G00Z[SAFE_Z];
N[N]X[XC]Y[YC];
N[N]G01Z[HOLE_DEPTH]F[FD];
N[N]G04X[DWELL];
$LL 99
$END_PICK
N[N]G00Z[SAFE_Z];
$ ------------------------- ends $1201 user defined cycle
$1205 This uses $IF / $ELSE / $ENDIF
Ramp Down Along Lines
$MSG
This ramps tool down from zero to
given depth along selected lines.
$
SAFE_Z
END_DEPTH
$ ------------------------- NC lines to be entered into program follow
$SELECT_TOOL
$PICK_LINES ''No prompt, so $PICK_LINES appears on bottom line
$IF LEN < TD
$MSG Line is too short for this tool
$ELSE
N[N]G00Z[SAFE_Z];
N[N]X[X1]Y[Y1];
N[N]Z[TD/10];
N[N]G01Z0.0F[FD];
N[N]G01X[X2]Y[Y2]Z[END_DEPTH]F[FC];
$ENDIF
$END_PICK
N[N]G00Z[SAFE_Z];
$ ------------------------- ends $1205 user defined cycle
$1206
Helical Milling 1 Pitch
SAFE_Z_RAPID
RAP_DOWN
FEED_DOWN
PITCH
$ ------------------- NC CODE STARTS HERE
$SELECT_TOOL
G00 Z[SAFE_Z_RAPID]
$PICK_CIRCLES SELECT CIRCLES FOR THREADING
$IF I_O = 1 GOTO 10 ''GHOST TOOL INSIDE
$IF I_O = -1 GOTO 20 ''GHOST TOOL OUTSIDE
$GOTO 99
$LL10 ''INTERNAL THREAD
$IF CW = 1 ''RIGHT HAND THREAD
N[N]G00X[XC]Y[YC];
N[N]G00Z[RAP_DOWN];
N[N]G01Z[FEED_DOWN]F[FC];
N[N]G01X[XC+(RAD-TD/2)*0.9]Y[YC+(RAD-TD/2)*0.1]F[FC];
N[N]G03X[XC]Y[YC+RAD-TD/2]Z[FEED_DOWN+PITCH/4]R[(RAD-TD/2)*0.9];
N[N]G03X[XC]Y[YC-RAD+TD/2]Z[FEED_DOWN+PITCH*0.75] R[RAD-TD/2];
N[N]G03X[XC]Y[YC+RAD-TD/2]Z[FEED_DOWN+PITCH*1.25] R[RAD-TD/2];
N[N]G03X[XC-(RAD-TD/2)*0.9]Y[YC+(RAD-TD/2)*0.1]Z[FEED_DOWN+PITCH*1.5]R[(RAD-TD/2)*0.9];
N[N]G00X[XC]Y[YC];
N[N]G00Z[SAFE_Z_RAPID];
$ELSEIF CW=0 ''LEFT HAND THREAD
N[N]G00X[XC]Y[YC];
N[N]G00Z[RAP_DOWN];
N[N]G01Z[FEED_DOWN]F[FC];
N[N]G01X[XC-(RAD-TD/2)*0.9]Y[YC+(RAD-TD/2)*0.1]F[FC];
N[N]G02X[XC]Y[YC+RAD-TD/2]Z[FEED_DOWN+PITCH/4]R[(RAD-TD/2)*0.9];
N[N]G02X[XC]Y[YC-RAD+TD/2]Z[FEED_DOWN+PITCH*0.75]R[RAD-TD/2];
N[N]G02X[XC]Y[YC+RAD-TD/2]Z[FEED_DOWN+PITCH*1.25]R[RAD-TD/2];
N[N]G02X[XC+(RAD-TD/2)*0.9]Y[YC+(RAD-TD/2)*0.1]Z[FEED_DOWN+PITCH*1.5]R[(RAD-TD/2)*0.9];
N[N]G00X[XC]Y[YC];
N[N]G00Z[SAFE_Z_RAPID];
$ENDIF
$GOTO 100
$LL20 ''EXTERNAL THREADS
$IF CW=1 ''RIGHT HAND THREAD
N[N]G00X[XC+(RAD+TD/2)*0.1]Y[YC+(RAD+TD/2)*1.1];
N[N]G00Z[RAP_DOWN];
N[N]G01Z[FEED_DOWN]F[FC];
N[N]G02X[XC]Y[YC+RAD+TD/2]R[(RAD+TD/2)*0.1];
N[N]G02X[XC]Y[YC-RAD-TD/2]Z[FEED_DOWN+PITCH*0.5]R[RAD+TD/2];
N[N]G02X[XC]Y[YC+RAD+TD/2]Z[FEED_DOWN+PITCH]R[RAD+TD/2];
N[N]G02X[XC-(RAD+TD/2)*0.1]Y[YC+(RAD+TD/2)*1.1]R[(RAD+TD/2)*0.1];
N[N]G00Z[SAFE_Z_RAPID];
$ELSEIF CW=0 ''LEFT HAND THREAD
N[N]G00X[XC-(RAD+TD/2)*0.1]Y[YC+(RAD+TD/2)*1.1];
N[N]G00Z[RAP_DOWN];
N[N]G01Z[FEED_DOWN]F[FC];
N[N]G03X[XC]Y[YC+RAD+TD/2]R[(RAD+TD/2)*0.1];
N[N]G03X[XC]Y[YC-RAD-TD/2]Z[FEED_DOWN+PITCH*0.5]R[RAD+TD/2];
N[N]G03X[XC]Y[YC+RAD+TD/2]Z[FEED_DOWN+PITCH]R[RAD+TD/2];
N[N]G03X[XC+(RAD+TD/2)*0.1]Y[YC+(RAD+TD/2)*1.1]R[(RAD+TD/2)*0.1];
N[N]G00Z[SAFE_Z_RAPID];
$ENDIF
$GOTO 100
$LL99
$MSG TOOL DIRECTION MUST BE INSIDE OR OUTSIDE
$LL100
$END_PICK
$ ------------------------- ends $1206 user defined cycle
$1208
Circle with MAHO G43 Lead-In
SAFE_Z_RAPID
RAP_DOWN
HOLE_DEPTH
$ ------------------------- NC lines to be entered into program follow
(MAHO CIRCLE)
$SELECT_TOOL
'' Tool dialog box provides Tool Number T, Tool Diam TD, Tool Length TL,
'' Offset OFS, Feed Down FD, Feed Cut FC and Spindle Speed S
T=[T] TD=[TD] TL=[TL] OFS=[OFS] FD=[FD] FC=[FC] S=[S]
$PICK_CIRCLES "ick Circles for MAHO G43"
N[N](CENTRE = [XC], [YC]);
N[N](CW = [CW], RAD = [RAD]);
$LET FRACTION = .8
$IF CW = 1
$LET ANGLE = 30.
$ELSE
$LET ANGLE = -30.
$ENDIF
$LET COSINE = COS(ANGLE)
$LET SINE = SIN(ANGLE)
$LET ARC_XCEN = XC + (X1 - XC) * (1. - FRACTION)
$LET ARC_YCEN = YC + (Y1 - YC) * (1. - FRACTION)
$LET XDIFF = X1 - ARC_XCEN
$LET YDIFF = Y1 - ARC_YCEN
$LET XSTART = ARC_XCEN + XDIFF * COSINE - YDIFF * SINE
$LET YSTART = ARC_YCEN + XDIFF * SINE + YDIFF * COSINE
N[N]G00 Z[SAFE_Z_RAPID];
N[N]X[ARC_XCEN]Y[ARC_YCEN];
N[N]Z[RAP_DOWN];
N[N]G01Z[HOLE_DEPTH]F[FD];
N[N]G01G43X[XSTART]Y[YSTART]F[FC]S[S];
$IF CW = 1
N[N]G02G42X[X1]Y[Y1]R[RAD * FRACTION];
N[N]G02X[XC + XC - X1]Y[YC + YC - Y1]R[RAD];
N[N]G02X[X1]Y[Y1]R[RAD];
$ELSE
N[N]G03G41X[X1]Y[Y1]R[RAD * FRACTION];
N[N]G03X[XC + XC - X1]Y[YC + YC - Y1]R[RAD];
N[N]G03X[X1]Y[Y1]R[RAD];
$ENDIF
N[N]G40;
N[N]G02X[ARC_XCEN]Y[ARC_YCEN]R[(RAD * FRACTION)/2];
N[N]G00Z[SAFE_Z_RAPID];
$END_PICK
$CANCEL_TOOL
'' $CANCEL_TOOL forces APS to display tool and Feeds/Speeds dialog box
'' even the tool is the same as the previous tool used.
$ ------------------------- ends $1208 user defined cycle
$ ---------------------- End of Post |
发表于 2003-12-7 01:19:01
QQ好友和群
QQ空间
腾讯微博
腾讯朋友
收藏
淘帖
赞一下！
发表于 2003-12-7 01:21:06
发表于 2003-12-9 01:44:08
发表于 2003-12-9 20:59:35
