//    ----------------------------------------
//    
//    The following SmartCAM code generator has been 
//    created to generate NC code for the respective 
//    machine and control combinations listed below. 
//    
//    Due to differences in programming styles, 
//    controller versions, and optional equipment, 
//    SmartCAMcnc DOES NOT and CANNOT guarantee
//    that the NC code generated is correct for any 
//    specific machine. Some modification to the code 
//    generator to match your setup and output 
//    requirements is likely necessary. 
//    
//    Modifications to code generators do not TYPICALLY
//    require a significant amount of time. SmartCAM 
//    customers with active SMA contracts are entitled 
//    to support for their code generators from the 
//    SmartCAMcnc Support Group. To contact them for 
//    support, please send an email to: 
//    Support@SmartCAMcnc.com. If you would like 
//    information on purchasing SMA for your SmartCAM 
//    products, please contact: Sales@SmartCAMcnc.com
//    
//    DISCLAIMER: It is the responsibility of the end 
//    user to confirm and verify that the NC code 
//    created by any code generator is accurate and 
//    will not cause a machine malfunction which 
//    could result in stock, tooling, machine, and/or 
//    personal injury. 
//    
//    SmartCAMcnc assumes no responsibility or 
//    liability for any damage caused or alleged to 
//    have been caused by the use of any of the code 
//    generators it provides.
//    ----------------------------------------

@COMMENTS

ALLIANT.NTS					10/19/89

Machine: Alliant RT 2V Vertical Milling Machine with
		 Anilam Crusader CNC Control

Machine File Name: ALLIANT.SMF

Template File Name: ALLIANT.TMP

Tape-to-Shape File Name: ALLIANT.TTS

Notes:

	1. This machine and template file have been set up to support the
	   following fixed cycles:

			G80 - Fixed Cycle Cancel
			G81 - Drill Cycle
			G82 - Spot Drill Cycle
			G83 - Peck Drill Cycle
			G86 - Tapping Cycle
			G85 - Boring Cycle


	2. Speeds in the Job Plan should be specified in revolutions 
	   per minute (RPM).  Feeds should be in inches per minute (IPM).
	   In order to produce code which will turn the spindle in a reverse
	   direction, type the spindle speed in Job Plan as a minus number.
     
	3. SmartCAM will automatically calculate the peck increment for each tool
	   to a value of 1/2 the diameter of the tool for all peck drilling
	   operations.  If you want to peck drill, remember to turn on the peck
	   drill hole operation ( Hole_Op - Peck_Drill) before creating the
	   Hole element and remember to specify the tool as a drill in Job Plan.

	4. SmartCAM will output all the necessary moves to turn cutter diameter
	   compensation on and off correctly (G40/G41/G42).  Any Profile in Shape
	   with an Offset of None needs no Lead_In or Lead_Out moves and will
	   produce code for the centerline of the toolpath.  No cutter compen-
	   sation codes will be output.  Any profile in Shape with either Offset
	   Right or Left will output code for the part profile rather than the
	   centerline of the toolpath and will output proper cutter compensation
	   commands.  If no Lead_In Lines are specified, SmartCam automatically
	   will add a perpendicular Lead_In Line equal to .050 greater than the
	   tool radius and start cutter compensation with this move.  In some
	   cases, this .050 movement may cause the tool to undercut another area
	   of the part.  This can easily be avoided using SmartCAM's Tool_Path
	   Lead_In and Lead_Out features, by creating a Lead_In Line of a smaller
	   amount.  If no Lead_Out Lines are specified, SmartCAM will retract the
	   tool in Z axis to the Z check plane or Z clearance plane (whichever is
	   greater) and then output a G40 in a block by itself to cancel cutter
	   compensation.  The operator may, at his option, specify Lead_In and
	   Lead_Out Lines to control the exact amount of movement used to turn on
	   and off cutter compensation.  Lead_In and Lead_Out Arcs may be used as
	   well.  The following procedure is recommended highly:
 
	5. If you wish to use Lead_In and Lead_Out Lines only, it is best to use
	   an Angle of 90 degrees and a Length greater than the tool radius.  If
	   you wish to use Lead_In and Lead_Out Arcs, it is best to use a Radius
	   equal to the same amount and an Angle of 45 degrees, then Lead_In
	   and Lead_Out Lines to those Arcs at an Angle of 90 degrees and a
	   length equal to the same amount.  Any time Lead_In and Lead_Out Arcs
	   are used, Lead_In and Lead_Out Lines are also recommended.
@START
%
#ONBLK G0 G40 G52 G70 G80 G90
 G29 T1001
 Z0 T0
 X#XPOS Y#YPOS
 T#TOOL

@TOOLCHG
< #FXD>
 G0 Z0 T0
 X#XPOS Y#YPOS
 T#TOOL

@END
< #FXD>
 G90
 G0 Z0 T0
 X#XHOME Y#YHOME
 G29 E
#OFFBLK%

@STPROF
< #ABSI>
< #FXD>
< #MOV>< X#XPOS>< Y#YPOS>

@ENDPROF
 #MOV Z#ZPOS
< #DCOMP>

@RAP
< #ABSI>
< #FXD>
< #MOV>< X#XPOS>< Y#YPOS>

@LINE
< #DCOMP>
< #MOV>< X#XPOS>< Y#YPOS>< Z#ZPOS>< F#FEED>

@ARC
 #MOV X#XPOS Y#YPOS I#XCTR J#YCTR< F#FEED>

@ZCLRMV
< #ABSI>
< #FXD>
< #MOV>< Z#ZPOS>

@ZCHKMV
< #FXD>
< #MOV>< Z#ZPOS>

@ZDPTHMV
< #MOV>< Z#ZPOS> F30.0#RESET(#FEED)

@FXD1
< #ABSI>
< G29 LV20=#FEED V21=#ZCHK
 #FXD>< X#XPOS>< Y#YPOS>< Z#ZDPTH>

@FXD2
< #ABSI>
< G29 LV20=#FEED V21=#ZCHK V22=#DWELL
 #FXD>< X#XPOS>< Y#YPOS>< Z#ZDPTH>

@FXD3
#EVAL(#V0=#ZCHK+.1)
< #ABSI>
< G29 LV20=#FEED V21=#V0
 #FXD>< X#XPOS>< Y#YPOS>< Z#ZDPTH>

@FXD4
< #ABSI>
< G29 LV20=#FEED V21=#ZCHK
 #FXD>< X#XPOS>< Y#YPOS>< Z#ZDPTH>

@FXD5
#EVAL(#PECK=#TLDIA/2)
< #ABSI>
< G29 LV20=#FEED V21=#ZCHK V23=#PECK
 #FXD>< X#XPOS>< Y#YPOS>< Z#ZDPTH>

@DWELL
 G04
@