Your focus when operating the Expert NURBS Cutter will be entering values in the Knowledge Editor. The following list of Cycle Parameters is for reference when altering parameter defaults, or making additional Cycles.
 Enter Table Name........ mltpc
Table name. Can not be edited.
 Enter Item Name......... XNURBS_CUT-ZIGZAG_XZ
Cycle name. Editing name enables making of new Cycles.
 Cycle Type.......(MLTPC) MLTPC SCUT2
Defines the type of cutting cycle and should not be edited.
Reserved, do not edit.
 Vert/Horz/Flow/Proj Cut V
Enter V for Vertical cutting, H for Horizontal cutting, F for Flow cutting, and P for polyline projection cutting.
 Rough Z Cut Increment (#)
An entry in this parameter automatically enables roughing. The value entered controls the maximum cutting depth for each roughing pass.
A total of 6 roughing methods are available with the Expert NURBS Cutter. They are divided into two categories, Vertical and Horizontal.
Vertical Cutting + Mode 1 = Offsets each roughing pass by  "Rough Z Cut Increment" +  "Stock Amount to Leave", moving in rapid when machine motions exceed  "Working Area Z Maximum".
Vertical Cutting + Mode 2 = Offsets each roughing pass by  "Rough Z Cut Increment" +  "Stock Amount to Leave", and proportionally distributes Z depth throughout the roughing activity without allowing tool to leave the stock material.
Vertical Cutting + Mode 3 = Shifts roughing motions in "Z" based on  "Rough Z Cut Increment" while compensating for  "Stock Amount to Leave", moving in rapid when machine motions exceed  "Working Area Z Maximum".
Horizontal Cutting + Mode 1 = Plunges straight down to each Z level, compensates for  "Stock Amount to Leave", roughs without following collective surface contours before proceeding to next lower Z level.
Horizontal Cutting + Mode 2 = Ramps down to each Z level, compensates for  "Stock Amount to Leave", roughs and makes a contour following pass before ramping down to next Z level.
Horizontal Cutting + Mode 3 = Plunges straight down to each Z level, compensates for  "Stock Amount to Leave", roughs and makes a contour following pass before plunging straight down to next Z level.
Y enables intersect cutting. Intersect cutting can be applied to all surface intersections in a drawing, or applied only to the intersections of selected sets of surfaces. If the surface drawing has already been defined to the system by previously making toolpath (a.GEO already exists), respond YES to the "Define Surfaces" prompt. You are then prompted "Group Surfaces into Sets?".
1. If your objective is to apply surface intersect toolpath on all surface intersections in the drawing, you should respond NO, and select all surfaces in the drawing when prompted to select objects.
2. If your objective is to apply surface intersect toolpath on intersections of selective sets of surfaces, you should respond YES. You are then given the opportunity to "Select Surfaces in First Set" and "Select Surfaces in Second Set". The "First Set" will disappear from the screen when you have completed the selection process for user feedback.
3. Upon completion of selecting objects you are prompted to, "Specify Minimum Angle that Defines Intersection Deg:". Respond according to your requirements.
Y enables CrossCut. Cross cutting only applies to vertical finishing motions. Cutting motions are produced on any surface(s) area(s) that meet the angle criteria, in the direction of the cutting motions. You are prompted during "Cut" for surface(s) angle criteria.
Y enables Recut. Recut, sometimes referred to as rest cutting, removes material left by a prior operation or tool. In Vertical cutting mode (entry V in ), the system will prompt for information regarding previous tool used. Toolpath is then produced on all surface areas not cut by the prior tool. In Horizontal cutting mode (entry H in ), no prompt occurs regarding previous tool, and vertical toolpath is produced on all surface areas that are nearly horizontal where XY motions could not be generated.
Y enables Surface Containment. If the surface drawing has already been defined to the system by previously making toolpath (a .GEO file exists), respond YES, to the "Define Surfaces" prompt. You are prompted during "Cut", to select surfaces to cut, followed by selection of surfaces to use for toolpath containment. This feature is not available when cutting directly from a solid.
Y enables String Containment. If the surface drawing has already been defined to the system by previously making toolpath (a .GEO file exists), respond YES, to the "Define Surfaces" prompt. You are prompted during "Cut" to select surfaces to cut and to select 2-D polyline(s) to use to contain toolpath. The XY boundary of a single closed polyline will contain the toolpath limits.
Y enables Plunge points. Plunge points apply only to roughing. In the roughing mode the system will make every attempt to plunge at the defined plunge locations. You are prompted during "Cut" to define plunge points.
Parameters  through  are used to define a working area (clip box). Normal system operation requires that parameter  "Working Area Z Maximum", contains a value equal to the value entered in parameter  "Material Z Loc(#)". Entry of a value different than the entry in  "Material Z Loc.(#)", is used only under special conditions.
 Description.....("TEXT") "X-Nurbs Cutting, Zigzag XZ Plane"
Text string used to describe Cycle.
Requires entry of where the top of the stock material is located. Cycle start position uses this entry to calculate feed distance to material. Normal system operation requires that parameter  "Working Area Z Maximum", contains a value equal to the value entered in parameter  "Material Z Loc(#)".
 Stock Amount to Leave... 0.0 Y
The first entry controls the amount of stock to leave. The second entry "Y" (without the quotes), indicates that you would like multiple stock allowances. You are prompted during CUT to select surface(s) for different stock allowance, and you are then prompted for a value.
 Slice Step Dir (POS/NEG) POS
Determines whether vertical cutting motions begin at X or Y zero and proceed positive, or begin at X or Y maximum and proceed negative.
***IMPORTANT NOTE***<R>The determination for CONVENTIONAL or CLIMB milling is automatically made by designating a POS or NEG answer to this parameter when using Horizontal finishing, as long as there is no entry in Parameter CW Horz. Cuts....(Y/N). A POS answer results in CONVENTIONAL milling, a NEG answer results in CLIMB milling. An entry of Y or N in Parameter CW Horz. Cuts....(Y/N), will override the automatic computation.
 Constant Step Over Dist. !*tr*
This entry defines the fixed distance between cuts. This entry is overridden when  "Define Scallop Size" is enabled with a Y entry.
Y enables Scallop Height Control for Vertical finishing. You are prompted during "Cut" for desired scallop height. Enter the desired scallop height at that time. You are then prompted for minimum step size. Minimum step size is a clamp to protect from excessive toolpath on unusually steep surface areas. A response of .001 for Inch, or .01 for Metric, is appropriate in most cases. A response too large will circumvent scallop height calculation.
 Vertical Cutting Angle. 0.0
Defines angle of Vertical toolpath. 0.0 = XZ, 90 = YZ. Any angle between 0 and 90 is valid. Negative angles are allowed. This parameter entry works in conjunction with  "Slice Step Dir (POS/NEG).
 Lace Cutting Paths (Y/N) Y
Y enables lace or zigzag cutting motions in Vertical and Horizontal cutting. Enter N to achieve uni-directional cuts in Vertical cutting. Enter N to achieve continuous direction cutting when using Horizontal cutting.
 Fall Over Mode (0/1/2/3)
Fallover Mode settings accommodate special Vertical finishing situations. The system default is Fallover Mode 3. In Fallover Mode 3, vertical finishing toolpath ends at the extents of the selected surfaces. Fallover Mode 1 and 2 cause toolpath to roll over the extents of the selected surfaces by tool radius. Mode 2 stops at tool radius, Mode 1 continues down in Z to "Working Area Z Minimum". Fallover Mode 0 causes toolpath to roll over as in mode 1, but also move away from the surface by a distance equal to tool radius. Fallover Mode settings are managed by the system for normal operation.
 CW Horz. Cuts......(Y/N)
This parameter applies only to Horizontal finishing. The default is no entry. No entry allows the entry in Slice Step direction to automatically control CLIMB or CONVENTIONAL cutting. N forces counter clock wise cutting. Y forces clock wise cutting direction. CCW toolpath is RED and CW toolpath is GREEN.
Lace cutting set to Y will cause zigzag (back and forth) horizontal finishing motions. This is particularly useful when cutting single or open multiple surfaces. Lace cutting should be set to N for normal multiple surface finishing.
 Task @ Lead-In (name/N) TPC-FEED
 Task @ Cut Start (name/N) TPC-CUT
 Run Tasks in Slices(Y/N) Y
Parameters  through  follow normal Router-CIM convention.
Parameters  and  follow normal Router-CIM convention
 Complete NC Program(Y/N) Y 1234
Y enables Complete NC Program which causes Router-CIM to go directly to NC Code after producing toolpath. The numeric value entered represents the Job Id.
 STR/END Tasks for NC Prg
This parameter allows the use of Start/End Codes when "Complete NC Program(Y/N)" is enabled. Entry in this parameter to enable Start/End Codes is: PROCTSK1 PROCTSK2