1. In the CAM Plan Manager, right-click on Operations, select Insert and then select the 2-1/2 axis milling operation from the form provided.  The operation will be added to the manager tree.
    

2. In the manager tree, select Parameters under the operation you just added and set them using the definition form provided.  Pick Accept when you are done.  Each 2-1/2 axis operation uses a unique definition form.  They are shown below under each operation type.  See 2-1/2 Axis Milling Operation Form Parameters for a definition of each parameter.
   
   Notice that (undefined) is shown next to Features under the 2-1/2 axis operation you just added.  This means that no features are yet defined for the operation.

 

3. Your CAM features (once you define them) are listed under the Geometry section of the manager tree.  Under Geometry, find the CAM component (i.e., part : name) and expand it (i.e., select to the left of the part) to list the CAM features currently defined for that component and select one.  It will now be listed under Features for the 2-1/2 axis operation you just created. The (undefined) flag will be removed.  
   
   To create a new CAM feature: Again, under Geometry right-click on the CAM component, select Add Feature and follow the forms and prompts.  You will be prompted to select geometry from the graphics window.

 

 

 

During 2-1/2 axis milling operations the tool will move at the rapid feed rate between milling areas (on air) with lifting.  Only regions where part material exists will the tool cut at the cutting feed rate.  The offset of part material is controlled by the Horizontal Clear parameter.

 

To apply this functionality, you need to add CAM surface features (not solid) defining the part material regions in additional to the path boundaries.  If no CAM surface feature is selected, all areas within the path boundaries will be cut with the cutting rates.

 

 

 

The spiral cut operation is a facing (area clearance) or pocketing technique, which advances the tool at each depth by proceeding toward or away from the part boundaries.

 

Sample Spiral Cut Operation (2-1/2 Axis)
 

 

 

The box cut operation is a facing (area clearance) or pocketing technique, similar to the zigzag cut except the cuts are all in the same direction. The tool is lifted between each cut.

 

Sample Box Cut Operation (2-1/2 Axis)
 

 

 

The zigzag cut operation is a facing (area clearance) or pocketing technique. It advances the tool at each depth though a sequence of straight parallel cuts, reversing the tool direction at the end of each cut.

 

 

Sample ZigZag Cut Operation (2-1/2 Axis)
 

 

 

With the contour cut operation, a medial or spine curve is calculated for each cutting zone. Tool movement proceeds in cuts generated parallel or perpendicular to that curve.
 

 

 

The profile cut operation cuts any number of open or closed curve boundaries (CAM Profile features) or CAM Components containing geometry profiles. Self-intersecting profiles are also supported as long as the Tool Location parameter is set to "on boundary." See 2-1/2 Axis Milling Operation Form Parameters for a definition of each parameter.  This allows engraving operations or complex patterns to be machined without error.

 

Sample Profile Cut Operation (2-1/2 Axis)
 

 

 

The Chamfer Cut operation will accept profiles, curves, surfaces or chamfer features.  The chamfer feature provides control for Offset, Draft, Depth, Chamfer Side and Spine Curves.  Cutter Tip Control is provided on the Cutting Parameters Tab of the Chamfer Opdef form.  The form also provides Corner Control Parameters.  See 2-1/2 Axis Milling Operation Form Parameters for a definition of each parameter.

 

 

Sample Profile Cut Operation (2-1/2 Axis)
 

 

 

Use the Helical Cut operation to machine male and female threads.  Cutting parameters include Pitch, Direction, Cut Order, Tolerance, Depth Thickness, Radial Thickness, Start Angle, Number of Passes and Step Distance.  

 

Path Control parameters are also available sand include Collision Checking, Return Level, Approach Distance, Engage and Retract Arc Radius % as well as Cutter Compensation.

 

See 2-1/2 Axis Milling Operation Form Parameters for a definition of each parameter.

 

 

 

 

 

The toolpath created by the Ramp Cut operation is similar to the toolpath created by Helical Cut operation for a hole feature.  However, the features used in Ramp Cut are general profiles and/or pocket features similarly used in other 2-1/2 Axis operations.

 

The Ramp Angle parameter (measured in degrees) is used as a tangent angle to control the toolpath.  Other parameters for this operation are similar to the Profile Cut operation.

 

The Profile Side (Left or Right) parameter is used to determine if the Ramp Cut toolpath is either on the left or right side of the feature profile.  The Cut Dir (Climb or Conventional) parameter determines the clockwise or counter-clockwise toolpath direction for closed profiles.  Open profile features are also supported.

 

Ramp Cut toolpaths start at the start point (Tool Home Start) and /or pre-drill point (Pre-Drill Points) similar to the Profile Cut operation.  The top plane is defined by the Top Point parameter.  Starting from the top plane, the toolpath then ramps down evenly as determined by the Ramp Angle until it reaches the bottom plane, defined by the Bottom Point parameter.

 

When the toolpath reaches the bottom plane, a line segment is created to reach bottom point (Tool Home End).  If this line segment is not the last segment of the base Profile Cut toolpath, which is created on the bottom plane, the Ramp Cut toolpath will continue (on the bottom plane) until it reaches the last point of the base toolpath.  The Side Cleanup parameter (if set to Yes) is used for a finish cut at the bottom plane.  Cutter Compensation is also available for this operation.  

 

See 2-1/2 Axis Milling Operation Form Parameters for a definition of each parameter.

 

 

 

 

 

• Note that any offset defined in the CAM Features for this operation will remain after all machining is completed. It will also be used in the ON boundary condition, in the TANTO, or PAST conditions. The following offsets would be added to the offset defined in the Feature.
   

• All 2-1/2 axis tool paths allow the subtypes "rest mill" and "clamp cleanup." In those cases a reference tool path should be selected ( ref oprn). If the subtype is set to "standard " the reference tool path will be ignored. In the case of "rest mill" the tool should be smaller than that used in the reference operation. For "clamp cleanup" the tool may be the same size or smaller than that used in the reference operation.
   

• This note may help to define cam features correctly and consistently for 2-1/2 axis milling operations with boundaries having islands. When machining 2D pockets with multiple cutting layers, islands defined from Cam Profiles assume infinite heights, so that no tool path can ignore them. Islands defined by any other cam feature remember their geometric heights. They will be ignored to obtain better and efficient cutting patterns if the current cutting z level is higher.