(CAM Manager) Operations 
2X
Mill (CAM Level)
2-1/2 axis milling operations include standard
path configurations such as spiral, box and zigzag as well as contour
and profile cuts. Geometry
for these tool paths can include CAM pocket, step, slot and profile features.
2-1/2 axis milling operations can also have containment features
assigned to them. The
clearance for containment surfaces is only determined by their feature
offset.
Since CAM profile features do not have a depth attribute, only one pass will be made unless the top and bottom of the stock specified on the Stock and Depth of Cut tab of the operation definition form (Opdef).
These tool path operations use the following:
Frames, speeds and feeds
Explicitly defined engage and retract macros or automatic engage and retract motions
Boundary and island cleanup and predefined access holes
Flexible step-over and depth of cut controls
Implicit stock definition using offsets
Any number of islands of varying depth and draft are allowed
How
to Define 2-1/2 Axis Milling Operations
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.
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.
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.
Spiral
Cut Operation (2-1/2 Axis)
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)
Box
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)
ZigZag
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)
Contour
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.
Profile
Cut Operation (2-1/2 Axis)
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)
Chamfer
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)
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.
