1. In the CAM Plan Manager, right-click on Operations, select Insert and the select the 3 axis milling operation from the form provided.  The operation will be added to the manager tree.
    

2. Select Parameters under the operation you just added and set the parameters using the definition form provided.  Pick Accept when you are done.  Each 3 axis operation uses a unique definition form.  They are shown below under each operation type.  See 3 Axis Milling Operation Form Parameters for a definition of each parameter.
   
   Notice that (undefined) is shown next to Features under the 3 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 3 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.

 

 

 

The 3 axis spiral cut operation is an area clearance technique which cuts any number of trimmed surfaces or solids using any number of closed boundaries to enclose the cutting motion. The tool advances at each depth by proceeding toward or away from part boundaries.

 

Sample Spiral Cut Operation (3-Axis)

 

 

 

The 3 axis zigzag cut operation is an area clearance technique which cuts any number of trimmed surfaces or solids using any number of closed boundaries to enclose the cutting motion. The tool advances at each depth through a sequence of parallel cuts, reversing the tool direction at the end of each cut.

 

Sample Zigzag Cut Operation (3-Axis)

 

 

 

The map cut operation cuts any number of trimmed surfaces or solids. The cutting motion proceeds in a series of parallel cuts in one or both directions. Cutting motion is limited by the extent of the part geometry.

 

No boundary is explicitly defined for this operation type.  When there is need for a part boundary the X, Y extent box of the part surfaces and/or solids are used.  See also 3 Axis Milling Operation Form Parameters for the "Top," "Bottom" and "Max Depth" parameters.

 

 

 

With the 3 axis 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 3 axis profile cut operation cuts any number of trimmed surfaces or solids using any number of open or closed curve boundaries to guide the tool centerline.

 

Sample Profile Cut Operation (3-Axis)

 

 

 

The 3 axis box cut operation is an area clearance technique, similar to 3-axis zigzag cut except the cuts are all in the same direction. The tool is lifted between each cut.

 

 

 

The side cut operation is a 2-1/2 axis tool motion controlled by depth of cut and surface or solid geometry. The tool can ramp from one depth down to the next and the cuts can be sorted based on cutting region or depth. This operation type relies, to some extent, on the same 2-1/2 axis milling techniques used in rough milling as well as the tool motion projection utility.

 

Sample Side Cut Operation

 

 

 

The iso cut operation uses the isolines (lines of constant U or V parameter value) of individual surfaces to guide the tool contact point. It is a 3 axis tool path which operates on one surface at a time. It can produce a very nice surface finish because it follows the surface "flow lines." However, it is NOT a gouge-free tool path.

 

 

 

With the Iso Parametric Cut operation the cutter contact paths follow the constant U or constant V parameter lines of the part surfaces.  This operation type can quickly provide efficient and smooth tool motion which can be difficult to achieve using any other tool control methods.  Because tool contact and path control comes directly from the surfaces, the tool is usually well placed even on near-horizontal and near-vertical part shapes.

 

A trade off is that there are a number of current limitations:

 

• This is NOT a gouge-free tool path.  Gouges or collisions will result if the tool cannot fit within the convex regions of the part surfaces or if other setup geometry encroaches on the resultant tool path.  Care should be taken in the definition of lead-in and lead-out definitions that those moves do not cause problems.
   

• Adjoining surfaces should meet in a near tangential condition.  Part surfaces should be selected in "continuous chains" and the tool path will determine the best parameter location and direction to follow when moving the tool between surfaces.  The tool path will not be able to continue a cut if the "next" surface in the sequence cannot be reached along the direction of the current cutting isoline.
   

• This is a Semi-finishing or finish tool path.  There is no internal tracking of stock and while cutting, the tool may collide with nearby stock.
   

• Surfaces should not be trimmed, or they should only be trimmed along iso-parametric lines.  Trimmed holes are ignored and surfaces that meet along a trimmed boundary will not be connected for cutting.
   

There are other functional limitations which may change over time:

 

• Cut density is only controlled by the number of cuts you request.
   

• If part surfaces are close and their edges match (within tolerance) the tool path operation will attempt to move through those shared edges.  That is, greater priority will be given to cutting over adjacent surfaces than to following the Cut Order setting on the Parameters form.
   

• Isolated surfaces (surfaces which are separated by position or only meet other part surfaces on sides which cannot be reached by following a consistent cut direction on adjacent surfaces) will always follow the Cut Order setting on the Parameters form.
   

• If  a group of part surfaces form a closed loop, the first surface to appear in that group will become the start or end surface for all cuts.  If part surface groups are open, all cutting will begin at one of the open ends (determined by the Cutting Mode parameter).  For example, to cut a sequence of part surfaces which are open, the Surface Feature can be defined with a Window Pick.  To cut a sequence of part surfaces which form a closed loop, the Surface Feature can be defined by picking the starting surface first and then Window Picking the remaining surfaces.

 

 

General Notes

 

• All surfaces in the Surface Feature Set are cut.  There should be no duplicate surfaces in the Surface Feature.  

• Since this operation attempts to determine how surface edges should be shared, confusion will result if more than two surfaces meet at a common (shared) edge.  

• If the Surface Tolerance specified is large (amounting to a significant fraction of the lengths of some surfaces) the edge matching algorithm may have difficulty in automatically sequencing the surfaces for cutting.

 

 

Cutting Parameter Notes

 

• Frame - Same as all other Operations.

• Speeds, Feeds - Same as all other Operations.

• Surface Tol - Same as all other Operations.

• Surface Thick - Applied normal to the part surfaces – Same as all other Operations.

• Step Type - Only “Number of Cuts”

• Step Value - 1=down center, 2=on edges, 3 or more includes edges with the additional cuts equally spaced.

• Cutting Mode - (Climb, Conventional) this setting and [ Tool ] [ Properties ] [ Tool Dirn ] determines the direction of the first cut in each region.

• Cut Pattern - (One way, Zig Zag), Same as all other Operations.

• Cut Order (Top to Bottom, Bottom to Top) - First cut in each region will be the highest or the lowest in that region.  Changing this setting will reverse the entire cut sequence in each cutting region.

• Top Limit % - Fraction of surface width used to bound high Side of tool path.

• Bottom Limit % - Fraction of surface width used to bound low Side of tool path.  (Sum of Top Limit % and Bottom Limit % must be >= 0%  and < 100% )

• Leads and Links - Between all cuts, tool path motions of less than the tool radius are connected with straight linear motions at the cutting Feed Rate.  Longer gaps use the Long Link values.

• The 3X Iso-parametric Operation type does not support Short links.

• Display - Same as all other Operations.

 

 

 

 

The peeling cut operation combines 2-1/2 axis motion in steep areas on the part and 3-axis motion in less steep regions. This improves machining efficiency and surface finish. You have complete control over the cutting pattern for the 3 axis motion.

 

The cutting can be limited to just the steep areas, the less steep areas, or both in one tool path. This operation relies, to some extent, on the same 2-1/2 axis milling techniques used in rough milling as well as the tool motion projection utility.

 

 

 

The rest cut operation removes material remaining after previous milling operations. This can be convenient and quicker (relying on a reference tool and surface analysis) or slower and more precise (relying on a reference operation and solid verification).

 

The precise technique allows rest milling to account for remaining stock after any number of milling operations by utilizing the work piece modeling capabilities obtained from verification.

 

This operation utilizes the same tool motion projector as other 3-axis operations. The rest mill path can use either a reference tool for cleanup, or a reference operation (after solid verification) to determine the regions with remaining material.

 

 

 

The pencil trace operation removes material in creases and tight curvature regions on the part. This is useful for both cleanup and from relieving material near steep surfaces in preparation for other milling operations. It utilizes the same tool motion projector as the other 3 axis operations do.

 

This operation utilizes the same tool motion projector as other 3-axis operations. The rest mill path can use either a reference tool for cleanup, or a reference operation (after solid verification) to determine the regions with remaining material.

 

Sample Pencil Trace Operation

 

 

 

The scallop removal operation is a 3 axis tool path that requires the input of either a map cut or a side cut reference operation. The reference operation is specified by selecting RefOprn from the Mill Tactic Operations Form and selecting the appropriate map cut or side cut operation.

 

The direction of the reference operation's cuts and surface steepness are used to determine regions which will need more machining. The regions and then the new tool path are computed. This operation can use a different tool than the reference operation. This operation relies, to some extent, on the same 2-1/2 axis milling techniques used in rough milling as well as the tool motion projection utility.

 

 

 

This is a 3 axis surface engraving operation (i.e., characters on parts). The input requirements for this operation are the surface part and the engraving characters. All of the input characters are considered as tool ON conditions.

 

 

 

• As with all operations involving surfaces, care should be taken to ensure the correct side of the surface to machine is either set in modeling (test by shading) or in the CAM surface feature set. Since solids always have the normal directed outward, this need not be set for CAM components containing solids or in CAM solid feature solid sets.
   

• 3 axis operations rely on controlling the tool center by computing a motion sequence and then projecting those motions onto the part geometry. This utility is powerful and relatively quick. It is especially useful for semi-finishing and finishing operations. It is not as effective working parallel to steep regions on the part.
   

• 3 axis operations rely on a CAM profile feature or stock geometry to help limit and direct the cutter motion over the part geometry. The mapcut operation uses the part extents to determine the region to cut. If it is not possible for the tool to contact the part while following the profile, no tool motion is generated through that region (unless a "bottom" Z is specified in the operation's definition form).  See 3 Axis Milling Operation Form Parameters for more about the parameters for each operation.
   

• With 3 Axis milling operations you can generate tool paths from open surface boundaries or silhouettes. Here are the conditions:
   

1. If there are no profiles added in the operation feature list, the system calculates profiles from the open surface boundaries.

2. If #1 above fails, the system tries to calculate surface silhouettes to generate the profiles.

3. The system will only use user specified profiles if any.

4. For 3 Axis Profile Cut and Surface Engraving, you must define profiles.