The Spiral Cut Operation Definition Form shown below is typical for the 2-1/2 axis operations.  Each operation form contains parameters according to the matrix of operations shown above.

 

 

2-1/2 Axis Spiral Cut Operation Definition Form - Cutting Parameters Tab	2-1/2 Axis Spiral Cut Operation Definition Form - More Cutting Parameters Tab
2-1/2 Axis Spiral Cut Operation Definition Form - Lead and Link Parameters Tab	2-1/2 Axis Spiral Cut Operation Definition Form - Stock and Depth of Cut Parameters Tab
2-1/2 Axis Spiral Cut Operation Definition Form - Appearance Parameters Tab

 

 

 

Frames, Speeds and Feeds

 

• Frame - This sets the alternate coordinate system defined within the setup for this operation.

• Speeds Feeds - Pick this button to set the speed/feed values for this operation's tool motions using the CAM Speed Feed Manager Form.   The name of the operation is also displayed to the right.

 

 

Cutting

 

Concave Corner (Profile Cut)

This refers to motions that are inserted when the tool changes direction at a concave corner. Select from the following:

 

• Standard - Insert a simple change in tool direction.

• Tusk Cut - When stepover is greater than 50% of the tool diameter, insert a move to clear material between cuts.

• D Loop - Insert circular moves to turn the tool (away from part boundaries).

• Fillet - With this corner control option, two adjacent segments, (line, line), (line, arc), (arc, line), or (arc,arc), will be filleted with the current Step Size as its radius, if these two segments are not against a wall. If either of the two segments is too short for a fillet, the radius will be one half of the Step Size for two more tries.  If the two segments are connected smoothly enough, no fillet will be necessary.  Smother tool path can be created with this option.

 

ConvexCorner (Profile Cut)

This refers to motions that are inserted when the tool changes direction at a convex corner. Select from the following:

 

• Fillet - With this corner control option, two adjacent segments, (line, line), (line, arc), (arc, line), or (arc,arc), will be filleted with the current Step Size as its radius, if these two segments are not against a wall. If either of the two segments is too short for a fillet, the radius will be one half of the Step Size for two more tries.  If the two segments are connected smoothly enough, no fillet will be necessary.  Smother tool path can be created with this option.

• Extend Tangent - Extends the corners tangent.

• Extend/Round Sharp - Extend the corners but round the sharp corners.  A junction with a Convex Angle less than Min Convex Angle is considered a sharp corner.

• d Loop - Insert circular moves to turn the tool (away from part boundaries).

 

Corner Control (Spiral)

This refers to motions that are inserted when the tool changes direction. Select from the following:

 

• Standard - Insert a simple change in tool direction.

• Tusk Cut - When stepover is greater than 50% of the tool diameter, insert a move to clear material between cuts.

• D Loop - Insert circular moves to turn the tool (away from part boundaries).

• Fillet - With this corner control option, two adjacent segments, (line, line), (line, arc), (arc, line), or (arc,arc), will be filleted with the current Step Size as its radius, if these two segments are not against a wall. If either of the two segments is too short for a fillet, the radius will be one half of the Step Size for two more tries.  If the two segments are connected smoothly enough, no fillet will be necessary.  Smother tool path can be created with this option.

 

 

• Extend Tangent - Extends the corners tangent.

• Round Corner - TBD

 

Cut Direction

If "Auto Cut Dir" is set to "No," use this parameter to select a cut direction.  The right mouse button will bring up the standard direction input options menu.

 

Cut Direction (Contour Cut)

• Radial - Cuts are created perpendicular to the region's medial curve.

• Parallel - Cuts are created parallel to the region's medial curve.

 

Cut Direction (Spiral and Profile Cut)

This determines the direction of cut. Select from the following:

 

• Climb / Conventional - Utilize the tool object's "cut dirn" (direction) property.

• CW / CCW - For Spiralcut, CW and CCW are not well defined for open profiles. If the resulting tool path is not desired, change to "Climb" or "Conventional" and recalculate the path.

 

Cut Order

Select from the following:

 

• Level First - Remove all material at one level (Z depth) before proceeding to the next.

• Region First - Remove all material from one boundary region (all depths) before proceeding to the next region.  This is relevant only if there is more than one z level being machined.

 

Profile Side

For the Ramp Cut operation, this parameter is used to determine if the Ramp Cut toolpath is either on the Left or Right side of the feature profile.  

 

Ramp Angle

For the Ramp Cut operation, this parameter (measured in degrees) is used as a tangent angle to control the toolpath.

 

Region Connect

This refers to the method of transitioning the tool from one machining region to another.  If it is not possible to move the tool without lifting, it will be lifted to a safe height above the region plus Vertical Clear. Select Tool Lift or No Tool Lift.

 

Slow Down Distance

This is the distance at which to decrease the feed rate before any turn in the path.  The feed rate will return to the cutting feed rate at the first linear motion greater than the slowdown distance.  The slowdown distance is specified in the Speed/Feed Form for this operation.

 

Spiral Progress

Select from the following:

 

• Step Inward - Cuts begin by following the part boundaries.  Subsequent cuts are each offset by a greater amount determined by the stepover value.  Each offset is connected by a linear move where possible.

• Step Outward - The reverse of "Spiral Inward" with cuts progressing by smaller offsets toward the part boundaries.

• Spiral Inward - Cuts begin by following the part boundaries and subsequent cuts are the result of a continuously increasing offset from the part boundaries.

• Spiral Outward - The reverse of "Spiral Inward" with cuts continuously progressing toward the part boundaries.

• Air Access Inward - The cutter will not touch the stock during engage/retract motion.  This increases cutter life and improves machining results

 

Step Type

This is the spacing of adjacent cuts when more than one cut is indicated by "No. of Cuts."  Select from the following:

 

• Absolute - Use this distance.

• Scallop Height - Compute the spacing from the tool and this scallop height.

• % of Tool Diameter - Compute the spacing from this percentage and the tool diameter.

 

Step Value

Use this value in conjunction with Step Type to control adjacent cuts.

 

Tolerance

This is the chord height tolerance applied to curves to control the density of tool path points.

 

 

 

Path Control

 

Tool Location

This determines the location of the tool in relation to the part or island curves.  Select from the following:

 

• On Boundary - center of tool touches boundary curves

• Tangent to Boundary - outer side of tool touches boundary curves

• Past Boundary - inner side of tool touches boundary curves

• On Part, Tan Island - center of tool touches part, side of tool touches island curves

• Past Part, Tan Island - inner side of tool touches part, side of tool touches island curves

 

Note that the On conditions condition will cause several of the stock offsets to be ignored for those boundary elements.
 

Overhang

This is only used in combination with boundaries to be cut with the "past" conditions of the Tool Location parameter shown above. This percentage of the tool diameter is added to the past condition to force the tool even farther outside the boundary.
 

Side Cleanup (Ramp Cut)

This indicates if a final clean up pass should be made on the part boundaries. If this is "yes" then there will be two passes along the boundaries.

 

Side Cleanup (Spiral, ZigZag, Box, Contour, and Profile Cut)

This indicates if a final clean up pass should be made on the part boundaries.  Select from the following options:

 

• None

• Cut with Levels - If the length of the cutting tool flute is not long enough (i.e., shorter than depth of cut), this option will perform side cleanup cuts by level as defined by the Depth of Cut parameters.

• Single Finish Cut - Perform one single finish cut.

• Scallop Cleanup (Box, Contour Cut) - perform cleanup passes for scallops only.

• Retract and Scallop Cleanup (Box, Contour Cut) - retract the tool and then perform cleanup passes for scallops only.

 

Island Cleanup

This indicates whether a final clean up pass should be made on the island boundaries. If this is "yes" then there will be two passes along the island boundaries.
 

Island Top Cleanup

For multiple passes at different depths, this directs the tool to make a final pass at the top of each island to ensure all stock is removed.
 

Pre-drill Points, Holes

This indicates locations where drilling operations will create access holes prior to executing this tool path. All tool motion at each depth will utilize these access holes as appropriate. Right-click the mouse for the standard point input options menu.
 

Tool Home Start , Tool Home End - These fines the start point and end point for this tool path operation.  Right-click the mouse for the standard point input options menu.  The tool home start point and tool home end point will be independent to each other. If the points are below the safety plane (which is Vertical Clear above the Top Point), it will be lifted up to the safety plane. For Vertical Clear refer to Auto Engage/Retract section of the General Tab. For Top Point refer to the Stock Data section of the Stock and Depth Tab.
 

Start Points - This indicates preferred regions on the boundaries to begin cutting. These points need only be in the neighborhood of the desired start points, the closest point on the boundary will be where cutting begins.  Right-click the mouse for the standard point input options menu.

 

 

Cutter Compensation

 

Cutter Comp

This specifies whether or not to output Cutter Compensation statements when generating the active tool path.  Cutter Compensation records will be output for planar motion in the XY, YZ or ZX plane of the default setup.

 

You can also set Cutter Compensation for all operations generated for a particular machine by selecting Programming from the CAM Machine Manager.  Cutter compensation is supported for output using the Flexpost post-processor. You can modify the Flexpost configuration file "fanuc10.fp" if different G codes are needed.

 

Cutter Compensation statements have the following format:

 

CUTCOM/side,plane

Example: CUTCOM/LEFT,XYPLAN

 

Select from the following options:

 

• None - No cutter compensation

• Offset - Cutter diameter compensation only

• Radius Offset - This option activates a new function for radius offset compensation for the Profile Cut, Chamfer Cut, and Ramp Cut operations.  If this option is selected, the Tool Location parameter will be forced to Tangent to Boundary.
  
  The Radius Offset option creates two sets of toolpaths, one visible set for output and display purposes and another internal set for using in both wireframe and solid verification.

 

 

Macros

 

• Full Approach - Macro object for the first entry for cutting this operation.

• Partial Approach - Macro object for subsequent entries during this operation.

• Full Retract - Macro object for the final exit from cutting this operation.

• Partial Retract - Macro object for previous exits during this operation.

 

 

Auto Engage/Retract

 

If no approach or retract macros are defined, these parameters allow for the flexible creation of engage and retract motions.

 

The following icons specify the type of approach during the engage/retract motions in the cutting plane.  These options are in conjunction with other auto engage/retract parameters such as Engage Arc Radius.  Select from the following icons:

 

	Linear - This adds a linear approach.
	Linear, Linear - This adds a linear line (with horizontal clearance) onto the linear approach.
	Linear, Circular - This adds a linear line (with horizontal clearance) onto the circular approach.
	Circular - This adds a circular approach.
	Circular, Linear - The added motions will be perpendicular to the tangent vectors of the lead in and out motions.  The length of the line segment is controlled by the "Horizontal Clear" parameter.  It is a 90 degree arc defined by the Engage Arc Radius parameter.
	Circular, Linear, Linear - This will engage from a pre-drill point to the start of the line tangent to an arc that is in turn tangent to the tool path.  The retract motion will be in the opposite path.  This option requires Pre-Drill Holes (refer to the Cutting tab below).
	Circular, Slope - This will engage from a pre-drill point to the start of an arc which is tangent to the tool path.  The retract motion will be in the opposite path.  This option requires Pre-Drill Holes (refer to the Cutting tab below).
	None - No approach during engage/retract motions is added.

 

Safe Dist (E1) and (E2)

These values are added to the clearance that is automatically detected to avoid hitting stock. This distance is applied after cutting and before linking/re-linking moves. You can specify a minimum safe distance to avoid any collisions.  Based on part geometry, it will determine the length of moves before linking the tool path for next cut.  E2 is used for two engage motions in the Linear - Linear Automatic engage and retract option.

 

Safe Dist (R1) and (R2)

R1 and R2 provides more user control on Linear - Linear Automatic engage and retract option.  R1 and R2 specify two Retract motions.

 

Engage Arc Radius

This specifies the engage arc radius. Use only when Engage, Retract (see above) is set to Circular or Circular, Linear.

 

Engage Overlap

This is a re-cut distance to obtain a smooth part surface when cutting closed loops along the part boundary.  One half of this distance is added at the beginning of the cut at the engage feed rate. The other half is added at the end of the cut at the retract feed rate.

 

Activation Range

Ordinarily, when the tool moves to an adjacent cut, it follows a straight path.  If an activation range is specified, auto-engage/retract sequences will be inserted for each cut within this range of the part's boundaries to ensure a good part finish.

 

Slop Angle

This parameter specifies the slop angle during the Circular - Slop Automatic engage and retract option.

 

 

Others

 

Traverse Type

In all traversals (except straight), the tool will take the shortest 2 axis move toward the next starting point. If that move is interrupted by part boundaries, the boundary will be followed to prevent gouging of the part.  The Horizontal Clear (see above) is added to the boundary to ensure that the tool does not contact the part.  Select from the following:

 

• Previous Plane - When moving the tool (but not cutting), move at the depth of the just-cut region plus Vertical Clear (see below).

• Clearance Plane - Always lift to the clearance plane of the setup.

• Traverse Straight - Vector directly to the start of the next cut. This is the only option can gouge the part.

• Blank Plane - Lift the tool to the top of the current region plus Vertical Clear (see below).

 

Vertical Clear

This is a safety lift distance (above the Top Point) for inter-cut moves. This Vertical Clear parameter and the Top Point parameter (see Stock and Depth Tab - Stock Data) together define the "safety plane."

 

Horizontal Clear

This is a safety gap around part boundaries for inter-cut moves.  This parameter is defined differently depending on the type (icon) of Auto Engage/Retract motion is selected.  See below.

 

Clamp and Table components are assigned the Horizontal Clear distance during toolpath operations to avoid tool breakage from collisions.

 

 

Plunge Type

Use this parameter to set the type of engage plunge motion.  Select from:

 

• Automatic - Plunge type is determined automatically

• Ramp - The plunge will ramp to the Vertical Clear distance.

• Straight - Use this to specify a straight plunge motion.

 

 

 

Depth of Cut

 

• Type
  
  Uniform Depth - This uses the maximum depth of cut for all depths, measured from the top of the region (see Stock Data below).
  Non-Uniform - This uses First Zcut (see below) for the first cut, Last Zcut above the lowest point in the region and then divides the region between evenly for the remaining depths of cut.
  Base Only - One pass is made at the lowest depth for the region.
  Base & Island Top - Like Base Only, but it also creates a cut at the top of each island.
  Island Top - This makes a cut at the depth of each island top.
   

• Max - This is the standard depth of cut used for determining the Z height of cuts.

• Min - Cuts will not be made closer than this depth apart, unless cuts are being placed at the depths of island tops.

• First Zcut - This is for non-uniform depths only, at top of the region.

• Last Zcut - This is for non-uniform depths only, at bottom of the region.

 

 

Stock Data

 

Use these parameters to define cutting depths.  If the CAM feature has its own depth (e.g., step, slot or pocket), and stock parameters are also defined, the top from the stock data will be used. The bottom will be the higher value between the stock bottom and the feature's actual bottom.

 

• Rough Cut Offset - This is a thickness to leave after the last rough cut is made. This is ignored if the boundary condition is on.
   

• Finish Cut Offset - This is a thickness to leave after a finish (optional) side clean cut is made. This is ignored if the boundary condition is on.
   

• Vertical Offset - This is a thickness of material to leave above the bottom of the region.
   

• Top Point - Use this to set the top of the part. This is not used when the top is already known from an existing CAM feature.  Enter a z value, an absolute coordinate value (x,y,z) or select a point from the graphics window. Point input options are available by right-clicking the mouse. This Top Point parameter and the Vertical Clear parameter (see General Tab - Auto Engage/Retract) together define the "safety plane."
   

• Bottom Point - Use this to set the bottom of the part. Like Top Point above, this is not used when the bottom is already known from the CAM feature.  Again, enter a z value, an absolute coordinate value (x,y,z) or select a point from the graphics window. Point input options are available by right-clicking the mouse.

 

 

 

 

 

See Tool Path Analysis and Appearance Options.

 

 

 

• OK - Update the operation definition with the new parameters and automatically updates the last modified date for this operation.

• Reset - Reset the form to the parameters already stored for this operation in the CAM plan. If this is a new operation, the contents of the form will default to values defined in your CAM Configuration files.

• Cancel - Close the form without saving any changes to the operation.

• Calculate -Calculate the tool path using on the current parameters.  You can also right-click on the operation in the CAM Plan Manager and select Calculate.  If a parameter is invalid, the Opdef form stays up and warning is given.  If no tool or feature is defined or if the tool path already exists and it is “Locked,” the parameters are saved, the Opdef form goes down and a warning is given.