The 3 Axis Spiral Cut Operation Definition Form shown below is typical for the 3 axis milling operations.  Each operation form contains parameters specific to that operation.  

 

3-Axis Spiral Cut Operation Definition Form - Cutting Parameters Tab	3-Axis Spiral Cut Operation Definition Form - More Cutting Parameters Tab
3-Axis Spiral Cut Operation - Lead and Link Parameters Tab	3-Axis Spiral Cut Operation - Appearance Parameters Tab

 

 

 

Frames, Speeds and Containments

 

Frame

Alternate coordinate system defined within the setup for this operation.

 

Speeds Feeds

The speed/feed values to use for this operation's tool motions.  Select from the list of speed/feed objects you have previously defined.  You can also pick Create to display the CAM Speed Feed Manager Form to create a new speed/feed object.

 

Containment

Displays the Containment Definition Form.  The value selected in the "Type" input field of the Containment Definition Form is also shown here.

 

 

 

Reference (Rest Cut)

 

Tool

A reference tool used to determine which regions could not be cut (using that tool).  It is used to determine regions where further machining would be required.

 

A list of previously created tools is displayed (see CAM Object Name List for using the list options).  The tool chosen should be appropriate for milling operation.

 

 

Thicknesses

 

Curve Thickness

Offset added to all curve geometry, may be positive (offset away from part boundaries, or negative (offset toward part boundaries).

 

Surface Thickness

Offset added to all surface geometry, may be positive (offset away from part surfaces, or negative (offset toward part surfaces).  If negative, the magnitude may not exceed the positive thick (optionally) specified for a given surface in a CAM feature plus the tool's corner radius.

 

Horizontal Thickness

Rather than applying the thick along the surface normal, this thick is applied in the X, Y plane only and away from the part surfaces.  It must be >= 0.  Performance note: tool path computation can be significantly faster for rough and side cut tool paths if "Horizontal Thick" and "Vertical Thick" are used and "surface thick" and the tool's corner radius are zero.

 

Vertical Thickness

This thick is applied along the tool axis (+/- Z).  It has the same effect as translating the tool path up or down by this amount.  Caution is advised when specifying negative values as gouging may occur.

 

 

Other

 

Bottom

If this value is less than the lowest tool path point, each cut will be lengthened to the part boundary.  The points added will be at this " bottom" depth.

 

Enter the 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.

 

Curve Tolerance

Chord height tolerance applied to curves to control the density of tool path points.

 

Cut Order

• Auto - automatically determine cut direction.

• High to Low - cuts should be made in a generally downward direction.

• Low to High - cuts should be made in a generally upward direction.

 

Cut Overlap

Recut distance to obtain smooth part surface when cutting closed loops.  This distance is added at the end of the cut (retracting the beginning of the cut) at the "cut" feed rate.

 

Cutting Order (Surface Engrave)

This parameter specifies the cutting order of the tool paths.

• Automatic - the system determines the best cutting order.

• Pick Order - The Cutting Order corresponds to the exact order selected

• Min Distance - The Cutting Order is determined by the closest position of the tool paths.

 

Cutting Mode

Determines the direction of cut. Select from the following:

 

• Climb - utilize the tool object's "Cut Dir" property.

• Conventional - same as "Climb"

• Center - centerline of tool motion lies ON the curve boundary.  (Profile Cut)

 

Cutting Mode (Iso Cut)

Used to set the step over direction of adjacent cuts.  Select from the following:

 

• Inc U - align adjacent cuts with the surface constant U parameter, from low U to high U.

• Dec U - align adjacent cuts with the surface constant U parameter, from high U to low U.

• Inc V - align adjacent cuts with the surface constant V parameter, from low V to high V.

• Dec V - align adjacent cuts with the surface constant V parameter, from high V to low V.

 

Max Depth

This value limits the maximum depth of cut.  The depth of the highest tool path point (the lower of: highest point computed or the "Top " point) and the depth of the lowest tool path point (the higher of: lowest point computed or the "Bottom " point) are divided evenly into a series of cuts which do not exceed the "Max Depth".

 

If "max depth" is defined and "Top" is higher than the highest tool path point calculated, then planar cuts may be created which clear away stock within the part's boundary.

 

Min Flat Length

Determines the smallest horizontal movement which could indicate the breaking of a cut into multiple cuts.

 

Min Steep Length

Determines the smallest upward/downward movement which could indicate the breaking of a cut into multiple cuts.  This field is only active when Cut Order is set to "High to Low" or "Low to High".

 

Number of Cuts

The number of adjacent cuts to make on each curve boundary.

 

Pre-drill Points

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.

 

A "Drill" type operation, with subtype "Access Hole" should be defined which indicates this operation as its "Ref Oprn."  Then, after this tool path has been calculated, the locations for the access holes and their depths will be computed automatically.  Select from the following:

 

• None - don't use or compute access hole locations

• Auto - automatically calculate all access holes after calculating the tool path.

• Input Points - you can pre-select the locations where access holes will be created, and the tool path will create motions to begin within those access holes at each cut depth.
  
  The depths of those holes will be calculated automatically.  If more access holes are required, they will be calculated automatically.  You are prompted to "Select Points."  The right mouse button brings up the standard point input menu.

 

Profile Side

Which side of the curve boundary to cut.  This is defined with respect to the cutting direction of the profile. The cutting direction is defined by the order in which the curves are selected for the CAM Feature Profiles.

 

In the case of CAM components (wherein a feature is not provided), the order of curves may not be well defined.  The best approach is to calculate the path and if its undesirable, reverse this parameter and recalculate the path.  Select Left or Right.

 

Side Cleanup

Indicates whether a final cleanup pass should be made on the part boundaries.  If this is "Yes" then there will be two passes along the boundaries.

 

Side Region

Controls the cutting region of the side cut tool paths without requiring you to create a stock or containment.  Select from the following:

 

• All Regions - Default, cuts all regions accessible to the cutter.

• Pockets Only - Limits tool path motion to those regions inside a pocket in the part (the complement of "outside only").

• Outside Only - Limits tool path motion to those regions which are not inside a pocket in the part.

 

Slope Limit

This parameter is only valid when "Bi-Direction" is set to "Optimal Perpendicular."

 

Slope Limit (Scallop Removal)

This angle determines which regions on the part will be machined.  Given the cutting direction of the reference operation, the regions needing further machining are determined from two criteria:

 

• The surface regions are more steep than the "Slope Limit."

• They lie outside that angle from the cutting direction of the reference operation.

 

Enter a value that is greater than 0 and less than 90.

 

Spiral Progress

• 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, 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.

 

Steep Angle

The allowable upward movement in a cut if "High to Low" is selected for the Cut Order or the allowable downward movement if "Low to High" is selected.  Any movement greater than this angle will cause a cut to be broken into multiple cuts.

 

Step Type

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

 

• Diam Percent - compute spacing from this percentage and the tool diameter.

• Center Dist - distance between tool center point along adjacent cuts.

• Contact Dist - distance between tool contact points on the part surface.  In the case of Rough tool paths, this is equivalent to "Center Dist".

• Scallop Height - the spacing between adjacent cuts is computed from the tool shape and this scallop height value.  In the case of 2- ½ axis tool motion, this is computed in the X Y cutting plane and the cut spacing is constant.

 

Step Value

Value to use in conjunction with Step Type to control adjacent cuts.

 

Surface Tolerance

Chord height tolerance applied to surface/solid geometry to control the density of tool path points.

 

Tolerance (Pencil Cut)

Chord height tolerance applied to surface/solid geometry to control the density of tool path points.

 

Tolerance (Rest Cut)

The machining tolerance for the finished part.

 

Tool Side (Surface Engrave Cut)

For this parameter, select include on, left and right from the driving curves.

 

• On - All curve offset are ignored.

• Left, Right - The cutting tool follows the corresponding left (or right) side of each driving curve when looking down from the z-axis. The left or right offset equals the sum of the curve offset and the tool radius.

 

Top

If this value is higher than the highest tool path point computed from the part geometry, it has no effect. If it is lower than that highest point, the tool motions above that depth are discarded, and each cut will be lengthened to the part boundary.  The points added will be at the depth of the lowest tool path point computed.

 

• Enter the 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.

 

Tool Location

Determines if tool side should touch the part or island curves (tan = outer side of tool, past = inner side of tool) or if the tool center should touch the curves (on).  Note that the ON condition will cause several of the stock offsets to be ignored for those boundary elements.

 

• Enter a value greater than 0 and less than 90.  Only surface regions which are more steep than this angle are isolated for further machining.  The "Cut Dir" along with the "Slope Limit" angle are then used to further limit the regions.  Cuts perpendicular to the "Cut Dir" are calculated in these regions.

 

 

Notes

 

• Top, Bottom and Max Depth provide a means of controlling the depth of cut.  After the tool motion is calculated, these values are used to limit or divide the tool path with respect to the Z axis (the tool axis vector).

• Cut Order, Steep Angle, Min Steep Length and Min Flat Length are intended to control the start points for cuts which are increasing or decreasing along the Z axis.  In the case of cuts which move both up and down, these parameters will determine where the cuts will be broken.

 

 

 

 

Pattern

 

Rest Type

Determines the type of rest cut pattern to use. Select from the following:

 

• Mapcut Rest - Uses a pattern similar to the Map Cut Operation.

• Peelcut Rest - Uses a pattern similar to the Peeling Cut Operation.

 

Cut Region

Determines which regions will be machined by this operation. (See "Slope Limit").  This field is only active when the Rest Type field above is set to Peelcut Rest.  Select from the following:

 

• Flat Regions - only generally flat regions will be machined, the tool motion will be determined by the "Cut Pattern."

• Steep Regions - only generally steep regions will be machined.  The tool motion will use the "side cut" cutting pattern.

• All Regions - all regions on the part will be machined.  The flat and steep motions will utilize the "Cut Pattern" and "Side Cut" motion types respectively.

 

Region Slope

Enter a value greater than 0 and less than 90.  Flat regions are those regions less steep than the "Region Slope".  Steep regions are those regions more steep than the "Region Slope."  This field is only active when the "Rest Type" field above is set to "Peelcut Rest".

 

Cut Pattern

Sets the cutting pattern. Select from the following:

 

• Zigzag - 3-axis zigzag motion.

• Box - 3-axis box cut.

• Spiral Inward - 3-axis spiral cut with "Spiral Progress" set to "Spiral Inward."

• Spiral Outward - 3-axis spiral cut with "Spiral Progress" set to "Spiral Outward."

• Step Inward - 3-axis spiral cut with "Spiral Progress" set to "Spiral Inward."

• Step Outward - 3-axis spiral cut with "Spiral Progress" set to "Step Outward."

• Contour Radial - 3-axis contour cut with "Cut Direction" set to "Radial."

• Contour Parallel - 3-axis contour cut with "Cut Direction" set to "Parallel."

 

Corner Loop

Inserts circular moves to turn the tool way from part boundaries.  After the tool reaches the turning point, it reverses, then follows a circular move into the next cut, moves back to the turning point and then proceeds along that next cut.  Select "Yes" or "No."  This option is only available when the Spiral Progress or Cut Pattern parameter is set to either Step Inward or Step Outward.

 

Auto Cut Direction

• Yes - set the cutting direction to be parallel to the longest linear boundary element.

• No - cutting direction will be determined by "Cut Dir."

 

Cut Direction

If "Auto Cut Dir" is set to "No," 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 (Map Cut)

Select a cut direction.  The right mouse button will bring up the standard direction input options menu.

 

Cut Direction (Rest Cut)

When "Zigzag" or "Box" is selected for "CutPattern" select a cut direction.  The right mouse button will bring up the standard direction input options menu.

 

Bi-Direction

This setting is only valid when "Auto Cut Dir" is set to "No." Select from the following:

 

• None - all cutting will take place in the "Cut Dir" direction.

• Perpendicular - after cuts are made in the "Cut Dir" direction, the same regions are machined in the perpendicular direction.

• Optimal Perpendicular - after cuts are made in the "Cut Dir" direction, cuts are made perpendicular to that direction in regions computed from the "Slope Limit".

 

Bi-dir Slope

This field is only active when "Bi-Direction" above is set to "Optimal Perpendicular."

 

Enter a value greater than 0 and less than 90. Only surface regions which are more steep than this angle are isolated for further machining.  The "Cut Dir" along with the "Bi-dir Slope" angle are then used to further limit the regions.  Cuts perpendicular to the "Cut Dir" are calculated in these regions.

 

Ramp Angle

If this value is > 0, the tool will ramp from the current cut depth down to the next.  The path is computed over the cut at that next depth.  Use of ramping motion removes the need for access holes.

 

Under Cut

If set to "Yes" the entire tool is used for computing a gouge-free path on the part.  If set to "No" then only the bottom of the tool is used.  If the part has a positive (or zero) draft it should not be necessary to select "Yes"; if the part has regions with a negative draft, or a tapered tool is being used then "Yes" should be selected.

 

 

Cut Overlap

Recut distance to obtain smooth part surface when cutting closed loops.  This distance is added at the end of the cut (retracting the beginning of the cut) at the "cut" feed rate.

 

 

 

Link Parameters

 

• Short/Long Link Type
  
  Tool path links can be classified as long or short using the % Short Link Limit parameter whose value is a percentage of the tool end diameter. Each path link has the following options.
  
  Automatic - The system calculates the path link in motions of the linear-arc-linear style.
  Z Lift Up - The tool lifts up along the Z-axis so that it traverses above the top of the part by at least the Safe Distance parameter.
  Straight - The tool moves directly from the end of the current cut path to the start of the next cut path while in cutting mode.
  Clearance - The tool lifts up a distance defined by Clear Z (see CAM Frame Manager before traversing to the next cut.
   

• % Short Link Limit-Tool path links can be classified as long or short using this parameter whose value is a percentage of the tool end diameter.

 

• Max Rotate Angle - This angle limits the axis rotational angle of each traversal movement.

 

• Smooth Distance - This parameter, if set greater than 0 (zero) will set the global joining and smoothing distance. This value cannot be larger than 2 * tool corner radius. The default value is 0 (zero).

 

• Save Distance - This value is 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.

 

• Max Plunge Length - This is a maximum distance for a plunge before the start of the actual cut.  It is a plunge move added before each lead In for safer tool engagement.  If this is left blank, it will default to the Safe Distance value above.   

 

 

Lead In Lead Out Parameters

 

 

• Type - This parameter sets the type of lead in. Select from the following:
  
  None - Lead in  is simply punching down and lead out is simply retracting in the direction of tool axis.
  Arc-Linear Ramp - Lead-in or out motion is in the form of an arc, linear or arc-linear. If Ramp Angle (see below) is set to zero, the motion lies in the xy-plane. The ramp angle is measured from xy-plane.
  Normal - Lead-in or out motion is in the form of an arc, linear or arc-linear, which lies in the plane normal to the tangent plane of the machining surfaces.
  Tool Axis Plane - Lead-in or out motion is in the form of an arc, linear or arc-linear, which lies in the plane of the tool axis direction and tool path tangent direction.

 

• Start Angle - This sets the lead in start angle in degrees.

• End Angle - This sets the lead in end angle in degrees.

• Radius - This sets the lead in radius.

• Linear Length - This specifies the length of a line which will form part of the Lead motion. For Lead In the order is first Line then Arc.

• Ramp Angle - This is only used when the lead in or out type (see above) is set to Arc-Linear Ramp.  It is measured from xy-plane.

 

 

Macros

 

• Use Macros - Select Yes to enable Macro Parameters

• 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.

 

 

 

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.