3D Profile Machining Operation

If set to True, an additive toolpath will be generated, suitable for extrusion heads.

Additive toolpaths are generated from lowest to highest Z levels with the lowest (starting) level at Z=Stock Surface.

For best results, this setting would be combined with a Waterline Rough 3D profile methods, and a small Depth Increment.

This method is very experimental at the moment and more work is needed to tie in with the post processor to control the extruder.

The tolerance used when automatic arc fitting is applied.

Zero will use an automatically calculated value.

Whether to apply arc fitting.

Arc fitting will make toolpaths smoother to machine and faster to calculate, but may introduce some inaccuracy.

When set to True, a toolpath for the back face of the model will be generated.

If the back face option enabled, a valid Back Face Zero Z setting should also be supplied.

To improve code generation speed, model faces pointing away from the front are ignored.

This can cause problems when the triangle winding order is inconsistent, so this behaviour can be disabled by setting Back Face Culling to False.

If the Back Face setting is enabled, this is the current Z coordinate that will be at Z=0 after the model is 'Flipped' about the Flip Axis.

The outer boundary shape, as determined by the Boundary Method setting, is extended by the distance give in the Boundary Margin setting.

It is recommended that a margin greater than 0 is used when using waterline profile methods in combination with Shape Outline boundary methods.

This property controls the shape of the area around the model to machine.

Boundary shapes options are:

Shape Outline - the outline shape of the source 3d models.

Bounding Box - a rectangle enclosing the source geometry.

Selected Shapes - A list of 3D or 2D shapes specified in Boundary Shape Ids.

A list of drawing entity IDs that represent the shapes to use to determine the boundary shape.

Angle in degrees from vertical to taper the outer boundary edge.

The clearance plane (offset from the work plane).

The clearance plane should be clear of the stock and any holding devices to allow free movement to any location.

A 2D Point, used with Clip Area Min to define a clipping area.

A 2D Point, used with Clip Area Max to define a clipping area.

If Clip Area Max and Clip Area Min coordinates are both 0, the machining area will not be clipped.

A multi-line gcode script that will be inserted into the gcode post after the current machining operation.

A multi-line gcode script that will be inserted into the gcode post before the current machining operation.

The feed rate to use when cutting.

Controls whether to cut to depth first or all cuts on this level first.

Depth increment of each machining pass. Determines the number of passes to reach the final target depth.

True: The toolpaths associated with this machining operation are displayed and included in the gcode output
False: The operation will be ignored and no gcode or tool paths will be produced for this operation.

The axis around which you would flip the stock to machine the back face.

Defines the type of lead in move to use.

Lead Move Type: None | Spiral | Tangent
Spiral Angle: Used by spiral and tangents to control ramp angle.
Tangent Radius : The radius of the tangent lead in
Lead Move Feedrate : The feedrate to use for the lead move. If 0, Cut Feedrate is used.

Refer to the lead move section for more information.

Defines the type of lead out move to use.

Refer to the lead move section for more information.

Maximum distance as a fraction (0-1) of the tool diameter to cut in horizontal transitions.

If the distance to the next toolpath exceeds MaxCrossoverDistance, a retract, rapid and plunge to the next position, via the clearance plane, is inserted.

Controls the direction the cutter moves around the toolpath.

Conventional | Climb | Mixed

If set to True, a negative mold toolpath is generated from a positive shape.

Each machine operation can be given a meaningful name or description.
This is output in the gcode as a comment and is useful for keeping track of the function of each machining operation.

An option that controls how the toolpaths are ordered in gcode output.

New (0.9.8) - A new, improved optimiser currently in testing.
Legacy (0.9.7) - Toolpaths are ordered using same logic as version 0.9.7.
None - Toolpaths are not optimised and are written in the order they were generated.

CamBam's waterline routines have been designed to work best with natural / curved shapes. Engineering shapes with perpendicular sides can potentially cause problems. If problems are encountered, setting Plane Slice Only to True can help but will only work with shapes that do not have any overhangs.

The feed rate to use when plunging.

List of drawing objects from which this machine operation is defined.

The method used to generate the 3D toolpath.

• Horizontal - Use a Z scanning method in horizontal direction.
• Vertical - Use a Z scanning method in vertical direction.
• Waterline Rough - Uses a series of waterline slices which are pocketed up to the boundary shape.
• Waterline Finish - Creates a profile using the tool offset at each waterline slice.

When Waterline Rough 3D profile method is selected, this option controls the pattern used to fill the pockets at each waterline layer.

The effects of each option can be seen when using the new Draw - Fill Region menu option.

Options are:

• Horizontal Hatch region filled with horizontal lines
• Vertical Hatch region filled with vertical lines
• Inside + Outside Offsets region filled with progressive offsets from outside in, unioned with offsets from islands radiating outward.
• Outside Offsets region filled with progressive offsets from outside in (like current pocket method).
• Inside Offsets region filled with offsets from islands radiating outward.

For Horizontal and Vertical 3D profile methods, this is the distance along each scan line (expressed as a fraction (0-1) of the cutter diameter), for each Z height test point.
Larger resolution values are faster but could result in some features being over cut.

Used control whether this should be a roughing or finishing pass.

For horizontal and vertical scanline operations:
If Roughing is selected, toolpaths at each Depth Increment are calculated.
If Finishing is selected, only the toolpath at the final Target Depth is calculated.

This is the amount of stock to leave after the final cut.

Remaining stock is typically removed later in a finishing pass.

Negative values can be used to oversize cuts.

For horizontal and vertical scanline methods, this property will suppress tool path segments steeper than a given gradient.

The value is specified in degrees where 90 degrees is vertical (Z).

A scanline finish with a reduced gradient threshold is useful when combined with a waterline finish operation. Waterline finish is best suited for steep areas but may result in uncut bands in shallow areas due to the limits its depth increment. Whereas scanlines work well on flat areas but can result in scalloped tool marks on steep model sides.

Using a Boundary Margin of (minus) the tool radius is recommended when using this property to restrict tool paths to shallow areas.

The direction of rotation of the spindle.

CW | CCW | Off

The pulley number or dial setting of the spindle for the target speed.

The speed in RPM of the spindle.

Corner to start profiling. Used in Horizontal and Vertical 3D profiling methods only.

Used to select a point, near to where the first toolpath should begin machining.
If a start point is defined, a small circle will be displayed at this point when the machining operation is selected. The start point circle can be moved by clicking and dragging.

The cut is increased by this amount each step, expressed as a fraction (0-1) of the cutter diameter.

For horizontal and vertical 3D profile methods, this is the distance between each scan line.

For waterline roughing, this is the distance between fill offset lines.

For waterline finishing, this value is not used.

The feed rate to use for crossover moves.

This is the Z offset of the stock surface at which to start machining.

Select a CAM Style for this machining operation. All default parameters will be inherited from this style.

The Z coordinate of the final machining depth.

This is the diameter of the current tool in drawing units.

If the tool diameter is 0, the diameter from the tool information stored in the tool library for the given tool number will be used.

The shape of the cutter

If the tool profile is Unspecified, the profile from the tool information stored in the tool library for the given tool number will be used.

EndMill | BullNose | BallNose | Vcutter | Drill | Lathe

Used to transform the toolpath.

Instructs the gcode interpreter whether or to use look ahead smoothing.

Constant Velocity - (G64) Smoother but less accurate.
Exact Stop - (G61) All control points are hit but movement may be slower and jerky.
Default - Uses the global VelocityMode value under machining options.

Used to define the gcode workplane. Arc moves are defined within this plane.
Options are XY | XZ | YZ