3D Profile Machining Operation
3D Profiles can be used to machine 3D objects from triangular mesh files. Currently 3DS and STL files are supported.
3D Profiles support the following features.
- Waterline roughing and finishing methods.
- Z scanline roughing and finishing methods.
- Front face and back face machining.
- Generation of negative molds from positive shapes.
- Restriction of machining boundary to save machining time.
- Experimental additive support for extrusion heads.
This method replaces the Bas Relief method in older CamBam versions.
See also:
3D Profile Tutorial,
3D Profile Tutorial - Back face
Properties
|
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= For best results, this setting would be combined with a This method is very experimental at the moment and more work is needed to tie in with the post processor to control the extruder. |
[New! 0.9.8N] |
The tolerance used when automatic arc fitting is applied. Zero will use an automatically calculated value. |
[New! 0.9.8N] |
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 If the back face option enabled, a valid |
|
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 |
|
If the |
|
The outer boundary shape, as determined by the It is recommended that a margin greater than 0 is used when using waterline profile methods in combination with |
|
This property controls the shape of the area around the model to machine. Boundary shapes options are: |
|
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. |
[New! 0.9.8] |
A 2D Point, used with |
[New! 0.9.8] |
A 2D Point, used with If |
|
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. |
|
|
|
The axis around which you would flip the stock to machine the back face. |
|
Defines the type of lead in move to use.
Refer to the lead move section for more information. |
[New! 0.9.8] |
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.
|
|
If set to |
|
Each machine operation can be given a meaningful name or description. |
|
An option that controls how the toolpaths are ordered in gcode output.
|
|
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 |
|
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.
|
|
When The effects of each option can be seen when using the new Draw - Fill Region menu option. Options are:
|
|
For |
|
Used control whether this should be a roughing or finishing pass.
For horizontal and vertical scanline operations: |
|
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. |
[New! 0.9.8N] |
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 |
|
The direction of rotation of the spindle. |
|
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 |
|
Used to select a point, near to where the first toolpath should begin machining. |
|
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. |
[New! 0.9.8] |
Select a CAM Style for this machining operation. All default parameters will be inherited from this style. |
|
A general purpose, multi-line text field that can be used to store notes or parameter data. |
|
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 ToolNumber is used to identify the current tool. If ToolNumber changes between successive machine ops a toolchange instruction is created in gcode. ToolNumber=0 is a special case which will not issue a toolchange. The tool number is also used to look up tool information in the current tool library. The tool library is specified in the containing Part, or if this is not present in the Machining folder level. If no tool library is defined the Default-(units) tool library is assumed. |
|
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.
|
|
Used to transform the toolpath. Warning! This property is experimental and may give unpredictable results.
|
|
Instructs the gcode interpreter whether or to use look ahead smoothing.
|
|
Used to define the gcode workplane. Arc moves are defined within this plane. |