Drilling Machining Operation
Used to create circular holes from selected point lists or circles.
Properties
|
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 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. |
|
Custom GCode script used for drilling if DrillingMethod=CustomScript Various macros can be used in this script which will be expanded by the post processor.
| - denotes a new line |
|
The feed rate to use when cutting. |
[New! 0.9.8] |
The depth increment controls the pitch of the spiral toolpath if This is the depth of cut for each loop of the spiral. |
[New! 0.9.8] |
For spiral drilling only. If |
|
Method used to generate the drilling instruction. Options are:
|
|
The time to pause at the bottom of the drill cycle. The unit of time measurement depends on the machine interpreter configuration and may be seconds or milliseconds. |
|
|
|
Used for spiral mill drilling and is the diameter of the hole required. If this is set to Auto, then the sizes of the selected shapes are used to calculate the hole diameter. |
[New! 0.9.8] |
For spiral drilling only. The distance to move in the lead out direction if |
|
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. |
|
Each machine operation can be given a meaningful name or description. |
|
An option that controls how the toolpaths are ordered in gcode output.
|
|
The incremental depth to drill before a retract. If 0, then doesn't peck drill. |
|
The feed rate to use when plunging. |
|
List of drawing objects from which this machine operation is defined. |
[New! 0.9.8] |
For peck canned cycles, retract to this value after each peck. |
|
Currently only supported by 3D Profile and Lathe machining 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. |
|
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. |
|
For spiral drilling only. If |
|
Used to select a point, near to where the first toolpath should begin machining. |
|
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. |