Machining Options

This property controls whether the I and J parameters for arc moves (G2, G3) use absolute coordinates or incremental, relative to the arc end points. If this setting is different to the way the CNC controller interprets arc moves, the resulting toolpath may look a mess of random arcs in the controller.

Default When default is set in the drawing's machining properties, the post processor Arc Center Mode will be used. A default value in the post processor will use Incremental (C-P1).

Absolute I & J are absolute coordinates of the arc center point.

Incremental (C-P1) I & J are coordinates of the arc center, offset from the first arc point. This is the typical incremental mode. In previous versions this option was just called Incremental.

Incremental (P1-C) I & J are offsets of the first arc point from the arc center.

Incremental (C-P2) I & J are arc center offsets from the second arc point.

Incremental (P2-C) I & J are offsets of the second arc point from the arc center.

This text is inserted at the end of the gcode output. It can contain multiple text lines or pipe characters '|' to denote new lines. It can also contain $macros. Common available macros are described in the post processor section.

This text is inserted at the beginning of the gcode output. It can contain multiple text lines or pipe characters '|' to denote new lines. It can also contain $macros. Common available macros are described in the post processor section.

This value is used when moving down to the stock surface or next cutting level.

If set to 0, the current machining operation's Plunge Feedrate is used (which can result in slow machining times).

If a non zero Fast Plunge Height is specified, a rapid move is used (G0) to the specified height above the stock. This can significantly improved cutting times in some files. A typical example might be 0.1 or Metric or 0.004 for Inches.

The default value is (-1), which will use one minor grid unit as the fast plunge height.

Adjusts the length of the holding tabs by scaling the length by these amounts. Outer Tab Scale is the length toward the toolpath and Inner Tab Scale is the length away from the toolpath.

A drawing point that will be used as the machining origin (X=0,Y=0) point when gcode is created.

The ellipsis button to the right of this property can be used to select a point in the drawing.

An 'X' icon will be displayed on the drawing at the machining origin point. This cross can be dragged to a new location using the mouse.

NOTE: MachiningOrigin replaces the GCodeOrigin and GCodeOriginOffset properties of earlier releases.

Controls how decimal numbers are output to the gcode file. This property is overridden by the Number Format specified in the selected post processor. See the Post Processor section for more information.

This is the location of the destination gcode file. Clicking the button to the right of this property will open a file browser.

A selection from a drop down list which contains a list of all the post processors available. The post processor controls how the gcode files are formatted and are user configurable using XML based post processor files.

This is a text field containing multiple macro definitions (one per line), of the format $macro=value. These macros can be used by the selected post processor and are a handy way of passing parameters from the drawing to the post processor.

Controls whether to regenerate toolpaths before creating gcode post.

• Always - Toolpaths will automatically be regenerated before posting the gcode.
• Prompt - Prompts whether or not to regenerate toolpaths before posting.
• If Needed - Toolpaths will be regenerated if machining properties or drawing objects change.

Prompt or If Needed are useful when the toolpaths take a long time to generate such as with some 3D operations.

True | False.

Show cut widths will shade the areas that will be cut. This feature currently only works when the drawing view has not been rotated. It should be easy to spot any areas that are not shaded and will therefore have stock remaining.

True | False.

Controls the visibility of a small arrow at the start point of each toolpath that indications the direction of machining.

True | False.

Controls the visibility of a dashed line that indicates rapid moves from one toolpath to the next.

NOTE: Rapids are currently only displayed within each machining operation. Rapids from one machining operation to the next are not yet shown but should be in the next release.

True | False.

Shows or hides the toolpaths. This is the same as using the View - Show Toolpaths menu option.

The stock object is used to define the dimensions of a block of material from which the part will be cut.

The properties of the stock object can be used to automatically determine some machining properties.

• If a machining operation or style's Stock Surface property is set to Auto, the stock's stock surface value will be used.
• If a machining operation or style's Target Depth property is set to Auto, the stock's stock surface and Z size will be used to determine the target depth, so a machining operation will by default machine all the way through the stock.

Stock properties:

Material: Informational text that describes the stock material.
Stock Offset: X and Y offset of the lower left corner of the stock block. For example, a stock offset of -10,-20 would position the stock 10 units to the left of the Y axis (X=0) and 20 units below the X axis (Y=0).
Stock Surface: The Z location of the top of the stock block.
Stock Size: The X, Y and Z dimensions of the stock block.
Color: Color to use when displaying this stock object.

Stock is undefined if the X,Y and Z sizes are all zero. Stock can be defined at the part or machining level. Stock defined at the part level will override and machining level stock definitions and will be used for all operations within the part.

The stock object dimensions can also be passed to simulators such as CutViewer when post processors with appropriate stock macros are included, such as the Mach3-CV post processor.

Select a default CAM Style for this part.
All machining operations in the part will use this style unless set otherwise in the machining operation's Style property.>/p>

This property is used to locate the style definitions used in the Part or machining operations.

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.

If left blank, the default tool library will be used (Default-{$Units}), otherwise the specified library will be used when looking up tool numbers.

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

All | Selected Only

When there are a lot of machining operations, it can get visually confusing as to which toolpath belongs to which machining operation. By setting Toolpath Visibility to Selected Only, only the toolpaths for the machining operation selected in the drawing tree are visible.

Constant Velocity | Default | Exact Stop

Controls the use of G61 and G64 commands in gcode output.

This global velocity mode setting can be overridden by individual machine operations. For example it may be useful to have a global value of Constant Velocity set for the drawing and use Exact Stop for finishing machine operations.

If Default is used, no velocity mode gcode is written (or the global velocity mode is used for machining operations).

Constant Velocity, sometimes referred to as 'Look Ahead', is a useful feature implemented in some CNC controllers so that motion is smoothed between control points. This is particularly useful with geometry that involves a sequence of many small movements, often trying to approximate a natural shape. The downside is a potential loss of accuracy.