Machining Options
Parameters that control how machining operation toolpaths are generated, as well as how gcode is produced, can be set by selecting the Machining folder in the drawing tree and inspecting the property window.
Note: In earlier CamBam versions, settings that controlled how toolpaths were displayed were also found in the Machining options. In version 0.9.8, these have been moved to the top level Drawing object of the file tree and are also accessible from the View menu.
Properties
|
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. |
|
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 If a non zero |
Inner Tab Scale, Outer Tab Scale New! [0.9.8i] |
Adjusts the length of the holding tabs by scaling the length by these amounts. |
|
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 |
|
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.
|
[0.9.8] moved from machining to first item in the drawing tree. |
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. |
[0.9.8] moved from machining to first item in the drawing tree. |
Controls the visibility of a small arrow at the start point of each toolpath that indications the direction of machining. |
[0.9.8] moved from machining to first item in the drawing tree. |
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. |
[0.9.8] moved from machining to first item in the drawing tree. |
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.
Stock properties:
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-CutViewer 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. |
|
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 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.
|
[0.9.8] moved from machining to first item in the drawing tree. |
When there are a lot of machining operations, it can get visually confusing as to which toolpath belongs to which machining operation.
By setting |
|
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 If |