www.kxcad.net Home > CAM Index > EdgeCAM Index >
The Code Wizard Document can control the type of output when using a driven tool.
Within the "C/Y Axis Functions" Tab (NC Style section) there are a number of options available as described here:
Support XC Interpolation – This switch only affects Axial ‘C’ axis
machining. When the switch is checked, the NC code will support Linear
and circular moves. The output method can be either in Polar or Cartesian
co-ordinates (see Program C axis Axial
cutting moves as Polar / Cartesian below).
When the switch is unchecked, all linear and circular moves will be converted to a series of linear moves with relation to the tolerance specified for each cycle.
Note: This switch can be overridden within EdgeCAM by using the command XC Interpolation (M-Functions menu).
Support Hole Canned Cycles (C and Y) – When this switch is checked, the Hole Cycles will use the canned cycle code specified within the Code Wizard (see C and Y G-Codes Tab, NC Style section).
When this switch is unchecked, all output will be directed through the linear feed and rapid C axis code constructors.
Support G98/G99 for Hole Cycles (C and Y) – When this switch is checked, the Code Wizard support the option of specifying a secondary retract plane for all Canned Hole cycles.
Reverse C Axis Sign
Check to reverse the sign of C angles on the main spindle, for example C90 becomes C-90.
Reverse C Axis Sign Sub Spindle
Check to reverse the sign of C angles on the sub spindle, for example C90 becomes C-90.
Reverse 0-360 Direction
Check to reverse the direction in which C angles are measured, for the main spindle, for example C90 becomes C270.
Reverse 0-360 Direction Sub Spindle
Check to reverse the direction in which C angles are measured, for the sub spindle, for example C90 becomes C270.
Convert Rapid Moves to High Feed when in Cartesian Mode – This switch only affects Axial ‘C’ axis machining.
Some controllers cannot perform rapid moves when the Cartesian mode has been evoked. To overcome this problem any rapid moves will be output as feed move but at a specified high feedrate (see Rapid Traverse Tab in the NC Style section).
Program C axis Axial cutting moves as Polar / Cartesian – This switch only affects Axial ‘C’ axis machining.
This option will select the type of output supported by the controller.
Polar – All linear and circular moves will be output where: X is the radius and C is the angular position.
Cartesian – All linear and circular moves will be output where: X is the co-ordinate and C is the Y co-ordinate. Note: Fanuc's Polar mode is in fact 'Cartesian', and Cartesian should therefore be selected.
Program Wrap Distance as Radius / Diameter – This switch only affects Radial ‘C’ axis machining.
If the controller requires a code and value to specify the radial distance to the set point of the tool, the value can be output as a radial or diametrical distance.