The Finish dialog box allows you to change the parameters of a finish feature to suit the part to be machined. It also operates like a Pattern Repeat (G73 on Fanuc®-style machines) cycle when multiple passes are used.
Posting Parameters
This box allows you to determine whether the code for the Finish Feature is output as a Canned Cycle or as Separate Moves.
Cycle Type - The options available change depending on the options selected.
Type box - This box allows you to select what type of operation is performed. You have the choice of Turn Rough, Turn Rough/Finish, Face Rough, and Face Rough/Finish.
X Stock - The total amount of stock removed in the X-axis.
Z Stock - The total amount of stock removed in the Z-axis.
NOTE: X Stock and Z Stock are unavailable when Number of Passes is set to one.
Z Allowance - This box determines how much material remains to be removed on the Z-axis.
X Allowance - This box determines how much material remains to be removed on the X-axis.
Number of Passes - This box allows you to specify a number of spring passes to perform on the profile.
Stock Diameter - This box indicates the start point of the toolpath generated by the system. This box is only available when you have selected Turn Finish from the type box.
Face Stock - This box indicates the start point of the toolpath generated by the system for Facing operations. This box is only available when you have selected Face Finish from the type box.
System Compensation
This box allows you to specify whether or not to use the tool collision detection when generating the toolpath.
Machine Compensation - This option allows you to select a method for applying tool nose radius compensation.
Off - When this option is selected, the system does not output any cutter compensation commands for the Finish operation.
Comp Left / G41 - When this option is selected, the system outputs the command, specified in the post processor, for Left Compensation within the Finishing operation.
Comp Right /G42 - When this option is selected, the system outputs the command, specified in the post processor, for Right Compensation within the Finishing operation.
Type
Default Rapid On Exit - When this option is selected, the system uses the default configuration for rapid moves to generate a rapid move after the completion of the feature. The default retract is Rapid on Exit to Tool Home X-Z.
Rapid on Exit to Tool Home X-Z - When this option is selected, after the operation has been performed, the system generates a rapid move in the X-axis first and then a rapid move in the Z-axis.
Rapid on Exit to Tool Home Z-X - When this option is selected, after the operation has been performed the system generates a rapid move in the Z-axis first and then a rapid move in the X-axis.
Rapid on Exit to Tool Home ZX - When this option is selected, after the operation has been performed the system generates a rapid move in the both the X-axis and the Z-axis on the same line.
Rapid on Exit to Cycle Start X-Z - When this option is selected, after the operation has been performed, the system generates a rapid move to the X-axis position issued at the beginning of the cycle and then a second move to the Z-axis position issued at the beginning of the cycle.
Rapid on Exit to Cycle Start Z-X - When this option is selected, after the operation has been performed, the system generates a rapid move to the Z-axis position issued at the beginning of the cycle and then a second move to the X-axis position issued at the beginning of the cycle.
Rapid on Exit to Cycle Start ZX - When this option is selected, after the operation has been performed, the system generates a rapid move to the X-axis and the Z-axis positions issued at the beginning of the cycle.
Rapid to Defined Point X-Z - When this option is selected the system generates a rapid move in the X-axis to the defined point and then a rapid move in the Z-axis to the defined point.
Rapid to Defined Point Z-X - When this option is selected the system generates a rapid move in the Z-axis to the defined point and then a rapid move in the X-axis to the defined point.
Rapid to Defined Point ZX - When this option is selected the system generates a rapid move in the X-axis and the Z-axis to the defined point.
No Rapid on Exit - When this option is selected the system does not generate a rapid move after the completion of the operation.
Lead In - Currently only a vector lead-in is available. This lead generates a linear movement by the user-specified distance from the beginning of each pass.
Lead In Z - This value indicates the distance and direction of travel, in the Z-axis, the system generates for the approach into the profile.
Lead In X - This value indicates the distance and direction of travel, in the X-axis, the system generates for the approach into the profile.
Lead Out - Currently only a vector lead-out is available. This lead generates a linear movement by the user-specified distance from the end of each pass.
Lead Out Z - This value indicates the distance and direction of travel, in the Z-axis, the system generates for the departure from the profile.
Lead Out X - This value indicates the distance and direction of travel, in the X-axis, the system generates for the departure from the profile.
NOTE: For a closer look at the handling of leads, please refer to Lathe Leads.
Rough Pass - Rough Tool
Insert Tab
Nose Radius - This value indicates the radius of the tool nose.
Tool Angle - This box allows you to specify the angle of the tool insert.
Cutting Angle - The angle between the reference point and the edge of the insert.
Theoretical Z - This value is defined as the imaginary sharp point of the tool in the Z-axis. This is value is generated automatically when the tool orientation and nose radius are input into the system and is not normally changed.
Theoretical X - This value is defined as the imaginary sharp point of the tool in the X-axis. This is value is generated automatically when the tool orientation and nose radius are input into the system and is not normally changed.
IC Diameter - The internal circumference of the insert.
Tool Label - This box is used to add a name to the tool, in the tool list, that allows you to easily identify the tool.
Insert Type - Located below the insert diagram; this box allows you to select the style of insert used.
Orientation Tab
Orientation Number - This box allows you to select a number. Each number corresponds to a direction the tool can face. This selection influences the ability of the tool to move into locations that are restricted by adjacent geometry.
NOTE: The Orientation Number is also the value that designates whether the cut is inside or outside of the geometry.
Mach Info Tab
Offset Register - This box indicates the register on the machine that stores the offset values.
Turret Position - This box indicates the location in the tool changer or turret in which the tool resides.
Home Position Z - This box indicates the home position in the Z-axis. The system utilizes this number when moving the tool to a home position and also uses this position to determine the starting location of the tool.
Home Position X - This box indicates the home position in the X-axis. The system utilizes this number when moving the tool to a home position and also uses this position to determine the starting location of the tool.
Feeds/Speeds
RPM - When this option is selected, the system generates the feeds and speeds in the posted program based on revolutions per minute.
CSS - When this option is selected, the system generates the feeds and speeds in the posted program based on maintaining a constant surface speed.
Spindle Direction
CW - When this option is selected the system outputs the command for Clockwise rotation of the spindle.
CCW - When this option is selected the system outputs the command for Counter Clockwise rotation of the spindle.
Maximum RPM - This box indicates the highest RPM the system is permitted to output for the specified tool.
Rough SFM/RPM - The surface feet per minute (for RPM) or revolutions per minute (for CSS).
Rough Feed - This box indicates the desired feed rate for tool movement.
Select Tool - This button allows you to select a previously defined and saved tool. All of the values input for the tool are applied to the drill operation.
Save - This button allows you to save the settings in this dialog box as the default settings for future parts.