The Thread dialog box permits you to change the parameters of a threading feature to suit the part to be machined.
Thread Type
Canned Cycle - When using the Canned Cycle method is selected the system outputs a threading operation in a standard G32 Threading Cycle.
Separate Moves - When using the Separate Moves option the system outputs several moves using the standard G76 threading output.
Thread Parameters
Threads Per Inch/MM - This box indicates how many crests occur for every unit of measure.
Thread Pitch - This box indicates the distance between crests of the thread.
Thread Height - This box indicates the distance from the minor diameter of the thread to the major diameter of the thread.
First Cut Amount - This box is used to specify the amount of material removed in the first pass of the thread cutting cycle.
Last Cut Amount - This box is used to specify the amount of material removed during the final pass of the Threading operation.
Number of Finish Passes - This box allows you to specify the number of finish passes the system outputs for the Thread.
Thread Lead-In Angle - This box allows you to select the angle of the approach into the thread. (0 degrees results in a perpendicular approach.)
Canned Cycle Chamfer Out - This box allows you to include a chamfer at the end of the thread that is generated and has two possible selections.
On - When this option is selected the Number of Leads box becomes available.
Off - When this option is selected the system does not perform the Chamfer Out operation.
Number of Leads - This box allows you to specify the number of threads used for the Chamfer Out and it must be between 0.1 and 9.9.
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.
Threading Tool
Insert Tab
Nose Radius - This value indicates the radius of the tool nose.
Tool Angle - This box allows you to select the included angle on the threading tool.
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.
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
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 - This option is selected by default.
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 is used to limit the rotation of the spindle. When calculating the speeds in the posted program the system limits the spindle speed to the value input into this box.
Speed - This box indicates the desired spindle rotation speed for the thread operation.
Pitch / Feed - This box indicates the desired feed rate for tool movement in the thread operation. This value is normally in inches (or millimeters) per revolution, and be equal to the thread pitch.
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 Thread operation.
Save - This button allows you to save the settings in this dialog box as the default settings for future parts.