The Rough dialog box permits you to change the parameters of a roughing feature to suit the part to be machined.
Posting Parameters
This box allows you to select the format for the posted operation. You is given the ability to choose between Separate Moves and Canned Cycles. When Canned Cycles is selected, the operations are posted using the proper canned cycle setup in the post processor. If Separate Moves is selected, the operations are long coded. If the Feature includes a Rough and a Finish, then both operations are posted in the selected format.
Cycle Type
Cycle Type - This box allows you to select what type of operation is performed. The types are Turn Rough, Turn Rough/Finish, Face Rough, and Face Rough/Finish.
Depth of Cut - This box indicates how much material is removed per pass.
Z Allowance - This box determines how much material is left for finishing on the Z-axis.
X Allowance - This box determines how much material is left for finishing on the X-axis.
Stock Diameter - This box indicates the major diameter of the bar stock that is being machined and is only visible when Turning Rough or Turning Rough/Finish is selected. This is also used to determine the where the toolpath begins cutting material on the outside diameter.
Face Stock - This box indicates the location of the front of the stock in the Z-axis and is only visible when Face Rough or Face Rough/Finish is selected. This is also used to determine where the toolpath begins cutting material on the face of the part.
System Compensation - This box allows you to specify whether or not the system compensates for the insert geometry and the tool nose radius. If this option is set to Off, the selected geometry is used as the program path. If this option is set to On, the system compensates for the tool nose radius and the insert geometry, producing a much different path. When using the Off option for System Compensation, it is recommended that you turn on the Machine Compensation option.
Machine Compensation
Off - When this option is selected, the system does not output any compensation commands in the posted program.
Comp Left / G41 - When this option is selected, the system outputs the Left compensation command in the posted program.
Comp Right / G42 - When this option is selected, the system outputs the Right compensation command in the posted program.
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.
Leadin Z - This value indicates the distance and direction of travel, in the Z-axis, the system generates for the approach into the profile.
Leadin 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.
Leadout Z - This value indicates the distance and direction of travel, in the Z-axis, the system generates for the departure from the profile.
Leadout 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 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 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.
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.
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 in the operation.
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 operation.
Save - This button allows you to save the settings in this dialog box as the default settings for future parts.