Milling Parameters Specific to Thread Milling
In addition to the common milling parameters, the following parameters control the tool path generated by a Thread milling NC sequence:
THREAD_DIAMETER
If you have specified the thread style as Internal, this parameter indicates the major thread diameter. If the thread style is specified as External, it indicates the minor thread diameter.
THREAD_FEED
Specifies the thread pitch.
THREAD_FEED_UNITS
The possible values are TPI (threads per inch), MM (millimeter per revolution), and INCH (inch per revolution).
THREAD_SERIES—The possible values are: UNC, UNF, M_COARSE, M_FINE.
TAPER ANGLE
The thread is cut with the specified taper angle. This enables creation of tapered threads for standard or custom purposes.
CUT_STYLE
• THREAD_CONTINUOUS—The thread is milled in a single by continuous motion, regardless of the number of inserts on the thread tool.
• THREAD_INTERRUPTED—The thread is milled in a series of motions that may overlap. The thread motion overlap is controlled by the following parameters:
◦ THREAD_OVERLAP—Is the distance (in degrees) that a thread motion will continue beyond its end before exiting and moving to the start of the next thread motion. Type a value other than 0 (in degrees).
◦ PICKUP_OVERLAP—Is the distance (in threads or degrees) that the start of the next thread motion will overlap the end of the previous thread motion. Type a value other than 0 (in threads or degrees).
 |
These parameters are only applied when the thread mill has more than one tooth.
|
CUT_TYPE
This option controls where the material is relative to the tool and has two values:
• CLIMB—The tool is to the left of material (assuming clockwise spindle rotation). Corresponds to the CLIMB value of the CUT_TYPE manufacturing parameter.
• CONVENTIONAL—The tool is to the right of material (assuming clockwise spindle rotation). Corresponds to the UPCUT value of the CUT_TYPE manufacturing parameter.
The following options define the beginning and end of the cut motion:
• Start Overtravel—Specifies the initial height of the tool above the start surface at the beginning of the tool path.
• End Overtravel—Specifies the height at the end of the tool path that the tool overtravels below the end surface.
• Thread Start Angle—Specifies the angle in the XY plane that determines where the thread mill starts to cut the thread.
The following parameters enable creation of multiple passes in a single tool path for a thread milling sequence.
INITIAL_DIAMETER
It is the diameter of a hole prepared for thread milling and is used in the computation of number of roughing passes.
PROF_STOCK_ALLOW
Specifies the amount of stock left by the sequence tool path.
THREAD_DIAMETER
It is the value used to calculate the final diameter machined by the last profile pass, and by the spring passes. Here the external thread final diameter is THREAD_DIAMETER + PROF_STOCK_ALLOW and the internal thread final diameter is THREAD_DIAMETER - PROF_STOCK_ALLOW.
Roughing Pass Parameters
• NUM_ROUGH_PASSES—Together with ROUGH_INCREMENT, allows you to create multiple roughing passes. This parameter is ignored if INITIAL_DIAMETER and ROUGH_INCREMENT are specified.
• ROUGH_INCREMENT—Specifies the amount of stock to remove with each cut for roughing passes.
• ROUGH_CUT_SPEED—The feed rate used for the profiling and roughing passes
• ROUGH_SPINDLE_FEED—The rate at which the spindle rotates for rough passes.
• SPINDLE_SPEED—The rate at which the spindle rotates for roughing passes, if ROUGH_SPINDLE_SPEED is not specified.
• CUT_FEED—The feed rate used for the roughing passes, if ROUGH_CUT_FEED is not specified.
Profile Pass Parameters
• NUM_PROF_PASSES—Together with PROF_INCREMENT, allows you to create multiple profiling passes horizontally offset from each other. The default value is 1. This is equivalent to a semi-finishing pass.
• PROF_INCREMENT—Specifies the amount of stock to remove with each cut for profile passes.
• SPINDLE_SPEED—The rate at which the spindle rotates for profile passes.
• CUT_FEED—The feed rate used for the profile passes.
Spring Pass Parameters
• NUM_SPRING_PASSES—The number of spring passes when the tool moves along the final thread diameter defined by THREAD_DIAMETER parameter.
• FINISH_SPINDLE_FEED—The rate at which the machine spindle rotates for spring passes
• FINISH_CUT_FEED—The feed rate used for spring passes.
• SPINDLE_SPEED—The rate at which the spindle rotates for spring passes, if FINISH_SPINDLE_SPEED is not specified.
• CUT_FEED—The feed rate used for spring passes, if FINISH_CUT_FEED is not specified.