Thread cycles


Thread cycle allows to generate passes (one ore more) for creating thread with specified parameters.

 

LatheThreadCycle

 

Threading area is specified by geometrical contour. Contour defines thread bottom diameter (inner diameter for external thread and outer diameter for inner thread). Second diameter is calculated by "Depth" parameter. Thread type - inner or outer - is specified by contour machining side (Perpendicular arrow near contour start point). Thread type - left or right - is specified by contour machining direction (Parallel arrow near contour start point) and spindle rotation direction. Contour approach and retract areas allows to set prolongation or chamfer for tool output.

The Properties window for the job assignment item has the following parameters.

 

LatheThreadCycleProps

 

Thread profile is specified by tool form and parameters in "Thread form".

Thread lead can be set by two ways. In the first case lead is defined as the distance between two same points of the profile, located on the neighboring threads. In the second case lead is specified by count of turns per length unit.

Value in "Depth" field defines thread profile height (difference between outer and inner diameters). This value must have positive value. Direction of this value calculates automatically and depends from contour "Machining Side" parameter.

"Thread angle" and "Inclination angle" parameters defines angle of tool plunge at each pass, if plunge mode is "Flank" or "Alternate Flank".

 

Thread angle

Inclination angle

 

 

Operation allows to create multistart threads by editing <Number of starts> and <Spindle start angle> parameters. Various cycle types use <Number of starts> differently. In ISO G76 numbers of starts sends to cycle as a parameter. But some machines have not this parameter in cycle. In this case it is possible to create multistart threads by making the same cycle with another <Spindle start angle> parameter value. Another way is using ISO G92 or ISO G32/33. In this case operation automatically generates passes with different spindle start angles.

Parameters in <Sequence> group defines numbers of starts and plunge mode for each pass.

Value in <Sequence> combobox defines plunge mode. The following types of strategies are available:

  • <Radial>. The direction of plunge is perpendicular to the axis of rotation.

 

image726

 

  • <Flank>. The plunge is made along one side of the ledge.

 

image728

 

  • <Alternate flank>. Plunge is made alternately along the two lateral sides of the ledge.

 

image730

 

  • <Modified flank>. Plunge with angle, specified at <Angle> parameter.

image732

 

Practically thread is processed by several passes. It allows to improve surface quality and reduce tool loading.

It is possible to specify number of passes by setting count directly or by setting first pass depth. In the last case number of starts calculates automatically from thread profile depth.

If cutting depth is constant, plunge to the next layer leads to increasing machining area and tool loading. It is possible to calculate cutting depth provides constant machining area and tool loading. "Determine cut depth from" parameter can accept two values: equal area and equal depth.

 

Equal area

Equal depth

 

In <Equal area> mode cutting depth decreases at each level. It is possible to set <Minimal cut depth>. If calculated depth becomes less than this value, minimal cut depth will be used.

To ensure the cleanliness of the surface last pass is performed with very small stock, and then the smoothering of the finished profile is performed several times without any stock. <Finish pass depth> parameter defines finish pass stock, <Finish pass count> parameter defines count of passes along ready profile, taking with finishing pass.

Thread toolpath can be generated in various format. We consider each of them separately.

 

Multipass thread cycle (ISO G76) allows you to use a single frame of the NC-program to set all parameters necessary for machine to make thread. Required depth is reached automatically by generating several passes. Among the parameters of the cycle there are start and finish point coordinates, taper angle (for taper threads), size of chamfer for tool out, profile angles, thread depth, passes count, plunge strategy and others. See NC control documentation for more information.

 

Example of NC program:

 

G01 X70 Z5.0 F1.0 M08            (Approach to start point)

G01 X70 Z5.0 F1.0 M08            (Approach to start point)

G76 P010060 

G76 X57.4 Z-24.0 P1.3 Q0.35 F2.0 (Calling G76 multipass thread cycle) 

G00 X200.0 Z150.0 M09            (Retract) 

 

Single pass thread cycle ISO G92 (can be G92, G78, G21 and others in different NC controls) generates closed set of moves for one threading pass. Picture below shows processing schema. Before calling this cycle tool is in Start point. Cycle is called by one frame of NC-program, defines thread start point, step, taper size, chamfer size and others. As a result of this frame the tool goes from Start to TSP point, thread to TEP point and returns to Start point. Usually threading is processed by several passes, so NC-program consists several cycle calls with various thread diameters.

 

 

Example of NC-program:

 

X60.0 Z20.0 M08 

G01 Z10.0 F1.0        (Approach to Start point)

G92 X29.4 Z-52.0 F2.0 (Calling cycle for one threading pass)

X28.9                 (Modal calling G92 cycle with another diameter value)

X28.5                 (Modal calling G92 cycle with another diameter value) 

X28.1                 (Modal calling G92 cycle with another diameter value)

X27.8                 (Modal calling G92 cycle with another diameter value)

X27.56                (Modal calling G92 cycle with another diameter value)

X27.36                (Modal calling G92 cycle with another diameter value)

X27.26                (Modal calling G92 cycle with another diameter value)

G00 X200.0Z150.0M09   (Retract)

 

Advanced (expanded) thread machining is processed by using ISO G32/G33 (can be different in various machines). This command activates continuous cylindric or taper threading mode with constant step. In this mode synchronization between tool movement and spindle rotation is enabled. All tool movements will processed in thread mode until the interpolation switching or rapid toolpath command will be detected. If tool moves parallel to the spindle rotation axis, cylindric thread will be formed. If tool moves both parallel and perpendicular to spindle rotation axis simultaneously, taper thread will be formed. It is possible to form special face thread, if tool moves perpendicular to spindle rotation axis. In this case groove looks like spiral of Archimedes will be formed at face.

G32/G33 command does not generate any moves, so all working tool moves, approaches, retracts, transitions to the next passes must be programmed in NC program directly.

Example of NC program:

 

G00 X60.0 Z10.0 M08 (Approach to Start point) 

G00 X29.4           (Approach to start of pass 1)

G32 Z-52.0 F2.0     (Threading synchronized with spindle)

G00 X60.0           (Return to Start)

Z10.0 

X28.9               (Approach to start of pass 2)

G32 Z-52.0          (Threading synchronized with spindle)

G00 X60.0           (Return to Start)

Z10.0 

X28.5               (Approach to start of pass 3)

G32 Z-52.0          (Threading synchronized with spindle)

G00 X60.0           (Return to Start)

Z10.0 

X28.1               (Approach to start of pass 4)

G32 Z-52.0          (Threading synchronized with spindle)

G00 X60.0           (Return to Start)

Z10.0 

X27.8               (Approach to start of pass 5)

G32 Z-52.0          (Threading synchronized with spindle)

G00 X60.0           (Return to Start)

Z10.0 

X27.56              (Approach to start of pass 6) 

G32 Z-52.0          (Threading synchronized with spindle)

G00 X60.0           (Return to Start)

Z10.0 

X27.36              (Approach to start of pass 7)

G32 Z-52.0          (Threading synchronized with spindle)

G00 X60.0           (Return to Start)

Z10.0 

X27.26              (Approach to start of pass 8)

G32 Z-52.0          (Threading synchronized with spindle)

G00 X60.0           (Return to Start)

Z10.0

X200.0 Z150.0 M09   (Retract)

 

 

 

See also:

Lathe Machining

Lathe contouring

Types of the job assignment elements (cycles)