Cycle 831 THREAD LONGITUDINAL
ISO programming
G831
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
This cycle enables you to execute longitudinal turning of threads.
You can machine single threads or multi-threads with this cycle.
If you do not enter a thread depth, the cycle uses thread depth in accordance with the ISO1502 standard.
The cycle can be used for inside and outside machining.
Related topics
- Cycle 832 THREAD EXTENDED optional longitudinal or plane thread, different taper threads, approach path and overrun path
Cycle sequence
The control uses the position of the tool at cycle call as the cycle starting point.
- The control positions the tool at rapid traverse at set-up clearance in front of the thread and performs an infeed movement.
- The control performs a paraxial longitudinal cut. When doing so, the control synchronizes feed rate and speed so that the defined pitch is machined.
- The control retracts the tool at rapid traverse to the set-up clearance.
- The control returns the tool at rapid traverse to the beginning of cut.
- The control performs an infeed movement. For the infeeds, to the angle of infeed Q467 is used.
- The control repeats this procedure (steps 2 to 5) until the thread depth is reached.
- The control performs the number of air cuts as defined in Q476.
- The control repeats this procedure (steps 2 to 7) until the desired Number of thread grooves Q475 is reached.
- The control returns the tool at rapid traverse to the cycle starting point.
While the control cuts a thread, the feed-rate override knob is disabled. The spindle-speed override knob is still active to a limited extent.
Notes
- With some machine types, the turning tool is not clamped in the milling spindle, but in a separate holder adjacent to the spindle. In such cases, the turning tool cannot be rotated through 180° (for example, to machine internal and external threads with only one tool). If, with such a machine, you wish to use an outside tool for inside machining, you can execute machining in the negative X diameter range and reverse the direction of workpiece rotation.
- Always position the tool in such a way that the control can approach the starting point at the end of the cycle without collisions.
- Do not program the angle of infeed Q467 to be larger than the thread edge angle
- This cycle can be executed only in the FUNCTION MODE TURN machining mode.
- The number of threads for thread cutting is limited to 500.
- In Cycle 832 THREAD EXTENDED, parameters are available for approach and overrun.
Notes on programming
- Program a positioning block to the starting position with radius compensation R0 before the cycle call.
- The control uses the set-up clearance Q460 as approach length. The approach path must be long enough for the feed axes to be accelerated to the required velocity.
- The control uses the thread pitch as idle travel path. The idle travel distance must be long enough to decelerate the feed axes.
- If the TYPE OF INFEED Q468 is equal to 0 (consistent chip cross section), then an ANGLE OF INFEED must be defined to be larger than 0 in Q467.
Cycle parameters
Help graphic | Parameter |
---|---|
Q471 Thread position (0=ext./1=int.)? Define the position of the thread: 0: External thread 1: Internal thread Input: 0, 1 | |
Q460 Setup clearance? Set-up clearance in radial and axial direction. In axial direction, the set-up clearance is used for acceleration (approach path) until the synchronized feed rate is reached. Input: 0...999.999 | |
Q491 Thread diameter? Define the nominal diameter of the thread. Input: 0.001...99999.999 | |
Q472 Thread pitch? Pitch of the thread Input: 0...99999.999 | |
Q473 Thread depth (radius)? Depth of the thread. If you enter 0, the depth is assumed for a metric thread based on the pitch. This value has an incremental effect. Input: 0...999.999 | |
Q492 Contour start in Z? Z coordinate of the starting point Input: –99999.999...+99999.999 | |
Q494 Contour end in Z? Z coordinate of the end point, including the thread runout Q474 Input: –99999.999...+99999.999 | |
Q474 Length of thread runout? Length of the path on which, at the end of the thread, the tool is lifted from the current plunging depth to the thread diameter Q460. This value has an incremental effect. Input: 0...999.999 | |
Q463 Maximum cutting depth? Maximum plunging depth in radial direction relative to the radius. Input: 0.001...999.999 | |
Q467 Feed angle? Angle at which the infeed Q463 occurs. The reference angle is the line perpendicular to the rotary axis. Input: 0...60 | |
Q468 Infeed type (0/1)? Define the type of infeed: 0: Consistent chip cross section (the infeed becomes less as the depth increases) 1: Constant plunging depth Input: 0, 1 | |
Q470 Starting angle? Angle of the turning spindle at which the thread is to be started. Input: 0...359999 | |
Q475 Number of thread grooves? Number of thread grooves Input: 1...500 | |
Q476 Number of air cuts? Number of air cuts without infeed at finished thread depth Input: 0...255 |
NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.
Change the following contents as needed:
- Tools
- Cutting parameters
- Feed rates
- Clearance height or safe position
- Machine-specific positions (e.g., with M91)
- Paths of program calls
Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.
In addition, test the NC programs using the simulation before the actual program run.
With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.
11 CYCL DEF 831 THREAD LONGITUDINAL ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
12 L X+80 Y+0 Z+2 FMAX M303 | ||
13 CYCL CALL |