Cycle 830 THREAD CONTOUR-PARALLEL
ISO programming
G830
Application
Refer to your machine manual.
This function must be enabled and adapted by the machine manufacturer.
This cycle enables you to execute both face turning and longitudinal turning of threads with any shape.
You can machine single threads or multi-threads with this cycle.
If you do not enter a thread depth in the cycle, the cycle uses a standardized thread depth.
The cycle can be used for inside and outside machining.
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 runs a thread cut parallel to the defined thread contour. 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
- Clamp the workpiece in such a way that there is no danger of collision if the control extends the contour by Q466, Q467.
- 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.
- Both the approach and overrun take place outside the defined contour.
Notes on programming
- Program a positioning block to the starting position with radius compensation R0 before the cycle call.
- The approach path (Q465) must be long enough for the feed axes to be accelerated to the required velocity.
- The overrun path (Q466) must be long enough to decelerate the feed axes.
- Before programming the cycle call, make sure to program Cycle 14 CONTOUR or SEL CONTOUR to be able to define the subprograms.
- 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.
- If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.
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 | |
Q461 Thread orientation (0/1)? Define the direction of the thread pitch: 0: L (parallel to the turning axis) 1: Perpendicular (perpendicular to the turning axis) Input: 0, 1 | |
Q460 Set-up clearance? Set-up clearance perpendicular to the thread pitch Input: 0...999.999 | |
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 | |
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 | |
Q465 Starting path? Length of the path in the direction of the pitch at which the feed axes are accelerated to the required speed. The approach path is outside of the defined thread contour. This value has an incremental effect. Input: 0.1...99.9 | |
Q466 Overrun path? Input: 0.1...99.9 | |
Q463 Maximum cutting depth? Maximum infeed perpendicular to the thread pitch Input: 0.001...999.999 | |
Q467 Feed angle? Angle at which the infeed Q463 occurs. The reference angle is formed by the parallel line to the thread pitch. 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 14.0 CONTOUR | ||
12 CYCL DEF 14.1 CONTOUR LABEL2 | ||
13 CYCL DEF 830 THREAD CONTOUR-PARALLEL ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
14 L X+80 Y+0 Z+2 R0 FMAX M303 | ||
15 CYCL CALL | ||
16 M30 | ||
17 LBL 2 | ||
18 L X+60 Z+0 | ||
19 L X+70 Z-30 | ||
20 RND R60 | ||
21 L Z-45 | ||
22 LBL 0 |