Cycle 830 THREAD CONTOUR-PARALLEL

ISO programming

G830

Application

 
Machine

Refer to your machine manual.

This function must be enabled and adapted by the machine manufacturer.

cyc830

This cycle enables you to run 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.

  1. The control positions the tool at rapid traverse at set-up clearance in front of the thread and performs an infeed movement.
  2. 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.
  3. The control retracts the tool at rapid traverse to the set-up clearance.
  4. The control returns the tool at rapid traverse to the beginning of cut.
  5. The control performs an infeed movement. For the infeeds, to the angle of infeed Q467 is used.
  6. The control repeats this procedure (steps 2 to 5) until the thread depth is reached.
  7. The control performs the number of air cuts as defined in Q476.
  8. The control repeats this procedure (steps 2 to 7) until the desired Number of thread grooves Q475 is reached.
  9. The control returns the tool at rapid traverse to the cycle starting point.
 
Tip

While the control cuts a thread, the feed-rate override knob is disabled. The feed-rate override knob is still active to a limited extent.

Notes

 
Notice
Danger of collision!
Cycle 830 executes the overrun Q466 following the programmed contour. There is a danger of collision!
  1. Clamp the workpiece in such a way that there is no danger of collision if the control extends the contour by Q466, Q467.
 
Notice
Danger of collision!
If the tool is pre-positioned at a negative diameter position, the effect of parameter Q471 Thread position is reversed. This means that the external thread is 1 and the internal thread 0. There is a risk of collision between tool and workpiece.
  1. 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°, e.g., 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.
 
Notice
Danger of collision!
The retraction motion is directly to the starting position. There is a danger of collision!
  1. Always position the tool in such a way that the control can approach the starting point at the end of the cycle without collisions.
 
Notice
Caution: Danger to the tool and workpiece!
If you program an angle of infeed Q467 wider than the side angle of the thread, this may destroy the thread flanks. If the angle of infeed is modified, the position of the thread is shifted in an axial direction. With a changed angle of infeed, the tool can no longer interface the thread grooves.
  1. Do not program the infeed angle Q467 to be larger than the thread edge angle
  • This cycle can only be executed 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

cyc830_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

cyc830_2

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.

 
Tip

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.

Example

11 CYCL DEF 14.0 CONTOUR

12 CYCL DEF 14.1 CONTOUR LABEL2

13 CYCL DEF 830 THREAD CONTOUR-PARALLEL ~

Q471=+0

;THREAD POSITION ~

Q461=+0

;THREAD ORIENTATION ~

Q460=+2

;SAFETY CLEARANCE ~

Q472=+2

;THREAD PITCH ~

Q473=+0

;DEPTH OF THREAD ~

Q474=+0

;THREAD RUN-OUT ~

Q465=+4

;STARTING PATH ~

Q466=+4

;OVERRUN PATH ~

Q463=+0.5

;MAX. CUTTING DEPTH ~

Q467=+30

;ANGLE OF INFEED ~

Q468=+0

;TYPE OF INFEED ~

Q470=+0

;STARTING ANGLE ~

Q475=+30

;NUMBER OF STARTS ~

Q476=+30

;NUMBER OF AIR CUTS

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