Cycle 860 CONT. RECESS, RADIAL

ISO programming

G860

Application

 
Machine

Refer to your machine manual.

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

This cycle enables you to radially cut in slots of any form.

You can use the cycle either for roughing, finishing or complete machining. Turning is run paraxially with roughing.

The cycle can be used for inside and outside machining. If the coordinate of the contour starting point is larger than that of the contour end point, the cycle runs outside machining. If the coordinate of the contour starting point is less than that of the contour end point, the cycle runs inside machining.

Roughing cycle sequence

  1. For the first recess with full contact, the control moves the tool at the reduced feed rate Q511 to the depth of the plunge + allowance.
  2. The control retracts the tool at rapid traverse.
  3. The control performs a stepover by Q510 x tool width (Cutwidth).
  4. The control then recesses again, this time with the feed rate Q478
  5. The control retracts the tool as defined in parameter Q462
  6. The control machines the area between the starting position and the end point by repeating steps 2 through 4.
  7. As soon as the slot width has been achieved, the control returns the tool at rapid traverse to the cycle starting point.

Multiple plunging

  1. For the recess with full contact, the control moves the tool at a reduced feed rate Q511 to the depth of the plunge + allowance
  2. The control retracts the tool at rapid traverse after each cut
  3. The position and number of full cuts depend on Q510 and the width of the tooth (CUTWIDTH). Steps 1 to 2 are repeated until all full cuts have been made
  4. The control machines the remaining material at the feed rate Q478
  5. The control retracts the tool at rapid traverse after each cut
  6. The control repeats steps 4 and 5 until the ridges have been roughed
  7. The control then positions the tool at rapid traverse back to the cycle starting point

Finishing cycle sequence

  1. The control positions the tool at rapid traverse to the first slot side.
  2. The control finishes the side wall of the slot at the defined feed rate Q505.
  3. The control finishes one half of the slot at the defined feed rate.
  4. The control retracts the tool at rapid traverse.
  5. The control positions the tool at rapid traverse to the second slot side.
  6. The control finishes the side wall of the slot at the defined feed rate Q505.
  7. The control finishes the other half of the slot at the defined feed rate.
  8. The control returns the tool at rapid traverse to the cycle starting point.

Notes

 
Notice
Caution: Danger to the tool and workpiece!
The cutting limit defines the contour range to be machined. The approach and departure paths can cross over the cutting limits. The tool position before the cycle call influences the execution of the cutting limit. The TNC7 machines the area to the right or to the left of the cutting limit, depending on which side the tool was positioned before calling the cycle.
  1. Before calling the cycle, make sure to position the tool at the side of the cutting boundary (cutting limit) where the material will be machined
  • This cycle can be executed only in the FUNCTION MODE TURN machining mode.
  • The tool position at cycle call defines the size of the area to be machined (cycle starting point)

Notes on programming

  • Program a positioning block to the starting position with radius compensation R0 before the cycle call.
  • Before programming the cycle call, make sure to program Cycle 14 CONTOUR or SEL CONTOUR to be able to define the subprograms.
  • If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.
  • FUNCTION TURNDATA CORR TCS: Z/X DCW and/or an entry in the DCW column of the turning tool table can be used to activate an oversize for the recessing width. DCW can accept positive and negative values and is added to the recessing width: CUTWIDTH + DCWTab + FUNCTION TURNDATA CORR TCS: Z/X DCW. A DCW programmed via FUNCTION TURNDATA CORR TCS is not visible while a DCW entered in the table is active in the graphics.
  • If multiple plunging is active (Q562 = 1) and the value Q462 RETRACTION MODE is not equal to 0, then the control issues an error message.
  • Finishing the contour requires programming tool radius compensation RL or RR in the contour description.

Cycle parameters

Help graphic

Parameter

Q215 Machining operation (0/1/2/3)?

Define extent of machining:

0: Roughing and finishing

1: Only roughing

2: Only finishing to final dimension

3: Only finishing to oversize

Input: 0, 1, 2, 3

Q460 Set-up clearance?

Reserved; currently no functionality

Q478 Roughing feed rate?

Feed rate during roughing. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute.

Input: 0...99999.999 or FAUTO

Q483 Oversize for diameter?

Diameter oversize on the defined contour. This value has an incremental effect.

Input: 0...99.999

Q484 Oversize in Z?

Oversize of the defined contour in the axial direction. This value has an incremental effect.

Input: 0...99.999

Q505 Finishing feed rate?

Feed rate during finishing. If M136 has been programmed, the value is interpreted by the control in millimeters per revolution; without M136, in millimeters per minute.

Input: 0...99999.999 or FAUTO

Q479 Machining limits (0/1)?

Activate cutting limit:

0: No cutting limit active

1: Cutting limit (Q480/Q482)

Input: 0, 1

Q480 Value of diameter limit?

X value for contour limit (diameter value)

Input: –99999.999...+99999.999

Q482 Value of cutting limit in Z?

Z value for contour limit

Input: –99999.999...+99999.999

Q463 Limit to plunging depth?

Maximum recessing depth per step

Input: 0...99.999

Q510 Overlap factor for recess width?

Factor Q510 influences the lateral infeed of the tool during roughing. Q510 is multiplied by the CUTWIDTH of the tool. This results in the lateral infeed factor "k".

Input: 0.001...1

Q511 Feed rate factor in %?

Factor Q511 influences the feed rate for full recessing, i.e. when a recess is cut with the entire tool width CUTWIDTH.

If you use this feed rate factor, optimum cutting conditions can be created during the remaining roughing process. In this manner, you can define the roughing feed rate Q478 to be so high that it permits optimum cutting conditions for each overlap of the cutting width (Q510). The control thus reduces the feed rate by the factor Q511 only when recessing with full contact. In sum, this can lead to reduced machining times.

Input: 0.001...150

Q462 Retraction behavior (0/1)?

With Q462, you define the retraction behavior after the recess.

0: The control retracts the tool along the contour

1: The control first moves the tool at an angle away from the contour and then retracts it

Input: 0, 1

Q211 Dwell time / 1/min?

A dwell time can be specified in revolutions of the tool spindle, which delays the retraction after the recessing on the floor. Retraction is performed only after the tool has remained for Q211 revolutions.

Input: 0...999.99

Q562 Multiple plunging (0/1)?

0: No multiple plunging: the first recess is made into the uncut material, and the subsequent ones are laterally offset and overlap by the amount Q510 * Width of the cutter (CUTWIDTH)

1: Multiple plunging; rough grooving is performed with full tool engagement into uncut material. Then the remaining ridges are machined. These are recessed successively. This leads to a centralized chip removal, considerably reducing the risk of chip entrapment

Input: 0, 1

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 860 CONT. RECESS, RADIAL ~

Q215=+0

;MACHINING OPERATION ~

Q460=+2

;SAFETY CLEARANCE ~

Q478=+0.3

;ROUGHING FEED RATE ~

Q483=+0.4

;OVERSIZE FOR DIAMETER ~

Q484=+0.2

;OVERSIZE IN Z ~

Q505=+0.2

;FINISHING FEED RATE ~

Q479=+0

;CONTOUR MACHINING LIMIT ~

Q480=+0

;DIAMETER LIMIT VALUE ~

Q482=+0

;LIMIT VALUE Z ~

Q463=+0

;LIMIT TO DEPTH ~

Q510=0.08

;RECESSING OVERLAP ~

Q511=+100

;FEED RATE FACTOR ~

Q462=+0

;RETRACTION MODE ~

Q211=3

;DWELL TIME IN REVS ~

Q562=+0

;MULTIPLE PLUNGING

14 L X+75 Y+0 Z+2 R0 FMAX M303

15 CYCL CALL

16 M30

17 LBL 2

18 L X+60 Z-20

19 L X+45

20 RND R2

21 L X+40 Y-25

22 L Z+0

23 LBL 0