Cycle 1025 GRINDING CONTOUR (#156 / #4-04-1)

ISO programming

G1025

Application

Use Cycle 1025 GRINDING CONTOUR in combination with Cycle 14 CONTOUR to grind open and closed contours.

Cycle sequence

  1. The control first moves the tool at rapid traverse to the starting position in the X and Y directions and then to clearance height Q260.
  2. The tool uses rapid traverse to move to set-up clearance Q200 above the coordinate surface.
  3. From there, it moves at the pre-positioning feed rate Q253 to the depth Q201.
  4. If programmed, the control performs the approach movement.
  5. The cycle starts with the first stepover Q534.
  6. If programmed, the control performs the number of idle runs Q456 after each infeed.
  7. This process (steps 5 and 6) is repeated until the contour or finishing allowance Q14 has been reached.
  8. After the last infeed, the specified number of air strokes at contour end Q457 are performed.
  9. The control performs the optional departure movement.
  10. Finally, the tool is moved at rapid traverse to the clearance height.

Notes

  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • The last stepover may be smaller depending on the input.
  • Keep in mind that the cycle takes M109 or M110 into account, if programmed. In this case, the control will display the feed rate of the center path of the milling tool. The feed rate shown in the status display may thus become lower for inside radii or become higher for outside radii.
  • Adapting the feed rate for circular paths with M109

Note on programming

  • If you want to program a reciprocating stroke, you need to define and start it before executing this cycle.

Open contour

  • Approach and departure movements for the contour can be programmed using APPR and DEP or Cycle 270.

Closed contour

  • In the case of a closed contour, only Cycle 270 is available for programming approach and departure movements.
  • When grinding a closed contour, it is not possible to alternate between climb and up-cut grinding (Q15 = 0). The control issues an error message.
  • If you programmed approach and departure movements, the starting position will shift with every infeed. If no approach and departure movements have been programmed, the control automatically generates a vertical movement and the starting position on the contour will not shift.

Cycle parameters

Help graphic

Parameter

Q203 Workpiece surface coordinate?

Coordinate on the workpiece surface referenced to the active datum. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q201 Depth?

Distance between the workpiece surface and the contour floor. This value has an incremental effect.

Input: –99999.9999...+0

Q14 Finishing allowance for side?

Lateral oversize that is to remain after machining. This allowance must be less than Q368. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q368 Side oversize before machining?

Lateral oversize that is present prior to the grinding operation. This value must be greater than Q14. This value has an incremental effect.

Input: –0.9999...+99.9999

Q534 Lateral infeed?

Amount by which the grinding tool is laterally infed.

Input: 0.0001...99.9999

Q456 Idle runs around contour?

Number of times the grinding tool executes the contour without removing material after every infeed.

Input: 0...99

Q457 Idle runs at contour end?

Number of times the grinding tool executes the contour without material removal after the last infeed.

Input: 0...99

Q207 Feed rate for grinding?

Traversing speed of the tool during grinding of the contour in mm/min

Input: 0...99999.999 or FAUTO, FU

Q253 Feed rate for pre-positioning?

Traversing speed of the tool when approaching the DEPTH Q201. The feed rate has an effect below the SURFACE COORDINATE Q203. Input in mm/min.

Input: 0...99999.9999 or FMAX, FAUTO, PREDEF

Q15 Up-cut / climb grinding (-1/+1)?

Define the machining direction of the contours:

+1: Climb grinding

-1: Up-cut grinding

0: Alternating between climb grinding and up-cut grinding

Input: -1, 0, +1

Q260 Clearance height?

Position at which no collision can occur with the workpiece. This value has an absolute effect.

Input: –99999.9999...+99999.9999 or PREDEF

Q200 Set-up clearance?

Distance between tool tip and workpiece surface. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

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 1025 GRINDING CONTOUR ~

Q203=+0

;SURFACE COORDINATE ~

Q201=-20

;DEPTH ~

Q14=+0

;ALLOWANCE FOR SIDE ~

Q368=+0.1

;OVERSIZE AT START ~

Q534=+0.05

;LATERAL INFEED ~

Q456=+0

;IDLE RUNS, CONTOUR ~

Q457=+0

;IDLE RUNS, CONT. END ~

Q207=+200

;GRINDING FEED RATE ~

Q253=+750

;F PRE-POSITIONING ~

Q15=+1

;TYPE OF GRINDING ~

Q260=+100

;CLEARANCE HEIGHT ~

Q200=+2

;SET-UP CLEARANCE