Cycle 1022 CYLINDER, FAST-STROKE GRINDING (option 156)

ISO programming

G1022

Application

 
Machine

Refer to your machine manual!

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

With the cycle 1022 CYLINDER, FAST STROKE GRINDING, you can grind circular pockets and circular studs. In the process, the control executes circular and helical paths in order to completely machine the cylinder surface. In order to achieve the required accuracy and surface quality, you can overlay the movement with a reciprocating stroke. The feed rate of the reciprocating stroke is usually so large that multiple reciprocating strokes per circular path are executed. This is equivalent to grinding with a rapid stroke. The lateral infeeds occur above or below depending on the definition. You can program the feed rate of the reciprocating stroke in the cycle.

Cycle sequence

  1. The control positions the tool above the cylinder based on the POCKET POSITION Q367. At FMAX, the control then moves the tool to the CLEARANCE HEIGHT Q260.
  2. At FMAX, the tool moves to the starting point in the working plane and then at F PRE-POSITIONING Q253 to the SET-UP CLEARANCE Q200.
  3. The grinding tool moves to the starting point in the tool axis. The starting point depends on the MACHINING DIRECTION Q1031. If you have defined a reciprocating stroke in Q1000, then the control starts the reciprocating stroke.
  4. Depending on the parameter Q1021, the control laterally infeeds the grinding tool. The control then infeeds in the tool axis.
  5. Infeed

  6. If the final depth has been reached, then the grinding tool moves for another full circle without a tool axis infeed.
  7. The control repeats steps 4 and 5 until the diameter of the finished part Q223 or the oversize Q14 has been reached.
  8. After the last infeed run, the grinding tool executes the IDLE RUNS, CONT. END Q457.
  9. The grinding tool leaves the cylinder on a semi-circular path to the safety clearance Q200 and stops the reciprocating stroke.
  10. At F PRE-POSITIONING Q253, the control moves the tool to the SAFETY CLEARANCE Q200 and then in rapid traverse to the CLEARANCE HEIGHT Q260.

Infeed

  1. The control infeeds the grinding tool in a semi-circle to the LATERAL INFEED Q534.
  2. The grinding tool executes a full circle and performs any programmed IDLE RUNS, CONTOUR Q456.
  3. If the area to be traversed in the tool axis is greater than the grinding wheel width B, then the cycle moves in a helical path.

Helical path

You can influence the helical path via a pitch in the parameter Q1032. The pitch per helical path (= 360°) is relative to the grinding wheel width.

The number of helical paths (= 360°) depends on the pitch and the DEPTH Q201. The smaller the pitch, the more helical paths (= 360°) there are.

Example:

  • Grinding wheel width B = 20 mm
  • Q201 DEPTH = 50 mm
  • Q1032 PITCH FACTOR (pitch) = 0.5

The control calculates the relationship between the pitch relative to the grinding wheel width.

Pitch per helical path = Maximale Zustelltiefe

The control covers the distance of 10 mm in the tool axis within a helix. The DEPTH Q201 and the pitch per helical path result in five helical paths.

Number of helical paths = Anzahl der Helixbahnen

Notes

 
Machine

The overrides for the reciprocation movements can be changed by the machine manufacturer.

  • This cycle can only be executed in the FUNCTION MODE MILL machining mode.
  • The control always starts the reciprocating stroke in the positive direction.
  • The last lateral infeed may be smaller depending on the input.
  • The control does not depict the reciprocating movement in the simulation. The reciprocating movement is depicted in the simulation graphics in the Program run, single block and Program run, full sequence operating modes.
  • You can also execute this cycle with a milling cutter. In the case of a milling cutter, the tooth length LCUTS equals the width of the grinding wheel.

Notes on programming

  • The control assumes that the bottom of the cylinder has a floor. For this reason, you can define an overshoot in Q1030 only at the surface. If you machine a through hole, for example, then you must take into account the lower overshoot in DEPTH Q201.
  • If Q1000=0, then the control does not execute a superimposed reciprocating movement.

Cycle parameters

Help graphic

Parameter

Q650 Type of figure?

Geometry of the figure:

0: Pocket

1: Island

Input: 0, 1

Q223 Finished part diameter?

Diameter of the fully machined cylinder

Input: 0...99999.9999

cyc1022_1

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

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

Q367 Position of pocket (0/1/2/3/4)?

Position of the figure relative to the position of the tool during the cycle call:

0: Tool pos. = Center of figure

1: Tool pos. = Quadrant transition at 90°

2: Tool pos. = Quadrant transition at 0°

3: Tool pos. = Quadrant transition at 270°

4: Tool pos. = Quadrant transition at 180°

Input: 0, 1, 2, 3, 4

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

Q1030 Offset to surface?

Position of the upper edge of the tool on the surface. The offset serves as the overshoot path on the surface for the reciprocating stroke. This value has an absolute effect.

Input: 0...999.999

Q201 Depth?

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

Input: –99999.9999...+0

cyc1022_2

Q1031 Machining direction?

Definition of the machining direction. The starting position arises from this.

–1 or 0: The control machines the contour from up to down during the first infeed cut.

+1: The control machines the contour from up to down during the first infeed cut.

Input: -1, 0, +1

Q534 Lateral infeed?

Amount by which the grinding tool is laterally infed.

Input: 0.0001...99.9999

Q1032 Factor for pitch of helix?

You can define the pitch of the helical path (= 360°) with the factor Q1032. This results in the infeed depth per helical path (= 360°). Q1032 is multiplied by the width B of the grinding tool.

Input: 0.000...1000

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

Q1000 Length of reciprocating stroke?

Length of the reciprocating movement, parallel to the active tool axis

0: The control does not perform a reciprocating motion.

Input: 0...9999.9999

Q1001 Feed rate for reciprocation?

Speed of the reciprocating stroke in mm/min

Input: 0...999999

Q1021 One-sided infeed (0/1)?

Position at which the lateral infeed occurs:

0: Lower and upper lateral infeed

1: One-sided infeed depending on Q1031

  • If Q1031 = -1, then the lateral infeed is performed above.
  • If Q1031 = +1, then the lateral infeed is performed below.

Input: 0, 1

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 type of contour grinding:

+1: Climb grinding

-1 or 0: Up-cut grinding

Input: -1, 0, +1

Q260 Clearance height?

Absolute height at which no collision can occur with the workpiece.

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 1022 CYLINDER, FAST-STROKE GRINDING ~

Q650=+0

;FIGURE TYPE ~

Q223=+50

;FINISHED PART DIA. ~

Q368=+0.1

;OVERSIZE AT START ~

Q14=+0

;ALLOWANCE FOR SIDE ~

Q367=+0

;POCKET POSITION ~

Q203=+0

;SURFACE COORDINATE ~

Q1030=+2

;SURFACE OFFSET ~

Q201=-20

;DEPTH ~

Q1031=-1

;MACHINING DIRECTION ~

Q534=+0.05

;LATERAL INFEED ~

Q1032=+0.5

;PITCH FACTOR ~

Q456=+0

;IDLE RUNS, CONTOUR ~

Q457=+0

;IDLE RUNS, CONT. END ~

Q1000=+5

;RECIPROCATING STROKE ~

Q1001=+5000

;RECIP. FEED RATE ~

Q207=+50

;GRINDING FEED RATE ~

Q253=+750

;F PRE-POSITIONING ~

Q15=+1

;TYPE OF GRINDING ~

Q260=+100

;CLEARANCE HEIGHT ~

Q200=+2

;SET-UP CLEARANCE