Cycle 1042 SHORT STROKE DEF. (#156 / #4-04-1)

ISO programming

G1042

Application

Use the definition cycle 1042 SHORT STROKE DEF. to define the reciprocation movement along the contour.

The contour to be machined must be shorter or only a little longer than the cutting edge of the grinding tool used. If the contour is longer, HEIDENHAIN recommends Cycle 1041 LONG STROKE DEF..

Cycle 1041 LONG STROKE DEF. (#156 / #4-04-1)

The reciprocation movement is defined using an interpolation position and the reciprocation movement up to the reversal points. The interpolation position is in the center of the reciprocating stroke.

The interpolation position facilitates programming of cylindrical grinding operations, especially for tapered workpieces. By programming in the workpiece coordinate system W-CS and flexible selection of the interpolation position, you can transfer the dimensions directly from the technical drawing. The control automatically calculates the movements along the contour.

Using Cycle 1042 SHORT STROKE DEF. combined with Cycle 1053 CONTINOUS CYLIND. GRIND., you can machine contours at diameter, step, or plane surfaces. Machining includes reciprocation movements and continuous infeed steps. This means that the infeed is even and performed without interruptions during the reciprocation movements.

Notes

 
Notice
Danger of collision!
If you program Q1058 PRE-POSITIONING MODE with 0, the control will ignore any safe positions. Q200 SET-UP CLEARANCE, Q260 CLEARANCE HEIGHT, and Q1031 SAFE DIAMETER have no effect. The control moves from the current position directly to the starting point. Risk of collision!
  1. If possible, program Q1058 not equal to 0
  2. Use a simulation to check the machining sequence
 
Notice
Danger of collision!
There must be sufficient room to incline the tool and approach it to the workpiece. Risk of collision during machining, especially for inside machining.
  1. Use the simulation to check the machining sequence
  • This cycle can be executed only in the FUNCTION MODE GRIND machining mode.
  • The cycle is CALL-active.
  • Use Cycle 1040 END CYLIND. GRINDING to reset the settings of Cycle 1042 SHORT STROKE DEF. at the end of cylindrical grinding.
  • The infeed direction directly affects the parameters to be programmed.
  • The following parameters are programmed depending on the infeed direction using X or Z coordinates:

  • Infeed direction

    X coordinate in the diameter

    Z coordinate

    X axis

    • Q368 OVERSIZE OF BLANK
    • Q1044 SUPPORT POINT OFFSET

    Z axis

    • Q1044 SUPPORT POINT OFFSET
    • Q368 OVERSIZE OF BLANK

Cycle parameters

Help graphic

Parameter

Q1040 Support position in X axis?

Position in the X axis of the ZX working plane

The interpolation position lies on the final contour and can be chosen as desired. For optimum results, use a dimensioned position in your drawing. This value has an absolute effect.

Input: 0...9999.99999

Q1041 Support position in Z axis?

Position in the Z axis of the ZX working plane

The interpolation position lies on the final contour and can be chosen as desired. For optimum results, use a dimensioned position in your drawing. This value has an absolute effect.

Input: –9999.9999...+9999.9999

Q1042 Infeed direction?

Axis and direction in which the control performs the infeed:

  • 0: X–
  • 1: X+
  • 2: Z–
  • 3: Z+

Selection using a selection menu (e.g., 0 I X–)

Input: 0, 1, 2, 3

Q368 Oversize before machining?

Oversize that is present on the finished part prior to the grinding operation. This oversize is effective in the direction opposite to the infeed direction.

In case of a radial infeed, the oversize refers to the diameter and is incremental.

Input: 0...99.99999

Q1043 Taper angle?

Definition of the apex angle of a cone:

>0: The cone becomes smaller towards its apex in the positive Z-axis direction.

<0: The cone becomes broader towards its apex in the positive Z-axis direction.

Input: -180...+180

Q1044 Offset of the support point?

Shifts the center of the reciprocation movement by the programmed value. The offset is perpendicular to the infeed direction. This value has an incremental effect.

Input: –9999.99999...+9999.99999

Q1000 Length of reciprocating stroke?

Length of reciprocation movement in mm

The interpolation position is at the center of the reciprocation movement.

With Q1044 SUPPORT POINT OFFSET, you can offset the center of the reciprocation movement.

Input: 0...+9999.9999

Q1001 Feed rate for reciprocation?

Speed of the reciprocating stroke in mm/min

Input: 0...999999

Q1049 Grinding wheel edge? (optional)

Definition of a grinding wheel edge or cutting edge of the grinding tool

Selection using a selection menu

Input: 100...760

Select grinding wheel edge

Q253 Feed rate for pre-positioning? (optional)

Traversing speed of the tool in mm/min. while approaching the pre-position

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

Q1058 Mode for pre-positioning? (optional)

Definition whether the control pre-positions the grinding tool and inclines it during machining:

0: The control does not pre-position the grinding tool and does not move it to any safe position. The tool is not inclined.

1: The control pre-positions the grinding tool and inclines it with Q531 ANGLE OF INCIDENCE.

2: The control pre-positions the grinding tool and inclines it using an automatically calculated inclination angle.

Input: 0, 1, 2

Positioning behavior in the definition cycles

Q260 Clearance height? (optional)

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

Input: –99999.9999...+99999.9999 or PREDEF

Q1031 Safe diameter? (optional)

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

At a diameter that is less than Q1040 SUPPORT POSITION X, the control assumes that you have programmed inside machining.

Input: 0...9999.99999 or PREDEF

Q200 Set-up clearance? (optional)

Distance between the tool and the contour at reversal point 1

This distance is measured in the direction opposite to the infeed direction. The set-up clearance is measured radially and is incremental.

Input: 0...99999.9999 or PREDEF

Q497 Precession angle? (optional)

Angle at which the control rotates the coordinate system around the tool axis.

This may be necessary if you have to bring the tool into a specific position due to space restrictions or to improve your view of the machining process.

Input: 0...359.99999

Q530 Inclination behavior? (optional)

Positioning behavior for inclined machining

1- MOVE: The control positions the rotary axes and performs compensation movements in the linear main axes. The compensation movements ensure that the relative position between the tool and the workpiece will not change during the positioning process.

2- TURN: The control positions the rotary axes only and does not perform any compensation movements.

Input: 1, 2

Q531 Angle of incidence? (optional)

Inclination angle of the tool relative to the workpiece

If you program Q1058=2, this parameter has no effect.

Input: -180...+180

Q533 Preferred dir. of incid. angle? (optional)

Selection of alternate possibilities of inclination. The inclination angle you define is used by the control to calculate the appropriate positioning of the rotary axis present on the machine. In general, there are two possible solutions. Via parameter Q533, you configure which solution option the control will use:

0: Solution that is the shortest distance from the current position.

-1: Solution that is in the range between 0° and –179.9999°

+1: Solution that is in the range between 0° and +180°

-2: Solution that is in the range between –90° and –179.9999°

+2: Solution that is in the range between +90° and +180°

Input: –2, –1, 0, +1, +2

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 1042 SHORT STROKE DEF. ~

Q1040=+0

;SUPPORT POSITION X ~

Q1041=+0

;SUPPORT POSITION Z ~

Q1042=+0

;INFEED DIRECTION ~

Q368=+1

;OVERSIZE OF BLANK ~

Q1043=+0

;TAPER ANGLE ~

Q1044=+0

;SUPPORT POINT OFFSET ~

Q1000=+0

;RECIPROCATING STROKE ~

Q1001=+1000

;RECIP. FEED RATE ~

Q1049=+120

;WHEEL EDGE ~

Q253=+750

;F PRE-POSITIONING ~

Q1058=+2

;PRE-POSITIONING MODE ~

Q260=+100

;CLEARANCE HEIGHT ~

Q1031=+100

;SAFE DIAMETER ~

Q200=+2

;SET-UP CLEARANCE ~

Q497=+0

;PRECESSION ANGLE ~

Q530=+1

;INCLINATION BEHAVIOR ~

Q531=+0

;ANGLE OF INCIDENCE ~

Q533=+0

;PREFERRED DIRECTION

Select grinding wheel edge

xx0: Selection of a cutting edge, without considering its length

The first two numerals define the cutting edge of the grinding tool to be used in the cycle.

By defining the cutting edge, the control will consider the tool angle from the tool table (e.g., the tiling angle ALPHA).

The tool angle is required if you programmed an automatic calculation of the inclination angle Q1058=2. The inclination angle depends on the cutting edge angle and the contour to be machined.

If you select this option, the control will not consider the cutting edge length when calculating the reciprocating stroke.

The control approaches reversal points 1 and 2 with the same grinding wheel edge.

Input

Cutting edge

Grinding wheel edge

Tool angle for inclination

120

1 – 2

1

ALPHA

210

2 – 1

2

ALPHA

230

2 – 3

2

BETA

290

2 – 9

2

ALPHA

320

3 – 2

3

BETA

560

5 – 6

5

ALPHA

650

6 – 5

6

ALPHA

670

6 – 7

6

BETA

690

6 – 9

6

ALPHA

760

7 – 6

7

BETA

Grinding pin
Special grinding pin
Cup wheel

Example for grinding wheel edge 120

x00: Selection of a grinding wheel edge

The first numeral defines the grinding wheel edge of the grinding tool to be used in the cycle.

The cycle with neither consider the cutting edge length nor calculate an inclination angle automatically (Q1058=2).

Selection options:

  • 100: Grinding wheel edge 1
  • 200: Grinding wheel edge 2
  • 300: Grinding wheel edge 3
  • 500: Grinding wheel edge 5
  • 600: Grinding wheel edge 6
  • 700: Grinding wheel edge 7
Grinding pin
Special grinding pin
Cup wheel

Example for grinding wheel edge 100

Examples: Q1049 Select grinding wheel edge

Example for grinding wheel edge 120

For machining, a grinding pin is used with parameter Q1049=120.

The control inclines the grinding tool, but does not consider the cutting-edge length.

Cylinder

Taper

Example for grinding wheel edge 100

For machining, a grinding pin is used with parameter Q1049=100.

The control neither inclines the grinding tool nor considers the cutting-edge length.

Cylinder

Taper