Cycle 1015 PROFILE DRESSING (option 156)

ISO programming

G1015

Application

 
Machine

Refer to your machine manual.

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

Use Cycle 1015 PROFILE DRESSING to dress a defined profile of your grinding wheel. The profile must be defined in a separate NC program. This cycle is based on the grinding pin tool type. The starting point and end point of the profile must be identical (closed path) and are located at a corresponding position on the selected wheel edge. Define the return path to the starting point in your profile program. You must program the NC program in the ZX plane. Depending on the profile program, the control either does or does not use tool radius compensation. The activated wheel edge is used as the preset.

This cycle supports the following wheel edges:

Grinding pin

Special grinding pin

Cup wheel

1, 2, 5, 6

not supported

not supported

Cycle 1030 ACTIVATE WHEEL EDGE (option 156)

Cycle sequence

  1. The control positions the dressing tool at the starting position with FMAX. The distance of the starting position from the datum is equal to the retraction values of the grinding wheel. The retraction values are relative to the active grinding edge.
  2. The control offsets the datum to the extent of the dressing value and executes the profile program. This process repeats itself depending on the definition of NUMBER INFEEDS Q1019.
  3. The control executes the profile program to the extent of the dressing value. If have programmed NUMBER INFEEDS Q1019, the infeeds repeat themselves. For every infeed, the dressing tool moves to the extent of the dressing value Q1013.
  4. The profile program is repeated without infeed in accordance with IDLE STROKES Q1020.
  5. The motion ends in the starting position.
 
Tip
  • The datum of the workpiece system lies on the active wheel edge.

Notes

 
Notice
Danger of collision!
When you activate FUNCTION DRESS BEGIN, the control switches the kinematics. The grinding wheel becomes the workpiece. The axes may move in the opposite direction. There is a risk of collision during the execution of the function and during the subsequent machining!
  1. Activate the FUNCTION DRESS dressing mode only in mode Program Run mode or in Single Block mode
  2. Before starting FUNCTION DRESS BEGIN, position the grinding wheel near the dressing tool
  3. Once you have activated FUNCTION DRESS BEGIN, use exclusively cycles from HEIDENHAIN or from your machine manufacturer
  4. In case the NC program is aborted or in case of a power interruption, check the traverse directions of the axes
  5. If necessary, program a kinematic switch-over
 
Notice
Danger of collision!
The dressing cycles position the dressing tool at the programmed grinding wheel edge. Positioning occurs simultaneously in two axes of the working plane. The control does not perform collision checking during this movement! There is a danger of collision!
  1. Before starting FUNCTION DRESS BEGIN, position the grinding wheel near the dressing tool
  2. Make sure there is no risk of collision
  3. Verify the NC program by slowly executing it block by block
  • Cycle 1015 is DEF-active.
  • No coordinate transformations are allowed in dressing mode.
  • The control does not graphically depict the dressing operation.
  • If you program a COUNTER FOR DRESSING Q1022, the control executes the dressing procedure only after reaching the defined counter in the tool table. The control saves the DRESS-N-D and DRESS-N-D-ACT counters for every grinding wheel.
  • This cycle can only be run in dressing mode. The machine manufacturer may already have programmed the switch-over in the cycle sequence.
  • Dressing

Note on programming

  • The angle of infeed must be selected in a way that the programmed profile always remains within the grinding wheel edge. If this condition is not met, then the dimensional accuracy of the grinding wheel is lost.

Cycle parameters

Help graphic

Parameter

cyc1015_1

Q1013 Dressing amount?

Value used by the control for the dressing infeed.

Input: 0...9.9999

Q1023 Infeed angle of profile program?

Angle at which the profile of the program is moved into the grinding wheel.

0: Infeed only at the diameter in the X axis of the dressing kinematic model

+90: Infeed only in the Z axis of the dressing kinematic model

Input: 0...90

Q1018 Feed rate for dressing?

Feed rate during the dressing procedure

Input: 0...99999

Q1000 Name of the profile program?

Enter the path and name of the NC program that will be used for the profile of the grinding wheel during the dressing process.

Alternatively, select the profile program via name option in the action bar.

Input: Max. 255 characters

Q1019 Number of dressing infeeds?

Number of infeeds of the dressing process

Input: 1...999

Q1020 Number of idle strokes?

Number of times the dressing tool moves along the grinding wheel without removing material after the most recent infeed.

Input: 0...99

Q1022 Dressing after number of calls?

Number of cycle definitions after which the control performs the dressing process. Every cycle definition increments the counter DRESS-N-D-ACT of the grinding wheel in the tool manager.

0: The control dresses the grinding wheel during every cycle definition in the NC program.

>0: The control dresses the grinding wheel after this number of cycle definitions.

Input: 0...99

Q330 Tool number or tool name? (optional)

Number or name of the dressing tool. You can apply the tool directly from the tool table via selection in the action bar.

-1: Dressing tool has been activated prior to the dressing cycle

Input: –1...99999.9

Q1011 Factor for cutting speed? (optional, depends on the machine manufacturer)

Factor by which the control changes the cutting speed for the dressing tool. The control handles the cutting speed of the grinding wheel.

0: Parameter not programmed.

>0: If the value is positive, then the dressing tool turns with the grinding wheel at the point of contact (opposite direction of rotation relative to grinding wheel).

<0: If the value is negative, then the dressing tool turns against the grinding wheel (same direction of rotation of the grinding wheel).

Input: -99.999...99.999

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 1015 PROFILE DRESSING ~

Q1013=+0

;DRESSING AMOUNT ~

Q1023=+0

;ANGLE OF INFEED ~

Q1018=+100

;DRESSING FEED RATE ~

QS1000=""

;PROFILE PROGRAM ~

Q1019=+1

;NUMBER INFEEDS ~

Q1020=+0

;IDLE STROKES ~

Q1022=+0

;COUNTER FOR DRESSING ~

Q330=-1

;TOOL ~

Q1011=+0

;FACTOR VC