Cycle 1015 PROFILE DRESSING (#156 / #4-04-1)
ISO programming
G1015
Application
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 is defined in a profile program created as a separate NC program. This cycle is based on the grinding pin tool type. The start and end points of the profile must be identical (closed path) and are located at a corresponding position at the selected grinding 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 grinding wheel edge is used as the reference point.
This cycle supports the following grinding wheel edges:
Grinding pin | Special grinding pin | Cup wheel |
---|---|---|
1, 2, 5, 6 | not supported | not supported |
Cycle run
- The control positions the dressing tool at FMAX to the starting position. 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 wheel edge.
- 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.
- The control executes the profile program to the extent of the dressing value. If you have programmed NUMBER INFEEDS Q1019, the infeeds repeat themselves. For every infeed, the dressing tool moves to the extent of the dressing value Q1013.
- The profile program is repeated without infeed in accordance with IDLE STROKES Q1020.
- The motion ends in the starting position.
- The datum of the workpiece system lies on the active grinding wheel edge.
Description of function
Procedure for profile dressing
- Defining the tool
- Define the grinding tool in the tool table
- Define the grinding tool type as grinding pin
- Defining the NC program
- Program the milling mode FUNCTION MODE MILL
- Program the grinding tool call
- Define Cycle 1030 ACTIVATE WHEEL EDGE
- Activate the dressing process with FUNCTION DRESS BEGIN
- Program the dressing tool call
The control does not exchange the active tool, but switches over by calculation.
- Define cycle 1015 PROFILE DRESSING and call up the profile program
- Deactivate the dressing process with FUNCTION DRESS END
- Program additional function M30
- Creating the profile program
- Program the desired profile as a contour
The contour must be closed. The active edge is the profile datum. You program the traverse path.
Applications for profile dressing
There are two applications for profile dressing:
- Shaping a grinding tool
- Resharpening a grinding tool
In the examples below, a grinding pin is dressed to suit the profile of a cup wheel.
Shaping a grinding tool
If the grinding tool does not yet have the desired shape, it must be shaped.
The figure displays the following information:
Depiction | Definition |
---|---|
Yellow | Desired profile |
Hatched | Finishing allowance from the grinding pin to the profile |
Red line | Profile program |
Green line | Diameter and length for the tool table |
Green dot | Current grinding wheel edge |
In order not to remove too much material in the first dressing process, the profile program must be relocated by at least the finishing allowance. The profile program datum can be relocated by enlarging the grinding tool radius and length in the tool table.
Define the grinding tool in the tool table to be so large that no part of the contour program will intersect the physical grinding tool.
HEIDENHAIN recommends defining the grinding tool diameter and length large enough in the tool table!
The profile datum is the active edge that you define with Cycle 1030 ACTIVATE WHEEL EDGE.
Resharpening a grinding tool
If the grinding tool already has the desired shape, you may resharpen it.
Depiction | Definition |
---|---|
Yellow | Desired profile |
Red line | Profile program |
Green line | Diameter and length for the tool table |
The profile datum is the active edge that you define with Cycle 1030 ACTIVATE WHEEL EDGE.
Notes
- Activate the FUNCTION DRESS dressing mode only in the Program Run operating mode or in Single Block mode
- Before starting FUNCTION DRESS BEGIN, position the grinding wheel near the dressing tool
- Once you have activated FUNCTION DRESS BEGIN, use exclusively cycles from HEIDENHAIN or from your machine manufacturer
- In case the NC program is aborted or in case of a power interruption, check the traverse directions of the axes
- If necessary, program a kinematic switch-over
- Before starting FUNCTION DRESS BEGIN, position the grinding wheel near the dressing tool
- Make sure there is no risk of collision
- Slowly prove-out the NC program
- You can execute this cycle in the following operating modes: FUNCTION MODE MILL, FUNCTION MODE TURN, FUNCTION MODE GRIND and FUNCTION DRESS.
- 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 be run only in dressing mode. The machine manufacturer may already have programmed the switch-over in the cycle sequence.
Note on programming
- The angle of infeed must be selected in a way to always maintain the programmed profile within the grinding wheel edge. If this condition is not met, the dimensional accuracy of the grinding wheel is lost.
Cycle parameters
Help graphic | Parameter |
---|---|
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 control shifts the profile for dressing. 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? (optional) Number of infeeds of the dressing process Input: 1...999 | |
Q1020 Number of idle strokes? (optional) Number of times the dressing tool moves along the grinding wheel without removing material after the most recent infeed. Input: 0...99 | |
Q253 Feed rate for pre-positioning? (optional) Traversing speed of the tool in mm/min for approach, withdrawal, and retraction movements This input value is optional. If it is not programmed, then FMAX applies. Input: 0...99999.9999 or FMAX, FAUTO, PREDEF | |
Q1006 Grinding wheel edge? (optional) Select the grinding wheel side to be dressed: -1: No selection 0: Face side 1: Shaft side This parameter may only be used if the dressing system is activated through a macro programmed by the machine manufacturer. Input: -1, 0, +1 | |
Q1022 Dressing after number of calls? (optional) 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: Factor for cutting speed not used >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.
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.
11 CYCL DEF 1015 PROFILE DRESSING ~ | ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
| ||
|