Workpiece shaping with FUNCTION SHAPING (#96 / #7-04-1)
Application
Contour planing, also known as shaping, enables you to create sealing surfaces with a high surface definition, for example. When FUNCTION SHAPING is active, the control automatically moves the tool toward the contour during traverse movements. Using FUNCTION SHAPING, this automatic tracking also enables you to perform engraving, engine turning, or beveling.
Contour planing is performed with turning tools (e.g., recess-turning tools RECTURN)
Related topics
- Entering tool data in the tool management
- Compensating turning tools in the NC program with FUNCTION TURNDATA CORR
Requirements
- Kinematics description
In order to track the tool, the control requires a kinematics description prepared by the machine manufacturer.
- Software option Adv. Spindle Interpol. (#96 / #7-04-1)
- Tool definition
- Tool type Turning tool
- Tool tip direction with DIRECT
- Tool axis Z
- FUNCTION MODE MILL active
Description of function
For shaping, activate a machine kinematics model in which the tool spindle is defined as rotary axis. This way, the control can track the tool along the contour.
You can use a basic rotation or 3D basic rotation to align the workpiece and carry out shaping even with a tilted working plane.
The control resets FUNCTION SHAPING in the following cases:
- FUNCTION SHAPING END
- M30
- Internal stop
Contour definition
Program the contour along which the control tracks the tool in FUNCTION SHAPING.
During shaping, the tool must be positioned perpendicular to the working plane. If you program the rotary axes within FUNCTION SHAPING, the control will display an error message.
Program the contour using only the following NC functions:
- Path functions except for approach and departure functions, without tool radius compensation
- TRANS DATUM
- TRANS ROT or Cycle 10 ROTATION
HEIDENHAIN recommends programming only the contour to be shaped within the FUNCTION SHAPING function. For example, if you are performing pre-positioning for the next contour, program the traverse movements after FUNCTION SHAPING END.
Tools for shaping
The required NC functions and software options for shaping vary, depending on the turning tool being used.
If the tool cutting edge is in the spindle center, you do not need the Adv. Function Set 2 software option (#9 / #4-01-1) for shaping. If the tool cutting edge is outside the spindle center, the Adv. Function Set 2 software option (#9 / #4-01-1) is required for shaping.
Tool cutting edge in spindle center
- Tool location point TLP in spindle center, front view and view from below
If the XL and YL parameters of the tool include the value 0, the tool location point TLP is in the spindle center. If you program FUNCTION TURNDATA CORR-TCS, the DXL syntax element must also include the value 0.
During shaping, the control turns the spindle in order to track the tool along the contour. While the spindle is turning, the tool location point remains at the same place for these tools.
Tool cutting edge outside the spindle center
- Tool location point TLP outside spindle center, front view and view from below
If the XL or YL parameters of the tool include a value unequal to 0, the tool location point TLP is outside the spindle center. If you program the DXL syntax element to be unequal to 0 inside FUNCTION TURNDATA CORR-TCS, you will also shift the tool location point.
During shaping, the control turns the spindle in order to track the tool along the contour. Rotation of the spindle leads to an offset regarding the original position of the cutting edge on these tools. The view from below shows you the offset at the tool location point TLP'. Without compensation, the tool would move away from the contour or damage the contour.
To compensate for this offset during machining and to keep the tool permanently at the contour, program M128 or FUNCTION TCPM with the selection of AXIS POS (#9 / #4-01-1).
Input
FUNCTION SHAPING BEGIN
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 FUNCTION SHAPING BEGIN | ; Activate shaping |
To navigate to this function:
Insert NC function All functions Special functions Functions Shaping SHAPING FUNCTION SHAPING BEGIN
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
FUNCTION SHAPING BEGIN | Syntax initiator for activating tracking |
FUNCTION SHAPING END
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 FUNCTION SHAPING END | ; Deactivate shaping |
To navigate to this function:
Insert NC function All functions Special functions Functions Shaping SHAPING FUNCTION SHAPING END
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
FUNCTION SHAPING END | Syntax initiator for deactivating tracking |
Notes
- For shaping tools, observe the information of the tool manufacturer about the minimum permissible inner radius
- Use relief-ground tools with suitable tool carriers
- If FUNCTION SHAPING is active, the control calculates the bisector from the current NC block and the next NC block. During the traverse movement, the control turns the spindle and thus the tool cutting edge. At the end of each NC block the tool cutting edge is positioned on the bisector to the contour.
- Refer to your machine manual.
If the shaping kinematics model is active, the tool spindle acts as an additional rotary axis. The tilting functions of the control permit only two rotary axes. To program a tilting function with the shaping kinematics model active, you must exclude the tool spindle from the calculation using M138.
In connection with the shaping kinematics model, the control activates M138 on a standard basis, if applicable.
- The NC function FUNCTION TURNDATA CORR is included in the scope of functionality of the Adv. Spindle Interpol. software option (#96 / #7-04-1).
You can use the NC function TURNDATA CORR-TCS just like a tool radius compensation to program the contour with the drawing dimensions.
Program structure for workpiece shaping
Here you see a possible program structure for workpiece shaping. Optional steps begin with If required. The third column contains further information or conditions for optional steps.
BLK FORM... | ||
Call tool for workpiece shaping | TOOL CALL ... | ; Turning tool with tool axis Z required |
If required, compensate for the tool | FUNCTION TURNDATA CORR-TCS... | |
Activate shaping kinematics | FUNCTION MODE MILL "..." | |
If required, exclude spindle from tilting using M138 | M138... | ; Only if you tilt the working plane after the shaping kinematics is active |
If required, tilt the working plane | PLANE SPATIAL... | |
If required, activate FUNCTION TCPM using AXIS POS | FUNCTION TCPM ... AXIS POS ... | ; Only if the tool cutting edge is outside the spindle center |
Activate FUNCTION SHAPING | FUNCTION SHAPING BEGIN | ; Activate tracking |
Shaping | L X... Y... Z... | ; Only linear axis movements permitted |
CC ... | ||
C X... Y... | ||
Deactivate FUNCTION SHAPING | FUNCTION SHAPING END | |
If required, deactivate FUNCTION TCPM | FUNCTION RESET TCPM | |
If required, reset the tilted working plane | PLANE RESET... | |
Activate milling kinematics | FUNCTION MODE MILL "..." | |
... |
Definitions
Engine turning
Engine turning is a process of mechanical engraving to produce patterns made of overlapping lines. This technique is used, for example, in printing technology and in the watchmaking and jewelery industries.
Beveling
Beveling is a special technique used to produce edges of highest surface quality, for example, in the watchmaking and jewelery industries.