Fundamentals
Application
The ISO 6983 standard defines a universal NC syntax.
On the TNC7 basic, you can program and execute NC programs using the supported ISO syntax elements.
Description of function
In connection with ISO programs, the TNC7 basic provides the following possibilities:
- Transferring files to the control
- Programming ISO programs on the control
- In addition to the standardized ISO syntax, you can program HEIDENHAIN-specific cycles as G functions.
- Coding in Klartext syntax allows you to use some NC functions in ISO programs.
- Testing of NC programs using Simulation mode
- Running NC programs
Contents of an ISO program
An ISO program is structured as follows:
ISO syntax | Function |
---|---|
I | File type ISO programs have an *.i file name extension. |
%NAME G71 | Start and end of the program |
G71 | Unit of measure: mm |
G70 | Unit of measure: Inch |
N10 N20 N30 ... | NC block numbers In the optional machine parameter blockIncrement (no. 105409), you define the increment between the block numbers. |
N99999999 | NC block number for the end of the program An NC program is incomplete without this NC block number. The control adds and updates the NC block numbers within the file automatically. The Program workspace exclusively shows successive numbers without taking the defined increment into account. |
G01 X+0 Y+0 ... | NC functions |
Contents of an NC block
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.
N110 G01 G90 X+10 Y+0 G41 F3000 M3 |
An NC block contains the following syntax elements:
ISO syntax | Function |
---|---|
G01 | Syntax initiator |
G90 | Absolute or incremental input |
X+10 Y+0 | Coordinates |
G41 | Tool radius compensation |
F3000 | Feed rate |
M3 | Miscellaneous functions (M functions) |
ISO example
Example task 1338459
Example solution 1338459
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.
% 1339889 G71 | |||
N10 G30 G17 X+0 Y+0 Z-40 | ; Workpiece blank definition | ||
N20 G31 X+100 Y+100 Z+0 | ; Workpiece blank definition | ||
N30 T16 G17 S6500 | ; Tool call | ||
N40 G00 G90 Z+250 G40 M3 | ; Clearance height in the tool axis | ||
N50 G00 X-20 Y-20 | ; Pre-positioning in the machining plane | ||
N60 G00 Z+5 | ; Pre-positioning in the tool axis | ||
N70 G01 Z-5 F3000 M8 | ; Feed to working depth | ||
N80 G01 X+5 Y+5 G41 F700 | ; First contour point | ||
N90 G26 R8 | ; Approach function | ||
N100 G01 Y+95 | ; Straight line | ||
N110 G01 X+95 | |||
N120 G24 R10 | ; Chamfer | ||
N130 G01 Y+5 | |||
N140 G24 R20 | |||
N150 G01 X+5 | |||
N160 G27 R8 | ; Departure function | ||
N170 G01 X-20 Y-20 G40 F1000 | ; Clearance height in the machining plane | ||
N180 G00 Z+250 | ; Clearance height in the tool axis | ||
N190 T6 G17 S6500 | ; Tool call | ||
N200 G00 G90 Z+250 G40 M3 | |||
N210 G00 X+50 Y+50 M8 | |||
N220 CYCL DEF 254 CIRCULAR SLOT ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
N230 G79 | ; Cycle call | ||
N240 G00 Z+250 M30 | |||
N99999999 % 1339889 G71 |
Notes
- The Insert NC function window allows you add ISO syntax, too.
- You can call a Klartext program within an ISO program (e.g., to benefit from the possibilities of graphical programming).
- You can call a Klartext program within an ISO program (e.g., to use NC functions that are available only for Klartext programming).
- If the ISO editor toggle switch is active, you can search for identical syntax elements in different NC blocks.
Searching for identical syntax elements in different NC blocks