Define monitoring sections with MONITORING SECTION (#168 / #5-01-1)
Application
The NC function MONITORING SECTION allows defining monitoring sections for process monitoring in the NC program.
Related topics
- The Process Monitoring workspace
Requirement
- Software option Process Monitoring (#168 / #5-01-1)
Description of function
MONITORING SECTION START is used to define the start of a new monitoring section and MONITORING SECTION STOP, to define the end of the monitoring section.
Define a separate monitoring section for each machining step to be monitored. Each monitoring section must be unique. If multiple monitoring sections have the same contents, make sure to name them differently.
HEIDENHAIN recommends ending each monitoring section with MONITORING SECTION STOP. Otherwise, the control will end the monitoring section automatically at the end of the program (END PGM).
For the following NC functions, the control ends the current monitoring section and starts a new one:
- MONITORING SECTION START
- TOOL CALL with tool change within a monitoring section
The control can only compare the machining operations if the traverses and machining time are identical for each execution. Thus, the monitoring section may only contain the machining operation itself (i.e., it may only begin after the tool call and pre-positioning). The programmed spindle speed must have been reached already.
Note the information on the program structure.
Input
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 MONITORING SECTION START AS "mill contour" | ; Beginning of monitoring section including additional designation |
To navigate to this function:
Insert NC function Special functions Functions Process monitoring MONITORING MONITORING SECTION
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
MONITORING SECTION | Syntax initiator for the monitoring section of process monitoring |
START or STOP | Start or end of the monitoring section |
AS | Additional designation Optional syntax element Only when START is selected |
Notes
- The control shows the beginning and the end of the monitoring section in the structure.
- If you change an NC block within a monitoring section, the previous recordings are no longer compatible. Comments are the only items you can change without further impact on monitoring. In order to monitor an edited monitoring section again, delete the existing recordings and define new "good parts".
- If you use different sizes of workpiece blanks, set process monitoring to a more tolerant setting or start the first monitoring section after pre-machining the workpiece blank.
Notes on the program structure
- The following NC functions are prohibited within monitoring sections:
- Stop of program run (e.g., M0, M1, or STOP)
- Call of an NC program (e.g., with CALL PGM)
Closed monitoring sections in a called NC program are permitted.
- Some NC functions may cause traverse differences, resulting in deviating machining times. This means that the program sequence is no longer reproducible and thus inadequate for process monitoring.
Avoid using the following NC functions within monitoring sections:
- Positions referring to the machine datum (e.g., M91 or M92)
- Automatic liftoff with M140 MB MAX
- Call of a replacement tool with M101
- Repeats with variable values (e.g., CALL LBL 99 REP QR1)
- Variable jump commands (e.g., FN 5)
- Variable or changing datum shifts (e.g., TRANS DATUM AXIS XQ1)
- Modifications of the spindle speed (e.g., M3 or TOOL CALL with the same tool as before)
- Combination with AFC sections (e.g., AFC CUT BEGIN)
The AFC function can be used jointly with process monitoring in an NC program. However, the process monitoring sections and AFC sections should not overlap.
- HEIDENHAIN recommends that you program a feed-rate value in the NC block before MONITORING SECTION START. Thus, the control will only position the tool once the programmed spindle speed has been reached.
- If you program MONITORING SECTION STOP without an associated MONITORING SECTION START, the control will display an error.
- The control monitors the movements in the W-CS workpiece coordinate system. If you perform the same machining operation at various positions in the machine, make sure to change the workpiece preset and not the workpiece datum.
- When monitoring machining operations with OCM cycles (#167 / #1-02-1), please note the following:
- Monitor roughing operations only.
- Always use the same tool (e.g., no resharpening during machining). Small deviations of the tool radius might result in deviating traverses.
- Pre-position the tool before calling the cycle. If the starting points deviate, OCM will generate different paths.
- Program the same speed for the cycle as in the tool call.