Block missing after data transmission to a TNC 4xx
NC FAQ1033
Frage:
Missing NC block after data transmission to a TNC 426/430. On a nearby iTNC 530 this behavior does not occur when the same program is used.
Initial situation:
A CAM system is used to generate a CNC program. A postprocessor is used to convert this program to HEIDENHAIN conversational format, appropriate for a TNC 426 (NC software no. 280 476-16) control. It is then transmitted to the control via TNCremo.
Error:
During editing as well as machining on the control, each NC block directly following a machining cycle is now missing.
Antwort:
Cause:
The postprocessor generates one tilde (~) too many in the last line of the machining cycle:
10 CYCL DEF 22 ROUGH-OUT ~
Q10=-0.8 ;PLUNGING DEPTH ~
Q11=+50 ;FEED RATE FOR PLUNGING ~
Q12=+1150 ;FEED RATE FOR MILLING ~
Q18=+0 ;COARSE ROUGHING TOOL~
Q19=+1000 ;RECIPROCATION FEED RATE ~ (Here is the superfluous tilde in the cycle!)
11 CYCL CALL (This block is then missing when the data is transmitted to the TNC 426/430)
This causes the program to be faulty.
Solution:
Adapt the postprocessor so that no tilde is generated in the last line of a machining cycle.
10 CYCL DEF 22 ROUGH-OUT ~
Q10=-0.8 ;PLUNGING DEPTH ~
Q11=+50 ;FEED RATE FOR PLUNGING ~
Q12=+1150 ;FEED RATE FOR MILLING ~
Q18=+0 ;COARSE ROUGHING TOOL~
Q19=+1000 ;RECIPROCATION FEED RATE
11 CYCL CALL
The iTNC 530 corrects this syntax error during loading, as opposed to the TNC 426/TNC 430.