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.