MAZAK SEQUENCE NUMBERS

[Anonymous]

I need help making some changes to my post.  I would only like the sequence number output above each new tool change.  Post attached 

[Arun.rs · Accepted solution]

HI @Anonymous 

Thanks for raising your concern via Forum .

Open post file in a 'Visual Studio Code' or 'Notepad++' to do the required modifications.

1. Define variable called  ' var sequenceNumberForToolChange; ' , you can define in '// collected state'

2. Search 'function writeBlock' , Add below condition in line number 202

if (properties.showSequenceNumbers || sequenceNumberForToolChange) {

3. Set the state as false for 'sequenceNumberForToolChange' in line number 217

sequenceNumberForToolChange = false;

Modified condition will be as below.

function writeBlock() {
  var text = formatWords(arguments);
  if (!text) {
    return;
  }
  if (properties.showSequenceNumbers || sequenceNumberForToolChange) {
    if (skipBlock && text) {
      writeWords2("/", "N" + sequenceNumber, arguments);
    } else {
      writeWords2("N" + sequenceNumber, arguments);
    }
    sequenceNumber += properties.sequenceNumberIncrement;
  } else {
    if (skipBlock && text) {
      writeWords("/", arguments);
    } else {
      writeWords(arguments);
    }
  }
  skipBlock = false;
  sequenceNumberForToolChange = false;
}

4. Search 'writeBlock("T" + toolFormat.format(tool.number), mFormat.format(6));'  in editor.

5. Write ' sequenceNumberForToolChange = true; ' before toolcall.

Regards

[Anonymous]

Thank you so much for your help works perfectly!!!!   I have another question, on the initial start of the program,  between all tool changes the machine goes to a safe position of:

G53 Z0

G53 X0 Y0 B0 C0

I would like to machine to go home in the only Z-axis and reposition "B & C" where necessary and eliminate the

G53 X0 Y0 B0 C0 

I have attached the new version of the post with the "N" number on tool change and G90 added for the "EIA" non-modal restart.

@Arun.rs 

[Arun.rs]

HI @Anonymous 

Thanks for the feedback.

If you don't want to output XYBC homing codes for every tool change and in program start, you can just comment it out with "//" in front of it. 

// if (insertToolCall) {
    // writeBlock(gFormat.format(53), gMotionModal.format(0), "X" + xyzFormat.format(0), "Y" + xyzFormat.format(0), "B" + xyzFormat.format(0), "C" + xyzFormat.format(0)); // retract
    //   forceABC();
    // } else {
    //   writeRetract(X, Y);
    // }

Save the file and test the post carefully.

Regards

[Anonymous]

@Arun.rs  this works but the problem is if you transitioning from an operation where C or B was not at 0 deg, nothing forces it back on the next operation to proper B C location.  I have attached a file, for example, after drill, the holes nothings reset B C going to tool 5