Prolight 3000 Turning Center

[Anonymous]

Greetings. I am working on a Prolight 3000 Turning Center and have had trouble getting correct G&M code. The closest I can get is with a modified¹ fanuc² turning post processor and editing the outputted code.

I've had to do the following to the G&M code to get it to function:

1. The G28 command will send the tool to the work zero³, not the machine zero, often causing a tool crash. I replace this with the two lines "G53 X0" and "G53 Z0" or remove it completely when it isn't an issue.
2. Tool Changes are done with an M06T## code instead of a T#### (Offsets are configured in the lathe control program)
3. The Lathe does not not recognize G97, I've had to replace the line "G97 S750 M3" with "S750 M3".
4. G3 is interpreted as G2 and vice versa.
5. The Prolight 3K control program will load file names with charactersand not just numbers.

Things that may help in diagnosing and address these issues.

Prolight 3000 Turning Center Manual
Prolight 3000 Turning Center Control Program
Link to Solidworks Sample Part w/ Turning Job
NC code that has been modified to "work" in the Prolight 3K control software simulation

   
Any help regarding this would be greatly appreciated.

¹: The Prolight 3K uses radius measurements instead of so I change that in the post processor base on what Achim recommended doing in this thread.
²: Base on the discussion in this thread I am assuming that this machine also uses modified fanuc code interpretation.
³:This may or may not relate to the G28 issue from this thread.

[damincin]

Hi,

My lathe with an Ah-ha controller has a few of the same issues.  So I can help with some of these.

#1. I've gotten rid of my G28s because they just don't work right (supposed to be supported, but I don't trust it.)  I don't use a G53, but replacing G28 with G53 like you want has been discussed here:

http://forums.autodesk.com/t5/computer-aided-machining-cam/fusion-lathe-cam-question/td-p/5751396

#2. If you just want the "Txx" part of the tool change, look in the post for the lines that read (I found 3 instances):
"writeBlock("T" + toolFormat.format(tool.number * 100 + compensationOffset));"

and change to something like:
"writeBlock("T" + toolFormat.format(tool.number));"

#3. Look for the line:
writeBlock(gSpindleModeModal.format(97), sOutput.format(tool.spindleRPM), mFormat.format(mSpindle));

get rid of the gSpindleModeModal.format(97), part.

#4. My lathe had this one... There are a number of ways to deal with this one, but what I did was look for the text "function onCircular(clockwise, cx, cy, cz, x, y, z, feed)"
You'll then see several lines that contain the text "gMotionModal.format(clockwise ? 2 : 3)".
Just reverse the "2" and the "3".  That will cause it to use the other.

#5. Get rid of all of this:

  if (programName) {
    var programId;
    try {
      programId = getAsInt(programName);
    } catch(e) {
      error(localize("Program name must be a number."));
      return;
    }
    if (properties.o8) {
      if (!((programId >= 1) && (programId <= 99999999))) {
        error(localize("Program number is out of range."));
        return;
      }
    } else {
      if (!((programId >= 1) && (programId <= 9999))) {
        error(localize("Program number is out of range."));
        return;
      }
    }
    if ((programId >= 8000) && (programId <= 9999)) {
      warning(localize("Program number is reserved by tool builder."));
    }
    var oFormat = createFormat({width:(properties.o8 ? 8 : 4), zeropad:true, decimals:0});
    if (programComment) {
      writeln("O" + oFormat.format(programId) + " (" + filterText(String(programComment).toUpperCase(), permittedCommentChars) + ")");
    } else {
      writeln("O" + oFormat.format(programId));
    }
  } else {
    error(localize("Program name has not been specified."));
    return;
  }


Ok.. I think that takes care of all of them.

Dave

[Anonymous]

Thanks damincin, after going through the post and changing what you mentioned everything works well and haven't encountered any issues yet. I decided just to get rid of the G28 code all together.

I attached the modified post processor for anyone else who may need it.