Heidenhain TNC 2500 Post Processor

[mathewXDZGT]

Hi

Looking for post processor change for my Heidenhain TNC 2500 controller.

I did a test file using the Heidenhain 407 generic post and found the tool change and drilling/tapping cycles did not work.

These are the main corrections made to get the file to work.

34 M9

35 L Z+0 R0 FMAX M91

36 M5

37 M1 #1 Remove M1 machine does not recognise

38 TOOL CALL 2 Z S7640 #2 Put M06 after each TOOL CALL

39 M3

94 CYCL DEF 1.0 PECKING

95 CYCL DEF 1.1 SET UP +7 #3 use - instead of + pecking SET UP

96 CYCL DEF 1.2 DEPTH -30

97 CYCL DEF 1.3 PECKG +30 #4 use - instead of + pecking PECKG

Can anyone help with modifying the Heidenhain 407 post.

Mathew

[ivan.stanojevic · Accepted solution]

Hi,

If you want to get rid of optional stop (m1), simply change property "optionalStop" to "no" when postprocessing.

I am not sure if I understood you well but if you want negative values for SET UP and PECKG you should search in your post for "function onDrilling(cycle)".

You will see all the codes which are responsible for drilling cycle.

Change these lines:

writeBlock("CYCL DEF 1.1 SET UP " + xyzFormat.format(cycle.clearance - cycle.stock));
writeBlock("CYCL DEF 1.3 PECKG " + xyzFormat.format(cycle.depth));

to look like this:

writeBlock("CYCL DEF 1.1 SET UP " + xyzFormat.format(-(cycle.clearance - cycle.stock)));
writeBlock("CYCL DEF 1.3 PECKG " + xyzFormat.format(-cycle.depth));

[mathewXDZGT]

Thanks Ivan,

Those two solutions worked.

The "-" for the drilling also looks like it needs to be applied the all drilling, counter boring and left/right tapping as well.

Still need the M06 after TOOL CALL.

This is the my first time dealing with post processors, do you have an example what and where to place code for the M06 inclusion.

Cheers

Mathew

[ivan.stanojevic]

Yes, you can apply "-" to all other cycles as well.

As for the M6 search for TOOL CALL line and change it to this:

  writeBlock(
      "TOOL CALL " + tool.number + SP + spindleAxisTable.lookup(spindleAxis) + " S" + rpmFormat.format(tool.spindleRPM), mFormat.format(6)
    );

[mathewXDZGT · Accepted solution]

After several attempts the only way i was able to get the M6 into the code was;

writeBlock(
"TOOL CALL " + tool.number + SP + spindleAxisTable.lookup(spindleAxis) + " S" + rpmFormat.format(tool.spindleRPM)
);
writeBlock( mFormat.format(6));

Mathew.

[Anonymous]

I am new to PP's how do you edit the pp. I also have the drilling cycles pluses instead of minuses.

Thanks

[Anonymous]

Thanks I didn't know you could open the file in a text editor, after reading the posts I figured it out.

Thanks