Convert a Absolute Post Processor to an Incremental

[ixlix]

Hi everyone,

I have a Thermwood 90 5 axis that has a post ive customised working nicely. We are trying to test being able to add in some cam generated code for holes etc to manually programmed incremental programs written by our cnc guy. 

Is there a way to get our current post processor to spit out the gcode in incremental? Or customise the post processor to do so?

Thanks

Alex

[bob.schultz]

Hello Alex,

You can get the post to output in incremental mode.  The key is to use 'createIncrementalVariable' instead of 'createVariable' for the axes formats and to output a G91 instead of the G90 code when incremental is in effect.  You can reference the Fanuc Incremental post, which we use to demonstrate incremental output.  You can search for the 'useIncremental' property in the post to see how it can be done.

[ixlix]

Thanks Bob. I gave it a go but seem to be getting an error in the cnc file. When i replace all the createVariable with createIncementalvariable in the xyzabc section, i get this error in the post.

..
Error(C:\Users\design\Documents\Alex\Thermwood 5-axis 0301817 Incremental.cps:163): TypeError: aOutput.disable is not a function
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Stack dump:
onOpen()@C:\Users\design\Documents\Alex\Thermwood 5-axis 0301817 Incremental.cps:162

Failed while processing onOpen().
Error: Failed to invoke 'onOpen' in the post configuration.
Error: Failed to invoke function 'onOpen'.
Error: Failed to execute configuration.
Stop time: Friday, February 16, 2018 12:29:13 AM
Post processing failed.

I have attached the Post processors, both absolute and the incremental version. I dont know my way around cam enough to know what else to change. The Fanc fie is quite different to the Thermwood one. 

Another issue i get with the Absolute one is the following, but not on every part. I have linked the part which does it, its just a test shape. 

Error: Error: Tool orientation is not supported for available machine axes.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Stack dump:
("Tool orientation is not supported for available machine axes.")@:0
onOpen()@C:\Users\design\Documents\Alex\Thermwood 5-axis 0301817 Absolute.cps:158

test part : http://a360.co/2EG9A7N

Thanks

Alex

[bob.schultz]

Hello Alex,

Thanks for supplying the post and part.  It seems that the 'disable' function is not in the createIncrementalVariable class.  You can change the definition back to createVariable for aOutput.

var aOutput = createVariable({prefix:"A"}, abcFormat);

It is also important to preset the position in each of the axes at the start of the program in the onOpen function.  Replace '0' with the correct value for each axis and you do have to call the 'format' function twice for each axis.

function onOpen() {
  xOutput.format(0);
  xOutput.format(0);
  yOutput.format(0);
  yOutput.format(0);
  zOutput.format(0);
  zOutput.format(0);
  bOutput.format(0);
  bOutput.format(0);
  cOutput.format(0);
  cOutput.format(0);

The reason for the error with the part you supplied is that the WCS in the Setup is not in the correct orientation.  It should match the tool orientation in the Swarf operation with the Z-axis pointing straight up.  Using your orientation the A-axis moves outside of its limits, which causes the error.

Hope this helps. 

[ixlix]

Thanks Bob, i'll give it a try on Monday.