Post processors for me spell confusion.

[JAZZCNC]

Suesi there's no great mystery to post processors really they do a very simple job. There main function is to format the G-code file so it complys with the control software requirements.
Because in industry there are many different machines with different Control software from different manufactures each with different models that talk sligthtly different then you need a translator and that's the job of the post processor.
If CAM software didn't use Post processors then you would need a software version for each Model of Machine and Control software it used.

Often industrial machines come with there own proprietary CAM software which outputs directly to the control software in the correct format.
Now often these proprietary softwares are limited in what they can do or designed just for one purpose and it's because of this why Cam software often gets used has it's more flexible. To do this and work with many versions of control software the CAM software needs to Post processors designed for each control software model.

Now the Control software like MAch3 or Linux cnc are generic Control Software designed to be used with many machine types and designs. So in there basic form don't dictate any specific machine data be inserted in the G-code so a basic generic Post processor is all that's needed.
Most CAM software have Generic post processors which only insert basic G-code Initialisation lines such has setting Metric or Imperial units etc.

Now this can change if you have Machine specific needs or want your machine to behave a certain why. In this case you would alter or write your own Post processor to suit your own needs.
An example of needing to do this would be an automatic tool changer that needs a specific macro file to work. Here you would have the post processor define a constant in the header Portion(top of Code) that points to a file location then inserts this Constant at every tool change thru out the G-code file.
This way you can have Custom machines that all use the Same Cam software and Control software but are setup very differantly regards Hardware like Tool changers etc. You just have a Post processor written for that machine.

Often you'll see Metric and Imperial Post processors with the Only differance being Metric inserts G21 Imperial G20 the rest will be exactly the same.!!

To give an idea of Formated and unformatted G-code with specific and generic post processors I've attached 3 files all work with or formated for Mach3.
1st is from BobCad Cam.
2nd is from Solid works
3rd is just a Genric

Has you'll see the Formatted ones insert much more NONE G-code lines for information that gets displayed on the screen while cutting. They also do other subtle things like Setting the Initialisation of machine. So setting Work offsets and cancelling any previous Modal commnads or Canned cycles etc.
A simple Example of Post inserted Code is the Solid works Post processor Sends the Machine to the home location on all axis (G53) before starting the Main G-code.
Bobcad does the same but only for the Z axis and sets it 10mm away from home (G53 Z10). Bobcad also gives much more information about tool etc that gets displayed on screen but has no affect on the actual cutting.

The genric G-code does nothing really other than set Cancel tool length offset (G49) and set Distance Mode to Absolute (G90).


Hope this helps but in a Nut shell if your using Mach3 or Linux cnc don't worry about it and just use a Genric Post thats set for the units your using if you can't find a Specific Post.