I thought a new board for post processors would be a good idea as a few variations are appearing.
Here is a post processor I knocked up to stick in all the required comment blocks to pass stock and tool information to CutViewer Mill.
It is also a good example of using the PostProcessorMacros field under the machining options, to pass information to the post processor.
The 'Mach3-CV' post uses the following macros...cut and paste all these lines into the PostProcessorMacros property. If you click the [...] button to the right you will get a multi-line text editor, which makes things easier to see.
$stock_length=150
$stock_width=150
$stock_height=12.7
$stock_x=75
$stock_y=75
$stock_z=12.7
Change the stock dimensions to suit. The stock_x/y/z macros are the stock origin offsets. In this example, the stock is centered about the origin, with the stock surface at z=0.
The PostProcessor and PostProcessorMacros can be set and saved to a cambam file, then this file used as DrawingTemplate (under tools options), so you don't need to keep setting these for new drawings.
With the CutViewer plugin installed and post processor set up, you should now be able to generate the gcode, then go Tools->Simulate with Cutviewer, to simulate without having to set up anything else in CutViewer.
EDIT: There are some limitations to this processor. At the moment tool diameter and taper are hard coded in as 0. If you want to simulate with ball/bull nose cutters then you would need to change the post manually.
