---------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
 Introduction:
  
 This is an extended version of the original fablab-mill-n-drill for PCB creation with Roland Modela 3-D Plotters by Marc Boon
 from the Netherlands.
 
 Projects of Francois de Wet from South Africa, which includes a Traffic Light Backup System and also a PIC Programmer required
 this extension which includes automaatic layer creation required to make it function more fluently. Francois is responsible for
 the design rules and his Fablab colleague, Oswald van Ginkel implemented the automatic layer creation and further functionality.
 Please e-mail oswald.vanginkel@gmail.com with SUBJECT: fablab-mill-n-drill if any help or explanation is required or a bug is
 found or feature is required.
 ---------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------

 Eagle Modela PC Board Manufacture Mini Help File:

* Install Fablab Milling And Drilling For Double Layer With Auto Layer Creation.

* Design your schematic/board layout in eagle.

* With the board layout selected: Click on the little magnifying glass (DRC : Design Rule Check) and load the design rules: 'fablab_doublelayer.dru',
        - the default ruleset is for making tracks with a 1/64 inch bit.
        - we usually replace the bit with a 1/32 inch one for making the holes! 
        - please experiment and do post feedback regarding rules that work for you on fablabpotchefstoom's discussions (facebook)

* Now after checking the design rules for your finished board layout, you are now ready to run the correct ULP (User Language Program) by clicking 
on the little ULP icon and selecting 'fablab-mill-n-drill-double-layer.ulp'.

* You are now presented with options for tool diameter (which should agree with the DRC above and the option to put a specified signal on the copper plane. Be wary of checking, 'mill holes larger to their size', as this might result in breaking thinner drill bits! But if you have large fixation holes you might be forced to do this (I recommend using at least a 1/32 inch drill bit for making any type of hole).

* After accepting the settings, wait for the ULP to complete - you can view the result of this tracing process by looking at the specially created layers: 100: DRILLBOT, 101: MILLTOP and 102: DRILLBOT. (Navigate to 'View>Display/hide layers...' for this)

* Now for the CAM part: Go to 'File>CAM Processor'

* From there load a job through 'File>Open>Job' and make sure you select: 'fablab-mill-drill-doublelayer.cam' 

* This presents you with the different tabs for each of the processes that your board has to undergo, namely milling of top countours and also of bottom contours. The drilling from the bottomside is also included (note that the board is flipped from left to right for the latter two processes) 

Flipping Diagram:

1:
        -> /
      /  B/T
   __T__ /
     B
2:
   <---- __B__
           T
3:
   __B__
     T

  <length>

* It is important that you specify the exact correct length (from left to right: measure it...) of your board (the workpiece itself, not the final product) for both the bottom milling and bottom drilling as the 'Offset' on 'X' on both these tabs!

* The machine settings is specified for each device type (in this case we have FABLAB_MILLING and FABLAB_DRILLING: each of these is specified in the eagle.def file)

* Now that you are satisfied with your settings you may 'Process Job'. (Note that the files for each of the job tabs is specified next to the 'File' button)

* It is very important that you use good double sided tape each time you fix the board. Bring the drill-bit (initially the one for drilling) down to the level of the board, before sending any commands from the computer.

* The files created by the CAM Processor: above.mill, below.mill and below.drill can each be sent to the Modela by doing for example: 
'cd C:\<path to your project *.brd and the cam processor files>' from command prompt
and then 'type below.drill > com1' if this is the serial port to which the Modela is connected. 

* After doing the bottom drilling, replace the drill bit with one appropriate for contours and again bring it down to the level of the board. Now commence with 'type below.mill > com1'.

* After sending this, you need to flip the board as in the flipping diagram, again fixing it with double-sided tape.  Now do 'type above.mill > com1'.

* If you really want to be smart you can create another job using an X offset of 0 and a device type FABLAB_DRILLING, but this time you only select the dimension layer instead of the 100 layer too, and voila the board is cut along the edges when sending the created file!

Further notes:
        - The depth and speeds at which the tracks is cut and the holes are drilled are specified under the [FABLAB_MILLING] and [FABLAB_DRILLING] 	headings within the eagle.def file. The codes is thus:
VS4 - this specifies a horisontal speed (along the X/Y axes) as 4 (I presume 4 inches per second).
!VZ3 - this specifies the speed along the Z axis as 3
!PZ-40,20 - this specifies the down position on the Z -axis as -40 (mils) from the zero position and the up position as 20 mils above the 0 position.
        - Please do experiment with these as boards with different thickness and copper hardness may require different settings.

