Our department has, in the student workshop, an LPKF ProtoMat 93S PCB prototyping machine. This will remove excess copper from blank PCB stock, drill the holes in the board, and cut out the finished PCB. It is an excellent way of quickly producing small boards.
To use the LPKF mill we recommend using the Eagle CAD system. Forget about Protel, it is expensive, crashes all the time and its libraries are awful.
Getting Text to work
Do not put your text on the solder layers. Make sure your design has two layers called tTopText (number 100) and tBottomText (number 101). Create these layers using the 'View->Display/Hide Layers' menu and click the 'new' button. Place the text into those layers. This allows you to create text on your board that is not insulated. Insulated text looks really ugly and is almost unreadable.
Getting the LPKF to cut your board out is an important step. To do this you should use the Dimension layer (Layer number 20) to draw a single track where you would like the cut-out to go. When importing into Boardmaster, make sure that the contour routing tool is chosen for this Layer.
There's some inconsistancy between the way Eagle generates the Gerber plotting data for octagons, and the way that CircuitCam interprets this data. This can lead to `disappearing pads' apparently, if any of the pads in your circuit are octagons. The fix to this problem was provided by Andrew Sterian in the news.cadsoft.de support forum (6 Nov 2001).
Additionally, it is necessary to make the octagons appear as circles to get a board that can be reliably-soldered: the pads get milled as octagons ok, but the track, rather than going to the edge of the pad, gets milled right to the hole (and is thus insulated from the rest of the pad) which means that the majority of solder you put between the pad and the leg of the component will not be electrically-connected to the track(s), leading to dangers of non-connections. However, quite usefully, within Eagle it's still an octagon, and any "copper pour" you put around the pins will be octagonal. The area between the pad and the pour area is milled out by the milling machine, with a circular pad and an octagonal "surround," so it actually looks pretty octagonal anyway.
， Close down Eagle
， Locate the file "eagle.def" (on Linux machines this is in /opt/eagle/bin)
， Make a backup of this file (eagle_orig.def or something)
， Search for the string "AMOC8" ... the line reads:
"%%AMOC8*\n5,1,8,0,0,1.08239X$1,22.5*\n"\ Octagons are emulated with a circle (using 8 vertices)
， Change the "22.5" to "0.0" ie:
"%%AMOC8*\n5,1,8,0,0,1.08239X$1,0.0*\n"\ Octagons are emulated with a circle (using 8 vertices)
， Comment out the line (ie, stick a ";" at the start of it):
;Octagon = "%%sOC8,%6.4f*%%\n" ; (code, diameter)
， Uncomment the line:
Octagon = "%%sC,%6.4f*%%\n" ; (code, diameter)
， Save the file (as "eagle.def")
， T01 0.024in
， T02 0.031in
， T03 0.032in
， T04 0.040in
All this will have created the following files (assuming your design is called "design")
Quit eagle, and save these files on a floppy disk. Make sure that the above files are on the floppy disk.
Start up the LPKF Mill (with the on switch), boot up the computer and insert your floppy disk.
， design.obo WiringSold Type: Gerber Ref: eaglegrb
， design.obt TextSold Type: Gerber Ref: eaglegrb
， design.odr Drill Type: Excellon Ref: eagledrl2
， design.ool Cutting Type: Gerber Ref: eaglegrb
， design.oto WiringComp Type: Gerber Ref: eaglegrb
， design.ott TextComp Type: Gerber Ref: eaglegrb
Still in the CircuitCAM program
Still in the CircuitCAM program
， eaglein.LMD Drill_Flash
， eaglein.LMD TextComp
， eaglein.LMD InsComp
， eaglein.LMD InsSold
， eaglein.LMD TextSold
The 'design.LMD' file is the one that will be used in the BoardMaster programme to actually control the Mill.
Now we are ready to use BoardMaster -- this is the software that controls the mill itself. Switch the Mill on and wait for it to warm up.
Now check the placement of your board. The screen should show an image of the Mill bed with your circuit. ove the Mill to each corner of your board and make sure that it is on a sensible piece of copper.Watch out for the pins that keep the board in place.
To cut out your board. Place a single thin track on the tDimension layer (layer 20). See above. Place the contour router tool into the collet so that it protrudes below by approximately 1.5 PCM widths. This means that the router will cut through the board.
The following from http://duvet.eee.nottingham.ac.uk/eagle/eagle2lpkf_at_eee.html
6. BOARD CUT-OUT
click Edit -> Contour Routing...
select "Source layer" ... "BoardOutline"
select "Destination layer" ... "CuttingOutside"
tool should be "Contour Router 2.0mm long"
click on the INSIDE of the BoardOutline layer (yellow) to select it
if you selected the correct object (the outline should go pale yellow)
then click the "select layer" button to select ALL objects in the BoardOutline layer
once selected, ERASE the layer (using the "X" button) - all the yellow should go
click near the grey CuttingOutside rectangle to select it
use the "+" and "-" keys on the keypad to move the "*" around the rectangle
press "Ctrl-g" to make a gap in the middle of one side
use the "+" and "-" keys to move the "*" around to the other side
press "Ctrl-g" to make a gap in the middle of the other side
de-select everything (right-click -> Cancel)
We have a lot of imperial drills (cheaper), but we only have metric Mill bits. This means that you need to do a collet change after the drilling phase. This is because we are out of metric drill bits. We are moving to using the imperial 1/8" mill and drill bits.