PCB Milling Preparation & Guidelines
Milling Conditions
Some simple sigle-sided and double-sided PCB can be milled in ECE workshop, but the following conditions must be met before a board will be considered for milling:
- Drill hole sizes:
- The smallest hole size is 25mil (0.025in)
- Any size 31mil or larger
- Clearance: A clearance of 20mil or more is preferable. You will be required to change the layout to maximize clearance for clearances less than 20mil. Other preferred clearances are 15, 11, 9, and 7mil. Clearances as small as 4mil are possible only if necessary.
- No reference designators on the component or solder layer
- Specify board dimensions (10.8in. by 8in. max.)
- Via pins (“nails” connecting solder side to component side traces via a mounting hole) require 32mil holes. Wire can also be used.
- Eyelets (rivets connecting solder side to component side traces via a mounting hole) require 40mil holes. Use for component mounting with connections on both sides.
- Supply “gerber 274x” files. No other formats are licensed for this machine.
- Drill files if needed (.dxf)
Tips for a successful layout
- Place as many tracks as possible on the circuit (back) side. Minimize the number of traces on the component (front) side.
- Keep tracks at least 0.1” from pins, especially on the component side.
- Avoid right angle turns, use two 45 degree turns. Use T trace intersections if you have to. Avoid Y trace intersections.
- Keep vias at least 0.1” from tracks or other holes.
- Use as few vias as possible
- It sometimes helps to swap IC pins to get a better layout. (Ex: A 7404 contains 6 inverters, sometimes changing which inverter is used will make the layout easier)
- Recommended trace width is 0.034in (0.8mm) (especially where it attaches to pads) which can be reduced to 0.017in (0.4mm) for crowded sections.
- Pad size should be at least 0.015” larger than hole size, 0.030” is recommended.
- In board layout DRC set the clearance of wires, pads and vias to .012 in. (3mm),
The clearance must be at least .011 - Via: hole diameter: 0.032”, pad diameter 0.055”
- Use the following sizes for eyelets (through hole via with hole for component) hole diameter: 0.040”, pad diameter 0.070. Eyelet Inside diameter is .029”
Suggested reading:
- PCB Design Tutorial, see good and bad routing and finishing touches).
- Tips for Designing PCBs
Gerber and drill files
Preparing Gerber and drill files from PCBnew
In PCBnew select “Plot” from main toolbar. Plot format “GERBER”, “back, front and Edges PCB.
The plot button will generate Gerber files “*-front.pho”, “*-Edges_PCB.pho” and “*-back.pho”.
The “Create drill” button will generate the drill file *.drl
Preparing the files from Eagle.
- Gerber 274x
- From the Control Panel , under “ CAM Jobs ”, open “ gerb274x.cam ”
- The “1 CAM Processor” window pops up
- Click “File”, “Open”, “Board” and open the “.brd” file for your project.
- Click “Process Job”. This will generate the “.sol” and “.cmp” files.
- drill.ulp
- Load the .brd file from the control panel under “Projects”. Type” run” in the command window, press enter.
- From the run window double click “drillcfg.ulp”. This will generate the.drl (rack file containing drill sizes)
- CAM – Excellon to generate the .drd file
- From the Control Panel , under “ CAM Jobs ”, open “ excellon.cam ”
- The “1 CAM Processor” window pops up
- Click “File”, “Open”, “Board” and open the “.brd” file for your project.
- Click “Process Job”. This will generate the “.drd” and “.dri” files.
Note: This page is from Jeff's word file.