The following guidelines will help you to produce your PCB for senior design. The guidelines will work for most PCB vendors.
These rules are based on Advanced Circuits "33 each" capabilities. They will work with most common manufacturers. Use their "Free DFM" tool before submitting your design. If there are any problems, fix them first - this will save you several days of work!
With Altium Designer, when using the PCB editor, open Design|Layer Stack Manager
 | Specify the core layer thickness as 62 mil |
| Add Top Dilectric and Bottom Dilectric, both with 0.5 mil Solder Resist thickness |
| If you're using a 4-layer board, add planes as appropriate |
With Altium Designer, when using the PCB editor, open Design|Rules...
| Routing | width = 6 mil minimum/preferred
| ||
| Electrical | Clearance = 7 mil minimum (this might be made smaller, but some projects with it set smaller have had manufacturing problems) | ||
| Manufacturing | Hole Size = 15 mil minimum | ||
| Routing | Routing Via Style Diameter = 27 mil min and preferred, 50 mil max | ||
| Routing | Routing Via Style Hole Size = 15 mil min/preferred/max | ||
| Mask | Solder Mask Expansion = 2.5 mil |
Regardless of what tools you use to create your PCB design, the only thing that you'll send to the manufacturer is a set of Gerber and Drill files. Thus, these are the most important files of all - please create them carefully and take some time to inspect them fully before submitting them. You must submit a set of Gerber files AND a set of drill files to the manufacturer.
Open up the a PCB document.
Select File | Fabrication Outputs | Gerber Files
Unless you have a reason to do otherwise, use the defaults all tabs except the "layers" tab.
For the layers, select the following:
 | Top/Bottom Layer (metal), Top/Bottom Overlay (silkscreen), Top/Bottom Solder Mask, Top/Bottom Paste |
| Any middle layers or planes you've added (for boards with more than two layers) |
| You probably do not need to check any of the mechanical layers |
| Do not check any layers under "Mechanical Layers to add to all plots" |
Click "OK" and your Gerber files will be generated.
View your Gerber files under the Camtastic.cam files and under "generated files". Carefully inspect the top/bottom metal layers (GTL and GBL) - these are your most important ones. If things are missing or extra metal is present, you'll need to fix this.
Open up the a PCB document.
Select File | Fabrication Outputs | NC Drill Files
Click "OK" and your drill files will be generated.
Inspect the Camtastic Drill file.
The drill files are in the Generated | Text Documents directory. You'll need the Roundholes.txt and (if applicable) Squareholes.txt files as well as the .DRR file.
Kevin Bolding January 08, 2008