Making printed circuit boards

Using ExpressPCB software and service

( )

First steps

Download latest version of schematic capture (ExpressSCH) and pcb (ExpressPCB) software from www.expresspcb.com. Read on-line help for both. On the ExpressPCB web site, read the "Tips for Designing PCBs".

Create schematic using ExpressSCH. Place every component on the schematic, including connectors that get signals and power on and off the board. If you create custom components, assign numbers to pins. Use Edit > Copy BOM to clipboard to as a BOM check. In your main BOM you need an entry for every component on the ExpressSCH BOM. In the schematic, File > Check schematic for netlist errors. Fix until you get no errors. Print the BOM and use as a checklist to ensure all components are placed on the PCB

Open new ExpressPCB file.

Drag outline handles to desired board size. Will open at 2.5" x 3.8", the size for the ExpressPCB MiniBoard service, your lowest cost option. Leave at this size unless your boards needs to be bigger.

Use Layout > Compute Board Cost to get pricing. Board cost depends only on board size and service. For lowest cost, choose 2-layer and standard or miniboard service. These don't have silkscreen (the lettering) or solder mask (green color) layering, but are musch less expensive. If making 10 or boards copies of the board, choose production service.

Create the board

Read the ExpressPCB help file and look at example Express.PCB files for hints.

Use the keyboard shortcuts. They will speed up operation considerably. Most important are: S=select, Z=zoom, +=zoom in, -=zoom out, F=zoom to fit, T=place trace, L=toggle between upper and lower layers, Space=end trace

File > Link schematic to PCB to connect the schematic file to the pcb file. Should you update the schematic, File > Refresh link to schematic to update the connection.

Place mounting holes. If mounting with 6-32 screws (recommended), use 0.200" round pad with 0.150" hole. Center of mounting holes 0.2" from each edge.

Place all components into the work area. Location doesn't matter yet. Assign a Part ID to each component by double clicking on component for the properties dialog box. Part ID must match Part ID on the schematic. Make custom components as needed, assigning numbers to all pins.

Place components that have defined relation to the enclosure. For example, right angle serial port connectors, or switches, or potentiometers that mount on the board but must stick through a hole in the enclosure. Double and triple check dimensions and placement.

Place ICs. Orient all in the same direction. Some shuffling may be required after other components are placed.

Place bypass caps at top of ICs.

Place large caps or other large components. If using TO-220 package components with heat sinks, allow room for heat sink.

Place smaller components.

Shuffle things as needed. Cluster related components together.

For traces, upper layer (red) run vertical, lower layer (green) run horizontal. While tempting to break this rule ("Gee, that pad is just there, I'll go vertical on this green trace for a bit, it won't hurt"), later in the layout you may regret your choice. Short sections of 45 deg are OK if you have to bump a trace up a bit and if it reduces the number of vias. Re-read the help file and the "Tips for Designing PCBs" for hints. Also, look at existing board files.

Lay down power line busses (e.g. +5 V and gnd) using 0.100 wide traces. If 0.100 doesn't fit, use 0.050.

Lay down high current lines using as wide a trace as possible (0.050 or 0.100)

Lay down signal lines with 0.012 traces. Use vias as needed to get from one side of the board to the other...but don't go overboard with vias. Vias are automatically placed when you change layers during a trace, or can be placed manually using a 0.056" round via.

No right angle turns on traces less than .050. If you have to get around an obstruction, build the detour with 45 deg turns.

You can use narrow 0.010 traces to fit between the pics of DIP ICs, but stay well away from the pads.

For laying signal and power traces to components, use the Highlight net connections button at the left. Clicking on a pad will highlight all the pads that must be connected. This greatly simplifies figuring out what goes to what. The nets will only be correct if the schematic was correct.

If a the highlighted net pad on a non-polarized component, e.g. a resistor, is at the opposite end from the simplest trace route, flip the component. When flipping, rotate the component but keep the text upright.

After traces are down, see if you can eliminate any vias by re-routing.

Finding optimal trace routes is fun. Somewhat like solving a puzzle.

If possible, add a ground plane for sensitive analog components. The ExpressPCB help file describes how.

If room, put a text label on the red layer to identify the board. If creating production service boards, place labels on the silkscreen layer.

Error check the board. Steps are below.

Error check the board

Run Layout > Compute Board Cost again as it can catch some errors.

Print a hard copy of the board. Lay the components (if you have them) on top and check that things fit)

Use the Highlight net pad button. Click on all pads of all components checking for proper connection. Check off on the BOM as you go to ensure you check all components. The message box at the bottom will alert for any missing components.

Set view to a single layer using buttons at lower right. Check that all traces end at a pad or a via. Check for overlapping traces on the same layer.

Print a hard copy of schematic. Using a highligher, mark a line on the schematic. Check that this connection exists on the PCB. Continue until all lines on the schematic are marked.

If you change even one trace, re-do the error checking.

Triple check before ordering. You are about to spend $50-$150 or more and it is irreversable if there is a mistake.

Final steps

Layout > Order Boards via the Internet to order the boards.