Designing PC Boards with ExpressPCB.

by Christopher Garber

When showing my first DIY headphone amplifier to a friend of mine, who happens to be an engineer, the result was very unsettling frown. After having a listen to the amp the frown did lighten up a bit but there was no pleasing him. When I asked what’s wrong he replied, “What you have here compared to your CD player is the difference between the engine of an Australian Holden, and a German BMW.” Straight away I knew he was talking about the breadboard, and the cables running around inside my case, and in all fairness it was an absolute mess.

Breadboards are great for prototyping equipment as it allows great flexibility to modify a design when needed; however the final product of a DIY project, ideally should have a neat PCB, few cables, and survive a shake test. Not only is a proper PCB neater but it is also more durable as there are no cables which can yank loose. This guide is for creating a simple PCB using the freely available tool ExpressPCB (http://www.expresspcb.com). As an example, I’ll design a small, basic Time Delayed Relay.

ExpressPCB is a software tool to design PCBs specifically for manufacture by the company ExpressPCB (no other pcb maker accepts ExpressPCB files). It is very easy to use, but it does have several limitations.

1. It can be likened to more of a toy then a professional CAD program.
2. It has a poor part library (which we can work around)
3. It cannot import or export files in different formats
4. It cannot be used to make prepare boards for DIY production (a limitation which we will work around).

I have used the ExpressPCB to design many PCBs (some layered and with surface-mount parts), and I am quite fond of the software. I print out pcb patterns and use the toner transfer method with an Etch Resistant Pen to make boards. However, ExpressPCB does not have a nice print layout. Here is how I design in ExpressPCB and clean up the patterns so they print nicely.

Preparing ExpressPCB for first use

ExpressPCB as I have already mentioned comes with a less then exciting list of parts. So before any project is started head over to Audiologica and grab the additional parts by morsel, ppl, and tangent, and extract them into your ExpressPCB directory. At this point start the program and get ready to setup the workspace to suit your style.

Click View -> Options. In this menu, setup the units for “mm” or “in” depending on how you think, and click “see through the top copper layer” at the bottom. The standard colour scheme of red and green is not nearly as pleasing as red and blue but that all comes down to personal taste. For the purposes of this tutorial, bright Red is the top layer, sky blue is the bottom layer, and a pink/purple is the intersection between the two layers.

The interface

When a project is first started you will be greeted with a yellow outline. This yellow outline is the dimension of the PCB. Typically after I position my parts and traces, I move them to their final position and then crop the PCB to the correct size. However, if I am designing a board with a certain size constraint, I crop the PCB to the correct size before I start.

On the left hand side is a vertical toolbar which from the top down has the following functions:

• • The select tool: It is fairly obvious what this does. It allows you to move and manipulate parts. When this tool is selected the top toolbar will show buttons to move traces to the top / bottom coper layer, and rotate buttons.
  • The zoom to selection tool: does just that.
  • The place pad: button allows you to place small soldier pads which are useful for board connections or if a part is not in the part library but the part dimensions are available. When this tool is selected the top toolbar will give you a large selection of round holes, square holes and surface mount pads.
  • The place component: tool allows you to select a component from the top toolbar and then by clicking in the workspace places that component in the orientation chosen using the buttons next to the component list. The components can always be rotated afterwards with the select tool if the orientation is wrong.
  • The place trace: tool allows you to place a solid trace on the board of varying thicknesses. The top toolbar allows you to select the top or bottom layer to place the trace on.
  • The Insert Corner in trace: button does exactly what it says. When this tool is selected, clicking on a trace will insert a corner which can be moved to route around components and other traces.
  • The remove a trace button is not very important since the delete key will achieve the same result.
    The remainder of the tools are sometimes useful, and fairly obvious in their purpose, but will not be discussed here.

Design Considerations

Before starting a project there are several ways to design a PCB and one must be chosen to suit the project’s needs.

• Single sided, or double sided?
  • When making a PCB you have the option of making a single sided board, or a double sided board. Single sided boards are cheaper to produce and easier to etch, but much harder to design for large projects. If a lot of parts are being used in a small space it may be difficult to make a single sided board without jumpering over traces with a cable. While there’s technically nothing wrong with this, it should be avoided if the signal travelling over the traces is sensitive (e.g. audio signals).
  • A double sided board is more expensive to produce professionally, more difficult to etch on a DIY board, but makes the layout of components a lot smaller and easier. It should be noted that if a trace is running on the top layer, check with the components to make sure you can get to its pins with a soldering iron. Large capacitors, relays, and similar parts which don’t have axial leads can NOT have traces on top unless boards are plated professionally.
• Ground-plane or other special purposes for one side?
  • When using a double sided board you must consider which traces should be on what side of the board. Generally I put power traces on the top of the board, jumping only to the bottom if a part can not be soldiered onto the top plane (like a relay), and visa versa. My Gilmore amp has all power and ground traces on the top of the board as well as one signal trace which would be three times longer if it was routed around the bottom.
  • Some projects like power supplies or amps can benefit from having a solid plane to use for ground. In power supplies this can reduce noise, and in amps it minimises the distance between parts and their ground connections, and keeps the ground signal as simple as possible. However, care must be taken with stubborn chips such as the TPA6120 amplifier from TI. The TPA6120 datasheet specifies not to run a ground plane under the pins or signal traces of this chip as the capacitance generated could effect performance negatively.

Creating a small project

 So now that these considerations have been taken into account we can start a small example. The project is a simple delayed relay circuit, powered by +12v/0v. As the power comes on the pot delays the charging of the capacitor. When the capacitor reaches the required voltage the darlington pair will switch forward voltage and the relay will activate. I use this in two of my headphone amplifiers to eliminate the power on thump by shorting the signal to GND during power-on.

For this project you will need to download a zip file with the required PCB parts. The zip file also includes the schematic, ExpressPCB file, pdf for editing, and a gif of the final result. It is availuable from here.

1. There are several ways to start a project like this. The two ways I use typically involve placing the most complex component and fanning out, or placing the power/signal traces at a board’s edge and working in. In this case I used the latter method. Place the pads for the power, 2 resistors, pot, and capacitor and link them up as in the schematic. (Hint: Print out the schematic and cross the traces with a red line as you add them. Reprint when it gets messy.)

2. Add the two transistors and the diode. When adding traces try to avoid right angles. Not only do 45 degree angles look nicer, have a shorter trace length, but some people also say right-angle trace affect the signal. (Hint: I used 1.53mm traces because they fit the holes nicely.)

3. Add the relay and the input / output pads. (Hint: The relay pads may not line up neatly since they didn’t fit exactly on the grid. The far bottom right button on the left toggles snap to grid.)

4. Finally select the whole project and move it so it lines up with the top left point on the yellow PCB outline, and adjust the PCB board size to fit. Add some optional text to one of the layers.

At this point the board is complete and ready to be sent to ExpressPCB for production. However using some simple tricks we can print an image suitable for the Toner Transfer, or the Photo Resist methods of making DIY PCBs.

Adding a Ground Plane

This tutorial board does not have a ground plane, but some designs benefit from covering a large portion of a board with a conductive plane tied to a certain net, usually the circuit ground. Capacitance is generated between traces routed under this plane between the nets which can reduce noise in a circuit. Express PCB v5.3 adds the option of creating a plane through the use of the Fixed Plane tool.Clicking “place a fixed plane” allows you to “draw a filled plane” or “draw a keep out area” for the plane at the top of the screen, along with which layer to draw it on. The plane will then be drawn onto the board and will route around all existing traces, holes and keep out areas. [The keep out areas should be placed where capacitance between parts and the plane need to be avoided, such as pins of high speed opamps except of course the connected pin.]

When a plane is added to a design, it surrounds all of the existing traces and pads, not connecting any of them. Those pads that need to be electrically connected to the plane must be individually selected by right clicking on the pad and selecting “top/bottom layer pad shape” and choosing either a solid or thermal pad. Solid pads are a straight solid link between the pad and the plane. There is nothing to distinguish the pad itself from the plane other then the hole. This is fine electrically, but when a weak soldering iron (less than 20W) is applied, the giant plane acts as a big heatsink, making it hard for solder to melt to it. Thermal pads leave the pad and plane separate, instead connecting them together by 4 very thin lines. This is still a perfect electrical connection for low current, but as heat has difficulty dispersing along the thinner lines, it is significantly easier to solder to them. Thermal pads make soldering easier, and solid pads make etching DIY PCBs an easier process.

Preparing the image

Unfortunately ExpressPCB does not offer export functions, and the printing function produces an image unsuitable for DIY PCBs. In order to prepare this image you will need an Adobe Acrobat PDF print driver (there are plenty of free ones available online), and image editing software capable of importing a PDF file. (I will use Adobe Distiller and Adobe Photoshop).

Note: Photoshop has very useful features for making PCBs. The PDF image is unsuitable because it is filled with dots. I tried removing the dots individually. While it is possible to remove the dots this way, it is tedious and painfully slow. Photoshop’s select-by-colour feature is definitely a winner here. The magic wand tool could also be used on each trace. Essentially whatever can be done to either remove the black dots, or the faster method of copying the traces to a new document, will work.

In Express PCB:

• Click file -> print.
• In the dialogue box select the PDF printer (Adobe PDF in the case of Distiller), select “bottom copper layer”, and “print in colour”. (Or top copper layer for 2 sided boards. Each layer is done separately.)
• Click Print.
  At this point you will have a pdf file with the following image:

In Photoshop:

• When Distiller is finished generating the PDF file, open it in Photoshop
• If asked for a resolution, select 300dpi.
• Click select -> colour range, and select the colour of the trace of the layer. (sky blue in my case for the bottom layer).
• Copy the resulting selection, click file -> new -> ok (check if resolution is alright), and Hit Control + V to paste the image as a new layer.
• Control + Click on the new layer will select it, click edit -> fill.
• Select Use: Black and click ok.

That’s it. All that is needed now is to print the image on a laser printer if using the Toner Transfer method. If using the Photo Resist method invert the image before printing. Also note that generally the top and bottom layers are printed separately, and the image will mirror itself when you do the transfer. When printing the top layer of a PCB, the image must first be flipped horizontally before being printed.

The finished product:

All files required for this tutorial are available here.

c. 2005 Christopher Garber (remove _nospam_).

Advertisement