I get asked (surprisingly) often about my PCB layouts and how I do them. Flattering obviously, but also a bit strange as I don’t really consider myself an expert on PCB layout at all. However, I can share are some “workflow” tips on laying out a board in the most effective way based on my experience.
Note that the below is based on using the freeware version of Eagle, but much of it should translate to other software packages without much difference.
The first step is to draw the schematic in the schematic editor. If I start from someone else’s published schematic I’ll normally print a copy on paper and mark on that which parts sizes I expect to use. This then becomes the reference for drawing the schematic in the editor. Once the schematic is drawn in it’s basic form I’ll check it, rename the parts and then run an electrical check to verify that nothing has been missed. If I am going from a published schematic I normally stick to the part names from the original schematic (because that makes for much easier troubleshooting if something’s amiss later on), otherwise I will make up something that is logical to me, usually going from input to output.
Then it is time to switch to the board editor. Most of my PCB layouts start out with mounting holes placed in the four corners (because that’s normally where I want them) and a ground plane drawn in the top layer. If I have a specific board size in mind I’ll restrict it straight away, otherwise I will keep the full area and then reduce the size as the layout progresses. I will also load my own standard design rules and tweak the parameters (mainly clearance) if required before I start, because then I will not make something that I have to revise later when the DRC (design rule check) fails.
I generally then start the actual layout process by placing the key components as I want them. Key components usually mean:
- Power and control devices (transistors/ICs and potentiometers/switches) that must extend over the edge of the board
- Power devices that need an onboard heat sink (heat sink is placed as well of course)
- Other ICs plus their associated decoupling parts as close to the IC as possible
- Key connectors (if they need to be in a certain position I fix that, otherwise I put them on the specific board edge where I believe it makes most sense to have them).
After this, the fun (or frustration) starts. Using the schematic on one side and the “ratsnest” command in Eagle to recalculate wires I start moving first the major and then the minor parts of the circuit around and positioning them to yield as short and as neat traces as possible. This requires several iterations and usually also putting the board away and coming back to it later because I tend to “go blind” after staring at the layout for too long at a time. Other tips that I use to simplify the layout process include:
- Every time I make a major change, I save the board as a different file version with a new revision number, because sometimes layout changes turn out to be “dead ends” and then it’s easier to return without having to do massive amounts of rework. Some of my more complex designs have 10-15 file revisions before getting to the final layout.
- I normally do the basic layout using one trace width, generally the smallest width I expect to use in the circuit. Once I have a layout I am reasonably happy with mechanically, I can enlarge key traces without having to do a lot of fiddly rework and without risking that I miss something. In general I also stick to using a few standard trace widths which makes it easier to quality check the layout later on in the process.
- I normally start with 45 degree trace angles for simple and consistent routing, and the in the last round of tweaks I may change some traces to be “odd” angles instead if it significantly helps the layout.
Once the layout is beginning to shape up and all traces are routed, I will start the actual layout screening process. This usually involves generating gerber files for the circuit and rendering them with circuitpeople.com and looking at each layer in isolation. For the copper layers I mainly try to look at a) whether the individual traces follow the most unbroken and logical path and b) whether the individual signals will flow through consistent trace widths. If not, i go back and make corrections accordingly. Once I start checking Gerbers, I also start adding text elements to the board because I now have a reasonable idea of where there is space for them.
I then pretty much repeat this process over and over again until I believe I can’t make any more improvements. Again, putting the board away for a day or more often helps and I often find that even a short break from something I am happy with means that when I come back I can make bigger optimisations than I though possible when I left it. Often during these breaks I also think up new features that may be worth including, such as multiple footprints for key components, additional labelling for connectors etc.
Eventually I get to a point that I am happy with the layout and then it is mainly the last checks of both the individual layers (using gerber renderings from circuitpeople) and the full board (using renderings from gerber-viewer.com, which allows displaying of multiple layers at the same time) plus the last tweaks to the silk screen. The last step is usually confirming that ERC and DRC are still error-free, and then printing off a sample of the board layout at 100% to check the final size. Seeing the board printed in actual size gives me a better impression of the size, even if I already know how big e.g. a 2” x 2” board is.
I will then place the PCB order and mark the last Gerber version with a tag in my Eagle project folder so that I can see later that this was the file version I sent off for manufacturing.