Here is what I found so far:
Paul's Everything you need to know about PCBs
1) use 12mil lines and 12mil spacing for signals.
2) use 25mil lines for power as a minimum. 50mil is best
3) for standard parts like caps, resistors and ICs use 60mil pads with 40mil holes
4) for the vias (to transfer the trace from 1 side to the other) use 40mil pads with 18mil holes
5) for resistors and axial ceramic caps use 400mil pad-to-pad spacing
6) for radial/film caps use 200mil pad-to-pad spacing
1mil = 0.001inch so 60mil = 0.060in
Note: when I say pad-to-pad it's really "hole-to-hole" but I'm using standard nomenclature. You want the resistor leads bent on 400mil spacings and 95% of caps used for filters are 5mm = 200mil spacing.
Overall looks ok. Just a couple suggestions.
Personally for analog circuits I don't run traces between IC pins. I'll run them up under the chip but not between the pins. Also, I like to come off the IC pin at a right angle, even if for only a short distance.
You don't have any bypass caps. Add a 100n cap to ground on each IC power pin as close to the pin as possible.
If the pots are off-board create pads for them. That way they don't have to be laid out as a trimmer footprint. That will free up your layout.
If you're using the ground plane as the actual signal ground make sure there are no unconnected islands.
The Big Ear wrote:
Why is it so important to have the caps as close as possible to the IC?
The bypass caps control (or try to) the noise on the power traces. The cap will filter noise on the trace before it gets to the ICs power pin, and will also filter noise created by an IC before it gets to the power trace.
Your CMOS chip is going to generate spikes on the power line as it switches, like when you flush the toilet and your wife is taking a shower... she yells. You want to put a capacitor close to the pin to keep that noise from getting to other components. Not the most technical explanation, but you get the idea.
It is quite a mental exercise, but once I get started on a design it is totally addictive. Recently one layout took me 3 months to complete Dead Banana just couldn't stop fussing over it, but it all worked when i built it so nanners
Usually I place chips and route power rails and ground 1st.
Once first draft is finished, I spend at least a few sessions refining the design, moving components to better positions, thickening up traces wherever appropriate.
When I think I am done i print out the schematic and check the PCB against it and mark off the schematic with a red pen to ensure every connection is correct. Then check all the pos, neg and ground connections are done and all route back to the power pins.
Always work from a schematic.
Build your prototype first
Make corrections to your prototype
Prototype with the actual production parts
Layout you pcb from the final schematic
Check spacing using production parts
Double check everything, and agin.
P.s. always work from an accurate schematic
Centralize everything off the Power Bus as much as you can. There's always exceptions, but that's a good place to start.
Strategically place resistors, diodes, caps, etc. so you can run traces in between the leads.
Don't hesitate to drag the pads to where you need them. Metal Bends! thumbs up
Jumpers, Jumpers, Jumpers!!!
Leave yourself a little space while you're laying the circuit blocks out. You can pull them closer after you optimize their placement.
Don't be afraid to rip stuff up and move it around. That's what the SaveAs is for. hihi
Routing traces manually is way way easier than dealing with the autorouter in my opinion! Just have a plan going in, and break it up into little chunks. You've got a pretty densely packed board there, and thru-hole means that routing can be more difficult. Set things to a 10mil grid and do 10mil traces, don't be afraid to get them right up next to each other or use small vias. Try to have bottom-side traces go one way, and top-side traces the other way.
Usually I construct little circuit blocks as densely as my DRC will allow, route them independently, then place them on the PCB, route power, and then connect the blocks to each other. That's going to be difficult with thru-hole on this layout I bet. 56 traces goes by extremely fast. You can hide power and ground connections in eagle by entering the command "ratsnest ! gnd +12v -12v", etc. and then do the same (minus the ! symbol) when you want to show them again.
If you're finding it extremely difficult or impossible to squeeze your layout onto this board, you might want to go to a second PCB, and use 0.1" headers to connect the boards.
Generally, it is best to place parts only on the top side of the board.
When placing components, make sure that the snap-to-grid is turned on. Usually, a value of 0.050″ for the snap grid is best for this job.
First place all the components that need to be in specific locations. This includes connectors, switches, LEDs, mounting holes, heat sinks or any other item that mounts to an external location.
Give careful thought when placing component to minimize trace lengths. Put parts next to each other that connect to each other. Doing a good job here will make laying the traces much easier.
Arrange ICs in only one or two orientations: up or down, and, right or left. Align each IC so that pin one is in the same place for each orientation, usually on the top or left sides.
Position polarized parts (i.e. diodes, and electrolytic caps) with the positive leads all having the same orientation. Also use a square pad to mark the positive leads of these components.
You will save a lot of time by leaving generous space between ICs for traces. Frequently the beginner runs out of room when routing traces. Leave 0.350″ – 0.500″ between ICs, for large ICs allow even more.
Parts not found in the component library can be made by placing a series of individual pads and then grouping them together. Place one pad for each lead of the component. It is very important to measure the pin spacing and pin diameters as accurately as possible. Typically, dial or digital calipers are used for this job.
After placing all the components, print out a copy of the layout. Place each component on top of the layout. Check to insure that you have allowed enough space for every part to rest without touching each other.
Placing Power and Ground Traces
AftPCB2er the components are placed, the next step is to lay the power and ground traces. It is essential when working with ICs to have solid power and ground lines, using wide traces that connect to common rails for each supply. It is very important to avoid snaking or daisy chaining the power lines from part-to-part.
One common configuration is shown below. The bottom layer of the PC board includes a “filled” ground plane. Large traces feeding from a single rail are used for the positive supply.
Placing Signal Traces
When placing traces, it is always a good practice to make them as short and direct as possible.
Use vias (also called feed-through holes) to move signals from one layer to the other. A via is a pad with a plated-through hole.
Generally, the best strategy is to lay out a board with vertical traces on one side and horizontal traces on the other. Add via where needed to connect a horizontal trace to a vertical trace on the opposite side.
A good trace width for low current digital and analog signals is 0.010″.
Traces that carry significant current should be wider than signal traces. The table below gives rough guidelines of how wide to make a trace for a given amount of current.
0.010″ 0.3 Amps
0.015″ 0.4 Amps
0.020″ 0.7 Amps
0.025″ 1.0 Amps
0.050″ 2.0 Amps
0.100″ 4.0 Amps
0.150″ 6.0 Amps
When placing a trace, it is very important to think about the space between the trace and any adjacent traces or pads. You want to make sure that there is a minimum gap of 0.007″ between items, 0.010″ is better. Leaving less blank space runs the risk of a short developing in the board manufacturing process. It is also necessary to leave larger gaps when working with high voltage.
When routing traces, it is best to have the snap-to-grid turned on. Setting the snap grid spacing to 0.050″ often works well. Changing to a value of 0.025″ can be helpful when trying to work as densely as possible. Turning off the snap feature may be necessary when connecting to parts that have unusual pin spacing.
It is a common practice to restrict the direction that traces run to horizontal, vertical, or 45 degree angles.
When placing narrow traces, 0.012″ or less, avoid sharp right angle turns. The problem here is that in the board manufacturing process, the outside corner can be etched a little more narrow. The solution is to use two 45 degree bends with a short leg in between.
It is a good idea to place text on the top layer of your board, such as a product or company name. Text on the top layer can be helpful to insure that there is no confusion as to which layer is which when the board is manufactured.
Checking Your Work
After all the traces are placed, it is best to double check the routing of every signal to verify that nothing is missing or incorrectly wired. Do this by running through your schematic, one wire at a time. Carefully follow the path of each trace on your PC layout to verify that it is the same as on your schematic. After each trace is confirmed, mark that signal on the schematic with a yellow highlighter.
Inspect your layout, both top and bottom, to insure that the gap between every item (pad to pad, pad to trace, trace to trace) is 0.007″ or greater. Use the Pad Information tool to determine the diameters of pads that make up a component.
Check for missing vias. ExpressPCB will automatically insert a via when changing layers as a series of traces are placed. Users often forget that via are not automatically inserted otherwise. For example, when beginning a new trace, a via is never inserted. An easy way to check for missing via is to first print the top layer, then print the bottom. Visually inspect each side for traces that don’t connect to anything. When a missing via is found, insert one. Do this by clicking on the Pad in the side toolbar; select a via (0.056″ round via is often a good choice) from the drop down listbox, and click on the layout where the via is missing.
Check for traces that cross each other. This is easily done by inspecting a printout of each layer.
Metal components such as heat sinks, crystals, switches, batteries and connectors can cause shorts if they are placed over traces on the top layer. Inspect for these shorts by placing all the metal components on a printout of the top layer. Then look for traces that run below the metal components.