Well… I think I have had another learning incident. I was routeing the logic on my PCB and feeling pretty good about how it was coming together. Then I realized I didn’t have the power routed. And with how I layed out my traces, power could not reach some of the IC’s. My question is, and I think I know the partial answer, is should the power, positive and negative be layed out first? I think so. Then how exactly should it be done? Should I use one side, maybe the back for the + and - (ground). Maybe running the power horizontally from both sides of the PCB and allowing a center section to be clear to route some logic? FYI, I’m trying to fit 26 IC’s, a voltage regulator, three connectors, a bunch of bypass cap’s, and a handful of resistors. Thanks Mike
Short answer: It is common to have a copper pour on at least one side of the board (assuming a two(2) layer board) assigned to the GND net to make half of the connections.
I’ve read a little about the pours. Should the pour be first and traces added after that? Mike What I mean is, Adding traces to the side of the pour.
There are two(2) key things to consider when using a copper pour.
“Show filled area in zones”, on the left vertical menu bar, really clutters up the visual display of the other layers on the board. Select the visibility level that you prefer for the task at hand.
Hint: If you use a large enough grid for the clearances of the design then it becomes likely that no manual routing of the GND net will be required.
Remember that the “b” Hotkey will rebuild the filled zone. Any additions or changes to copper traces will affect how the the filled zone is rebuilt.
Thanks, I’ll give it try. Mike
A copper zone is not a magic thing. If you simply add a copper zone to a two layer board without thinking about that from the get go then you will not get good ground connections! Even if DRC says everything is connected you might have ended up with two pads that are quite close to each other having a connection only over a thin and long part of the zone.
A copper zone is a good and easy way to get uninterrupted power planes if and only if the zone is on its own layer. This is the major benefit of increased layer count. If your time is more expensive than the upgrade to a 4 layer board then i would suggest you go that way. If not then you might need to start over.
If you need to stay on 2 layers then you need to follow a few rules from the start. One layer is for horizontal connections only the other for vertical. You then add a zone for one power supply line (most likely GND) to both sides and stitch it together to get something as close to an uninterrupted zone as feasible with a two layer setup.
Another option is to try and avoid putting traces on the second layer as that will leave one nearly uninterrupted layer. Then you only need to carefully check if the few traces that interrupt this plane are something to worry about (and if necessary add something on the top layer to bridge this interruption there).
TlDr: zones on a two layer board are an art in of itself. If you can afford it go with a 4 layer setup and have one inner layer exclusive to GND.
A 6 mill copper width is good for 0.225Amps with a 1C temperature rise; and is a fairly common minimum for modern fab houses. With proper grid spacing between parts, there will be more than one copper path to the different devices; none of which are stated to be high current devices.
26 ics is getting up there, so the next logical step is to consider 4 layer Board, of it gets too tight on 2L.
4L are also better Thermally, and have better RFI and EMC and lower ground noise.
The pours auto-adjust to where the traces are not…
On tight 2 layer boards, I like to route Power/Gnd as traces and then pour last, and do another pass that increases pour copper by compressing signals. That ensures you have connections everywhere, and copper fill where possible.
Reading this I imagine an old PCB with many DIL14 7400 serie ICs organised as matrix. Assume we have each ICs pin 7 (GND) right down, and pin 14 (VCC) left up. Under each row of ICs (or betwean ICs pin rows) there were the GND horizontal track connected to all pins nr 7, and over all ICs row there were the VCC horizontal track connected to all pins nr 14. Then GND tracks were connected at far right of PCB, and VCC at far left od PCB. Blocking caps were positioned between each ICs in row connecting theirs VCC and GND traces. All rest connections were done by horizontal tracks at the layer at which the power is done and vertical at other layer.
Rene, thanks for the thoughts. This is my first PCB. I was thinking that a 2 layer board would be cheaper than 4. I’m a retired engineer and time is not really a problem. But that being said, maybe I should look in to the cost differential. I don’t mind starting over, this is a learning project besides a functional project Mike
My minumin trace is set at 10 mils. You say that 6 mils would allow two traces between pins? Maybe I should try that. THanks Mike
Thanks I’ll have to investigate the cost of a 4 layer board. It would make things a little easier. But being a SS supported person I have to watch the penny’s. Thanks Mike
YUP. This is a 7400 board. I’m attempting to make a PCB of one of my wire wrap boards. This PSB would be a replacement for my I/O card on my 8080 computer. The wire wrap board has 2 PPI’s and 2 UART’s on it. The PCB will have only one PPI. But as I go things are getting tight. Thanks Mike
Look at those old times boards. They hat two traces on the top layer, both parallel and passing under the ICs lengthwise. All ICs nicely aligned in a grid makes this technique easier to follow.
74 series in DIL is no problem with two layers.
Nick
I found a site www.s100computers.com. There are a number of s100 boards, mostly likely made in this century. I see that they have horizontal traces on the front and probably vertical traces on the back. I’ll give this a try thanks Mike
One other note if you opt for 4 layer board Mike, route the power traces on the outer layers. Better heat dissipation. For really high current traces I have also seen PCBs where the solder mask was left off for specific traces and “busbars” soldered to the traces by hand afterwards. This is extreme though.
That is only an issue if you really have high power stuff (>1A)
I would assume that in this case it is simply meant as “the supply lines” which will carry in the order of a few mA.
For supply lines like these it is typical to have uninterrupted planes on the inner layers as it reduces the number of things you need to think about with regards to EMC. (one full layer GND, one layer for the positive supplies if possible large uninterrupted regions for the same supply)
First serious money I have ever earned was for Chronocomparator (don’t know if I name it correctly - the device to measure and calibrate digital watches speed) I have done (being those time a student) in 1981.
It was based on 7400 serie.
I’ve got 2x my father months salary for it. That price still was 4x less then the price for factory made such device. I had a chance to see such device working but could’t look inside as it was at guaranty. The biggest unknown for me was how to build the antenna to receive 32768Hz from watch.
And I’ve got into a problem of 8 hour time constant in electronic 
I put reference 1MHz clock into a thermostat (quartz case surrounded by aluminium sheet + heating transistor + thermistor) in a styrofoam box. It stabilized its frequency in about 15 minutes. But once I decided to run my device for whole day and noticed that after about 8 hours it lost accuracy. The reason was 7400 serie power consuming. Temperature inside my device (it was about 15x15x30cm) rise over temperature I set in thermostat.
If he really has old 7400 TTL serie ICs (probably not) then each one is about 20mA. 26 Ics x 20mA = 0.5A.
Yes all the IC’s are 7400 TTL chips and the current draw is closer to 0.625 Amperes. I am still hoping to fit all the traces on a two sided board, but we will see. Had some family stuff come up and have not been able to work on the PCB, but will start again soon. Thanks for the help Mike