I would like suggestions from experiences pcb designer on the order in which I should lay out the track for a complex 4 layer board. In a 6x6cm board, I have 150 parts of which there are 36 ICs (16 of which are Dual FETs and 16 photo detectors), 33 LEDs, a high density connector and the remaining are resistors and caps. Only one LED will ever be turned on at a time and for approximately 20 seconds, 1 second delay then the next LED. There is no high speed switching. The detectors and the LED selector are I2C at that is only 100Khz clock. The I2C clock is not “active” after the desired LED and detector are selected.
Should I lay the power and ground first? Should I lay the longest runs first? etc. etc. I realize by asking this question that the responses will be highly subjective. Please chime in! Thanks!
I allocate one inner layer as ground. Once you have a good ground plane power becomes much less critical.
Placement is the hard part. I guess the LEDs and connector have fixed locations, so the other parts have to be placed to minimise total track lengths
That many components and ICs on a board that size sounds like a challenging board to route. Component placement will be crucial to success.
You haven’t told us much about the board so it’s difficult to give any specific advise. Typically I would route the most critical parts of the circuit first. For high speed logic or analog circuitry where noise is a primary concern you might want to start with your PDN. Then the high speed logic and/or analog sections where short traces are preferred. I find it is usually easier to route shorter traces first.
with a repeating cell, take the time to pack one very tightly, (which may mean routing a few to check inter-cell packing) and then consider a script to clone that placement on the needed XY’s
I’ve been making boards for years, but just started with KiCad.
I usually first arrange the parts roughly by function and get the ratlines somewhat organized by moving and arranging the parts.
Then I arrange the power distribution, a task made much easier if you can put a ground plane on the bottom. I’ve never made a 4 layer board but envy the ability to have a + plane as well.
Then I usually start with localized traces that nothing crosses, just 'cause it’s easy work. Then I attack any buses or groups of tracks that go together.
Lastly, I weave in any long traces that wander from one part of the board to another.
Chrystals, bypass caps and other distance critical things are done VERY early. Like as part of power distribution.
Once you have a solid and unbroken ground plane and have smd decoupling right next to each power pin, a power plane is a waste of track routing possibilities
Again, knowing nothing about the circuitry on the board such a statement is rather dangerous if not misleading.
You can almost never go wrong by having a power plane and it always frees up space on your signal layers. Without a power plane you need to pay even more attention to your PDN analysis. Without a power plane you end up with two adjacent signal layers which could also cause problems. We don’t know if there is any impedance control needed on the board, etc. And there is more to decoupling than just having caps close to power pins.
I usually have multiple power rails, so power planes are likely to be fragmented anyway.
The OPs question is about a board with many leds, so probably a display or illuminator, neither of which are in transmission line territory.
Power distribution may well an issue to be considered if many leds switch together and planes are not always the answer to this if supply noise is a critical elsewhere.
I would probably be using power planes in a 6 layer design
I don’t see how you can jump to conclusions about a board based on how many LEDs it has. Perhaps it’s a stereo preamp with an LED VU meter? You might like that to be somewhat quiet. It might be a digital Yahtzee game, but having it reset every time it rolled 5 6’s wouldn’t be cool either. Either way it doesn’t change what I stated previously.
Multiple power rails are pretty common. You can get away with properly split power/ground planes if you know what to avoid. I also have boards with multiple power rails, multiple voltages many of which are also split between digital and analog. I wouldn’t even consider not having a power plane.
Anyway, I was simply stating my opinion that you far too easily dismissed the use of a power plane for what would seem like an already difficult board based on the number of power connections for 36 ICs, regardless of how many LEDs there are.
I am not trying to argue, sometimes power planes are necessary, sometimes useful and sometimes a waste.
What is more important for any non trivial board with a digital clock is to have a ground plane or FCC/CE compliance is unlikely
Split power planes work well when a board can be nicely partitioned core - IO - interface - analog (like a PC motherboard) , but mine have just about every IC needing 2 rails, so not so simple
On 4 layer boards I often use the second inner layer as a power plane to begin with, but I don’t take much care to not fragment it as I would with a ground plane. If it’s a complex board the power plane often end up with both traces from other power rails and sometimes signals too. But it doesn’t matter, but it sure makes initial routing easy when you can just nail down both the ground and power pins to begin with. You don’t start eating off of the power plane before you have to, and it often ends up with only short traces going over other traces on the top or bottom signal plane.
Typically the second layer, that is the first inner layer from the component side, is the ground plane. On a smd board much of your routing is on the component layer so it makes a little more sense to have the next layer as your reference plane. It also allows stitching vias to thermal pads etc without punching holes in your power plane (assuming you use blind vias). It can also provide a bit more shielding for the components themselves.
A continuous power plane is often just as important as a continuous ground plane. The power plane can be split into multiple power planes if done carefully. What “carefully” means depends on the circuit design.
Running signal tracks on your power plane makes it less like a plane and more like a bunch of big tracks, especially if you’ve already split it. It can no longer function as a reference plane. Perhaps it’s time for more layers?
1.21Gigawatts: How did you manage to quote me like that? All I get when I press the reply button is a link to your post and your avatar in the upper right corner of my post. I will reply you in paragraphs accordingly.
Yes, I took for granted everyone used the second layer as ground plane. You will see when you read my post again that I never mentioned putting either power planes or tracks on the second layer.
Define “often”. More often than not I will say that normal routing of power tracks are considered sufficient.
Yes, as I said, my power plane will get segmented if it turns out I need it for signals or other power tracks. You assume I use a power plane for impedance benefits, but if you read my post again I explain it is only for making routing easier. If I need a continuous power plane, then yes, I might need an extra layer. But if you take care to only route short tracks that go roughly in the same direction, there’s no need.
Below I have attached an example using the method I describe, where I end up using many more signals on the power plan than I wanted for. This was due to a revision with the addition of a few signals and not enough time to redo an entire space constrained board. If you look at it in full resolution, you can see how I originally intended it, the plane is VDDS and only a few VDDR tracks. It keeps the layout tidy and simple. The addition of the other signals demonstrates two things:
I was lucky I has an almost unused layer for emergency routing.
There is still plenty of track width left on my uA VDDS plane even though I had to cut it horizontally in half in the middle.
