Routing ICs VCC/GND on pcb between its own pins

Hi,

Many ICs have a a couple routes to GND or VCC
I have three questions..

Is it ok to:

  1. Route 1 line to the IC per power/ground and the rest route underneath the IC between its own pins?

  2. Route power/ground to the IC from the source and directly from that IC pins route those lines ahead to other electronic parts/rest of board?

  3. I know some ICs are different than others, but as a general rule of thumb would you consider routing the VCC underneath the IC or the CLK lines? Not sure of the effects those ICs can have on the signal and I guess it would be better not to gamble with CLK lines..

by looking at the datasheet i don't necessarily see any recommendation from the manufacturer, e.g i know the atmega328 has vcc and avcc etc, but on arduino these gnds etc are all connected together, so they are also not really following best practice i think..

2 sided board - run ground plane on both sides. Run wider VCC trace to power pins as needed. Keep traces away from crystal traces, only have Gnd plane under the crystal. 10mil traces for signals, 20-24 for VCC, wider if having high current flows - there are online trace width calculators you can use.
Everything else: no long parallel traces with data & clock lines, have clock cross other signals at right angles where possible. By clock, SCK for SPI is the only really critical signal.
Don't forget 0.1uC cap on each VCC/AVcc pin of Every device on board.
Keep analog traces away from digital as best you can.

CrossRoads:
no long parallel traces with data & clock lines, have clock cross other signals at right angles where possible. By clock, SCK for SPI is the only really critical signal.

Thanks for the elaborate answer :slight_smile: most of it i managed to find lately only and you reassure the knowledge i gained, always gain new info..

  • You mean no parallel traces for VCC with the data or clock? or that data and clock shouldn't be parallel as well?
  • Right angles, as 90 degrees? I dont understand how does that look over the other trace, even if you meant 45 degrees..

I didn't get answered for some of the original questions, i think.. or if it's not in what you replied, than i shouldn't take it into consideration at all :smiley:
I wanted to know if its possible to route power/ground traces to an IC than between itself to pins that need power or to even other electronics and whats better to route under IC, VCC or CLK traces, if it matters..

Right angles, as 90 degrees? I dont understand how does that look over the other trace,

One track in one side of the board and the other track on the other.

Basically what you are trying to do is to minimise the capacitance between the tracks to prevent signals coupling between them.

Grumpy_Mike:
One track in one side of the board and the other track on the other.

Basically what you are trying to do is to minimise the capacitance between the tracks to prevent signals coupling between them.

Yeah i understood the double sided idea, and they go on either side of thepcb…
i attached an image with 4 trace options below to try and make our life easier with this :wink: what i understood is number 2, but it sounds like you recommend me to go for option number 3, but between option number 3 or 4 i didnt think like there should be a difference so i thought you guys must be really speaking of some awkward number 1

or do you mean something completely different and that you meant that any traces that go “over” one another should be perpendicular

123.png

Routing under the IC is not critical.
VCC with large current flow and SCK with fast edges can have some impact on close, parallel traces.
Leave some separation, or run the traces at right angle.
Make the signal path for both as short as you can, don't wander all over the board with them if you can help it.

Number one is a nonsense you should always route wires to be as short as possible.
Do not run lines in parallel first and then dive over just do it.

Grumpy_Mike:
Number one is a nonsense you should always route wires to be as short as possible.
Do not run lines in parallel first and then dive over just do it.

yeah i know number 1 is absolutely idiotic :smiley:
did you mean that any traces that go “over” one another should be perpendicular ?

CrossRoads:
Make the signal path for both as short as you can, don’t wander all over the board with them if you can help it.

but there are times where you must route VCC all over the place, is that ok? you can see below the outer circular trace line which is all VCC, i am going to make them fatter soon…

#2 would be good.
#4 is not bad.
#3, avoid right angle, the etching process can eat the inside corner more, making the trace more prone to failure. Keep the close parallel path, and parallel overlapping between layers, to a minimum.
#1, that’s just bad routing, just go straight across. If the path is needed to go around something, then do it as a couple of turns, avoid the right angle, same as #3.
Here’s a board I did recently. You can look close and say “bad routing for reason #x, bad routing for reason #y
but what you can’t tell from the routing is the functionality.
If you follow the CLK path from the upper 2x3 header, you will see it goes to every device on the left, and parallels the thicker power trace. However, in this case the power is a pretty low current level, there are plenty of decoupling caps, so there would be little likelyhood of current surges bothering the clock lines, and it only parallels one line for a very short amount. The signal it parallels is a MOSFET gate drive line, so any crosstalk would just get masked by the comparatively slow turn on and turn off times of the MOSFET.
Same with the long traces going out to the gates. One gate control signal is likely to have little affect on another.
What you also don’t see is the ground plane that covers the majority of the board, ground plane that was maximized by moving signals to allow wide free path from the power MOSFETs back to the screw terminals, by adding Ground vias to connect up layers, by moving signals away from pads, and sometimes changing layers to let the ground plane get to places it otherwise would not be.

All this comes from experience designing and having to debug errors in other designs where not as much care was taken, or signal density didn’t allow it, and the resulting signal glitches had to be addressed in other ways.

CrossRoads:
#2 would be good.
#4 is not bad.
#3, avoid right angle…

Yes yes, we are speaking of the same thing

CrossRoads:
have clock cross other signals at right angles where possible

So i didn’t quite get the point here with right angles but if I did get your over idea in the first quote i think im good, also checked your design i see i undertsand…

Thanks a lot for the elaborate explanation! thumbs up! cool info…

This is a close parallel clock trace to vcc? really? its like 6mm no??

I see in your design on IC2 pin number 13 (i think), a trace goes over a pin, is that normal?

Your design really shows a good demonstration of the vertical/hortizonal layer strategy with vias that i read about but couldn’t implement myself due to the oval shape and in turn parts placement

sorry to be a pain in the ** but i still dont understand what i came to this post with… :slight_smile:
if i can route vcc to an IC’s vcc pin and to trace from that same VCC pin to other pins of the same IC that need power… or to other electronics’ power pin… does the current or whatever electricity terminology get affected by that VCC pin or the power just goes through “around” that pin, powering it and continues on like the pin isn’t even there, to the other electronic part

The separation between all traces and pads is at least 10mm. I don’t do 6, that’s too easy to short things together when soldering.

Yes, having a trace connect to a pad in multiple places is normal.

Routing Vcc to multiple places - there is resistance in any wire, so many ohms/inch based on copper thickness and width, so the overall resistance increases with wire length. Your little thin trace is bad, that needs to be thicker. What you can do to help is rotate each LED perpindicular to the board edge the way the LEDs at 12:00, 3:00 and 9:00 are. Then you can run a nice fat VCC trace around the outside of the whole board. Then there will be minimal (and likely unmeasureble) voltage drop as you go down the line.
Do you have a ground plane? I’m thinking yes based on the lack of traces connecting pins I know are grounded, such as the 22 pF caps.
Looks like you need VCC connected to several LEDs and all 4 ICs still? With a fat VCC trace running around the board, you can drop Vcc in from the ring to the power pins easily, down the middle of the chips, and get all the LEDs too.

Thanks croassroads.. couldnt get near a computer so couldnt reply sooner..

I selected all traces and turned them to 10mil and haven't got aroundt to make the VCC back to 24mil..

The reason the LEDS are not perpindicular is that before I had a different design and I connected them to ground plane, forgot them like that..
I cant seem to manage to route 24mil traces straight out of the pins anyways when the LED is in an angle, the route needs to start very short and than straight off go in 45 degrees or it gets too close to ther pin beside it.. sounds like asking for trouble

Yes I need to connect VCC still to all points you mentioned..

Last question I guess before i wrap up this one and ship it out.. i understand tracing 45 degrees staright of the pin isn't a good practive.. Is it possible to route VCC from the power source to the external vcc "outer ring" in my design (the one you referred to) at 2 or more places? for some kind of awkward redundancy or maybe better signal..

i understand tracing 45 degrees staright of the pin isn't a good practive.

There is nothing wrong with that.
Connecting to the outer ring in several places is fine.
Starting thinner at the LED leg and getting thicker as soon as space permits is fine also. I often have to do that with SMD parts, where 8-10mil is the width of the pad, and there are adjacent pads, so that's all you can get right at the part.
LEDs with 25.4mm pitch can have 16mil at the pad and then widen out to 24 just away from the pad, especially where signals are leaving the LED on the opposite side, or off the ends.