3
\$\begingroup\$

In a 4 layer board it's advised to have power and ground plane as internal layer, but due to space crunch on my board I want to lay a few tracks on the internal layer.

Is it okay to do it ? If yes then is there any precaution to take while doing so ?

\$\endgroup\$
2
  • \$\begingroup\$ How much do you need to worry about the EMI? What's the purpose and nature of your device? \$\endgroup\$ – Nick Alexeev Jan 1 '17 at 1:11
  • \$\begingroup\$ @NickAlexeev The purpose of the device is RF communication(BLE) of some sensor readings. \$\endgroup\$ – U7786 Jan 2 '17 at 9:07
13
\$\begingroup\$

Tip. Keep ground as an inviolate layer, and use the 3 other layers for signals and power.

Treat power as a signal. While there are theoretical benefits to having a power plane, it is rarely worth it. The cost of dedicating a whole plane to power is too high, in terms of real estate. The time saving of 'not having to think' about power distribution is actually a problem, because it means that you tend not to think about power distribution!

A good layup is critical signals on the top (where you can keep an eye on them), ground as layer 2, then layers 3 and 4 as a strict Manhattan grid of power and less critical signals.

The point about using a Manhattan wiring grid is that you always have a consistent way to get from A to B, you never have a tricky rip-up and reroute of half the board, late in the layout process. Those are the frustrating times when some people yield to the temptation to 'just run a little track through the ground plane', then you do it again and the next thing you know, the ground has fallen apart like a lace curtain.

Route power like this. Put a bulk electrolytic capacitor at the power entry to the board. Put a 10nF at every package power pin. Now think. Where can you tolerate voltage drops? Where must you have isolation between groups of components conducted via the power rails? What is the power consumption of each block. Now route tracks sufficiently wide for the current, and use series resistors, inductors, ferrite beads, or LDO regulators to achieve the desired rail voltages and inter-block isolation.

You don't always need a ground plane of course, only for RF and very high speed logic. A good alternative is to use a Manhattan pair of layers to lay an XY grid of ground tracks, connected at every intersection. Then you have 2 clear layers and two half layers for the rest of your signals and power. If you have a few critical signal tracks, then you can add a local ground under just those few.

\$\endgroup\$
5
  • \$\begingroup\$ You mean a separate layer for signals & Power or can they be mixed as per requirement while keeping the ground plane separate? \$\endgroup\$ – U7786 Dec 31 '16 at 10:03
  • \$\begingroup\$ @user33944 added to answer \$\endgroup\$ – Neil_UK Dec 31 '16 at 12:18
  • \$\begingroup\$ Thanks @Neil_UK , the details were helpful, actually I'm developing a RF application and you have already mentioned a few specifics about the same. \$\endgroup\$ – U7786 Dec 31 '16 at 13:43
  • \$\begingroup\$ @Neil_UK -- see section 10.7.1 of Electromagnetic Compatibility Engineering. In short, digital currents return in the plane under the trace, whether it be a power plane or a ground plane. Your approach can work provided that you can get away with a single routing layer for high speed/RF signals...but, this denies you the ability to use PCB-embedded capacitance layers, which are a very good thing to have at high frequencies. \$\endgroup\$ – ThreePhaseEel Dec 31 '16 at 18:06
  • \$\begingroup\$ Also, I would recommend against going for inter-block isolation unless you are doing total isolation (i.e. all power and signals into and out of the block are isolated) \$\endgroup\$ – ThreePhaseEel Dec 31 '16 at 18:10
3
\$\begingroup\$

Sure, you can put traces on any layer, you do however lose some of the benefits of having planes.

Slots can become antennas, but this can be mitigated somewhat by stitching across them on other layers.

\$\endgroup\$
6
  • \$\begingroup\$ Thank you @Jasen . Can you please tell or guide me to a source to know the benefits of having planes and not having the same (Power & Ground) as ordinary traces. One I understand might be the interference that can be avoided by having a ground plane in between . \$\endgroup\$ – U7786 Dec 31 '16 at 8:33
  • \$\begingroup\$ Also what's the basic difference between a signal layer and plane? \$\endgroup\$ – U7786 Dec 31 '16 at 8:34
  • \$\begingroup\$ a plane is just a layer that's a pour \$\endgroup\$ – Jasen Dec 31 '16 at 8:36
  • \$\begingroup\$ Okay, So any trace having a lot of interconnects like GND would benefit from using a plane instead of layer . \$\endgroup\$ – U7786 Dec 31 '16 at 8:38
  • \$\begingroup\$ Think about how the current gets to and back from each power consumer on the board - think of the planes as big wide traces, and anything that cuts across the flow is potentially problematic. Also keep in mind that you want both the supply and return paths to be as similar as possible, otherwise you get a loop formed by the differences in path, and that can start to look like a loop antenna radiating interference. \$\endgroup\$ – Chris Stratton Dec 31 '16 at 8:53

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.