1
\$\begingroup\$

I have made a few PCB's over the past few months as I have started to learn about design. All of the circuit boards have been Arduino based, so nothing to powerful. I design them up in Eagle and I know this is bad, but I have just used the Auto-router for everything, including the ground and power lines.

My boards have worked fine with this (maybe except for one thing), but I know this is very bad practice. I have been doing some research on ground planes and from what I have read I have not found a reason not to use them on your 2 layer PCB. Should I always add a ground plane to the bottom of my circuit board? When I look at other example boards in Eagle like the Arudino Mega, I notice it does not have a ground plane and I would like to know why someone would not use one. Also, is it okay to run signal wires through your ground plane?

One other question I have is when is it okay to use the Auto-router. From what I found online it should be fine to auto-route signal wires, and that I should manually route ground and power traces. And that these traces should be much thicker than the signal traces.

My last question is about ground loops. I think I have paranoid myself about ground loops and think that they are always gonna happen. As long as I have everything attached to ground on my board (and I only have one common ground), then there should be no issue in having a ground loop correct?

Thank you for the help, I am still very much a beginner with all of this.

\$\endgroup\$
1
\$\begingroup\$

This is a hard question to answer fully.

Things that argue in favor of having a ground plane:

  • high speed digital busses
  • SDIO
  • SDRAM
  • DDR
  • USB
  • Ethernet
  • RF signals

Things that don't really need a ground plane

  • Analog Audio (but still needs attention to noise issues)
  • SPI bus (marginal...)
  • I2C bus
  • I2S (digital audio)
  • Low-speed ADC's (1MHz or less)

Personally, I always try to route my signals on a single layer and use the bottom as a ground plane for simple utility boards. Careful placement is critical to achieve this. If needed I will run a few traces on the ground plane, but I try to keep them as short as possible.

For production 2-layer boards that don't need a ground plane, I still try to fill all unused space with copper on top and bottom, and use GND vias to interconnect in lots of places. I try to avoid having large sections of copper on top that are not bonded to the bottom, and vice verse. I will move stuff around a bit to make sure I get good interconnection and continuity of GND.

For 4 layer boards, I always use a ground plane and try very hard to have zero tolerance for traces or any nets other than ground on that plane. Typically there is also a generic "power" plane. On that one I will allow power fills or power traces usually.

A lot of this is to make sure the board can pass radiated emissions testing. If you don't need to do that, you only have to worry that the board works. You can be a lot less stringent.

In the end, any design that meets all its requirements is good enough. It is not necessarily a problem to just use the autorouter, but be careful if your board has any of the things in my list that generally require a ground plane. Or maybe route those things first, then let the autorouter take over.

\$\endgroup\$
1
\$\begingroup\$

A ground plane should be used to provide a nice, solid, low impedance path to ground. Some people, and almost all hobbyists (generalising), use it as a lazy way to hook up the ground connection as obviously this is used in a lot of places. In an ideal world, this means no other traces through it, and direct connection to the relevant pins. You may (will) have to break these rules in a real 2-layer board, but you can get much closer on a 4 layer board.

In something like an Arduino clone, you can happily use a ground plane and it is likely to work fine. Likewise, you can split the plane with signals, especially if you have no sensitive analog components, on projects like this. It's good practice not to, of course, but don't get too hung up at this stage of learning.

Which leads to autorouter. As a (weakly held) general rule, don't use it! While it may find paths for you, it is likely that thinking more about your component placements and general layout will be far more beneficial as a beginner. The real power of the autorouter is actually for advanced users who have to route out 1000s of pins from tiny ICs. Typically, you lay out as much you can (be bothered) by hand - this will usually make you place components logically, rather than just spattered all over the board. For a design the size you are describing, don't use it. Personally, I route sensitive signals first (local decoupling, small signal analog, fast digital etc), then power/ground, then hook the remaining airwires.

On a single board, you will not have a ground loop. Unless for some reason you have two different power supplies feeding the board. Ground loops tend to be more of a problem in small signal analog, less so in digital designs and it's easier to isolate with digital protocols.

\$\endgroup\$
  • \$\begingroup\$ So in 2 layer PCBs I should route gnd conns rathet than connect gnd to gnd plane? But 4 lyr pcbs use one layer as gnd plane? \$\endgroup\$ – SilvioCro Feb 9 at 22:05
  • 2
    \$\begingroup\$ @SilvioCro No, don't take that as a rule. A ground plane is fine on a 2-layer board, just be aware of what you are doing and the limitations. You will be able to get closer to the ideal on a 4 layer board. The main thing is to think about where the current flows, and how your signals interact. \$\endgroup\$ – awjlogan Feb 9 at 22:08
1
\$\begingroup\$

Decades ago I worked near a guy who cranked out the assembly-level device-drivers for a conveyor-belt distribution system. He also designed moderate-performance embedded-systems for where a PC_AT was overkill; in some cases, large amounts of Input/output pins were needed, and he happily cranked out custom I/O expanders, using a AutoRouter.

I once happened to examine the 2-layerPCB I/O Expander, which used TTL logic, and noticed the long-thin 1/16" GROUND trace that Daisy-Chained around the several dozen TTL ICs. I asked him, and he replied "Has never been a problem."

However, about 4 years later (he having died in a plane crash) and I had moved from systems-and-PCBs to systems-and-silicon. My boss asked "xxxxx called from YYYY company. They wonder if we have any ideas as to why these embedded systems will randomly go into MCU_reset?"

I, without a pause, simply stated "The grounds he (the deceased) used are not planes, but long thin Daisy_Chains. Tell xxxxx to convert those PCBs to Ground_plane PCBs."

WHy was this ----- Daisy_Chain grounds a problem?

Here is the math. Assume TTL, assume noise immunity of at most 1 volt.

If we find inductive spikes or kicks in the Ground that reach even 1/2 volt, we have found the problem.

What will we find?

Assume the Ground Trace runs 3 sweeps across the PCB, of 8" each, 24" total, or 4/5 meter and thus approximately 4/5 of microHenry, or 800 nanoHenries.

Assume the TTL logic power demands exhibit 10mA peaks that rise in 10 nanoSeconds.

Is this a problem?

V = L * dT/dT

V = 800nH * 10mA/10nS = 800 nH * 1mA/1nS = 800 * 0.001 nH/nS = 0.8 volts

Thus with just ONE (ONE) TTL gate causing Ground currents, the entire PCB is at risk.

TWO CHOICES:

(1) Use a Ground GRID (My first large TTL project, with 75 SSI TTL, never had sproblems; it used X and Y wires running past each of the ICs; thus each IC had at least two GND returns coming from wherever the TTL signal ended up. The GRID was made of 5 banks of 15 ICs; thus from left to right there were 5 parallel wires (#22 bus wire), of length about 15 inches or 30 inches round-trip in air or about 3 nanoSeconds electrical-length for a Standard TTL speed of 10 or 15 nanosecond gate prop-delay (tho the IDD surges are what I am discussing here)

(2) use a Ground Plane; the premier prototyping technology at that time was WIREWRAP from Augat or Robinson_NUget. I could not afford those, so a ground-grid was my (successful) solution. By the way, each TTL IC had 0.1uF soldered between pin 7 and 14 (for those 14-pin DIPs), and all the VDD surges were well provided right at the IC.

\$\endgroup\$

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.