Useful add-ons for PCB prototypes?

Go To Last Post
13 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

This question is prompted by some good ideas I've seen here, and a few I've had on my own.  I thought it would be useful to collect them in one place.

 

So the question is, what types of add-ons are useful to include in a new PCB design, which can be either populated or left unpopulated?

 

I'll prime the pump.

 

1) A few GND pads.  I make them the size to take a 0.025" square pin.  When I was stupid I'd lay out boards with no place to attach a scope ground probe!

 

2) A few LEDs for debugging.  One nice arrangement is a single LED hex digit, driven by 4 output pins, but even individual LEDs are very useful.  And a place to clip on a scope probe, either on the LED lead, or a separate pin as in #1.

 

3) Pads on unused port pins. 0.025" compatible is good.

 

4) Power pads in parallel with the power connector.  Sometimes I don't want to add a connector and mating connector, I just want to solder a couple of wires to the board.

 

I'll stop here - keep 'em coming!

 

Last Edited: Wed. Dec 10, 2014 - 02:23 AM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I'm certainly not an expert in PCB layout / design, but a couple common suggestions to the first timer's posting their layout are:

 

Add mounting holes.  Use them to eventually put the PCB in an enclosure, or while debugging, put a bolt through the holes to hold it up off the table.

 

Add a name and version number. 

If a PCB goes through a few revisions it makes it much easier to identify which version one has before them.

Additionally, if you pull the board out of a stack of old PCBs to modify for some quick test, it is helpful to be able to identify the board against a bunch of old board schematics. 

 

It goes without saying that chips and headers should have some sort of Pin #1 marker.

 

JC

 

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

If the chip use has a USART bring that out to a small header even if not used.

John Samperi

Ampertronics Pty. Ltd.

www.ampertronics.com.au

* Electronic Design * Custom Products * Contract Assembly

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Great ideas above.

 

- 2 push buttons

- 2 LEDs

- Pin header

- testpoints for all relevant signals tracks running under chips.

- Tent all vias but those I'll use as testpoints.

- GND pin at some corner just to hook up instruments

- 'firewall' jumpers between major board blocks, so I can debug problems without cutting tracks

- thicker tracks around pads likely to break apart, like thru-hole connectors, heavy parts, etc.  Altium s/w calls them "teardrops"

- Stretch pads of SOIC footprints so I can use any narrow/wide/jedec types available

- Always mark the pin 1 on the JTAG and any other header.

 

while(!solution) {patience--;}

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0
  • jumper on the power rail in various places so as to be able to measure the current drawn in major sections
  • jumper to isolate drive signal to fets or transistors so that drive can be applied manually or via external signals
  • grounding resistors on base or gate (N-Fet) so that those devices do not switch on randomly

 

Ross McKenzie ValuSoft Melbourne Australia

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

If the chip has JTAG (or equivalent), use it!!

Top Tips:

  1. How to properly post source code - see: https://www.avrfreaks.net/comment... - also how to properly include images/pictures
  2. "Garbage" characters on a serial terminal are (almost?) invariably due to wrong baud rate - see: https://learn.sparkfun.com/tutorials/serial-communication
  3. Wrong baud rate is usually due to not running at the speed you thought; check by blinking a LED to see if you get the speed you expected
  4. Difference between a crystal, and a crystal oscillatorhttps://www.avrfreaks.net/comment...
  5. When your question is resolved, mark the solution: https://www.avrfreaks.net/comment...
  6. Beginner's "Getting Started" tips: https://www.avrfreaks.net/comment...
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Pads for an inductor on AVcc.

"Experience is what enables you to recognise a mistake the second time you make it."

"Good judgement comes from experience.  Experience comes from bad judgement."

"Wisdom is always wont to arrive late, and to be a little approximate on first possession."

"When you hear hoofbeats, think horses, not unicorns."

"Fast.  Cheap.  Good.  Pick two."

"We see a lot of arses on handlebars around here." - [J Ekdahl]

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 1

Add a name and version number. 

If you have room, but a big white rectangle of silkscreen ink in one of the corners, so you can mark it up with a sharpie...

 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

1. Where both analog & digital circuitry exists on the same PCB, place ferrites or small inductors between digital & analog circuitry that share Vcc, Vee and analog & digital common ground returns, to reduce digital noise levels on the analog side of things.

 

2. Where both analog & digital circuitry exists on the same PCB and where elevated analog & digital return currents are present, tie all common analog & digital ground returns carrying elevated current flow to a single common entry point on the PCB, minimizing cross coupling of ground noise into the analog side of things.  This would include running separate ground returns from on-board power supplies - run a separate "isolated" ground return from each voltage regulation system to a common point and the place of power entry.

 

3. The supply lines between the raw DC power source and the PCB should be ran with the largest gage and the shortest length as practical.

 

4. Where both analog & digital circuitry exists on the same PCB, it is critically important that each digital IC have an appropriate "Despiking" capacitor across the Vcc & GND and Vee & GND pin pair and placed as close as possible to the IC, itself.

 

5. When analog & digital circuitry both share the same PCB, it is highly suggested that, where possible, the analog circuitry and the digital circuitry be keep in separate sections of the PCB.  This facilitates reduced interference to analog circuitry due to radiated digital noise.  Isolation of the analog & digital circuitry also helps with PCB power buss isolation and management, as well.

 

6. Where analog or digital signals breach the boundaries of the others sphere of influence, I.E. an analog signal breaching the digital sections and sphere of influence, that analog signal should be guarded on both side along it's path of travel, helping guard against magnetic radiation from the digital circuitry.  The same goes for a digital signal entering the analog section.

 

7.  Where greater immunity of external signal radiation is critical, micro-strip (also known as strip-line) methods should be used to further manage analog-side noise immunity and increased digital-side waveform quality, better transmission line impedance control and reduction of radiated emissions.

 

8. When looking at digital signals capable of sub-nano second rise & fall times, use a scope probe whose GND lead is as short as possible.  This helps reduce inductive ringing, post transition, providing a more accurate representation of the digital signals you are attempting to observe.  It also aids in timing measurement, as well.

 

In my experience over more than four decades of bench work, lack of attention to good PCB power buss structure has been a very common design oversight.  It seems engineers often take great pride and joy in the details of the exotic, and the fun stuff.  I've often heard engineers say "Oh, I can get a power supply anywhere!", never realizing that good on-board PCB power buss structure concepts are even more important then the exotic or the fun stuff.  In fact, I've seen a few really great designs fail because of poor PCB power buss structuring and the PCBs had to be totally re-laid out, from scratch.

 

Not only will these guidelines help in establishing accurate, stable analog ADC readings, these practices will help ensure that all on-board analog circuitry exhibits the most noise free operation possible. 

You can avoid reality, for a while.  But you can't avoid the consequences of reality! - C.W. Livingston

Last Edited: Wed. Dec 10, 2014 - 07:13 PM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

analog signal should be guarded

Is it OK to use a single ground plane for guarding both analog and digital signals on a PCB?   For example, consider the Arduino where the analog pins are connected as shown in the attached picture (where the ground plane is THE shared ground plane.)   Would it be better to have a separate ground plane just for guarding the analog traces (presumably isolated with more ferrite?)?

 

Attachment(s): 

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

For ADCs, such as what is within the 8-bit family of AVRs, the layout isn't terribly critical, unless you are measuring say, micro-volt levels and then amplifying those levels to be compatible with the AVR ADC operating levels.

 

Where it really gets stinky is when you are using external ADCs that are say, a 12, 14 or 16 bits.  Where the minimum design requirements of the AVR ADC would be acceptable for the AVR ADC, using a 12, 14 or 16 bit ADC under the same PCB layout philosophy would be a waste of the higher bit ADCs.  The reason is  because the least significant 2, 4 or 6 bit of the 12, 14 or 16 bit ADCs would probably get lost in the noise.

 

The fact is, using a 12 bit ADC, you could probably get away with just designing up a double sided PCB, with careful layout.  But with 14 and 16 bit ADCs, a multi layer PCB would be a must, where the ADC analog input signals and other analog signals could be better protected and routed.  This is also where the analog and digital GND planes would most definitely require some sort impedance between the analog and digital GNDs, such as a Ferrite or small inductor.

 

The key here is impedance and not just simply resistance.  Impedance, while related to resistance, differs from resistance in that, a typical resistor passes both DC and AC current nearly equally well.  But when using a Ferrite or inductor,  these passive components readably pass DC current undisturbed but they react to AC current by way of inductive reactance: XL = 2*Pi*F*L. where, 2*pi = 6.28, F is the frequency of the noise and L in the inductance of the ferrite or inductor. 

 

To determine the actual impedance (Z), the equation is: Z = sqr(R^2 + L^2).  Where if viewed as a right triangle, the adjacent side (or base) = R, the opposite side = L and the hypotenuse = Z.  Or, as those goofy mathematicians call it, Pythagorean Theorem.

 

http://www.electronics-tutorials.ws/inductor/ac-inductors.html

http://en.wikipedia.org/wiki/Pythagorean_theorem

 

Ideally, at DC levels, the impedance will be very near zero Ohms.  But at those pesky frequencies that might cause problems in a mixed analog/digital power bus structure, you want the impedance between GND systems to be as high as possible, but still practical.

 

The Screen shot that you have attached would be an improvement to running just a free trace and it will help to isolate channel to channel coupling, as well as providing some shielding from nearby radiated energy.

You can avoid reality, for a while.  But you can't avoid the consequences of reality! - C.W. Livingston

Last Edited: Thu. Dec 11, 2014 - 10:03 AM
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

G0NZ4L0 wrote:

- Stretch pads of SOIC footprints so I can use any narrow/wide/jedec types available

This is a generally useful idea if you'll be hand-soldering the prototypes too.  I find a little extra pad length makes it much easier to solder small SMD packages, as the solder from the tip/solder wire has a place to gain a foothold in order to flow onto and under the device pin.  Without that foothold it becomes too easy to just solder the top of the pin, without the solder flowing to the pad.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

@kk6gm: True. Also happened quite often over here with some old DIY boards.

while(!solution) {patience--;}