PCB Design Tips / General Science and Electronics / Forums

Forums

4hv.org :: Forums :: General Science and Electronics

« Previous topic | Next topic »

PCB Design Tips

Move Thread

LAN_403

nrhoades

Mon Sept 17 2007, 01:51AM

Registered Member #610 Joined: Wed Mar 28 2007, 09:44PM
Location: Middletown, RI
Posts: 110

I am compiling design tips for PCB Design. Anything to add?

Layout Design Tips:

Route by hand - Autorouters can connect all of your nets but they usually do a terrible job. Take the time to route every trace by hand. If you use shortcuts, you may pay for it.

Minimize length - Place components as close to each other as possible. Work to minimize trace length. Long traces have higher
impedances and will slow your signal propagation.

Think about wavelength - If the traces on your board are comparable to the wavelength of your signals then power transmission becomes an issue. Make your traces as short as possible.

Eliminate islands - Remove any little isolated pieces of copper ("islands") especially when using high frequencies. They can act like resonators and pick up noise.

Maximize width - Maximize the width of your traces to reduce impedance. Make all of your power connections nice and fat.

Bypass capacitors - Use bypass capacitors for each IC or localized function. A bypass capacitor is simply a lowpass capacitor connected between power and ground as close to the IC as possible. If the IC demands an inrush of current, then charge will be drawin from the bypass capacitor instead of the power rail capacitor. This prevents a temporary voltage droop in the entire system. Common values are 0.1uF and 0.01uF, though the datasheets of the parts will usually specify what to use. Ceramic capacitors (and the like) are best because of their low internal impedance.

Use ground plane if possible - A ground plane is a section of copper dedicated to providing the lowest impedance return path to ground as possible. I use double-sided copper boards and dedicate the backside to ground. The advantage to this is that ground can be referenced anywhere through a via.

No smaller then 0805 - You will hate life trying to surface-mount anything smaller then an 0805 package. A hot-air pencil makes the job much easier and is highly recommended over a soldering iron.

Leave copper for support - Leave an isolated copper pad for mechanical support under any screws, nuts, bolts, heat-sinks, or large objects to be mounted to the board. You may also want to think about leaving corner pads for mounting the entire PCB board.

Use sockets - Use sockets if you have any DIP packages. That way the chips are easy to replace if they die.

Prepare for mistakes - It is guaranteed that mistakes will be made the first time around. This is the prototyping process. Design your board to work, not to look pretty.

...

Mon Sept 17 2007, 02:26AM

Registered Member #56 Joined: Thu Feb 09 2006, 05:02AM
Location: Southern Califorina, USA
Posts: 2445

Also, be extremely careful when laying out the power rails, especially when using a mixed signal (ie, high power/high frequency and analog). If something needs clean power run a trace strait from the power coming in, and use some filtering.

Make sure that any connectors on the board have plenty of copper on the bottom of the board that you can solder them to.

If there is high voltages make sure to leave plenty of room (especially when you are going to have flux and crap on the board).

For parts that dissipate a lot of power (microprocessors, high brightness LEDs, ucc's, diode, etc, etc), make sure that the pins are on a nice big area of copper, as the pins are the most effective way to heatsink devices. Often times the ground pins will be a part of the copper plate the die is mounted on.

thedatastream

Mon Sept 17 2007, 07:02AM

Registered Member #505 Joined: Sun Nov 19 2006, 06:42PM
Location: Yorkshire!
Posts: 329

It's more than possible to hand solder 0402 capacitors - any smaller and it can start to get really tricky. You don't even need a hot air pencil, a normal Weller soldering iron with a fine point will do.

I would agree with your comments about Autorouters - certainly none of the ECAD guys here use them.

I would add that the return path for currents is just as important as the transmission path. There was a thread on this subject maybe a few months ago that NeilThomas contributed some good points in.

Also, avoid any breaks in the ground plane underneath high speed signals from transmitter to receiver. The ground plane forms part of the transmission line and any breaks will screw up the impedance and give you reflections. Really comes into play with frequencies over 50MHz

Dr. Slack

Mon Sept 17 2007, 07:11AM

Registered Member #72 Joined: Thu Feb 09 2006, 08:29AM
Location: UK St. Albans
Posts: 1659

Nice try, I appreciate the effort, but the field is complicated and I'm not sure a "few tips" will help much. But my tuppence worth

1) Appreciate whether you are laying out a simple low frequency board (resistors, switches, LEDS, static loads), a head-banging RF board, or a board that appears only to use lowish frequencies but bites you in the bum because of fast edge (microcontrollers, IGBTs, anything with logic that stores state (D latches, 555s)). Wavelength/10 is a better length limit than wavelength. By the way, logic edges can be very fast, with ACMOS having frequency components to 1GHz.

2) make sure you can mount it OK, screw holes etc.

3) Build a good dedicated place to clip your scope GND or your meter 0v for debugging at layout time, you might want good probe points for your power rails as well. I've damaged many a board as the grounded croc-clip snakes all over the board having jumped off its precarious IC pin8.

4) If a simple low frequency board, then use autorouters if you like, no point buying a dog and then barking yourself.

5) wide power traces, adequate heatsink lands, all that good stuff.

6) For any other type of board, use a ground plane, whether you think you will need it or not, period. You can often get away without, but if you have to read tips to understand how to lay out a circuit board, then you probably won't appreciate which occasions are which. Ground plane with holes in is usually OK (or a fully connected XY grid of ground traces), ground plane with slots in usually isn't (a partially connected grid of ground traces), and a ground trace that snakes around like a signal trace trying to be routed is usually a disaster. Treat every signal as half a transmission line, the other half is the corresponding ground path, then you can start thinking nH per mm or pF per mm for the parasitics, and you can start visualising how the return currents will couple unexpectedly into other bits of the circuit, and can flow round holes, but not across slots.

ConKbot of Doom

Fri Sept 21 2007, 03:46AM

Registered Member #509 Joined: Sat Feb 10 2007, 07:02AM
Location:
Posts: 329

Ive attended a seminar about grounding/ground planes on circuit boards, and it was similar to most of the things being stated here... Just a few things I'd like to comment on...

At high frequencies, trace inductance, not resistance is the real problem, and the path of lowest inductance for a return current, is directly under the signal trace, even if you have a solid ground plane. For high-frequency work, a ground plane is the most important thing.

Other stuff like traces between leads... avoid them if you can, if not you'll have to be careful when you do go to etch the board and solder.

I personally wouldnt want to go smaller then 603 with SMD components, though I haven't done any with a real fine point, only a 3mm or so chisel tip. Too small and the surface tenson of the solder gets to be a pain, and reflow looks more and more like it would be worth it.

Dr. Who

Tue Sept 25 2007, 10:23PM

Registered Member #326 Joined: Sat Mar 18 2006, 01:12PM
Location: Glasgow, Scotland
Posts: 66

As well as using a 0.1u capacitor on each power/ground pin pair, use 1 or 2 10u capacitors on the board for LF decoupling.

For fast digital devices such as FPGAs, PCI, ECL, USB, etc, read the databook carefully, and follow the manufactuer's recommendations on layout, decoupling, track length, etc. rigorously.

Built test points onto the board. For digital circuits, add test points with pinouts and connector types that match those of your logic analyser.

Leave enough space around chips to make room for IC test clips, and to facilitate removal/replacement.

Dr. Slack

Fri Sept 28 2007, 06:52AM

Registered Member #72 Joined: Thu Feb 09 2006, 08:29AM
Location: UK St. Albans
Posts: 1659

I am compiling design tips for PCB Design. Anything to add?

I notice there's a "printed circuit board" page on the HvWiki, which doesn't show up if you search "PCB". Perhaps when you've collected your tips, you'd present them there?

Bjørn

Fri Sept 28 2007, 08:27AM

Registered Member #27 Joined: Fri Feb 03 2006, 02:20AM
Location: Hyperborea
Posts: 2058

"PCB" is too short to be indexed by the search engine. If you use "Go" instead it will find the page since there is a redirect from "PCB" to "Printed circuit board".

The difference between "Seach" and "Go" is that "Go" will go to an article automatically if the title is an exact match, if not it will do the same as "Search".

Design tips like these are exactly the sort of information that the wiki is meant for. Just keep adding to this thread, sooner or later someone will get inspired and and put it in the wiki.

Moderator(s): Chris Russell, Noelle, Alex, Tesladownunder, Dave Marshall, Dave Billington, Bjørn, Steve Conner, Wolfram, Kizmo, Mads Barnkob