I’m not a board designer. I’m an embedded programmer guy. I’ve seen the schematics of a quite a few boards, but I am unclear on several items.
When choosing bypass capacitors, does it matter if they are ceramic, tantalum, etc?
What about capacitors for the power supply/voltage regulator? Do these need to be a specific type (electrolytic, etc)?
How close is “close enough” to power connections for bypass caps?
What should be the minimum trace size for power traces? Is the 0.012 sufficient for a 3V3 source with no more than 500mA? It seems so based upon the trace width calculators I’ve used online (they say about 6mil).
Should the output capacitor for the power supply/regulator be placed near the output of the supply? I suspect this is the case.
What about the filter caps and series terminators on the USB? The app note from NXP says to route D+ and D- on the bottom of the board, but makes no mention of the placement of caps and resistors. Should these be near the connector, or near the part?
I’m considering the 1206 form factor for SMT caps and resistors. They look large enough to solder by hand. Anybody know if these are too small to hand solder?
I too come from a programming background and had to figure out these problems. The answers I will give mostly come from trial/error, working with development kits, and talking with hobbyist. I can’t back this up scientific theories.
Boring answer: follow what is given in the regulator’s datasheet. If it is polarized use tantalum, otherwise use ceramic.
I never had to use anything other than tantalum or ceramic cap so far. Tantalum are usually smaller than other electrolitic capacitors and unless you need something in the micro Farad range and above you always find what you need with Tantalum.
Close enough is “as close as possible while still being able to solder it”. I used to pack everything very thightly only to realise it was a pain to solder or modify. At less than 1cm you should be alright
Yes, near the output of the supply. Your ICs that will draw power from this supply will each have their own bypass capacitor as well.
I would guess they go closer to the chip but it doesn’t really mather since most of the noise will come from the cable and connectors.
The first SMD package I had to work with was 0603 (1608 in metric) which at first seems really small but not so hard to solder with tweezers and a good iron tip. I guess it depends on how much space you have to fit your components. Also, if you use ICs with packages such as TSSOP, your 1206 resistors will seem disproportionate compared to the pin size of the IC.
I hope that helps you, but I think I will also learn from the following posts!
Yes, to a point. Look and read up about capacitor ESR. Bypass caps generally should be low-ESR, so ceramic is preferred unless you need high values.
Linear voltage regulators may or may not specify what they need. If the value is small enough, ceramic. Mid-ranges go for tantalum, and large (22uf+ for me) go electrolytic. If its an AC circuit, such as after a bridge rectifier, you need to be more choosy. Some tantalums just can’t handle being a reservoir capacitor (too high of an ESR, plus a tendency to fail). Electrolytic are best here.
Can you get the capacitor closer without ripping up your entire board? If so, its too far away
The trace calculators will help you here. Remember, small long traces have resistance, which you may want to avoid. If you have the space, make them bigger.
Yes.
Keep the overall USB length on the board as short as reasonably possible. The part location doesn’t particularly matter if you follow the above rule
I regularly hand solder 0603, without any vision assistance devices or even paste and reflow. 1206 is huge . 0402 is a real pain without paste or a microscope. 0102 is dust. If you want something easy, 0805 is a good compromise. They don’t scatter all over when you sneeze. And always buy many spares.
My trick with two pad devices is to put a dab solder down on one pad of the PCB first, grab the component with tweezers, reheat the first pad while pushing the device flat onto the board. Do several devices in the area, then go around and solder the (now laying flat) second pad. Its somewhat harder to control exact solder amounts, but can be very quick. Holding the device and applying wire solder seems to require 3 hands for me, lest I end up with tombstoned parts or generally crooked stuff.
Buy small tweezers! and don’t be shocked when your good quality tweezers are $20. I’ve found good sales/clearances at Techni-Tool.
Just a note about the capacitors. This is especially important if you’re doing digital work, but also applied to analogue stuff.
You should have one small value (100nF is the usual, but 10nF can be Ok too) ceramic across the power rails to every chip on the board. More, if the chip has multiple rails. You should also have a minimum of one larger electrolytic (20 to 100uF) per three chips. More, if you’re using tantalums, which tend to have have lower ESR than aluminium foil caps.
The elctrolytics are there largely for their high ESR value, which damps out oscillations on the power rails which are caused by the fast switching of digital circuitry. If you leave them out, it’ll go bananas.
theatrus is right too, your ceramic decoupling caps should be as close as you can realistically get them to the chips. If they’re too far away you might as well leave them off, as the series inductance will destroy any effect they’d have and they could even ring, which would be a Bad Thing.
As for the component sizes, 0603 isn’t too bad to work with by hand. I mix in some 0805’s too, as I can get two traces to run under them in a pinch, which helps cut down on vias.
theatrus is right too, your ceramic decoupling caps should be as close as you can realistically get them to the chips. If they’re too far away you might as well leave them off, as the series inductance will destroy any effect they’d have and they could even ring, which would be a Bad Thing.
I often place them on the other side of the board from the IC. Then, you can get them as close as you want. not great for cheap manufacturability but for a 1 off it's fine.
I don’t know what it is either. But I am given a note when I try to post saying that my post is being sent to moderation because of the use of a “forbidden word.” And trying to track down the word, whatever it is, ends up requiring me to remove entire paragraphs.
I’m not in the bypass spam group yet, but I’ll try to post.
In the ARM group, I posted a link to a schematic. The link didn’t work well, so I did some research and I think I have a better method now. And rather than have everything over there, I’m reposting the contents here.
I replaced the RC circuit on the reset with a supervisory circuit.
I removed the R-packs and replaced them with smaller 0603 resistors. I liked the bussed R-packs for pullups/pulldowns, but the parts were just too large.
I’m especially interested in people taking a look at the power supply (LM1117 regulator based) and the RS232 interface.
I can hand solder 0603 parts faster than a through hole part (no need to turn the board over or clip off excess leads off parts). The easiest way I’ve found to hand solder them (usually, I use solder paste and hot air) is to melt a small blob of solder on one pad, take the part with tweezers and re-melt the solder and place the part, then solder the other terminal as normal. 1206 is really easy to hand solder.
I use 0603 because it means I can get decoupling caps closer to the IC. Especially with fine pitch high pin count ICs, it can be tough routing the traces out if there’s a huge 1206 decoupling capacitor on every power pin, and it forces you to move the capacitor further from the IC just to get the traces out (this is more of a problem with an IC with pins on all four sides when mounting to a home made board, where I can’t put vias under the chip). 0603 size parts let me get decoupling capacitors within 1 or 2mm of the power pin in question. (If I’m using something like a CPLD, if I’m not using all the pins on the IC, I will leave the pins adjacent to power pins unused so that there’s no traces to worry about close to the power pins, and I can get the decoupling capacitor really close to the power pin).
I normally use 0805 parts, as they are relatively easy to handle and I have plenty of them. I picked up a complete reel of 0805 100 nF capacitors on Ebay - they will see me out, and then some.
I recently tried Sparkfun’s hot plate method of soldering SMD devices and other than the ridiculous cost of solder paste, it seems to work really well. I don’t even use a solder mask. I have a small amount of solder paste in an old contact lens case and I use a toothpick to dab the paste onto the pads. 0805 and 0603 parts are very easy to do this way. Smaller than that and I have to go looking for a magnifying glass to make sure I’m hitting only the pads. The only problem with this method is you can’t really do double-sided SMD boards.
For the other design questions, it’s a little more complicated. Long traces have resistance and inductance that shorter traces don’t have. As a general rule, I try to keep any signals with high switching speeds as short as possble. Since USB D+ and D- are clocked at 48MHz (and the rest of my design is only running at 8MHz), I make D+ and D- as short as possible as a top priority. The placement of the the other components will dictate how long the remaining traces are, so all that’s needed is to work from the highest speed switching signal to the lowest.
Also as others have said, decoupling caps always need to be close to their respective IC’s. I usually hand route these first before giving the autorouter a shot at solving the routing problems.
One other thing. Beware of running two independently switching signals in parallel over a long distance. They will cross-talk onto one another and you’ll wind up with garbage on the other end of the transmission line.
Thanks for the link! I’ll keep that in mind for next time. It was my own laziness that led me to buy Kester no-clean paste - I didn’t search the forums first.
Thanks to everyone for their help! Now that I’m no longer on the “forbidden word” list, it is much easier to post.
I’ve cleaned up my schematic, and updated the layout. I’ve ordered the parts and the boards, and should have everything next week. For those that are interested, here’s both (in Eagle):
I crammed everything into a 2"x3" board. I have a BOM, that shows about $20 in parts total (single unit quantities). I ordered boards from Advanced Circuits ($33 each proto).
