6 ms·

PCB Design Tutorial for Startups

102 points by poindontcare 10y ago

honkhonkpants 10y ago
A long article that says almost nothing. Instead of choosing trace widths and layer count and component sizes at random, take a week to read and understand the very useful book "High Speed Digital Design" by Howard Johnson. Despite the name it concerns itself more with the analog domain than with the digital. Very useful information about the behavior of traces and holes in boards.
- pmorici 10y ago
  I didn't want to be critical of it but as someone who went through the process of designing and manufacturing my own hardware product to sell a couple years ago that was my thought as well. Really long and very little insight into the real difficult parts.
  - mng2 10y ago
    Yes, it seems much more like a high-level overview than an in-depth tutorial.
  - jwr 10y ago
    As someone who has actually designed manufacturable boards I'd say the same. In addition the article has some strange recommendations: * don't use QFN — I see no reason to, on the contrary, these are great packages (see my other post in this thread) * 0603 minimum size for passives — huh? I see no reason not to go down to 0402, which is both easy to manufacture (assembly costs are the same, component costs are usually lower), and easy to prototype (just get a large desk magnifying glass and a good pair of tweezers and you're good to go).
- tomkinstinch 10y ago
  High Speed Digital Design is a great book (a "handbook of black magic," as its subtitle professes), and it is a nice complement to Horowitz and Hill's The Art of Electronics. You're exactly right that the former addresses way more analog details than the title suggests, and at high frequencies the analog stuff really matters. A passive component is never simply a capacitor, resistor, or inductor. We just call it one based on the dominant characteristic. At particular frequencies the characteristics can change so much that designs have to take the difference into account. Application notes and manufacturer references also contain a wealth of information. TI's Op Amps for Everyone (a great reference in general) has a chapter (17) devoted to PCB design: http://web.mit.edu/6.101/www/reference/op_amps_everyone.pdf http://web.mit.edu/6.101/www/reference/op_amps_everyone.pdf Beyond comprehensive references, you can pick up things from articles as you go; I learned the trick of using two back-to-back Schottky diodes to reduce the ground plane potential difference to <0.3V from a PDF like this one: http://www.ti.com/lit/an/slyt499/slyt499.pdf http://www.ti.com/lit/an/slyt499/slyt499.pdf Trade magazines with articles are another great resource, like Circuit Cellar or EDN.
- bsder 10y ago
  Johnson's book is good, but it is WAY overkill for the vast majority of PCB design that you can do as a hobbyist. I can sum up what you need to know for high speed design in a nutshell: 1) True high-speed design has a sample PCB layout in the datasheet or application note. Follow it RELIGIOUSLY. 2) If you don't have any specific notes about layout, put a single 50 Ohm resistor in series on any communication link clock line (aka JTAG-TCK, SPI-SCK, etc.) at the source. Too many chips these days are capable of launching and responding to a clock edge that has GHz components on a link that's supposed to be KHz. That 50 Ohm series resistor knocks the edge rates down to where they should be.
bsder 10y ago
A couple things that I wish people had pointed out before I got started with PCB's: 1) You will spend your life reading datasheets. 2) Datasheets lie. 3) You will spend way more time in component selection than schematic design or board layout. 4) You will spend way more time creating component footprints than in schematic design or board layout. 5) Lay out the board by hand. You will waste more time fighting an autorouter than if you just laid it out. 6) A 6 layer board is not that much more expensive than a 4 layer board and is VASTLY easier to lay out. 2 layer boards should be avoided unless you you are a masochist or every fraction of a penny really counts. Some of the given advice is a bit off. 1) He doesn't put enough emphasis behind avoiding BGA. BGA should be avoided like the plague. Period. It will only cause excruciating pain. 2) Small QFN isn't that hard to deal with ... if you tweak the PCB footprints a touch (make sure you have .5 mm of bare copper outside the package outline and you can treat them like QFP). 3) 0603 is actually pretty small. Most people should stick with 1206/1210.
- asimuvPR 10y ago
  Mind sharing more about BGA?
  - bsder 10y ago
    You mean, other than for me to threaten to stick a red hot poker in your eye if you use it? :) BGA isn't "impossible" for a hobbyist. But it's a huge amount of work for very little gain. All advice here also applies to what people refer to as CSP (chip scale package) as well. 1) BGA packages generally require better than normal PCB rules in order to actually "fan out" the signals to routing. BGA packages can put a lot of signals in a small area (that's why people like them), and you wind up needing very small pitch traces and vias to get everything out. You may even need an 8-layer board to pull it off 2) You can't really inspect BGA without X ray equipment. I don't know of any hobbyist X-ray machines yet (that actually might be a good project...) 3) BGA is prone to strange failures if you don't get ALL the balls down properly. You can get things like unpowered chip sectors because a Vdd ball is a little flaky (chip manufacturers don't always spend money reinforcing the on-chip power grid if they think you are using balls). 4) If you have a "small" (less than 40 pin) BGA, there is almost always a QFN option that is easier to work with and is almost the same size. 5) Thermal management of a BGA can be tricky. There is normally better heat flow out the top of a chip than down into a board, but BGA's normally want to push heat into the board. That having been said IF YOU MUST use a BGA: 1) Use a contract manufacturer Really. This is the best advice. I got some very tiny CSP chip boards done for like $50 per board for 20 boards. Even if your time is only worth $20/hour, the crossover point is 50 hours of work. You'll spend lots more than that if you're playing with BGA. 2) If you have a small number of balls, see if you can adjust the footprint such that you can hand solder things by having copper stick outside the package outline. I can't give you any general advice as this is specific to every chip. However, I have successfully routed things like power regulators which only have a small number of balls this way. I have also routed some bigger things like FPGA's this way (you can reorganize the output pins) where I simply didn't even try to use any pins not on the outermost edges. However, you are at the mercy of the manufacturer as to how many power balls you need hooked up properly. 3) Use a reflow oven. There are lots of reflow oven things on the market for <$500. If you get things placed right, a reflow oven gives you decent results. 4) Don't try to hand rework. Accept that you're going to throw the board out if there is a short. Yes, I'm sure lots of people have done things and been successful with BGA. However, if you do enough, you will find you are at the mercy of luck rather than consistency with BGA unless you let folks who have reflow and X-ray machines do the work.
jwr 10y ago
Here's something I don't get: why discourage people from using QFN packages? QFNs are only a problem if you are hand-soldering your boards with a traditional soldering iron. Which is nuts. These days everyone should have a soldering station with both traditional iron and hot air — and soldering QFNs using hot air is straightforward and easy. Besides, the article is about manufacturing, so you aren't likely to solder those QFNs yourself. So why discourage them? I think QFN and DFN packages are fantastic. They save lots of board space (and believe me, board space matters a lot in all designs, more than you think!), have good thermal properties, lack of leads makes for better low-inductance connections, less material means lower price. And most still have pitch of 0.5mm or more, so you can use the same design rules and same PCB pricing. Everything is great about them. BGAs are a different matter, but not for the reason most people think: they are problematic not because they are difficult to solder, but because you need much tighter PCB parameters to be able to route all the signals. In particular, via size is the biggest problem. You need really small vias that can be placed between four BGA balls. I dislike the hate being poured onto QFNs. I think it is a relict of the past: back when hot air was expensive and "strange" and people tried to solder everything by hand using a soldering iron, QFNs were the enemy. But these days they should not be. The unfortunate effect of hobbyists hating QFNs is that some manufacturers (Freescale/NXP, notably) later class certain chips as "hobbyist" and don't provide QFN packaging at all. And believe me, if you're designing a wearable device, the difference in size between a QFN-64 and an LQFP-64 is monstrous. Providing no real advantages, because both have 0.5mm pin pitch. So, while I would agree with the author that BGA packages are best avoided, I would encourage everyone to actually go ahead and use QFN/DFN packages. They are better in every respect.
turnip1979 10y ago
I'm in the Bay area and a hardware hobbyist (software is my full time gig). I see tons of meetups for SW but almost nothing for electronics hardware. Any recommendations?
zw123456 10y ago
Nice overview article. I have been doing PCB's for about 3 decades and here are just a couple of little tricks I have learned over the years, some are too long to go into here, but just a couple quickies maybe will help someone out: 1) Often the chip manufacture provides BSDL files which often times contain the foot print info and a lot of CAD tools have macros that will read them in and create your foot print for you. 2) There are often foot print libraries already out there you can download or are provided by the CAD software. But in either case, don't trust them, there are often errors, get your parts first, do the PCB layout, print it out on a good printer (usually the CAD SW will print it to scale and test fit everything. 3) There is a big difference between doing prototype boards and production boards. For prototype boards, make them big because you will have mistakes and will probably have to black wire (cut a trace and fix) it. I often use 2 layer or 4 layer for prototypes because it is easier to do fixes. If you CAD SW does auto layout then it is not that big of a deal as long as the board is large enough for it to route everything for you. For Production PCB's it is a different story and a lot more work to do right and I recommend farming it out if you can afford to. 4) I agree that part selection is critical but also, if you have simulation software either a separate program or in your CAD system, doing simulations can save you a lot of time. If you don't have simulation SW check into it, there are some decent free ones to learn on but to get serious you have to pay a lot. 5) For complex designs, I do separate prototype boards, one with the FPGA on it, another with the MCU and another one with the analog on it and so or, sort of a unit test approach (sort of like dev-ing SW) that way you can swap out sections that aren't working for you without throwing away a board full of parts, it is more effort but if you plan it out it can save you time and money. 6) I agree with the BGA comments, don't use those types of components unless you have a reflow oven and know how to use it, it is easier to debug QFN and QFP type packages since all the leads are exposed for inspection. You can often get parts in either package type and when you go to production you can always swap out to the smaller package later. If you have to use those for prototyping check if the manufacturer has a prototype board for it already it can be easier to just use an off the shelf one. A lot of people say the first board is a throw away, but that can be expensive for a production one so I have learned these tricks for prototyping so when you get to production you can avoid that bad first board.
- mschuster91 10y ago
arcticbull 10y ago
Also, ChipQuick is great. It's super-low melting point solder you can use to easily rework SMD components. This thing has saved my ass too many times to count as a hobbyist :) Was able to get away without a reflow station for the small stuff I've been working on. http://www.chipquik.com/store/index.php?cPath=200 http://www.chipquik.com/store/index.php?cPath=200

102 points by poindontcare 10y ago

A long article that says almost nothing. Instead of choosing trace widths and layer count and component sizes at random, take a week to read and understand the very useful book "High Speed Digital Design" by Howard Johnson. Despite the name it concerns itself more with the analog domain than with the digital. Very useful information about the behavior of traces and holes in boards.

pmorici 10y ago
I didn't want to be critical of it but as someone who went through the process of designing and manufacturing my own hardware product to sell a couple years ago that was my thought as well. Really long and very little insight into the real difficult parts.
- mng2 10y ago
  Yes, it seems much more like a high-level overview than an in-depth tutorial.
- jwr 10y ago
  As someone who has actually designed manufacturable boards I'd say the same. In addition the article has some strange recommendations: * don't use QFN — I see no reason to, on the contrary, these are great packages (see my other post in this thread) * 0603 minimum size for passives — huh? I see no reason not to go down to 0402, which is both easy to manufacture (assembly costs are the same, component costs are usually lower), and easy to prototype (just get a large desk magnifying glass and a good pair of tweezers and you're good to go).
tomkinstinch 10y ago
High Speed Digital Design is a great book (a "handbook of black magic," as its subtitle professes), and it is a nice complement to Horowitz and Hill's The Art of Electronics. You're exactly right that the former addresses way more analog details than the title suggests, and at high frequencies the analog stuff really matters. A passive component is never simply a capacitor, resistor, or inductor. We just call it one based on the dominant characteristic. At particular frequencies the characteristics can change so much that designs have to take the difference into account. Application notes and manufacturer references also contain a wealth of information. TI's Op Amps for Everyone (a great reference in general) has a chapter (17) devoted to PCB design: http://web.mit.edu/6.101/www/reference/op_amps_everyone.pdf http://web.mit.edu/6.101/www/reference/op_amps_everyone.pdf Beyond comprehensive references, you can pick up things from articles as you go; I learned the trick of using two back-to-back Schottky diodes to reduce the ground plane potential difference to <0.3V from a PDF like this one: http://www.ti.com/lit/an/slyt499/slyt499.pdf http://www.ti.com/lit/an/slyt499/slyt499.pdf Trade magazines with articles are another great resource, like Circuit Cellar or EDN.
bsder 10y ago
Johnson's book is good, but it is WAY overkill for the vast majority of PCB design that you can do as a hobbyist. I can sum up what you need to know for high speed design in a nutshell: 1) True high-speed design has a sample PCB layout in the datasheet or application note. Follow it RELIGIOUSLY. 2) If you don't have any specific notes about layout, put a single 50 Ohm resistor in series on any communication link clock line (aka JTAG-TCK, SPI-SCK, etc.) at the source. Too many chips these days are capable of launching and responding to a clock edge that has GHz components on a link that's supposed to be KHz. That 50 Ohm series resistor knocks the edge rates down to where they should be.

bsder 10y ago

A couple things that I wish people had pointed out before I got started with PCB's: 1) You will spend your life reading datasheets. 2) Datasheets lie. 3) You will spend way more time in component selection than schematic design or board layout. 4) You will spend way more time creating component footprints than in schematic design or board layout. 5) Lay out the board by hand. You will waste more time fighting an autorouter than if you just laid it out. 6) A 6 layer board is not that much more expensive than a 4 layer board and is VASTLY easier to lay out. 2 layer boards should be avoided unless you you are a masochist or every fraction of a penny really counts. Some of the given advice is a bit off. 1) He doesn't put enough emphasis behind avoiding BGA. BGA should be avoided like the plague. Period. It will only cause excruciating pain. 2) Small QFN isn't that hard to deal with ... if you tweak the PCB footprints a touch (make sure you have .5 mm of bare copper outside the package outline and you can treat them like QFP). 3) 0603 is actually pretty small. Most people should stick with 1206/1210.

asimuvPR 10y ago
Mind sharing more about BGA?
- bsder 10y ago
  You mean, other than for me to threaten to stick a red hot poker in your eye if you use it? :) BGA isn't "impossible" for a hobbyist. But it's a huge amount of work for very little gain. All advice here also applies to what people refer to as CSP (chip scale package) as well. 1) BGA packages generally require better than normal PCB rules in order to actually "fan out" the signals to routing. BGA packages can put a lot of signals in a small area (that's why people like them), and you wind up needing very small pitch traces and vias to get everything out. You may even need an 8-layer board to pull it off 2) You can't really inspect BGA without X ray equipment. I don't know of any hobbyist X-ray machines yet (that actually might be a good project...) 3) BGA is prone to strange failures if you don't get ALL the balls down properly. You can get things like unpowered chip sectors because a Vdd ball is a little flaky (chip manufacturers don't always spend money reinforcing the on-chip power grid if they think you are using balls). 4) If you have a "small" (less than 40 pin) BGA, there is almost always a QFN option that is easier to work with and is almost the same size. 5) Thermal management of a BGA can be tricky. There is normally better heat flow out the top of a chip than down into a board, but BGA's normally want to push heat into the board. That having been said IF YOU MUST use a BGA: 1) Use a contract manufacturer Really. This is the best advice. I got some very tiny CSP chip boards done for like $50 per board for 20 boards. Even if your time is only worth $20/hour, the crossover point is 50 hours of work. You'll spend lots more than that if you're playing with BGA. 2) If you have a small number of balls, see if you can adjust the footprint such that you can hand solder things by having copper stick outside the package outline. I can't give you any general advice as this is specific to every chip. However, I have successfully routed things like power regulators which only have a small number of balls this way. I have also routed some bigger things like FPGA's this way (you can reorganize the output pins) where I simply didn't even try to use any pins not on the outermost edges. However, you are at the mercy of the manufacturer as to how many power balls you need hooked up properly. 3) Use a reflow oven. There are lots of reflow oven things on the market for <$500. If you get things placed right, a reflow oven gives you decent results. 4) Don't try to hand rework. Accept that you're going to throw the board out if there is a short. Yes, I'm sure lots of people have done things and been successful with BGA. However, if you do enough, you will find you are at the mercy of luck rather than consistency with BGA unless you let folks who have reflow and X-ray machines do the work.

jwr 10y ago

Here's something I don't get: why discourage people from using QFN packages? QFNs are only a problem if you are hand-soldering your boards with a traditional soldering iron. Which is nuts. These days everyone should have a soldering station with both traditional iron and hot air — and soldering QFNs using hot air is straightforward and easy. Besides, the article is about manufacturing, so you aren't likely to solder those QFNs yourself. So why discourage them? I think QFN and DFN packages are fantastic. They save lots of board space (and believe me, board space matters a lot in all designs, more than you think!), have good thermal properties, lack of leads makes for better low-inductance connections, less material means lower price. And most still have pitch of 0.5mm or more, so you can use the same design rules and same PCB pricing. Everything is great about them. BGAs are a different matter, but not for the reason most people think: they are problematic not because they are difficult to solder, but because you need much tighter PCB parameters to be able to route all the signals. In particular, via size is the biggest problem. You need really small vias that can be placed between four BGA balls. I dislike the hate being poured onto QFNs. I think it is a relict of the past: back when hot air was expensive and "strange" and people tried to solder everything by hand using a soldering iron, QFNs were the enemy. But these days they should not be. The unfortunate effect of hobbyists hating QFNs is that some manufacturers (Freescale/NXP, notably) later class certain chips as "hobbyist" and don't provide QFN packaging at all. And believe me, if you're designing a wearable device, the difference in size between a QFN-64 and an LQFP-64 is monstrous. Providing no real advantages, because both have 0.5mm pin pitch. So, while I would agree with the author that BGA packages are best avoided, I would encourage everyone to actually go ahead and use QFN/DFN packages. They are better in every respect.

turnip1979 10y ago

I'm in the Bay area and a hardware hobbyist (software is my full time gig). I see tons of meetups for SW but almost nothing for electronics hardware. Any recommendations?

zw123456 10y ago

Nice overview article. I have been doing PCB's for about 3 decades and here are just a couple of little tricks I have learned over the years, some are too long to go into here, but just a couple quickies maybe will help someone out: 1) Often the chip manufacture provides BSDL files which often times contain the foot print info and a lot of CAD tools have macros that will read them in and create your foot print for you. 2) There are often foot print libraries already out there you can download or are provided by the CAD software. But in either case, don't trust them, there are often errors, get your parts first, do the PCB layout, print it out on a good printer (usually the CAD SW will print it to scale and test fit everything. 3) There is a big difference between doing prototype boards and production boards. For prototype boards, make them big because you will have mistakes and will probably have to black wire (cut a trace and fix) it. I often use 2 layer or 4 layer for prototypes because it is easier to do fixes. If you CAD SW does auto layout then it is not that big of a deal as long as the board is large enough for it to route everything for you. For Production PCB's it is a different story and a lot more work to do right and I recommend farming it out if you can afford to. 4) I agree that part selection is critical but also, if you have simulation software either a separate program or in your CAD system, doing simulations can save you a lot of time. If you don't have simulation SW check into it, there are some decent free ones to learn on but to get serious you have to pay a lot. 5) For complex designs, I do separate prototype boards, one with the FPGA on it, another with the MCU and another one with the analog on it and so or, sort of a unit test approach (sort of like dev-ing SW) that way you can swap out sections that aren't working for you without throwing away a board full of parts, it is more effort but if you plan it out it can save you time and money. 6) I agree with the BGA comments, don't use those types of components unless you have a reflow oven and know how to use it, it is easier to debug QFN and QFP type packages since all the leads are exposed for inspection. You can often get parts in either package type and when you go to production you can always swap out to the smaller package later. If you have to use those for prototyping check if the manufacturer has a prototype board for it already it can be easier to just use an off the shelf one. A lot of people say the first board is a throw away, but that can be expensive for a production one so I have learned these tricks for prototyping so when you get to production you can avoid that bad first board.

mschuster91 10y ago

arcticbull 10y ago

Also, ChipQuick is great. It's super-low melting point solder you can use to easily rework SMD components. This thing has saved my ass too many times to count as a hobbyist :) Was able to get away without a reflow station for the small stuff I've been working on. http://www.chipquik.com/store/index.php?cPath=200 http://www.chipquik.com/store/index.php?cPath=200