Top Tips for Designing PCB's so they are Manufacturable.

[mrpackethead]

Whats your top tips for designing PCB's that are manufacturable??   or improve cost and reduce faults.

[mrpackethead]

(1) Spend lots of time on reviewing solder stencil apertures.  Really take the time to understand how they should be set up. 
(2) Reduce the BOM as much as you practically can.
(3) Double sided placement is somethign you really want to do for a good reason. If you can fit it on one side do that.  Even if it requires some extra board space.  (4) A 4 layer board might end up signifincatly smaller than a 2 layer, and end up being cheaper.

[T3sl4co1l]

I have the luxury of a full automated DFM service at the local shop I work for. Good for checking footprints, primarily.

Tim

[brabus]

Keep in mind stress on ceramic caps.
Do not put ceramic caps near the edge of the board;
Do not put ceramic caps near screw holes;
Do not put ceramic caps next to wire screw contacts;
Do not put ceramic caps in the preferred flexing direction of the board (happens with long thin boards);
The list continues...

Rule of thumb: Keep some very well made boards (a couple of Motherboards/embedded boards, some PCBs from an LCD TV, something from a smartphone, something industrial, etc.) on your desk and periodically check if your board looks like them. If you see major differences, you are probably screwing something up. :-D

[BrianHG]

Any traces under SMD resistors/capacitors should be dead center.  Same goes for any traces between pins on SO-8-14-16... packages.  (You wouldn't believe how many designs I see where you have a trace hugging one of the 2 pads to the minimum spacing manufacturing rule...)

Keep vias drill hole to either board manufacturer's recommended hole size, or larger by at least 1 full mil, keep extra angular ring around the vias.  If you do not need a test point, tent the vias.

Space out traces to 8 mil spacing at least unless you really need the occasional compact point, or are paying for a high spec PCB.

Keep everything away from the edge of the PCB and do not fill planes of place traces, except for an optional single ground trace, under or inside mid layer around mounting screws.

Run multiple parallel vias when feeding high current power traces.

[SMTech]

For SMT:

Put fiducials on your PCB, do not place them symmetrically and keep them at least 5mm away from the edges (conveyors and fixtures cover at least 3mm of the board).
If you panelise it, put a border on the panel, put fiducials on that too.
Fiducials are not defined using silkscreen or soldermask.
Define fiducials as components so their locations are automatically included in the pick and place file.
Make any individual panel over 50mmx50mm (which is still pretty small).
If you have connectors that overhang the board rout out underneath the overhang in the panel border so the border can be safely removed without breaking the connector.
Weird and wonderful connectors often need special tooling, or a harder to source specific part number with a pick assist tape/clip, don't use them just for the sake of it.
Surface mount is a != cheaper, sometimes it is both mechanically better and cheaper to use a conventional PTH part, at least until you get to high volumes where this might change the economics.
Thermally balance the copper traces to your components if you have a tiny trace to one end and a huge trace to the other you risk tombstoning or jauntiness.
If you follow current IPC & guidelines for footprints you should be fine when it comes to creating your stencil layer. Be sure to break up large pasted areas into smaller ones however - this is usually covered in the datasheet.
Read your datasheets! For some devices (QFNs seem to be the primary suspect) the package might not match the one you have in your CAD library even tho' it might seem the same at first glance. The center pad might be bigger/smaller and the outer pads might be shorter/longer.


For PTH:

Check your apertures and pad sizes.
Keep things away from the edges if it needs wave soldering.

In general:

If your board is an odd shape put it in a square panel with routing and scoring as appropriate, don't leave huge gaping holes in the panel, particularly if that PCB needs to go through wave solder later - keep it nice and rigid.
If you can avoid a custom cable, do so.
At scale some of these rules change, special tooling will remove some DFM requirements and introduce others - work with your manufacturer.
Thermally balance your board: top and bottom should have similar copper coverage, if one has way more than the other, your board WILL warp. That can cause stress on the components as well as being a pain to handle and looking bad.
Specify parts that exist, there is no point asking for a 1uF NPO 0805 100V capacitor just because the datasheet has suggested NPO is better.
If assembly looks fiddly, it will cost you more and increase the risk of build errors, costly rework and maybe even damage.

[Ice-Tea]

Not mentioned yet (oddly...): make sure the parts in your BOM are not unobtanium.

Digikey and/or Farnell are not the Holy Grail but if they don't stock it there's a decent chance it should not be on your board.

[SMTech]

Not mentioned yet (oddly...): make sure the parts in your BOM are not unobtanium.

Digikey and/or Farnell are not the Holy Grail but if they don't stock it there's a decent chance it should not be on your board.

In a similar vein, avoid single source, where possible all your parts should have available generic alternatives (or at least multiple vendors) that fit in the same footprint.

[ar__systems]

Not mentioned yet (oddly...): make sure the parts in your BOM are not unobtanium.

Recently most of stuff is turning into unobtanium...

My tip:

make sure the circuit can tolerate (not necessarily function at) input voltage in the entire range from zero to the intended voltage level. I.e. if the board is normally powered by 24V, you should be able to safely apply any voltage in 0-24V range  for prolonged time without entering any unstable states, erratic or undefined behavior. Helps with testing production units.

[asmi]

1. keep in mind that parts are three-dimensional and think about how the board is going to be assembled to make sure you can reach all pads with multimeter and soldering iron. Learnt this one when I had a short on some pads of a QFN which I couldn't reach with my iron without touching other parts, so I had to take these parts off first. Utilize 3D view capabilities of whatever eCAD you use for that.
2. when you place connectors along the perimeter of the board remember that in many cases connecting cable is wider than the actual connector. Otherwise you might not be able to connect all cables at the same time if you place several connectors too close to each other.

[Mr. Scram]

Maybe using multiple nested footprints so a shortage won't stump you?

[wraper]

Any traces under SMD resistors/capacitors should be dead center.

If you have a leeway to put a trace under them, either those are large components or your footprint is crap prone to tombstoning. EDIT: or your PCB is expensive to produce.
Example of crappy footprint many people make v. Unless adhesive is placed under component, such a large gap should be avoided.

[rx8pilot]

My top tip is to assemble your own designs.

I have learned a lot from my own bad ideas leading to various manufacturing challenges.

[T3sl4co1l]

Any traces under SMD resistors/capacitors should be dead center.

If you have a leeway to put a trace under them, either those are large components or your footprint is crap prone to tombstoning. EDIT: or your PCB is expensive to produce.
Example of crappy footprint many people make v. Unless adhesive is placed under component, such a large gap should be avoided.

Although taking that too far is equally bad.  If you can't route at least a thin trace under an 0805 or larger, your rules are wrong.  That's one pet peeve of the aforementioned DFM tool I use: it contains a SM-782 land pad gap maximum check.  Which is superseded by 7351, and the DFM guys know it.  They just leave it in as information.  So, even a full enterprise tool like this, you cannot follow blindly, you must use good judgement, as is always the case.

Just as well, tombstoning isn't a risk on 0805s and up.  It is a moderate risk on 0603, and a serious risk below there, and you probably won't get a trace between pads on those sizes.

Tim

[wraper]

Although taking that too far is equally bad.  If you can't route at least a thin trace under an 0805 or larger, your rules are wrong.

0805 is what I consider on a large side. But I would not suggest routing under 0603. BTW 0805 tombstones quite easily. Different thermal mass on the pads and components like ferrite beats, and here you go. I had an issue with certain 0805 ferrite bead on certain PCB (it's fine on another PCB with the same footprint), simply switched to ferrite bead from different supplier and it became fine.

[LapTop006]

make sure the circuit can tolerate (not necessarily function at) input voltage in the entire range from zero to the intended voltage level. I.e. if the board is normally powered by 24V, you should be able to safely apply any voltage in 0-24V range  for prolonged time without entering any unstable states, erratic or undefined behavior. Helps with testing production units.

Ideally nothing should be damaged by short overvoltage at a few volts over too.

Also consider what happens if polarity is reversed. Not always important, but sometimes it's cheap enough to add a diode or other protection even if it shouldn't matter.

[mrpackethead]

>Put fiducials on your PCB, do not place them symmetrically and keep them at least 5mm away from the edges (conveyors and fixtures cover at least 3mm of the >board).

the symmetric bit is important.  If you accidently load a panel into your Machine around the wrong way, or even upside down it is good if the machine cant' find the fiducial, and errors out.        My yamaha's will give or take look in the general area +/- about 2mm to find the fid..     Its good to  put fids on both individual PCB's and the panel itself.  Some of how this shoudl be done will be dependant a little bit on how your PNP system is se tup.   I use 2mm Fids on my panels, and 1mm round fids on my PCB, and have a decent amount (.5mm ) of solder mask pull back on them to make sure its easy to find.    You can also set up bad block fids as well.     Again, this is all stuff that you will never learn in a book.. Ask your PNP contractor or ifyou are doing it yourself,  figure it out.

>If you panelise it, put a border on the panel, put fiducials on that too.

Other thigns worth doign. Fids for paste stencils,  On the tooling strips ( yes, please use a tooling strip so you dont' have parts hard up against the rails ).  Do useful thigns like  text that says..   " TOP SIDE "    /  " THIS SIDE TO FRONT"    Very helpful as you load into the line.     Even consider using Big Arrows etc.   Make it easy for operators.   On My Yamaha line,  to make it easy , i have an alignment hole that is 5,5mm from the bottom left corner of the board. Again this is specific to the line its going to be made on.   everything you can do to make it easier results in high quality output.  Less faults.

>Fiducials are not defined using silkscreen or soldermask.

BUZZ if you do.  Minus 10points. Go Straight to Jail do not pass Go. Do not collect $200.

>Define fiducials as components so their locations are automatically included in the pick and place file.

Yes, this is a very good idea.   Add them as parts in yoru default templates so you dont' forget to put them in!   In my automation scripts, which build my PNP files, i have mine set up to be called FIDTOP1 FIDTOP2  which means it cand find them and deal to them directly.      Your vendor may use them differently.

>Read your datasheets! For some devices (QFNs seem to be the primary suspect) the package might not match the one you have in your CAD library even tho' it >might seem the same at first glance. The center pad might be bigger/smaller and the outer pads might be shorter/longer.

And dont' trust librarys that you got from the internet, make sure you've checked them!! or better still actually do them yoruself.  After a while you'll get resonably good at it, and its not a big issue.      ( QFN's are my fav IC package, they just work so well and are the easiest to reflow if you do it properly. )


>If your board is an odd shape put it in a square panel with routing and scoring as appropriate, don't leave huge gaping holes in the panel, particularly if that PCB >needs to go through wave solder later - keep it nice and rigid.

yeah..   again, talk with whoever is going to run the boards, and see how it will work together.

If you can avoid a custom cable, do so.

> yES. THATS just a way to spend lots of money or time.

>At scale some of these rules change, special tooling will remove some DFM requirements and introduce others - work with your manufacturer.
>Thermally balance your board: top and bottom should have similar copper coverage, if one has way more than the other, your board WILL warp. That can cause >stress on the components as well as being a pain to handle and looking bad.

As a general rule and there are times to break this.. if you are doing a four layer board, keep your two internal layers with as much solid pour on them. and our outside layers with just signal traces.. Its a good starting point.

>Specify parts that exist, there is no point asking for a 1uF NPO 0805 100V capacitor just because the datasheet has suggested NPO is better.
>If assembly looks fiddly, it will cost you more and increase the risk of build errors, costly rework and maybe even damage.

And check that they are availalbe. At design time, take the time to see if the parts are widely avaialble from multiple suppliers..   If only one has it, better think hard.

[Rerouter]

For mounting holes where you will be screwing against the board, put a ring of Vias where the screw head will rest, It will lessen how much the PCB can flow away from that point over time,

Standardize your drill sizes where possible to a smaller subset, if your doing large runs it means less cam time for the operators,

Inside (concave) corners on pcb edges should be rounded of have a designed cut in for a 2.5mm routing bit,

If you have wire solder pads, reinforce the pads with vias to reduce the risk of pad tearing.

Remove solder mask under QFN's where possible, Technically they are more reliable long term if the fillet is thicker, but its harder to get production yield.

Use a good revision naming scheme for your design files, so if you have to do an update because the fab cannot source a certain part, Its clear which is the latest that should be used.

[D3f1ant]

Don't put silkscreen overlay under QFN or other leadless parts that have no standoff.

I have had a part sit not quite flat because of a thick silkscreen, causing soldering issues. The footprint generator in AD often places silkscreen under parts that should fit flat.

[ChristopherN]

We're doing very small runs of special equipment, here is my list:

• Avoid cables with special connectors. If you have enough space and your signals are low frequency just use solder pads.
• Solder pads for cables should always be clearly marked, use a bigger font than normal for those. The same applies to connectors.
• Test your PCB with the housing it will go into, either in CAD or by printing it on paper and glueing the print to a piece of cardboard. I've seen many projects that had to be redone cause some parts did not fit at the last assembly test with many 100s of units already scheduled for production.
• Make sure all parts of the PCB that need to be touched after assembly (e.g. for wires, test points, headers for firmware updates, ..) can actually be reached without tearing the whole thing apart or breaking your fingers.
• Select a housing that is bigger than your PCB if you want to use watertight PG fittings for you cables. Many manufacturers do not leave enough room so connectors can not be installed correctly. This leads to leaks an damaged PCBs.
• Do a basic thermal test for each project, not just the PCB. Housings and other stuff will have a big impact on airflow and your whole thermal management.
• Be careful if you use PCBs as mechanical references, for example for mounting displays that should be visible in a cutout in the housing. Use bigger screw holes so the production worker can adjust the two parts to match.
• Use proper screws and spend time on finding matching bits / drivers. It will really bite you if you have to use the screw more than once and the head is gone.
• Add proper test points to everything you want to test. It's a pain to get pogo pins that go on connectors and such to work reliable. Avoid having test adapters that need to have a 3D pogo pin structure cause you want to test on high connectors and stuff.
• Leave enough room between test points. It's a pain if you have to contact 6 test points that are spaced like a 1.27mm pitch header.

I have so much more on my mind regarding this, someone should write a book

[IconicPCB]

Set routing rules sensibly.
Dont push the envelope just because the design software allows you.
Think about diamond shaped fiducials.

[mrpackethead]

Think about diamond shaped fiducials.

Why?

[Rerouter]

Apart from from "diamond fiducial" pulling the most interesting google image threads I've ever encountered, I don't see why a diamond shape would be preferential to any other, so long as the manufacturers tooling can recognize it?

[SMTech]

Here's the list of defined fiducial types on an Essemtec machine. Personally I have only ever encountered round ones typically 1 to 1.3mm in diameter and they seem to work perfectly well for me.
I find the Annulus type quite useful for those boards where I have to resort to using mounting holes or vias in place of a true fiducial.

[MudAndSnow]

Visualize yourself building the product as fast as you can while checking documents as little as possible.

Make it easy to find and access anything that production people need (test points, programmer connections, mounting holes, etc). 

When I worked in production the most common solution to problems was my generally very friendly boss yelling "read the production binder!"  Don't assume people will read your instructions. They might read all of it on first build, could miss steps, and probably won't even glance at it for refresher the next day.

Try to keep fragile components away from screw holes. Boards dont always get gently placed straight onto mounting points and screwdrivers sometimes slip. If someone hits and cracks a ceramic cap when their driver slips, they might not replace it and it might still pass QA.

If you have parts that might need to be glued down (large parts with small connection to PCB), try to leave room for not only glue (rtv or whatever) but also for the glue applicator.

If the PCB is having a spray (conformal coat) applied, think about the shadows created by large parts when spraying on an angle. If you put a bunch of large electrolytics in a 'U' shape with some small parts in the middle of the 'U', theres a chance those small parts won't get coated.