Getting a PCB right the first time

[ZeroResistance]

How does one ensure that a PCB that is to be sent a board house is free of errors.
By errors, my main concern is if the footprints are of the correct dimensions and their pin layout is correct. I don't want to receive a board where an I package IC used like LQFP64 in not of proper size or maybe its inverted/mirrored and that renders the pcb useless.

I guess one way would be to print the board on a sheet of paper to 1:1 scale and actually place the real world footprint on it and eyeball it for correctness.

But I'd like to hear from the learned and esteemed members here what techniques they use so that these errors don't occur? Do you have any systems in place that ensure an error free pcb?

Of course in addition to incorrect footprints there would be a number of other issues like incorrect schematic symbol, or a  error in connection in the schematic, and I'm open to hear about how to prevent / detect these too.

[MagicSmoker]

I have done exactly as you surmised: print the footprint on paper and place the component on top of it. After you've made a few dozen (to hundreds) of footprints you get confident enough to skip this step, but it still occasionally saves my bacon. For example, I recently made a footprint for a new high voltage TO-247 variant (I4 package) and printing it out before sending off the board caught a mistake in the pin offsets.

As for checking pin assignments for accuracy, this is somewhat more difficult because you are essentially proofreading your own work. If you don't have a colleague that can help (I don't) then the best advice I can give is to set it aside for a day or two so you forget the details then go back and double-check the datasheet against the library symbol.

[iMo]

ALWAYS (!!) double-triple-check ALL your layers you are going to send with the "gerbview"..
It allows you to measure the distances on the layer pretty well.

[ZeroResistance]

I have done exactly as you surmised: print the footprint on paper and place the component on top of it. After you've made a few dozen (to hundreds) of footprints you get confident enough to skip this step, but it still occasionally saves my bacon. For example, I recently made a footprint for a new high voltage TO-247 variant (I4 package) and printing it out before sending off the board caught a mistake in the pin offsets.

As for checking pin assignments for accuracy, this is somewhat more difficult because you are essentially proofreading your own work. If you don't have a colleague that can help (I don't) then the best advice I can give is to set it aside for a day or two so you forget the details then go back and double-check the datasheet against the library symbol.

Most of the times I don't have the physical part at hand, and so have to rely on the dimensions of the datasheet. However I think I may have to rethink that and probable get some samples of the critical parts, before sending the pcb for manufacture.

[T3sl4co1l]

Us commercial designers often have access to review procedures (semi/automated DFM (design for manufacture) checks), which is a great help, but also still quite limited, depending on just how fully featured it is of course.  (For example, the one I use often, is really limited to checking footprints and spacing, and only those that are in the database.  Anything not in the database, basically comes back with a note "we couldn't tell, check this manually".)

There is value in mitigation.  Put 0-ohm jumpers on your RXD/TXD pins, you'll confuse them eventually and it's an easy hack to swap them back.
MCU pins with source-termination resistors are handy test points and for rewiring.
Use easy-to-handle parts (0805 chips?), leave enough space between components that you can hand-solder them (or whatever processes you have access to).
Use relatively large pads, so you can hand-solder them, or put on alternate parts if needed (say, replacing an 0805 resistor with a SOD-123 diode, or a 1206 chip?).
Prefer general-purpose parts, in widely available packages (SOT, SOIC, TSSOP..), and check the pinouts not just for your preferred parts but check for possible pin-compatible substitutes as well.
Download IPC-7351 (preferably a newer version (a or b), but any will do), read and understand how leads and pads are dimensioned, and check your footprints against them.  Tweak the dimensions to suit your process (e.g., extra toe length for hand soldering).

As for personal review -- when you don't have access to, or budget for, any of these services, you're just checking it yourself -- that's down to the user, obviously.  Some people are great at spotting a needle in a haystack.  Often it takes a lot of experience to spot these sorts of things.  You're literally inspecting thousands of objects.  Expect to make mistakes, but also take your time, and interact with your design.  "Handle" it, as well as you can with a CAD model; generate 3D views, get a feel for how the connections are routed in space.  Check your memory of the part pinouts, top and bottom; recheck them against the datasheet.

Got a bullshit datasheet that's showing the footprint backwards, or not labeling things, or the drawing is full of fuck?  Ask, maybe someone has experience with that part, or can look it up in a database.

Personally, I do a lot of faffing around on PCB layouts, idly shoving traces, prettying things up.  This mitigates the fatigue of staring at thousands of objects, and provides a different way to interact with and inspect them.  This also gives me the time and perspective to contemplate other issues, like circuit strays, EMC performance, DFM, DFT (design for test), and so on.  (Besides the value this faffing actually generates, I do -- if I do say so myself, and based on others I've seen -- do the actual layout work very quickly, so I have plenty of time to spend in this way, compared to the average service.)

Tim

[Bassman59]

Also, after you've gotten the footprints and pinouts all correct, you'll still screw up the mechanical part. Does it fit into the box? Are the mounting holes and connectors and such in the right place? Did the mechanical drawing of the enclosure front panel make any sense? Did you pay attention to the keepouts so that parts aren't butting up against the metalwork?

[tszaboo]

It doesnt need to be perfect as first try. That's what the prototype is for. I always schedule a prototype into the project plan, no matter how much management is screaming because of it. In fact, you should make a huge bone-headed mistake that ensures that they dont send the prototype into production, so all the other small mistakes can be corrected. If you dont have one, they will send it into production, the first time they see an LED blink on a board.

[djacobow]

It doesnt need to be perfect as first try. That's what the prototype is for. I always schedule a prototype into the project plan, no matter how much management is screaming because of it. In fact, you should make a huge bone-headed mistake that ensures that they dont send the prototype into production, so all the other small mistakes can be corrected. If you dont have one, they will send it into production, the first time they see an LED blink on a board.

Yeah, I'm happy if my prototype can be *made* to work, or at least prove out the parts of the design that had "worried me." If that means some cut traces, added bodges, and parts flipped upside down, that's fine.

When I make a board and find lots of errors and things I want to fix to make the board better, more manufacturable, etc, it doesn't upset me too much. When my board has ONE such error, that actually ticks me off more. I guess that may or may not be logical, depending how how much time I spent on the board trying to get it "perfect". 

[KL27x]

the footprints are of the correct dimensions

Recommended footprint mechanical drawings are almost always included in the datasheet for a component.

maybe its inverted/mirrored and that renders the pcb useless.

I don't think there's a cure for dyslexia. 

There are only a couple or regular gotcha's I can think of that are always on my checklist for Eagle, aside from obvious ERC and DRC's.
View the unrouted signals layer by itself (to make sure it's completely empty, of course) in case there are any almost-connected signals that leave tiny gaps.
Check clearances and soldermask to make sure vias are tented/untented as intended.

[tautech]

All of the above plus a few little things gleaned from many SS home etched PCB's without overlays.

Component orientation markings.
Amend IC and active component footprints for the copper to show pin 1 or add an adjacent copper dot as a pin 1 signifier.
Same for polarized caps, make one pad square and/or add a + into the copper closeby.
Diodes often have a polarized footprint but adding a K in copper closeby never hurts.
Mark polarized headers, just a + and GND/Neg/- is plenty.
Unconnected copper = No Net.

Measurements
Double check scaling of prints and final artwork is correct, if you haven't got calipers......GET SOME !
Don't skimp on TH drill hole size, anyone that reworks your board will thank you.
Annular rings, make them as large as is practical and when clearance is a problem elongate them.
Watch for insufficient trace clearances when using elevated voltages....overlays and conformal coatings can help manage this.
Always consider rework when laying out a PCB so that some poor bugger doesn't have to remove 1/2 the components from the PCB to remove just the one they want. Particularly important for SMD PCB's !
Use medium or low density class passive footprints for anything that might be hand soldered or reworked.

Finally, does the PCB make sense in that are polarities to each and every polarized component are correct.

Oh, and DRC !