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

[oldnewb]

Screaming Circuits, a prototype assembly shop in the Portland area (Oregon, USA), publishes the occasional newsletter ("Circuit Talk") that makes for good nerd reading material.  They cover the many ways to screw up a board design, so future engineers can learn from others' mistakes.  PDFs of each issue are available on their Web site:

    https://screamingcircuits.com/about/news

[ar__systems]

Screaming Circuits, a prototype assembly shop in the Portland area (Oregon, USA), publishes the occasional newsletter ("Circuit Talk") that makes for good nerd reading material.  They cover the many ways to screw up a board design, so future engineers can learn from others' mistakes.  PDFs of each issue are available on their Web site:

    https://screamingcircuits.com/about/news

I'm not sure they should be listened to. I opened up the last one and this is what they write:

In five years we may no longer have components larger than 0402.

Yeah right. Ridiculous. And they are supposed to be "in the industry".

[wraper]

In five years we may no longer have components larger than 0402.

Yeah right. Ridiculous. And they are supposed to be "in the industry".

LOL, you still have heat to dissipate. There is no way around it  .

[jolshefsky]

These are all great ideas ... I have a checklist right in my board-file template on a non-manufacture layer so each project has the list right there to look at. Some things that I haven't seen yet:

• Run the design rule check one last time.
• Make holes where wires will be directly soldered (especially when hand-soldered) about 25% larger than than the nominal wire diameter. Make the annular ring larger (by percentage) than for component pads. Think about strain relief (or its absence).
• Consider making your own footprint for every part you're using. Only use outsourced footprints after you've confirmed they're well designed.
• Ensure no pads make unexpected contact with the case metal.
• Look at the gerber files directly in local software: something separate from your design system.
• Open the drill file in a text editor and look for weird drill sizes (it's not a complicated file format, and each drill size is listed.) Go back to your design and confirm if you find two drill sizes that are almost identical—see if you can change them both to the same size.
• Round off the sharp outer corners with curves in the board outline so the boards are more pleasant to handle. (Except when there's a good reason not to.)

[rx8pilot]

Wishing the DRC in Eagle could detect the absence of fiducials of some sort.

I forgot to put fids in a design a few months back which was a pain to deal with. There were no reliable features on the board, so I had to manually align the PCB on each pass through the P&P. Only had to do 30pcs and it was still enough pain to make a permanent mark.

I think I will make a Python script that parses the Eagle files to make sure each PCB includes fids and the in-house part number, and revision number. So easy to forget those.

[T3sl4co1l]

Round off the sharp outer corners with curves in the board outline so the boards are more pleasant to handle. (Except when there's a good reason not to.)

I like to take this a step further and add rout slots around the board as well, and specify v-score through the tabs.  The board depanels very cleanly with minimal burrs.

It is more steps, though.

Where a rough, rectangular board is all that's needed, I'll still spec v-score.  Ugly but cheap.

Tim

[schmitt trigger]

Lots of good advice here.

-If your board uses many leadless or very small components, place a few test point in strategic signals, and label the signal names.

-annotate your board as much as possible. I know, I know, some components are way too small to be annotated individually.

-always include the board part number and layout revision level. Allow an area for a sticker label which has the BOM and software revisions.

-connectors, specially those which connect to the outside world, suffer from lots of stress. Use ALL of the provided anchor pins.

[mrpackethead]

-annotate your board as much as possible. I know, I know, some components are way too small to be annotated individually.

I would say annotate for a reason.  dont' do it just because you can. 

[mikeselectricstuff]

Plenty of test points, annotated on the silkscreen. More so for prototypes. Don't forget a few scope ground points too.
Connect any unused MCU/FPGA pins to test pads, just in case.
Pads and alignment holes for bed-of-nails jigs for test and programming.
Unless your resist is white, put a rectangular block of silkscreen somewhere, so you can mark boards with a permanent marker ( number, tested, programmed, faulty, whatever). If your silkscreen is white, put an outline box so you know where any pen marks should go.
Don't put traces on an inner layer if it can go on the surface - you never know what you may need to track-hack.

If possible, sleep on a layout before ordering.

 

[mrpackethead]

Plenty of test points, annotated on the silkscreen. More so for prototypes. Don't forget a few scope ground points too.

yes. vias are useful for that, until you tent them. better to be deliberate about it, and mark them up.  Remember that you need to be able to get a scope tip into the test point!  You might want to consider putting in test pins/loops.

Connect any unused MCU/FPGA pins to test pads, just in case.


Or even a header pin if you have space.  As you say, just in case, and some time down the track you might just need it for somethign.



Pads and alignment holes for bed-of-nails jigs for test and programming.

yes, think about how you are going to test and program.     I'm love the cables from http://www.tag-connect.com/



If possible, sleep on a layout before ordering.


have lunch and dinner.

[rx8pilot]

If possible, sleep on a layout before ordering.

This may be the most important tip of them all.
Seems like every time I order at the end of the day, those are the ones with the dumbest mistakes.

[KL27x]

Check the soldermask layer, esp in Eagle. You can easily tent/untent vias unintentionally.

Check paste layer to make sure you aren't putting paste on pads where you don't want it.

Check "unrouted traces" layer all by itself. Sometimes the ground plane doesn't quite reach areas, and you can't see it until you do this, leaving a 0.1mm gap between a pad and the ground plane. (Done this, and... uh.. where's the engineering inquiry when you need it?)

If you are doing any ongoing dev with the firmware, you can lay down a small area of solid white silkscreen for annotating with sharpie.

Beware that any insigificant but carelss things you leave on the board may turn into "engineering inquiries," otherwise known as questions. You don't want questions, because questions add time/days to your turnaround. If you're intentionally doing something that looks goofy, try to preempt a question by including that info when you submit the quote/RFQ.

Write down the dimensions of your board. You're going to fill out the form halfway and find out you don't know the dimensions. And the quote page will timeout.

If you're using a new manufacturer, be sure to put in multiple quantities, even some many times larger than what you originally anticipate. Some manufacturers have huge price changes over certain quantities. Once you find that magic number, it might save you tons of money in the future. 500 pieces might cost less than 400.

[PartialDischarge]

This thread should be sticky

yes, think about how you are going to test and program.     I'm love the cables from http://www.tag-connect.com/

Didn't know those existed, I usually make my own with pogo pins from mouser, a PCB board, a broken drill, and a small amount of epoxy

[mrpackethead]

Didn't know those existed, I usually make my own with pogo pins from mouser, a PCB board, a broken drill, and a small amount of epoxy

That is an impressive amount of effort. nice.  I have been using the tag connect ones for some time and programed Lots of boards with them

[ar__systems]

yes, think about how you are going to test and program.     I'm love the cables from http://www.tag-connect.com/

They look so cool, I immediately want to order. But when I think about it for a minute, what value does this bring in? My standard is 5x1 0.1" header. When space is limited I go with 5x1 2mm, and when it is super limited I use 5x1 1mm. 1mm is PITA to work with, but it is even smaller when the tag-connect. 2mm is about the same area as TC and quite comfortable to work with.  For production I can leave pin underpopulated. I like to double the two pins in a center as a serial port output for debugging. So if I have to I can solder in two pins and get debug info out of the board. 5x1 also can be installed on either side of the board, but 2x3 can't, because the piount will be mirrored.

The plastic hooks on TC seems to be subject to frequent breaking.

[mikeselectricstuff]

yes, think about how you are going to test and program.     I'm love the cables from http://www.tag-connect.com/

They look so cool, I immediately want to order. But when I think about it for a minute, what value does this bring in? My standard is 5x1 0.1" header. When space is limited I go with 5x1 2mm, and when it is super limited I use 5x1 1mm. 1mm is PITA to work with, but it is even smaller when the tag-connect.

I also was looking for a 5-way in-line version for the standard PIC ISP header but they don't seem to do them.
I use 2.54,2 and 1.27mm versions depending on size constraints - with an in-line header it's fairly easy to solder some pogo pins to some protoboard to get similar functionality.
You don't need the board locks for production programming, and for development you can just solder a header on.

[Kjelt]

Wishing the DRC in Eagle could detect the absence of fiducials of some sort.
I forgot to put fids in a design a few months back which was a pain to deal with. There were no reliable features on the board, so I had to manually align the PCB on each pass through the P&P. Only had to do 30pcs and it was still enough pain to make a permanent mark. 

Buy a K40 laser from China for $400 and you can burn some sort of feducials after and at the same time print a unique pcb or barcode on the pcb to differentiate individual pcb's.

[mikeselectricstuff]

Wishing the DRC in Eagle could detect the absence of fiducials of some sort.
I forgot to put fids in a design a few months back which was a pain to deal with. There were no reliable features on the board, so I had to manually align the PCB on each pass through the P&P. Only had to do 30pcs and it was still enough pain to make a permanent mark. 

Buy a K40 laser from China for $400 and you can burn some sort of feducials after and at the same time print a unique pcb or barcode on the pcb to differentiate individual pcb's.

When I did it, I just used some calipers to scratch a cross a fixed distance from the PCB corners, which was good enough

[Kjelt]

When I did it, I just used some calipers to scratch a cross a fixed distance from the PCB corners, which was good enough 

On 30 consecutive pcbs within 0,1mm accuracy 

[ar__systems]

When I did it, I just used some calipers to scratch a cross a fixed distance from the PCB corners, which was good enough

I simply take a couple of 0603 parts closer to corners of PCB and use them as fiducials.  Though after having to do that a couple of times you learn not to repeat that mistake

[mrpackethead]

yes, think about how you are going to test and program.     I'm love the cables from http://www.tag-connect.com/

They look so cool, I immediately want to order. But when I think about it for a minute, what value does this bring in? My standard is 5x1 0.1" header. When space is limited I go with 5x1 2mm, and when it is super limited I use 5x1 1mm. 1mm is PITA to work with, but it is even smaller when the tag-connect.

I also was looking for a 5-way in-line version for the standard PIC ISP header but they don't seem to do them.
I use 2.54,2 and 1.27mm versions depending on size constraints - with an in-line header it's fairly easy to solder some pogo pins to some protoboard to get similar functionality.
You don't need the board locks for production programming, and for development you can just solder a header on.

I dont' use the ones with the plastic locks on them.   Kind of defeats the purpose for me. as i'm wanting somethign small.  Big advantage i see is that they are just single sided, so you dont' consume lots of board ). Makes layout easier.  and it often means you can get them very close to the relevent IC.     I started out with .1" headers as well, but am using these a lot.   Where i need to have a test jig as well, i have just used some standard pogo pins and created the layout.

Mike, Microchips ICSP port is technicallyk not 5 pin, its 6. I know lots of times the 6th pin is not used.  Look at a Pickit it has 6 pins.  I've pretty much ditched usign Pickits because they are just too slow, and use the ICD3 and ICD4..     Sadly the ICD4 does not have support for all the older IC's yet.

We've programmed thousands of parts using them and they work.. Not the only answer to the problem of course.

[ar__systems]

Yes, Pickit is 6 pins, but I'm yet to encounter an MCU that requires 6th pin to be programmed. I worked probably with like 30-50 different one including pic24, dspic, pic32

[mrpackethead]

Yes, Pickit is 6 pins, but I'm yet to encounter an MCU that requires 6th pin to be programmed. I worked probably with like 30-50 different one including pic24, dspic, pic32

Most of the new pics support Low voltage programming,  which requries the use of the 6th pin (PGM ).   There are times that you wont' want to use HVP ( High voltage programming ). LVP allows programming to occur at the VCC level of the Chip  ( 3.3V / 5V or so )..      Its worth a read up on this topic.

[mrpackethead]

PCB Surface Selection.

HASL is cheap, but often problematic.   ENIG can be a better alternative/

[mikeselectricstuff]

Yes, Pickit is 6 pins, but I'm yet to encounter an MCU that requires 6th pin to be programmed. I worked probably with like 30-50 different one including pic24, dspic, pic32

Most of the new pics support Low voltage programming,  which requries the use of the 6th pin (PGM ).   There are times that you wont' want to use HVP ( High voltage programming ). LVP allows programming to occur at the VCC level of the Chip  ( 3.3V / 5V or so )..      Its worth a read up on this topic.

Many of the newer PICs (not sure exactly which but noticed when I was fixing some broken PICkits) don't use HV on MCLR, so LVP is redundant on those. I can't think of many scenarios where HV programming on MCLR is a problem - worst-case a series resistor may be needed. I've never seen a need to use LVP - as far I'm concerned the ISP header is always 5 pins. 
Pickit is slow on larger parts but has the huge benefit of programmer-to-go mode for standalone operation, which AFAIK isn't yet implemented on PK4 ( last time I looked there wasn't even any mention in the docs).