In a similar vein, I discovered and have started using the Tag-Connect TC2030-USB to program/troubleshoot my boards. While it's technically/originally intended as a way to do JTAG debugging, I am completely enamored with the ability to drop a footprint on my PCB and be able to connect to it without having to place a relatively expensive connector (or a connector at all) that I don't necessarily want users interacting with.
They're fine for one guy using them on the bench but they are a nightmare for mass production. The 50-mil pitch is annoying to make work with a bed-of-nails fixture, the clips are fundamentally incompatible with production lines, either robot or human, the parts are expensive, and the cycle life is not there.
I have had one too many arguments with firmware people who think these things are sufficient for production that I am just done with them by now. There are other ways to do it.
The only actual issue I had with Tag is that it takes up more space than an array of aggressively placed test points would. Which is still acceptable in some designs.
If you can't hit a massive, enormous 1.27mm pitch connector complete with dedicated indexing holes with your jig, I can't fathom how that would be the fault of the connector.
No, it is not. You may think my contract manufacturers lack skill. (No comment from me.) But I have to live with them and make things work.
I try to get my CMs involved in design early. I think it is telling that whenever I give them choices, they reject Tag-Connect and pick one of the other options. Every. Single. Time.
The connector that was specifically flat-out hard rejected was the TC-2070 14-pin version. The number of pins was part of the problem. Apparently (this was a while back now so I may be misremembering) they had trouble with the density at 0.050": 6 pins gives you a lot more room on the sides to squeeze stuff in than 14 does. So they have to do it with a special premade block that comes in and hits the pads, and that block was nearly-but-not-quite unobtainium for the 14-pin version. The CM hated the Tag-Connect in general and wanted it gone, so we didn't trust them too much, but then we tried to build the fixture in house and prove them wrong... after that experience I have joined them in their hatred.
The fact of the matter is that there are many, many other good ways to do it, so it's not Tag-Connect or nothing. Castellations are right out in HVM because of the cost hit, so that rules out Edge-Connect and friends. Würth has WE-SKEDD which looks like the same general thing as Tag-Connect but I've not had cause to try it.
My favorite thing to do, if space allows, is to just put down the unshrouded surface-mount header. Cortex and ESP parts nominally use a standard 0.050" header and you can just place it down. Then don't populate it, and you've got an array of pads that are long enough to stagger test probes on to in a bed-of-nails, or for bench use it is very easy to hand-solder the header on. Plus it's surface-mount so the space below the header is available for use (often things like pull resistors or ESD diodes go nicely here). The biggest wrinkle here is the solder stencil. You do not want to have paste put on these pads if you're not soldering the header, because you badly want your test pins to hit clean ENIG finish and not flux-covered no-clean solder (doubly nasty to probe, even clean solder is bad enough). So it's harder to do a small run of 100 bench-debug boards with headers then the rest as production. You usually end up just soldering the header by hand (or having the CM do it), which is OK.
Otherwise it's traditional pogo pads all the way. This is pretty much required anyway whenever the board is too small for other methods (did I mention Tag-Connect is huge? Tag-Connect is HUGE.) and it works great as long as you were already planning on fixturing.
With the information you're giving, my decision would probably be to take the non-clip TC2030 or TC2050 (I've never needed 14 pins) footprint and overlay the footprint for a regular 1.27mm SMD connector on top of it. Cortex debug connector should be a good fit but I haven't checked.
That seems to be the "get your cake and eat it" (though it does mean you're spending the space and drilling the holes for TC.) But still -
> They're fine for one guy using them on the bench
If you're insistent on Tag-Connect, that's a pretty good way to go. Those legs are a big part of the problem and so the No-Leg version helps a lot. But then it also falls out of the board....
Seriously, I tried to like Tag-Connect. I did like it before supporting a CM and a hardware team trying to use it (and lose the cables...). Now I just plain don't think it adds value over the alternatives. The header is three cents. Three. Cents. The cable is $39 (with legs, $34 without). That buys you over 1,000 headers and then you can use the free cables that come in the box with all the debug probes and live in the pile over there in the shop.
Bending the little pins also works (they will tend to bend themselves after a little while of use anyway), but at the cost of making insertion a little harder as well. I found that to be the best compromise for me, but YMMV.
Just put normal test pads next to the tag connect, a bit more spaced out. A bed of nails in the production line connects to that, the tag connect can be used for bench development.
I've been doing a cheap DIY version of Tag-Connect for some STM32 projects (6-pin debug). I just put the holes for a pin header near the edge of the board, and use a pogo clip to connect [0]. (These are readily available on AliExpress in various sizes.)
I think they probably mean standard through-holes. It's the old trick where you stagger the holes just enough that the flex of the pinheaders still let's them be inserted, but have just enough friction to stay in place while you're flashing or whatever.
Right, plated through holes, but with almost no exposed anular ring. As little as I can get away with without getting mask sprayed down into the hole.
For 100 mil pitch, 25 mil square pins: 36 mil holes, 6 mil off center, 12 mil hole to hole.
The short side of a generic pin header is the side that goes in the holes, so the long side is free to accept dupont sockets and shunts the same as if you had the same pins soldered in the pcb. So the cable is just ordinary programmer fly wires with female dupont ends. You don't even need to make an actual cable.
If space is tight on the pcb then it does use up more pcb than pads that leave the other side free. And pogo pins are going to be a lot faster for producing something in numbers.
I don't mind buying nice stuff like a fancy purpose made good-working tool for myself but I'm always making open source projects and one design goal is to require as little as possible, and as generic and universal as possible from the user. So I avoid fancy special things where possible. It's not designing for commercial production runs nor designing for one-off for myself, it's designing to a kind of a platonic ideal to strip away anything unnecessary and yet try to meet 2 opposing goals at the same time as much as possible: Don't require special tools that make things work reliably because of how fancy the tool is, and don't require the user to be a zen master craftsman that can attain a successful result with rocks and nails. Try to make the process reliable and repeatable while still only requiring basic materials and supplies. As much as possible anyway.
Pogo pins are pretty common these days and not exactly exotic or expensive any more so maybe I can start using them.
Then again, the through holes do 2 extra things besides make the connection.
With pads you need to aim/register the pins to land on the pads, and you need to hold them there. That means aiming with your eyes and holding with at least one hand, or it means adding some kind of extra registration and grabbing features to both the pcb and the cable, like extra drill holes or slots and extra plastic shapes on a special cable-end etc. Or no extra features on the board and instead a whole clamping jig that holds both the board and the pins.
Since these are holes that pins go in to, you don't need any other form of registration to aim the pins at the pads. The pins go in the holes.
And they hold onto the pins themselves, so you don't need any other form of retention.
It's just like plugging a plug into a socket where the socket provides all that naturally.
I have one board that needs two different connections like that, one for jtag and one for power and to temporarily close a jumper to write-enable the cpld. So a 4-pin and a 6-pin, 2 different cables in 2 different places. The entire board is slightly smaller than a DIP-28 so no room for any real connectors. You just stick the cables in and two different cables hold themselves with zero hands while you operate the flashing software. The wires are all plain dupont wires stuck on the pins, no solder, and 2 of the pins just have a generic jumper on them. It's completely basic and not-special and works perfect.
I have another board that needs 28 pins in a small space.
For that one I used 2.0mm pitch pins in straight rows not staggered, but with the holes only 1.7mm apart. In that case it's the long side of the pins that goes into the holes, and the short side is soldered into a programming adapter pcb that goes into a programmer. The pins are in 2 sets of 2x7. Each set of 2x7 has 2 straight rows of 0.72mm holes 1.7mm apart. What happens there is, as the pins start to lean over, the top of the pins hit the opposite side of the hole on the top of the pcb, and don't want to go any further. The pins wedge solid and make 4 points of contact, 2 on bottom and 2 on top, and the board won't go any further even though the pins only just poke out the top and there is still almost 2mm of travel left. So you have a lot of remaining travel to just push a little more if you get a bad connection. It works great and no special parts anywhere.
Doesn't it require ENIG? I wanted edge connector for my pcb project but it adds $20 to the price of pcb, that's just too much. Anyone knows card edge alternative? I'm thinking pin header but that's not very user friendly. Edge card can be inserted blindly even if you don't see the connector, pin header would probably just bend irl.
I've done HDMI edge connectors like this using plain HASL without too much trouble. Just don't forget to remove all soldermask on the connector path, they'll dirty out quickly otherwise.
But, now I do ENIG everywhere because it's often the same price as lead-free HASL (or so close it does not matter), while looking way cooler. I've started to take quite seriously leaded stuff now, especially since low temperature lead-free solder exists (SAC305).
ENIG sounds expensive right? Double the cost of your board or w/e? IMO it's no big deal because::
- A: If you want a 6 or more layer board at some places, you have to get ENIG anyway, and solving routing puzzles isn't my idea of fun.
- B: The PCB price is a small portion of the overall price anyway; parts and SMT dominate. So you're paying 2x as much on 15% of the total or w/e.
There are USB-A drives which do this, and in my experience they are far less durable than ones which have an actual connector. Given the thinness, this is going to be too easily snapped off.
FWIW, my slightly more than anecdotal evidence is that 1.6mm is the default thickness at JLCPCB and PCBWay, and they will subtly encourage you to switch to that width if you don't want to pay more or wait longer for them to fill a sheet.
Every IC prototype board (eg Proto Advantage) and all of those Adafruit breakout boards are 1.6mm.
For these reasons, 1.6mm sure seems like a default if there is one. Is there some JEDEC standard or similar which proves me officially wrong? Happy to learn if so.
It's not 1.6mm, it's actually 1/16", and it's been the standard since the days of yore. It's a super common inch measurement so it's not really a surprise to see it here, if you know your inches. There's tons of 1/16" plywood, for example.
A "thick" PCB was commonly 3/32" (0.093") and a "thin" one 1/32" (0.031"). Now of course it's all made in Asia so the metric dimensions predominate (0.8mm, 1.6mm, 2.4mm), but the legacy remains.
And of course PCBs aren't really any of these thicknesses, they're whatever the glass weaves press down to in the lamination press....
Your answer prompted me to do some further research. It's true that IPC-2221A does reference 1/16th as a historical precedent.
That said...
Lawrence Berkeley is an American institution, and it's fair to say that your perspective is American-centric. Without rehashing the ages old argument, it is still true that the US stands with Liberia and Myanmar in your steadfast refusal to standardize on the metric system.
It's your prerogative to conclude that this is an Asian thing, but it's very much an almost everyone else thing.
I will concede that it drives me nuts that not only does the lumber industry still use inches here, it's also officially and somehow legally not even accurate in inches. Why we can't have nice things...
Where does LBNL come into this? The reference in IPC-2221 is to NBS Report 4283 from 1956. Neither of those have anything much to do with LBNL.
I reject your assertion that my comments are America-centric. This a technology that was primarily developed in America and is now predominantly no longer manufactured there (Asia is not in America). It is rather natural for each place to use the units of measure they favor, so it is natural for what was a very common customary unit dimension of 1/16" to become a reasonably round metric dimension of 1.6mm. This is how things develop in the world.
Thanks for calling that out; the IPC-2221A doc I was viewing was on the LBNL domain and my brain incorrectly inferred that the folks who had worked on the IPC spec were employed by LBNL.
Still, IPC is also based in America, which brings us to the same place. While every org has to be based somewhere, the notion that the entire world should use imperial measurements simply because America does is pretty much the definition of America-centric in my books.
The ground truth is that we're talking about a de-facto standard, not a hard one. Given the actual difference between 1.6mm and 1/16", the ease of working in base 10, PCBs are mostly made in Asia and the flogged horse that the entire rest of the planet thinks in metric... it's no surprise to me that 1/16" has become a historical footnote.
I've found 0.8mm to make much more reliable connections, since the specification says that the tongue should be 0.7mm. 0.6mm will disconnect if the cable is angled in any way.
0.8mm is definitely out of USB 3.0 official spec and might damage the plug. The Spec requires 0.7mm with contacts and 0.6mm without, i.e., 0.05mm for the contact. See:
i wonder how often you can plug/replug the connector in this case. how will the pcb material hold up? with my press-fit or clip-fit (is that a term?) 3d prints, ive noticed that 20 cycles can be sufficient to induce substantial 'loosening'.
It’s likely in the order of 10-30, especially with something like ENIG as a finish. If you wanted more cycles, you’d want to switch to a hard gold finish which would likely increase the cost substantially.
This is truly only for a debug port, not anything else.
That's cool but I am not sure how a customer of mine would feel if I shipped a board to them like that. (I could see trying it on a project for myself, though.)
The problem with USB-C connectors for hobby projects is that they are ass to solder by hand—I’m still looking for one that would use a larger pitch by shorting the four USB pin pairs for either orientation. If you’re shipping something to a customer, I think it’s fair to assume that you don’t really have that problem :)
They're also ass to make PCBs for. The second you need 2oz or higher you start to really push the limits of what most prototype shops can do.
This is a pretty standard 2.0 receptacle, you've only got 0.2mm between pads if you follow their footprint (literally the limit for soldermask bridges on 2oz at JLCPCB): https://gct.co/download?type=PDFDrawing&name=USB4105.pdf
Get a hot air gun: it'll make your life way easier. You can tin the pads with a soldering iron, put the connector on and squirt some flux on the leads, and then just blow hot air until it reflows into place.
What do you do if the structural through-holes already have solder in them, that wick doesn’t seem to get? I’ve been trying to put a new USB C port onto my switch for quite a while now. (Now that I think about it, I can probably just shorten the prongs on the port and add solder after for structural strength).
I have the SS-02, and I like it - I had one of the cheap blue ones first, but the pliable rubber tip really makes a difference. If you’re soldering smd by hand, it’s more than worth the $20
The answer to almost every question in soldering is 'more flux'. Solder wick has flux in the center of the braid, but it's hard to get it into tight places like structural through-holes. Adding your own liquid/paste flux will make the wick much more effective.
Melt the solder and thwack the board on something hard? So the board stops but the molten solder doesn't.
Sometimes though you just have to pile on solder and flux because the via is small enough that surface tension and heat dissipation means its never coming out
I often add solder to make it easier for the wick to get everything. If the original assy was Lead-Free, using low temp solder (I can has lead? As a treat?) may make a difference here as well. Flux pen on the solder wick also seems to help especially if your wick is kinda crusty.
How would tinning those tiny pads not create a massive bridge between them? Does the bridge somehow go away in the reflow phase? (Not familiar with reflow at all)
To add to the sister comments, you can quite easily remove such bridges by adding flux and then touching each individual pad with a fine tipped soldering iron. It sometimes takes a few tries, but eventually the solder that’s touching the solder mask will either be wicked onto the iron or move onto one of the neighboring pads. (The trick is to touch just the pads with the iron, and not to try to attack the solder bridge itself.)
Do you find the 6-pin charge-only Type-C connectors too small? Or the 16-pin 2.0-only ones? They seem reasonably hand-solder-friendly but I admit I've been fortunate enough to have the factory handling them for me.
Yeah, I find the 16-pin ones a little beyond my skill. They also feel silly—why can’t I have one with just six pins for D±, VBUS, GND, and CC1/2? I guess I could have a factory make a bunch of modules like that for me, but it definitely feels like a thing that should already exist.
(There are passive A-to-C adapters, so I see no reason why I couldn’t short pin pairs like that.)
I have soldered the 12-pin, power-only USB-C connectors. The real breakthrough came though when I tried a hotplate rather than soldering iron for the USB-C connector.
Could you clarify? As far as I can tell, GND is A1/B1 and A12/B12, VBUS is A4/B4 and A9/B9, D+ is A6/B6, and D− is A7/B7, and each A pin swaps with its B counterpart when I flip the connector.
Only one side of the cable is going to be lit, but you don't know which one it is: it depends on whatever happened upstream. So you have to be able to handle either side being lit up. You can't easily do that with a single set of contacts because of how D+/D- is handled (it would be a literal X-shaped crossover), so now you're kind of stuck.
It ends up just not being worth the trouble if you need the USB 2.0 pair. But power-only is much easier and, guess what, pretty available in the market.
The 6-pin Type-C provides 2 pins each for power, ground, and CC. (DO NOT LEAVE CC OUT. THIS IS WHY A LOT OF RECENT USB STUFF MISBEHAVES. GET CC1/2 RIGHT PLEASE.)
The 16-pin adds 10 more: 4 for D+/D-, 2 more each for power and ground, and then they add 2 more for SBU as well. I'm not entirely sure why SBU is important enough but I'd guess it's because it's physically vertically next to CC so probably helps the mechanicals to leave it in.
There actually do exist 8-pin guys like this https://www.lcsc.com/product-detail/C47326494.html (among others) that add D+/D- only to the 6-pin connectors. I can't imagine they work terribly well most of the time but they must have some use? They do seem to be from Asian vendors only, which might mean something.
(Side note: the way Type-C handles D+ and D- has caused me so much pain. I get that it was a difficult problem to solve... but there had to be a better way than this, right? Probably not, but I can still whine.)
I was glad to see this at first (because I did page through Mouser and LCSC a bit before I came back here to continue my bitching and found nothing). Then I actually looked at the drawing, and— Excuse me, is that really a USB-C socket that only works in one orientation?.. The drawing shows that the socket has both CC1 (A5) and CC2 (B5) but only one of the two copies of D+ (A6 but not B6) and D- (A7 but not B7). Seriously? Even I don’t hate my users that much.
Yep. I couldn't believe it existed either. I was even curious enough to ask an LLM about it and got the same response: it doesn't know of a use beyond creating frustration.
I guess past-me was smart when drawing USB-C connector symbols in my library and this one doesn't exist there for a reason!
This is very cool! What is the practical intent, given USB ports are 69c each? To save vertical space? I am thinking: Neat this is elegant and would work! But I can't think of any scenarios (off-the-cuff.) where I would choose this.
I have no idea how easy it is to implement this in KiCAD, but if it is - prototyping with this can be faster if you're eg making something like a DIY keyboard. Fewer things to solder, which is very nice if you struggle with it.
In a similar vein, I discovered and have started using the Tag-Connect TC2030-USB to program/troubleshoot my boards. While it's technically/originally intended as a way to do JTAG debugging, I am completely enamored with the ability to drop a footprint on my PCB and be able to connect to it without having to place a relatively expensive connector (or a connector at all) that I don't necessarily want users interacting with.
https://www.tag-connect.com/solutions-target-devices/usb-ser...
They have FTDI versions as well, for those who want the full USB boot/reset treatment.
Also, they have another connector for attaching to castellated edges. I think it's just so clever.
They're fine for one guy using them on the bench but they are a nightmare for mass production. The 50-mil pitch is annoying to make work with a bed-of-nails fixture, the clips are fundamentally incompatible with production lines, either robot or human, the parts are expensive, and the cycle life is not there.
I have had one too many arguments with firmware people who think these things are sufficient for production that I am just done with them by now. There are other ways to do it.
This reads like a skill issue to me.
The only actual issue I had with Tag is that it takes up more space than an array of aggressively placed test points would. Which is still acceptable in some designs.
If you can't hit a massive, enormous 1.27mm pitch connector complete with dedicated indexing holes with your jig, I can't fathom how that would be the fault of the connector.
Not sure how this got down voted.
This is truth.
>> This reads like a skill issue to me.
> Not sure how this got down voted.
You’ll notice the parent comment could have gotten the point across without sounding toxic, by just dropping the “skill issue” paragraph.
See also: https://news.ycombinator.com/newsguidelines.html (the section about how to write a good comment).
No, it is not. You may think my contract manufacturers lack skill. (No comment from me.) But I have to live with them and make things work.
I try to get my CMs involved in design early. I think it is telling that whenever I give them choices, they reject Tag-Connect and pick one of the other options. Every. Single. Time.
The connector that was specifically flat-out hard rejected was the TC-2070 14-pin version. The number of pins was part of the problem. Apparently (this was a while back now so I may be misremembering) they had trouble with the density at 0.050": 6 pins gives you a lot more room on the sides to squeeze stuff in than 14 does. So they have to do it with a special premade block that comes in and hits the pads, and that block was nearly-but-not-quite unobtainium for the 14-pin version. The CM hated the Tag-Connect in general and wanted it gone, so we didn't trust them too much, but then we tried to build the fixture in house and prove them wrong... after that experience I have joined them in their hatred.
The fact of the matter is that there are many, many other good ways to do it, so it's not Tag-Connect or nothing. Castellations are right out in HVM because of the cost hit, so that rules out Edge-Connect and friends. Würth has WE-SKEDD which looks like the same general thing as Tag-Connect but I've not had cause to try it.
My favorite thing to do, if space allows, is to just put down the unshrouded surface-mount header. Cortex and ESP parts nominally use a standard 0.050" header and you can just place it down. Then don't populate it, and you've got an array of pads that are long enough to stagger test probes on to in a bed-of-nails, or for bench use it is very easy to hand-solder the header on. Plus it's surface-mount so the space below the header is available for use (often things like pull resistors or ESD diodes go nicely here). The biggest wrinkle here is the solder stencil. You do not want to have paste put on these pads if you're not soldering the header, because you badly want your test pins to hit clean ENIG finish and not flux-covered no-clean solder (doubly nasty to probe, even clean solder is bad enough). So it's harder to do a small run of 100 bench-debug boards with headers then the rest as production. You usually end up just soldering the header by hand (or having the CM do it), which is OK.
Otherwise it's traditional pogo pads all the way. This is pretty much required anyway whenever the board is too small for other methods (did I mention Tag-Connect is huge? Tag-Connect is HUGE.) and it works great as long as you were already planning on fixturing.
With the information you're giving, my decision would probably be to take the non-clip TC2030 or TC2050 (I've never needed 14 pins) footprint and overlay the footprint for a regular 1.27mm SMD connector on top of it. Cortex debug connector should be a good fit but I haven't checked.
That seems to be the "get your cake and eat it" (though it does mean you're spending the space and drilling the holes for TC.) But still -
> They're fine for one guy using them on the bench
If you're insistent on Tag-Connect, that's a pretty good way to go. Those legs are a big part of the problem and so the No-Leg version helps a lot. But then it also falls out of the board....
Seriously, I tried to like Tag-Connect. I did like it before supporting a CM and a hardware team trying to use it (and lose the cables...). Now I just plain don't think it adds value over the alternatives. The header is three cents. Three. Cents. The cable is $39 (with legs, $34 without). That buys you over 1,000 headers and then you can use the free cables that come in the box with all the debug probes and live in the pile over there in the shop.
You can get retaining clips to hold it on. While these can be a bit fiddly, I’ve found them good enough for bench testing with no legs tag connect
https://www.tag-connect.com/product/tc2030-retaining-clip-bo...
Bending the little pins also works (they will tend to bend themselves after a little while of use anyway), but at the cost of making insertion a little harder as well. I found that to be the best compromise for me, but YMMV.
We do smaller production runs of typically 100-1000 boards and have had good luck with the Tag connectors for programming them.
Out of curiosity what are the other ways?
Just put normal test pads next to the tag connect, a bit more spaced out. A bed of nails in the production line connects to that, the tag connect can be used for bench development.
This is the way
0.1" header holes slightly staggered to grip inserted headers can work great and you don't need to have a special expensive cable on hand to use it.
I've been doing a cheap DIY version of Tag-Connect for some STM32 projects (6-pin debug). I just put the holes for a pin header near the edge of the board, and use a pogo clip to connect [0]. (These are readily available on AliExpress in various sizes.)
[0] https://www.adafruit.com/product/5433
I do exactly the same on my boards and use that same clip.
Back in my undergrad days I built a similar clip out of a broken clothes peg, hot glue, and some 2.54mm headers. It worked well.
Maybe you like this - "paw connect", a whimsical version of the footprint for this connector:
https://github.com/LeoDJ/Paw-Connect
I just use ordinary straight pin headers and stagered via holes. The board just has vias and the cable just has a plain pin header not even pogo pins.
Why vias? So the pins don't go all the way through? Wouldn't any disparity in the lengths of the pins make that pin not touch?
I think they probably mean standard through-holes. It's the old trick where you stagger the holes just enough that the flex of the pinheaders still let's them be inserted, but have just enough friction to stay in place while you're flashing or whatever.
Right, plated through holes, but with almost no exposed anular ring. As little as I can get away with without getting mask sprayed down into the hole.
For 100 mil pitch, 25 mil square pins: 36 mil holes, 6 mil off center, 12 mil hole to hole.
The short side of a generic pin header is the side that goes in the holes, so the long side is free to accept dupont sockets and shunts the same as if you had the same pins soldered in the pcb. So the cable is just ordinary programmer fly wires with female dupont ends. You don't even need to make an actual cable.
If space is tight on the pcb then it does use up more pcb than pads that leave the other side free. And pogo pins are going to be a lot faster for producing something in numbers.
I don't mind buying nice stuff like a fancy purpose made good-working tool for myself but I'm always making open source projects and one design goal is to require as little as possible, and as generic and universal as possible from the user. So I avoid fancy special things where possible. It's not designing for commercial production runs nor designing for one-off for myself, it's designing to a kind of a platonic ideal to strip away anything unnecessary and yet try to meet 2 opposing goals at the same time as much as possible: Don't require special tools that make things work reliably because of how fancy the tool is, and don't require the user to be a zen master craftsman that can attain a successful result with rocks and nails. Try to make the process reliable and repeatable while still only requiring basic materials and supplies. As much as possible anyway.
Pogo pins are pretty common these days and not exactly exotic or expensive any more so maybe I can start using them.
Then again, the through holes do 2 extra things besides make the connection.
With pads you need to aim/register the pins to land on the pads, and you need to hold them there. That means aiming with your eyes and holding with at least one hand, or it means adding some kind of extra registration and grabbing features to both the pcb and the cable, like extra drill holes or slots and extra plastic shapes on a special cable-end etc. Or no extra features on the board and instead a whole clamping jig that holds both the board and the pins.
Since these are holes that pins go in to, you don't need any other form of registration to aim the pins at the pads. The pins go in the holes.
And they hold onto the pins themselves, so you don't need any other form of retention.
It's just like plugging a plug into a socket where the socket provides all that naturally.
I have one board that needs two different connections like that, one for jtag and one for power and to temporarily close a jumper to write-enable the cpld. So a 4-pin and a 6-pin, 2 different cables in 2 different places. The entire board is slightly smaller than a DIP-28 so no room for any real connectors. You just stick the cables in and two different cables hold themselves with zero hands while you operate the flashing software. The wires are all plain dupont wires stuck on the pins, no solder, and 2 of the pins just have a generic jumper on them. It's completely basic and not-special and works perfect.
I have another board that needs 28 pins in a small space. For that one I used 2.0mm pitch pins in straight rows not staggered, but with the holes only 1.7mm apart. In that case it's the long side of the pins that goes into the holes, and the short side is soldered into a programming adapter pcb that goes into a programmer. The pins are in 2 sets of 2x7. Each set of 2x7 has 2 straight rows of 0.72mm holes 1.7mm apart. What happens there is, as the pins start to lean over, the top of the pins hit the opposite side of the hole on the top of the pcb, and don't want to go any further. The pins wedge solid and make 4 points of contact, 2 on bottom and 2 on top, and the board won't go any further even though the pins only just poke out the top and there is still almost 2mm of travel left. So you have a lot of remaining travel to just push a little more if you get a bad connection. It works great and no special parts anywhere.
Oooh that's a great trick! Thanks, I'll try that on my next board.
I had good experience with carefully spaced holes in PCB and a 50 mil header, see https://jacdac.github.io/jacdac-docs/ddk/firmware/jac-connec...
You might be interested in this "SKEDD" connector:
https://www.we-online.com/katalog/media/o210254v410%20ANE011...
https://www.digikey.com/en/products/detail/w%C3%BCrth-elektr...
I wish the cables weren't so expensive! They do wear out after a while; had one die that way. Using the 2030-NL STM32 6-pin one.
Same, enamored and I’m not even the EE. Elegant, no cost on the product side, and I don’t have to take the board out of the case to access it.
If you're interested in other PCB edge connectors, here's an HDMI one I designed:
https://forum.kicad.info/t/hdmi-pcb-edge-connector-for-raspb...
Doesn't it require ENIG? I wanted edge connector for my pcb project but it adds $20 to the price of pcb, that's just too much. Anyone knows card edge alternative? I'm thinking pin header but that's not very user friendly. Edge card can be inserted blindly even if you don't see the connector, pin header would probably just bend irl.
I've done HDMI edge connectors like this using plain HASL without too much trouble. Just don't forget to remove all soldermask on the connector path, they'll dirty out quickly otherwise.
But, now I do ENIG everywhere because it's often the same price as lead-free HASL (or so close it does not matter), while looking way cooler. I've started to take quite seriously leaded stuff now, especially since low temperature lead-free solder exists (SAC305).
ENIG sounds expensive right? Double the cost of your board or w/e? IMO it's no big deal because::
> solving routing puzzles isn't my idea of fun.
This just illustrates how different people are: I sometimes make PCBs just to route them! It's by far the most fun part for me.
the only people who gonna use this footprint is hobbists, and they care a lot about cost.
Eh for a hobbyist it's simpler and more robust to just put a connector on the board or use a test clip. I use clips like these: https://www.aliexpress.com/item/1005007622121847.html
You can choose your spacing: 1, 1.5, 2, or 2.54mm.
There are USB-A drives which do this, and in my experience they are far less durable than ones which have an actual connector. Given the thinness, this is going to be too easily snapped off.
I mostly use these for prototyping. Even gold-coated fingers still suffer from abrasion after many inserts so there is no way these are durable.
What PCB thickness is optimal? The USB-C tongue on a shieldless part I use is ~0.7mm, which is a pretty thin PCB.
They say "use 0.6 mmm"
https://x.com/AnasYMalas/status/1982060711670067350
That is a very thin PCB. For anyone reading this, 1.6mm is standard.
No…. It really depends where/what industry/what type/how many layers.
I would say 1.6mm is pretty thick but it depends.
Fully agree with the "it depends".
FWIW, my slightly more than anecdotal evidence is that 1.6mm is the default thickness at JLCPCB and PCBWay, and they will subtly encourage you to switch to that width if you don't want to pay more or wait longer for them to fill a sheet.
Every IC prototype board (eg Proto Advantage) and all of those Adafruit breakout boards are 1.6mm.
For these reasons, 1.6mm sure seems like a default if there is one. Is there some JEDEC standard or similar which proves me officially wrong? Happy to learn if so.
>For these reasons, 1.6mm sure seems like a default if there is one.
If you do consumer (phone/tablet/pc) a lot of boards are 0.8mm(12L) or 0.6mm for example.
If you do automotive/drones/industrial it’ll become thicker (2 oz copper).
DirtyPCB defaults to 1.2mm. I measured a couple random dev/breakout boards around and got 0.8/1.2/1.6.
It's not 1.6mm, it's actually 1/16", and it's been the standard since the days of yore. It's a super common inch measurement so it's not really a surprise to see it here, if you know your inches. There's tons of 1/16" plywood, for example.
A "thick" PCB was commonly 3/32" (0.093") and a "thin" one 1/32" (0.031"). Now of course it's all made in Asia so the metric dimensions predominate (0.8mm, 1.6mm, 2.4mm), but the legacy remains.
And of course PCBs aren't really any of these thicknesses, they're whatever the glass weaves press down to in the lamination press....
That's really interesting, thanks.
Your answer prompted me to do some further research. It's true that IPC-2221A does reference 1/16th as a historical precedent.
That said...
Lawrence Berkeley is an American institution, and it's fair to say that your perspective is American-centric. Without rehashing the ages old argument, it is still true that the US stands with Liberia and Myanmar in your steadfast refusal to standardize on the metric system.
It's your prerogative to conclude that this is an Asian thing, but it's very much an almost everyone else thing.
I will concede that it drives me nuts that not only does the lumber industry still use inches here, it's also officially and somehow legally not even accurate in inches. Why we can't have nice things...
Where does LBNL come into this? The reference in IPC-2221 is to NBS Report 4283 from 1956. Neither of those have anything much to do with LBNL.
I reject your assertion that my comments are America-centric. This a technology that was primarily developed in America and is now predominantly no longer manufactured there (Asia is not in America). It is rather natural for each place to use the units of measure they favor, so it is natural for what was a very common customary unit dimension of 1/16" to become a reasonably round metric dimension of 1.6mm. This is how things develop in the world.
Thanks for calling that out; the IPC-2221A doc I was viewing was on the LBNL domain and my brain incorrectly inferred that the folks who had worked on the IPC spec were employed by LBNL.
Still, IPC is also based in America, which brings us to the same place. While every org has to be based somewhere, the notion that the entire world should use imperial measurements simply because America does is pretty much the definition of America-centric in my books.
The ground truth is that we're talking about a de-facto standard, not a hard one. Given the actual difference between 1.6mm and 1/16", the ease of working in base 10, PCBs are mostly made in Asia and the flogged horse that the entire rest of the planet thinks in metric... it's no surprise to me that 1/16" has become a historical footnote.
I've found 0.8mm to make much more reliable connections, since the specification says that the tongue should be 0.7mm. 0.6mm will disconnect if the cable is angled in any way.
0.8mm is definitely out of USB 3.0 official spec and might damage the plug. The Spec requires 0.7mm with contacts and 0.6mm without, i.e., 0.05mm for the contact. See:
https://www.usb.org/sites/default/files/USB%20Type-C%20Spec%...
Pages 42 and 44.
+copper+ENIG is going to make that 0.7mm
i wonder how often you can plug/replug the connector in this case. how will the pcb material hold up? with my press-fit or clip-fit (is that a term?) 3d prints, ive noticed that 20 cycles can be sufficient to induce substantial 'loosening'.
It’s likely in the order of 10-30, especially with something like ENIG as a finish. If you wanted more cycles, you’d want to switch to a hard gold finish which would likely increase the cost substantially.
This is truly only for a debug port, not anything else.
Plug an OTG cable in and connect to that, so you don't repeat plug-unplug?
What about the force transferred by the connector wiggling? I think You'd need a very good mechanical design on the case to make it all work.
That's cool but I am not sure how a customer of mine would feel if I shipped a board to them like that. (I could see trying it on a project for myself, though.)
The problem with USB-C connectors for hobby projects is that they are ass to solder by hand—I’m still looking for one that would use a larger pitch by shorting the four USB pin pairs for either orientation. If you’re shipping something to a customer, I think it’s fair to assume that you don’t really have that problem :)
They're also ass to make PCBs for. The second you need 2oz or higher you start to really push the limits of what most prototype shops can do.
This is a pretty standard 2.0 receptacle, you've only got 0.2mm between pads if you follow their footprint (literally the limit for soldermask bridges on 2oz at JLCPCB): https://gct.co/download?type=PDFDrawing&name=USB4105.pdf
Get a hot air gun: it'll make your life way easier. You can tin the pads with a soldering iron, put the connector on and squirt some flux on the leads, and then just blow hot air until it reflows into place.
What do you do if the structural through-holes already have solder in them, that wick doesn’t seem to get? I’ve been trying to put a new USB C port onto my switch for quite a while now. (Now that I think about it, I can probably just shorten the prongs on the port and add solder after for structural strength).
A good solder sucker is your friend.
I have the SS-02, and I like it - I had one of the cheap blue ones first, but the pliable rubber tip really makes a difference. If you’re soldering smd by hand, it’s more than worth the $20
The answer to almost every question in soldering is 'more flux'. Solder wick has flux in the center of the braid, but it's hard to get it into tight places like structural through-holes. Adding your own liquid/paste flux will make the wick much more effective.
Melt the solder and thwack the board on something hard? So the board stops but the molten solder doesn't.
Sometimes though you just have to pile on solder and flux because the via is small enough that surface tension and heat dissipation means its never coming out
Doesn't a pump make quick work of this?
Frequently not. It's always handy to know about extra techniques in soldering.
You can also scale this up in a solder oven and remove almost every single component. Used this for reversing a PCB a few times.
A desoldering pump (manual model, $10 or so for a decent one) is very suitable for removing solder from through-holes, if that is the main issue.
I often add solder to make it easier for the wick to get everything. If the original assy was Lead-Free, using low temp solder (I can has lead? As a treat?) may make a difference here as well. Flux pen on the solder wick also seems to help especially if your wick is kinda crusty.
How would tinning those tiny pads not create a massive bridge between them? Does the bridge somehow go away in the reflow phase? (Not familiar with reflow at all)
Yes, the surface tension of melted solder pulls the solder to just the pad areas (assuming you don’t have far too much)
Make sure there is soldermask between the pads. This makes soldering much easier!
(If your foundry can't fabricate it, then make the pads thinner until they can fabricate the soldermask.)
Using with a little flux while tinning usually prevents the pads from bridging
To add to the sister comments, you can quite easily remove such bridges by adding flux and then touching each individual pad with a fine tipped soldering iron. It sometimes takes a few tries, but eventually the solder that’s touching the solder mask will either be wicked onto the iron or move onto one of the neighboring pads. (The trick is to touch just the pads with the iron, and not to try to attack the solder bridge itself.)
Do you find the 6-pin charge-only Type-C connectors too small? Or the 16-pin 2.0-only ones? They seem reasonably hand-solder-friendly but I admit I've been fortunate enough to have the factory handling them for me.
Yeah, I find the 16-pin ones a little beyond my skill. They also feel silly—why can’t I have one with just six pins for D±, VBUS, GND, and CC1/2? I guess I could have a factory make a bunch of modules like that for me, but it definitely feels like a thing that should already exist.
(There are passive A-to-C adapters, so I see no reason why I couldn’t short pin pairs like that.)
I have soldered the 12-pin, power-only USB-C connectors. The real breakthrough came though when I tried a hotplate rather than soldering iron for the USB-C connector.
You cannot do that because of how the connector flips over.
(Believe me, I have tried to make it work.)
Could you clarify? As far as I can tell, GND is A1/B1 and A12/B12, VBUS is A4/B4 and A9/B9, D+ is A6/B6, and D− is A7/B7, and each A pin swaps with its B counterpart when I flip the connector.
Only one side of the cable is going to be lit, but you don't know which one it is: it depends on whatever happened upstream. So you have to be able to handle either side being lit up. You can't easily do that with a single set of contacts because of how D+/D- is handled (it would be a literal X-shaped crossover), so now you're kind of stuck.
It ends up just not being worth the trouble if you need the USB 2.0 pair. But power-only is much easier and, guess what, pretty available in the market.
The 6-pin Type-C provides 2 pins each for power, ground, and CC. (DO NOT LEAVE CC OUT. THIS IS WHY A LOT OF RECENT USB STUFF MISBEHAVES. GET CC1/2 RIGHT PLEASE.)
The 16-pin adds 10 more: 4 for D+/D-, 2 more each for power and ground, and then they add 2 more for SBU as well. I'm not entirely sure why SBU is important enough but I'd guess it's because it's physically vertically next to CC so probably helps the mechanicals to leave it in.
There actually do exist 8-pin guys like this https://www.lcsc.com/product-detail/C47326494.html (among others) that add D+/D- only to the 6-pin connectors. I can't imagine they work terribly well most of the time but they must have some use? They do seem to be from Asian vendors only, which might mean something.
(Side note: the way Type-C handles D+ and D- has caused me so much pain. I get that it was a difficult problem to solve... but there had to be a better way than this, right? Probably not, but I can still whine.)
> There actually do exist 8-pin guys like this https://www.lcsc.com/product-detail/C47326494.html
I was glad to see this at first (because I did page through Mouser and LCSC a bit before I came back here to continue my bitching and found nothing). Then I actually looked at the drawing, and— Excuse me, is that really a USB-C socket that only works in one orientation?.. The drawing shows that the socket has both CC1 (A5) and CC2 (B5) but only one of the two copies of D+ (A6 but not B6) and D- (A7 but not B7). Seriously? Even I don’t hate my users that much.
Yep. I couldn't believe it existed either. I was even curious enough to ask an LLM about it and got the same response: it doesn't know of a use beyond creating frustration.
I guess past-me was smart when drawing USB-C connector symbols in my library and this one doesn't exist there for a reason!
This is very cool! What is the practical intent, given USB ports are 69c each? To save vertical space? I am thinking: Neat this is elegant and would work! But I can't think of any scenarios (off-the-cuff.) where I would choose this.
I have no idea how easy it is to implement this in KiCAD, but if it is - prototyping with this can be faster if you're eg making something like a DIY keyboard. Fewer things to solder, which is very nice if you struggle with it.
Here is a similar project in the sense that it uses no connectors on the PCBs, using a SOIC-8 clip to bite into the board. I think it's pretty clever.
https://github.com/SimonMerrett/SOICbite/
I was looking for this for a while!
Very clever packaging of a connector
[flagged]
[flagged]