i received the latest pre-production cards yesterday and have tested one of them: it works.
however (and this is the whole point of doing pre-production prototypes) in endeavouring to use automated assembly and solder paste it was discovered that the VIAs underneath the pads for the JAE DC3 Micro-HDMI connector are sucking the solder paste in and down, leaving the pins not properly connected.
the factory's engineer hand-soldered the 10 samples, but we cannot possibly do 1,000 PCBs by hand.... so it is necessary to do some test PCBs to work out how to get these connectors, with utterly tiny pins (0.25mm wide) to stick, given that the tracks simply have to come up from underneath using VIAs.
VIAs coming up on a pad is generally bad because it's a hole down which the solder paste simply... sucks down.
if anyone knows any tricks i would appreciate hearing them. i was thinking of creating the pad with a triangular end, placing the VIA right at the end so that the solder paste can't "wick away". anyone got any other ideas?
l.
--- crowd-funded eco-conscious hardware: https://www.crowdsupply.com/eoma68
On Jun 15, 2017 10:02 AM, "Luke Kenneth Casson Leighton" lkcl@lkcl.net wrote:
if anyone knows any tricks i would appreciate hearing them. [...] anyone got any other ideas?
Can you share a screenshot or PDF or imgur link to the PCB layout around the connector? A direct link to the GERBERs would work too.
On Thu, Jun 15, 2017 at 3:11 PM, Neil Jansen njansen1@gmail.com wrote:
Can you share a screenshot or PDF or imgur link
is the source code of the imgur proprietary service available so that i can host my own version of imgur without being monitored?
.... tell you what, i'll make a news update on a server that i have access to, where i know it's entirely libre-hosted software by people that i trust :)
http://rhombus-tech.net/allwinner_a10/news/
how's that? :)
so.. you can see, the right-hand pads are really *really* close to the edge of the PCB. so for that exact same reason it's impossible to bring the tracks in on the top layer.
now, examination of one of the samples which was not properly assembled (by hand), the DC3 connector was placed 1mm too far back.. but the pins were still successfully wired to the pads (right at the very end). so in theeeoorryyyy.... the left-most pads could be moved up to 1mm to the left, then the right-most pads extended so that extra amounts of solder paste can be dropped on them.
thoughts appreciated.
l.
On Thu, Jun 15, 2017 at 5:10 PM, Luke Kenneth Casson Leighton lkcl@lkcl.net wrote:
.... tell you what, i'll make a news update on a server that i have access to, where i know it's entirely libre-hosted software by people that i trust :)
http://rhombus-tech.net/allwinner_a10/news/
how's that? :)
Not bad, but you should be careful with your trust: that page has been vandalized, to restore, you should add back the missing "o":
http://rhombus-tech.net/allwinner_a10/news/EOMA68_A20_bottom.rev2.4.png instead of : http://rhombus-tech.net/allwinner_a10/news/EOMA68_A20_bottm.rev2.4.png
For the third picture to show up properly...
okaay so the HDMI connection isn't so hot on these 2.7.4 boards. it works... but there is significant line-interference under certain circumstances, even for 720p50. 1080p60 there is huge amounts of interference resulting in green horizontal lines. *sigh* i'll just have to have another go at the layout... blech.
2017-06-15 21:01 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
okaay so the HDMI connection isn't so hot on these 2.7.4 boards. it works... but there is significant line-interference under certain circumstances, even for 720p50. 1080p60 there is huge amounts of interference resulting in green horizontal lines. *sigh* i'll just have to have another go at the layout... blech.
How about having GND tracks parallel to each Tx/Rx pair. Creating a sink for EM signals to drain into instead of crossing over.
---GND----0 ---Tx------[ ] ---Rx------[ ] ---GND----0 ---Tx------[ ] ---Rx------[ ] ---GND----o
2017-06-16 8:55 GMT+02:00 mike.valk@gmail.com mike.valk@gmail.com:
2017-06-15 21:01 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
okaay so the HDMI connection isn't so hot on these 2.7.4 boards. it works... but there is significant line-interference under certain circumstances, even for 720p50. 1080p60 there is huge amounts of interference resulting in green horizontal lines. *sigh* i'll just have to have another go at the layout... blech.
How about having GND tracks parallel to each Tx/Rx pair. Creating a sink for EM signals to drain into instead of crossing over.
---GND----0 ---Tx------[ ] ---Rx------[ ] ---GND----0 ---Tx------[ ] ---Rx------[ ] ---GND----o
Looking at the schematics I see that is already being done. I do however see a lot of gaps between GND tracks. Especially on the blue layer.
Too bad the HDMI pads are so close to each other otherwise you could have had a GND track run between them fully enclosing the HS pads.
To the left I see that all HDMI tracks are routed trough some chips. What are those? Magnetics, impedance matchers? I mention that because on the blue tracks the'res a log of extra track for matching track length. maybe that should that be done before those chips.
Also the pads are shortened. I hope that's on purpose.
2017-06-16 9:33 GMT+02:00 mike.valk@gmail.com mike.valk@gmail.com:
2017-06-16 8:55 GMT+02:00 mike.valk@gmail.com mike.valk@gmail.com:
To the left I see that all HDMI tracks are routed trough some chips. What are those? Magnetics, impedance matchers? I mention that because on the blue tracks the'res a log of extra track for matching track length. maybe that should that be done before those chips.
Just a design thought on track length. Because of impedance matching HF tracks should be of equal length. And to minimize their EM emission the need to run parallel. But when changing direction you get an inner and outer track where the outer track becomes longer. To mitigate that you have those curly lines scattered around, usually at the end. Those cost a lot of room.
Since the schematics already show two layers with HF signal tracks why not place the Tx and Rx track on top of each other. Result: Parallel tracks. And very close to each other. Equal lengths on "curves". And minimize the curly tacks.
I know that this introduces issue when you need tracks crossing. But that could be solved by cross bridging... Hmm how am I going to visualize that in text....
T R x x | | Tx_____ / | | \ / | | o Tx/Rx---< | | >----Rx/Tx o | | / \Rx_____/ | | | |
ASCII art needs monospace font...
Tx/Rx on the left come in stacked. Before the bridge they split Rx passes a via to the Tx layer. leaving the Rx layer free for other tracks to pass on the Rx layer. After the bridge Tx passes the via the the previous Rx layer and Rx continues on the Tx layer, The swapped layers. Both Rx and Tx have passed a keeping a match via count for impedance matching.
On Fri, Jun 16, 2017 at 11:06 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
Since the schematics already show two layers with HF signal tracks why not place the Tx and Rx track on top of each other. Result: Parallel tracks.
the impedance of different layers is different, so no this does not work. or forces you to do a stack analysis. and simulations. which cost tens of thousands of dollars.
l.
Op 16 jun. 2017 15:57 schreef "Luke Kenneth Casson Leighton" <lkcl@lkcl.net
:
On Fri, Jun 16, 2017 at 11:06 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
Since the schematics already show two layers with HF signal tracks why not place the Tx and Rx track on top of each other. Result: Parallel tracks.
the impedance of different layers is different, so no this does not work. or forces you to do a stack analysis. and simulations. which cost tens of thousands of dollars.
Bleh. It looked so pretty in my mind. ;-(
So different layers have different copper thickness.
l.
_______________________________________________ arm-netbook mailing list arm-netbook@lists.phcomp.co.uk http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook Send large attachments to arm-netbook@files.phcomp.co.uk
On Fri, Jun 16, 2017 at 8:40 PM, mike.valk@gmail.com mike.valk@gmail.com wrote:
Bleh. It looked so pretty in my mind. ;-(
i knoow... btw can you possibly investigate why, when you hit "reply", the ">"s are not added?
So different layers have different copper thickness.
in a stack you tell the factory what thicknesses you want, as well as what material in between, and what thickness of that, too. so you get different capacitance on different layers. thus, the problem is: you cannot guarantee the impedance will be identical on different layers. so having differential pairs on different layers is the worst possible thing you could do.... *unless* you have access to PCB simulators. which are ultra-expensive.
l.
2017-06-17 11:17 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
On Fri, Jun 16, 2017 at 8:40 PM, mike.valk@gmail.com mike.valk@gmail.com wrote:
Bleh. It looked so pretty in my mind. ;-(
i knoow... btw can you possibly investigate why, when you hit "reply", the ">"s are not added?
I was using gmail in HTML mode, apparently. I've found a switch. Hopefully this works better.
N.B. Was this a problem before the auto HTML conversion on the list?
So different layers have different copper thickness.
in a stack you tell the factory what thicknesses you want, as well as what material in between, and what thickness of that, too. so you get different capacitance on different layers. thus, the problem is: you cannot guarantee the impedance will be identical on different layers. so having differential pairs on different layers is the worst possible thing you could do.... *unless* you have access to PCB simulators. which are ultra-expensive.
So it doesn't have to be a problem. As long as you control the layers that have traces have the same thicknesses.
.On Wed, Jun 21, 2017 at 9:35 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
2017-06-17 11:17 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
On Fri, Jun 16, 2017 at 8:40 PM, mike.valk@gmail.com mike.valk@gmail.com wrote:
Bleh. It looked so pretty in my mind. ;-(
i knoow... btw can you possibly investigate why, when you hit "reply", the ">"s are not added?
I was using gmail in HTML mode, apparently. I've found a switch. Hopefully this works better.
it does. yay!
N.B. Was this a problem before the auto HTML conversion on the list?
yes. i am constantly having to hand-edit people's replies to add line-breaks. it's been amazingly tedious.
in a stack you tell the factory what thicknesses you want, as well as what material in between, and what thickness of that, too. so you get
So it doesn't have to be a problem. As long as you control the layers that have traces have the same thicknesses.
technically correct but far too much risk and hassle. you end up tying the PCB layout to a specific PCB manufacturing factory.
l.
2017-06-21 13:00 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
.On Wed, Jun 21, 2017 at 9:35 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
2017-06-17 11:17 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
On Fri, Jun 16, 2017 at 8:40 PM, mike.valk@gmail.com mike.valk@gmail.com wrote:
i knoow... btw can you possibly investigate why, when you hit "reply", the ">"s are not added?
I was using gmail in HTML mode, apparently. I've found a switch. Hopefully this works better.
it does. yay!
For those wonder how. https://www.youtube.com/watch?v=kDP3VcmsYtg
in a stack you tell the factory what thicknesses you want, as well as what material in between, and what thickness of that, too. so you get
So it doesn't have to be a problem. As long as you control the layers that have traces have the same thicknesses.
technically correct but far too much risk and hassle. you end up tying the PCB layout to a specific PCB manufacturing factory.
Hmm. If only we could include parameterised sections in the design to accommodate that.
l.
arm-netbook mailing list arm-netbook@lists.phcomp.co.uk http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook Send large attachments to arm-netbook@files.phcomp.co.uk
On Wed, Jun 21, 2017 at 12:00:07PM +0100, Luke Kenneth Casson Leighton wrote:
.On Wed, Jun 21, 2017 at 9:35 AM, mike.valk@gmail.com
in a stack you tell the factory what thicknesses you want, as well as what material in between, and what thickness of that, too. so you get
So it doesn't have to be a problem. As long as you control the layers that have traces have the same thicknesses.
technically correct but far too much risk and hassle. you end up tying the PCB layout to a specific PCB manufacturing factory.
Are there high-frequency risks/problems with switching back and forth between the layer pair so that each trace travels equal distances on layer X and on layer Y?
Wolfram
On Wed, Jun 21, 2017 at 6:26 PM, Wolfram Kahl kahl@cas.mcmaster.ca wrote:
On Wed, Jun 21, 2017 at 12:00:07PM +0100, Luke Kenneth Casson Leighton wrote:
.On Wed, Jun 21, 2017 at 9:35 AM, mike.valk@gmail.com
in a stack you tell the factory what thicknesses you want, as well as what material in between, and what thickness of that, too. so you get
So it doesn't have to be a problem. As long as you control the layers that have traces have the same thicknesses.
technically correct but far too much risk and hassle. you end up tying the PCB layout to a specific PCB manufacturing factory.
Are there high-frequency risks/problems with switching back and forth between the layer pair
there are. the more VIAs you have the more EMI there is. R.F. (and HDMI is R.F.) does not travel in a straight line: if you have an abrupt change of direction (a corner or a VIA) the signal actually tries to just keep going in a straight line!
the best track layouts use curves not 45 degree transitions. the best layouts have no track changes at all, are as symmetrical as possible, are completely surrounded symmetrically by the exact same amount of space on either side, and the exact same number of vias on both sides of the track. and also are impedance matched in terms of distance between the pairs, width of the tracks, *and* the distance between layers *and* the dielectric constant of the insulation between the layers.
it's a pretty heavy-duty amount of requirements.
l.
2017-06-21 20:04 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
On Wed, Jun 21, 2017 at 6:26 PM, Wolfram Kahl kahl@cas.mcmaster.ca wrote:
On Wed, Jun 21, 2017 at 12:00:07PM +0100, Luke Kenneth Casson Leighton wrote:
.On Wed, Jun 21, 2017 at 9:35 AM, mike.valk@gmail.com
in a stack you tell the factory what thicknesses you want, as well as what material in between, and what thickness of that, too. so you get
So it doesn't have to be a problem. As long as you control the layers that have traces have the same thicknesses.
technically correct but far too much risk and hassle. you end up tying the PCB layout to a specific PCB manufacturing factory.
Are there high-frequency risks/problems with switching back and forth between the layer pair.
there are.
Every set of parallel wires act as both inductors and capacitors. https://www.engineersgarage.com/sites/default/files/imagecache/Original/wysi....
With DC inductance is less of a problem. But with HF signals you don't want return signals canceling out the main signal.
That's why the lines need to be parallel and of equal length.
And why I hate the length matching only on the end of the line.
the more VIAs you have the more EMI there is. R.F. (and HDMI is R.F.)
HDMI is HF, High frequency, which causes RF, Radio Frequency's, emissions.
EMI, Elektro Magnetic Interference, is the result of RF hitting your signal line and creating noise and distortion.
Every electrical current causes an EM field. But with DC it is static. With HF is dynamic making to harder to read the signal properly and without errors.
the best track layouts use curves not 45 degree transitions.
That might not be true. Curves might actually be more problematic. When the signal hits a wall it deflects. Like light on a mirror. With curves the signal starts bouncing in zigzag pattern. Making the distance traveled more unpredictable. And in worst case the signal starts traveling backwards creating echo's.
HF Signals also tend to move on the outside of a conductor/track.
I guess that's why via's are so bad. The are round and change route at 90 degrees, downward or upward. So the signal starts bouncing and echoing. Creating RF noise.
But with BGA IC's you have no other option than to use VIA's and sometimes signals need to cross so you have to as well.
the best layouts have no track changes at all, are as symmetrical as possible, are completely surrounded symmetrically by the exact same amount of space on either side, and the exact same number of vias on both sides of the track. and also are impedance matched in terms of distance between the pairs, width of the tracks, *and* the distance between layers *and* the dielectric constant of the insulation between the layers.
it's a pretty heavy-duty amount of requirements.
l.
arm-netbook mailing list arm-netbook@lists.phcomp.co.uk http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook Send large attachments to arm-netbook@files.phcomp.co.uk
Luke Kenneth Casson Leighton lkcl@lkcl.net writes:
.On Wed, Jun 21, 2017 at 9:35 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
2017-06-17 11:17 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
On Fri, Jun 16, 2017 at 8:40 PM, mike.valk@gmail.com mike.valk@gmail.com wrote:
Bleh. It looked so pretty in my mind. ;-(
i knoow... btw can you possibly investigate why, when you hit "reply", the ">"s are not added?
I was using gmail in HTML mode, apparently. I've found a switch. Hopefully this works better.
it does. yay!
N.B. Was this a problem before the auto HTML conversion on the list?
yes. i am constantly having to hand-edit people's replies to add line-breaks. it's been amazingly tedious.
Hi Luke,
Does whatever is your favoured editor not have a widget for that sort of thing?
In notmuch+emacs one is editing mails in emacs Message mode, which means you can re-wrap a paragraph, with the quotes being done as one would hope, by simply hitting M-q (Alt-q on my keyboard) when in the offending paragraph.
While one could spend one's life trying to teach people how these things were generally done in the '80s, I came to the conclusion that the steady influx of Internet newbies meant that became a Sisyphean task some time in the '90s, and then got significantly worse when Microsoft inflicted a mail client on the world that punishes people for using email the way we'd prefer.
Using better tools seems likely to be the shorter route to inner calm.
Having said that, I did try to persuade Ron to edit out the 'Original Message' line of his mails, since that makes emacs ignore the whole mail as an empty top-post. He managed to do it a couple of times before the strain became too much, so he was trying before he became trying ;-)
On the plus side, people that resolutely stick to talking in their own preferred style, rather than taking into account the preferred style of their audience, helpfully tag themselves as not being worth one's time.
Cheers, Phil.
Hi,
On Thu, Jun 22, 2017 at 10:28:21AM +0200, Philip Hands wrote:
Luke Kenneth Casson Leighton lkcl@lkcl.net writes:
yes. i am constantly having to hand-edit people's replies to add line-breaks. it's been amazingly tedious.
Does whatever is your favoured editor not have a widget for that sort of thing?
I usually use 'fmt' to create line-breaks semi-automatically. Many text editors for Unix like systems (e.g. vi) allow to invoke external programs as filters to manipulate (part of) the text.
Example for vim to insert line-breaks into the current line:
:.,.!fmt
Example for vim to re-adjust line-breaks of a paragraph:
!}fmt
But you all knew this already anyway. ;)
It still is more tedious to have to adjust the text for a reply than to just have a nicely formatted plain text mail to start with.
Thanks, Erik
On Thu, Jun 15, 2017 at 11:10 AM, Luke Kenneth Casson Leighton < lkcl@lkcl.net> wrote:
is the source code of the imgur proprietary service available so that i can host my own version of imgur without being monitored?
Lol, no clue, dude. imgur is what us plebs without principles or motivation use :-) Use whatever works for you.
so.. you can see, the right-hand pads are really *really* close to the edge of the PCB. so for that exact same reason it's impossible to bring the tracks in on the top layer.
OK so if I were laying that out, I wouldn't ever put a via in the middle of a pad, not a full time electrical engineer, I only do hobby boards in quantities of less than 100. Tomorrow I'll ask around at work to see if any of the EE's have any advice. They do all sorts of crazy things in a production environment that I would never dream of.
On Fri, Jun 16, 2017 at 3:47 AM, Neil Jansen njansen1@gmail.com wrote:
so.. you can see, the right-hand pads are really *really* close to the edge of the PCB. so for that exact same reason it's impossible to bring the tracks in on the top layer.
OK so if I were laying that out, I wouldn't ever put a via in the middle of a pad,
there's not really any other options: you can see how little clearance there is to the edge of the board: it's flat-out impossible to bring tracks in either in between those two sets, or round the back... and you don't want to anyway: they're differential pairs (up to 1ghz clock rate) because this is HDMI.
not a full time electrical engineer, I only do hobby boards in quantities of less than 100. Tomorrow I'll ask around at work to see if any of the EE's have any advice. They do all sorts of crazy things in a production environment that I would never dream of.
there's a way - it just has to be found.
l.
2017-06-16 8:19 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
there's not really any other options: you can see how little clearance there is to the edge of the board: it's flat-out impossible to bring tracks in either in between those two sets, or round the back... and you don't want to anyway: they're differential pairs (up to 1ghz clock rate) because this is HDMI.
Hmm. Then how are other users of this connector doing it? This seems like a generic problem. The solder technique is generic afaikt. 1. Either they are using smaller width tracks and are passing between the left hand pads. 2. They have via's right to the pads. But that's very close to the edge.
The options I see... . find other schematics using this connector. . Use smaller width tracks. . Cut the pads tight a little shorter and place the via's to the right creating a bottleneck but stil far enough from the edge . The above but to the left, via's in the middle.
On Fri, Jun 16, 2017 at 7:51 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
2017-06-16 8:19 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
there's not really any other options: you can see how little clearance there is to the edge of the board: it's flat-out impossible to bring tracks in either in between those two sets, or round the back... and you don't want to anyway: they're differential pairs (up to 1ghz clock rate) because this is HDMI.
Hmm. Then how are other users of this connector doing it? This seems like a generic problem. The solder technique is generic afaikt.
- Either they are using smaller width tracks and are passing between the
left hand pads.
like i said: there's not enough room to get that many tracks between the pads, and it would violate differential-pair rules to do so.
- They have via's right to the pads. But that's very close to the edge.
exactly.
The options I see... . find other schematics using this connector.
none.
. Use smaller width tracks.
can't.
. Cut the pads tight a little shorter and place the via's to the right creating a bottleneck but stil far enough from the edge
possible.
. The above but to the left, via's in the middle.
possible but risky.
2017-06-16 8:54 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
On Fri, Jun 16, 2017 at 7:51 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
. Use smaller width tracks.
can't.
Was afraid of that
. Cut the pads tight a little shorter and place the via's to the right creating a bottleneck but stil far enough from the edge
possible.
. The above but to the left, via's in the middle.
possible but risky.
Depends on how near to can get to left hand pads or the egde on the right and were the pads in the connector have most tolerance.
Speaking of near the edge. The tracks on the board seem awfully close the boards cutoff edge. Doesn't that create a problem for cutting them out?
On Fri, Jun 16, 2017 at 8:03 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
. Cut the pads tight a little shorter and place the via's to the right creating a bottleneck but stil far enough from the edge
possible.
. The above but to the left, via's in the middle.
possible but risky.
Depends on how near to can get to left hand pads or the egde on the right and were the pads in the connector have most tolerance.
Speaking of near the edge. The tracks on the board seem awfully close the boards cutoff edge.
yyep they are.
Doesn't that create a problem for cutting them out?
no but it does cause an imbalance in the differential pairs unless the tracks come in dead-straight from the left, and it also means that ground shielding isn't possible.
normally the connector would be at least 20-30 mil away from the edge so that ground vias could be placed all along the right-hand edge. that's near-flat-out impossible. the best that can be hoped for is that the three pins (in grey) which are GND will do the job of creating an EMI shield instead.
l.
2017-06-16 9:07 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
On Fri, Jun 16, 2017 at 8:03 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
Speaking of near the edge. The tracks on the board seem awfully close the boards cutoff edge.
yyep they are.
Doesn't that create a problem for cutting them out?
no but it does cause an imbalance in the differential pairs unless the tracks come in dead-straight from the left, and it also means that ground shielding isn't possible.
normally the connector would be at least 20-30 mil away from the edge so that ground vias could be placed all along the right-hand edge. that's near-flat-out impossible. the best that can be hoped for is that the three pins (in grey) which are GND will do the job of creating an EMI shield instead.
I was talking about the photo's not the connector.
On Thu, Jun 15, 2017 at 11:10 AM, Luke Kenneth Casson Leighton < lkcl@lkcl.net> wrote:
After thinking about it a bit more, what about a blind via? They can even be filled with copper by the board house. I'm assuming this is a 6-ish layer board, yea?
Since you didn't mention that it was blind or otherwise, i'm assuming you have regular-old normal vias, probably non-tented? A blind via will by the very physics and geometry wick away less solder, because it takes up less volume. And if it's filled with copper or whatever the board house can fill them with, it will take up no solder at all.
See 'A', 'B', and 'C' on the (GASP!) imgur link. http://imgur.com/a/L0lmS
Would this work?
Hi, about vias, some PCB houses have special technique for vias in a pad (VIP for short). Look up on YT how it's done. Here is one of results from quick search https://www.pcbcart.com/pcb-capability/via-in-pad.html
16 cze 2017 14:53 "Neil Jansen" njansen1@gmail.com napisał(a):
On Thu, Jun 15, 2017 at 11:10 AM, Luke Kenneth Casson Leighton < lkcl@lkcl.net> wrote:
After thinking about it a bit more, what about a blind via? They can even be filled with copper by the board house. I'm assuming this is a 6-ish layer board, yea?
Since you didn't mention that it was blind or otherwise, i'm assuming you have regular-old normal vias, probably non-tented? A blind via will by the very physics and geometry wick away less solder, because it takes up less volume. And if it's filled with copper or whatever the board house can fill them with, it will take up no solder at all.
See 'A', 'B', and 'C' on the (GASP!) imgur link. http://imgur.com/a/L0lmS
Would this work? _______________________________________________ arm-netbook mailing list arm-netbook@lists.phcomp.co.uk http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook Send large attachments to arm-netbook@files.phcomp.co.uk
On Fri, Jun 16, 2017 at 2:44 PM, Marek Pikuła marek@pikula.co wrote:
Hi, about vias, some PCB houses have special technique for vias in a pad (VIP for short). Look up on YT how it's done. Here is one of results from quick search https://www.pcbcart.com/pcb-capability/via-in-pad.html
interesting. so... they plug the VIA with resin then put copper on top of that. i'll run it by mike's factory, see if he's heard of it.
l.
I'm on mobile at work, I've confirmed with an EE here that does this sort of thing all the time.
The good news is that your easiest bet is to just ask the board house to fill the vias with epoxy, they can plate over that, and it's very common these days. He said that filling a normal via (not blind or buried) with epoxy is going to be cheaper than what I previously proposed (using blind vias).
The better news is that you can actually rework your current boards by filling the offending vias with epoxy, if they're otherwise usable. A pneumatic shot dispense system would be needed but they're cheap and available now thanks to China.
There isn't really any bad news. He said it's extremely common, we do it probably 100's of times on our boards at work , which are incredibly dense and expensive. No issues at all, it's extremely reliable to do this, even across temperature ranges and vibration.
On Fri, Jun 16, 2017 at 2:59 PM, Neil Jansen njansen1@gmail.com wrote:
I'm on mobile at work, I've confirmed with an EE here that does this sort of thing all the time.
The good news is that your easiest bet is to just ask the board house to fill the vias with epoxy,
awesome. that's two great ideas. via-over-pad (which involves resin-filling as well).
l.
Op 16 jun. 2017 16:03 schreef "Luke Kenneth Casson Leighton" <lkcl@lkcl.net
:
On Fri, Jun 16, 2017 at 2:59 PM, Neil Jansen njansen1@gmail.com wrote:
I'm on mobile at work, I've confirmed with an EE here that does this sort of thing all the time.
The good news is that your easiest bet is to just ask the board house to fill the vias with epoxy,
awesome. that's two great ideas. via-over-pad (which involves resin-filling as well).
So the PCB factory is not the party populating the board?
l.
_______________________________________________ arm-netbook mailing list arm-netbook@lists.phcomp.co.uk http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook Send large attachments to arm-netbook@files.phcomp.co.uk
On Fri, Jun 16, 2017 at 8:44 PM, mike.valk@gmail.com mike.valk@gmail.com wrote:
So the PCB factory is not the party populating the board?
correct. PCB manufacturing is a specialist task. PCB assembly is a specialist task. larger companies can be big enough to have both sets of specialists and equipment in-house. mike's factory is not one such company.
l.
On Fri, 16 Jun 2017 15:01:08 +0100 Luke Kenneth Casson Leighton lkcl@lkcl.net wrote:
On Fri, Jun 16, 2017 at 2:59 PM, Neil Jansen njansen1@gmail.com wrote:
I'm on mobile at work, I've confirmed with an EE here that does this sort of thing all the time.
The good news is that your easiest bet is to just ask the board house to fill the vias with epoxy,
awesome. that's two great ideas. via-over-pad (which involves resin-filling as well).
l.
How about a third? I'm no EE (I'd like to be, but that's another story), so take this with a grain of salt. Use kapton tape to cover the holes. That will resist the heat the down and up side being that you have to manually apply and remove it afterwards and it will not leave a trace like epoxy so you can use the VIA holes.
Sincerely, David
On Sat, Jun 17, 2017 at 3:30 AM, David Niklas doark@mail.com wrote:
How about a third? I'm no EE (I'd like to be, but that's another story), so take this with a grain of salt. Use kapton tape to cover the holes. That will resist the heat the down and up side being that you have to manually apply and remove it afterwards and it will not leave a trace like epoxy so you can use the VIA holes.
nice idea... *thinks*... the holes are 6mil (0.15mm) wide. i would be concerned that tape would let air through, or would house an air bubble underneath. if epoxy resin is a standard technique that's been tried, tested and proven, i'd prefer it.
l.
On Fri, Jun 16, 2017 at 1:51 PM, Neil Jansen njansen1@gmail.com wrote:
After thinking about it a bit more, what about a blind via?
no. they're insanely expensive and only justifiable with very high MOQs. current PCB costs are only around $1.50 in volume. prototyping costs would be through the roof.
for this project the PCB has to be manufacturable at reasonable cost in small all the way up to mass volume.
l.
On 16 Jun 2017, at 12:02 AM, Luke Kenneth Casson Leighton lkcl@lkcl.net wrote:
...
if anyone knows any tricks i would appreciate hearing them. i was thinking of creating the pad with a triangular end, placing the VIA right at the end so that the solder paste can't "wick away". anyone got any other ideas?
l.
Is it an issue of gravity? Perhaps it might be possible to apply the solder paste to the board in an upside down orientation (or even just at a high angle)?
On Thu, Jun 15, 2017 at 3:16 PM, Bluey bluey@smallfootprint.info wrote:
Is it an issue of gravity? Perhaps it might be possible to apply the solder paste to the board in an upside down orientation (or even just at a high angle)?
the solder paste is applied with a stencil and (literally) a squeegee. it sticks quite happily, and stays there even if the board's upside-down.
the problem is not the solder paste as it's applied, but when the board's put into the oven. that's where, when it reaches melting temperature (240C or so?) it flows into the via holes... which are something like 0.15mm wide (6 mil, aka 6 1/000ths of an inch).
given that the pads themselves are only 7mil (0.2mm) wide, and only about 25mil (1mm appx) long, there's far too little solder paste so it just gets sucked down the hole.
you cannot place the components upside-down on the PCB before they go into the oven, if you do that they will simply fall off.
l.
2017-06-15 16:02 GMT+02:00 Luke Kenneth Casson Leighton lkcl@lkcl.net:
i received the latest pre-production cards yesterday and have tested one of them: it works.
however (and this is the whole point of doing pre-production prototypes) in endeavouring to use automated assembly and solder paste it was discovered that the VIAs underneath the pads for the JAE DC3 Micro-HDMI connector are sucking the solder paste in and down, leaving the pins not properly connected.
How about placing the connector on a small flex-PCB and then connect the flex-PCB to the hard-PCB? Then you don't have to worry about the correct mount height of the connector, leaving you with a bigger variety of connectors. But then you'll need find another way to fixate the connectors to the card housing. 3D print?
Also you can test connectors independently of the whole board.
I understand such a change might be to big to do in terms of time and costs.
Just trying to think outside the box here ;-)
On Wed, Jun 21, 2017 at 9:43 AM, mike.valk@gmail.com mike.valk@gmail.com wrote:
How about placing the connector on a small flex-PCB and then connect the flex-PCB to the hard-PCB? Then you don't have to worry about the correct mount height of the connector, leaving you with a bigger variety of connectors.
a... a... oh! awesome idea! actually might be able to get away with a separate daughterboard. can't use a flex PCB, mounting these connectors is enough of a bitch as it is.
But then you'll need find another way to fixate the connectors to the card housing. 3D print?
PCB interlocks. size of cutout matches size of daughterboard.
Also you can test connectors independently of the whole board.
very true.
I understand such a change might be to big to do in terms of time and costs.
space. and EMI (over the connector).
Just trying to think outside the box here ;-)
i could potentially try it for the passthrough card, which is a lower production cost.
l.
arm-netbook@lists.phcomp.co.uk
-
Bluey -
David Niklas -
Erik Auerswald -
Luke Kenneth Casson Leighton -
Marek Pikuła -
mike.valk＠gmail.com -
Neil Jansen -
Philip Hands -
Vincent Legoll -
Wolfram Kahl