[Arm-netbook] EOMA68-A20 2.7.4 pre-production prototypes received and working

[Luke Kenneth Casson Leighton]

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

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-n

[Neil Jansen]

On Jun 15, 2017 10:02 AM, "Luke Kenneth Casson Leighton" <***@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.
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@fil

[Luke Kenneth Casson Leighton]

Post by Neil Jansen
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachment

[Vincent Legoll]

On Thu, Jun 15, 2017 at 5:10 PM, Luke Kenneth Casson Leighton

Post by Luke Kenneth Casson Leighton
.... 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":

Loading Image...
instead of :
Loading Image...

For the third picture to show up properly...

[Luke Kenneth Casson Leighton]

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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-netboo

[m***@gmail.com]

Post by Luke Kenneth Casson Leighton
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
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large

[m***@gmail.com]

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton
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.
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-netbook@

[m***@gmail.com]

Post by m***@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.
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attach

[Luke Kenneth Casson Leighton]

Post by m***@gmail.com
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@files.phcomp.co

[m***@gmail.com]

Post by m***@gmail.com
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-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@files.phcomp.co.uk
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook

[Luke Kenneth Casson Leighton]

Post by m***@gmail.com
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?

Post by m***@gmail.com
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachm

[m***@gmail.com]

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com
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?

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@f

[Luke Kenneth Casson Leighton]

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com
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!

Post by m***@gmail.com
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.

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@files.phc

[m***@gmail.com]

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton
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.

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton
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.

Post by Luke Kenneth Casson Leighton
l.
_______________________________________________
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to

[Wolfram Kahl]

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton
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

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-n

[Luke Kenneth Casson Leighton]

Post by Wolfram Kahl

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to a

[m***@gmail.com]

Post by Luke Kenneth Casson Leighton

Post by Wolfram Kahl

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton
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.
Loading Image....

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.

Post by Luke Kenneth Casson Leighton
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.

Post by Luke Kenneth Casson Leighton
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.

Post by Luke Kenneth Casson Leighton
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.
_______________________________________________
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-netb

[Philip Hands]

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com
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!

Post by m***@gmail.com
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.

[Erik Auerswald]

Hi,

Post by Philip Hands

Post by Luke Kenneth Casson Leighton
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

[Neil Jansen]

On Thu, Jun 15, 2017 at 11:10 AM, Luke Kenneth Casson Leighton <

Post by Luke Kenneth Casson Leighton
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.

Post by Luke Kenneth Casson Leighton
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.
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@files.phcomp.co.u

[Luke Kenneth Casson Leighton]

Post by Neil Jansen

Post by Luke Kenneth Casson Leighton
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.

Post by Neil Jansen
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Sen

[m***@gmail.com]

Post by Luke Kenneth Casson Leighton
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.
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send lar

[Luke Kenneth Casson Leighton]

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton
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.

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.

Post by m***@gmail.com
2. They have via's right to the pads. But that's very close to the edge.

exactly.

Post by m***@gmail.com
The options I see...
. find other schematics using this connector.

none.

Post by m***@gmail.com
. Use smaller width tracks.

can't.

Post by m***@gmail.com
. 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.

Post by m***@gmail.com
. The above but to the left, via's in the middle.

possible but risky.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-netbook@

[m***@gmail.com]

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com
. Use smaller width tracks.

can't.

Was afraid of that

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com
. 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.

Post by m***@gmail.com
. 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?
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attach

[Luke Kenneth Casson Leighton]

Post by m***@gmail.com

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com
. 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.

Post by m***@gmail.com
. 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.

Post by m***@gmail.com
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@f

[m***@gmail.com]

Post by Luke Kenneth Casson Leighton

Post by m***@gmail.com
Speaking of near the edge. The tracks on the board seem awfully close the
boards cutoff edge.

yyep they are.

Post by m***@gmail.com
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.
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-netb

[Neil Jansen]

On Thu, Jun 15, 2017 at 11:10 AM, Luke Kenneth Casson Leighton <

Post by Luke Kenneth Casson Leighton
http://rhombus-tech.net/allwinner_a10/news/

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-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large

[Marek Pikuła]

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" <***@gmail.com> napisał(a):

On Thu, Jun 15, 2017 at 11:10 AM, Luke Kenneth Casson Leighton <

Post by Luke Kenneth Casson Leighton
http://rhombus-tech.net/allwinner_a10/news/

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-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@files.phcomp.co.uk
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments t

[Luke Kenneth Casson Leighton]

Post by Marek Pikuła
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-

[Neil Jansen]

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.
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachmen

[Luke Kenneth Casson Leighton]

Post by Neil Jansen
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-netbook

[m***@gmail.com]

Post by Neil Jansen
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-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@files.phcomp.co.uk
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments

[Luke Kenneth Casson Leighton]

Post by m***@gmail.com
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@file

[David Niklas]

On Fri, 16 Jun 2017 15:01:08 +0100

Post by Luke Kenneth Casson Leighton

Post by Neil Jansen
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

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-netbook@

[Luke Kenneth Casson Leighton]

Post by David Niklas
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-n

[Luke Kenneth Casson Leighton]

Post by Neil Jansen
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@file

[Bluey]

Post by Luke Kenneth Casson Leighton
...
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)?


_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments t

[Luke Kenneth Casson Leighton]

Post by Bluey
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.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments t

[Andrew Bolin]

Date: Thu, 15 Jun 2017 15:02:07 +0100
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.
...

if anyone knows any tricks i would appreciate hearing them.
Can you enlarge the solder mask for these pads, thus providing enough
solder to both fill the via and make the connection?

This is the standard recommendation when using thermal pads / thermal vias.
_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-netbook

[Luke Kenneth Casson Leighton]

On Sun, Jun 18, 2017 at 11:57 PM, Andrew Bolin

Post by Andrew Bolin
Can you enlarge the solder mask for these pads, thus providing enough
solder to both fill the via and make the connection?
This is the standard recommendation when using thermal pads / thermal vias.

indeed. this was the recommendation of mike, at the factory. there
is however veery little room to do that.

buut... *deep breath*... a closer examination of the 10 samples shows
that the DC3 connector is more complex than i initially thought. the
4 through-hole ground connectors on the metal case are not just simple
through-hole pins: the two back ones have an additional lip which i
did not anticipate being there.

looking at the datasheet this "lip" is supposed to be in direct
contact with the board (not down a hole or over the edge of the PCB or
anything) but that does not explain why the outer set of pins are in
contact with the PCB but the inner set are not.

the only thing that i can think of is: either the connector was
damaged during (as part of) its installation with a heat-gun, or it
was already damaged and the outer pins bent downwards.

i'll have to inspect the samples i have here more closely.

l.

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-

[m***@gmail.com]

Post by Luke Kenneth Casson Leighton
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 ;-)

_______________________________________________
arm-netbook mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-***@fil

[Luke Kenneth Casson Leighton]

Post by m***@gmail.com
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.

Post by m***@gmail.com
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.

Post by m***@gmail.com
Also you can test connectors independently of the whole board.

very true.

Post by m***@gmail.com
I understand such a change might be to big to do in terms of time and costs.

space. and EMI (over the connector).

Post by m***@gmail.com
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 mailing list arm-***@lists.phcomp.co.uk
http://lists.phcomp.co.uk/mailman/listinfo/arm-netbook
Send large attachments to arm-netbook