Maker Pro
Maker Pro

PCB manufacture

R

rickman

Jan 1, 1970
0
I had some PCBs made with 22 boards per panel (small boards). I
wanted a single panel for prototypes, but it turned out I could get 6
panels for only $500 more. This would get me through the first round
of production if I didn't need any changes. The day the maker was
supposed to ship them, I got an email saying they had a poor yield and
only got 116 good boards out of 7 panels vs the 132 I ordered.

So now I have a concern about the quality of the boards. I was told
the failed boards had problems with the plating in the 10 mil holes I
used for vias. They claim that the "good" boards have no quality
issues. My concern is that the vias may be marginal and open once
they are temperature cycled a bit.

I am not sure how to handle this with the vendor. I guess I could
just flat out tell them that I am concerned with investing some
$18,000 building up over 100 boards only to have my customer see
failures in the field. I don't feel like they have done 100% on this
since they did not provide the quantity I requested.

They have offered to rebuild the entire set of panels if I am not
happy with the result, but that would be a week delay. I also don't
know if they are willing to let me use one of the current panels and
remake the rest.

Anyone have experience with 10 mil via holes and reliability issues?
If you have a problem with an order like this, is it reasonable to use
one panel and reject the rest?
 
L

linnix

Jan 1, 1970
0
Anyone have experience with 10 mil via holes and reliability issues?
If you have a problem with an order like this, is it reasonable to use
one panel and reject the rest?

As you have figured-out, pushing the process limit could be
expensive. We would not go below 16 mil holes, even if we need bigger
boards. Are you sure you can't use bigger holes?
 
R

rickman

Jan 1, 1970
0
As you have figured-out, pushing the process limit could be
expensive. We would not go below 16 mil holes, even if we need bigger
boards. Are you sure you can't use bigger holes?

Sure, I can use bigger holes. But I can't use bigger pads. It was
hard enough to make the layout work with 10 mil holes and 24 mil
pads. This board is very small and defined by the customer's
requirements. It is a daughter card on an existing product so I have
no flexibility in size except for extending one end which I have
already done as much as possible. Even that does not do a lot for the
density issue since the board is over 5 times longer than it is wide.
Extending the length more just means I have longer lines to try to
squeeze through the same bottlenecks around the chips and
connectors.

I guess I am confused about "process limits". I have seen vendors
that claim to have capability for hole sizes down to 6 mil. They just
say that they can't guarantee that the hole will not be plated closed
which is fine with me. So I don't see where 10 mil holes should be a
real issue. Did I pick a poor PCB maker? Am I just not grasping the
realities of PCB manufacturing?
 
D

DaveN

Jan 1, 1970
0
rickman said:
Sure, I can use bigger holes. But I can't use bigger pads. It was
hard enough to make the layout work with 10 mil holes and 24 mil
pads. This board is very small and defined by the customer's
requirements. It is a daughter card on an existing product so I have
no flexibility in size except for extending one end which I have
already done as much as possible. Even that does not do a lot for the
density issue since the board is over 5 times longer than it is wide.
Extending the length more just means I have longer lines to try to
squeeze through the same bottlenecks around the chips and
connectors.

I guess I am confused about "process limits". I have seen vendors
that claim to have capability for hole sizes down to 6 mil. They just

Did the vendor you chose give this claim? If not then there's your problem,
choose a different vendor.
 
D

DaveN

Jan 1, 1970
0
DaveN said:
Did the vendor you chose give this claim? If not then there's your
problem, choose a different vendor.

Sorry, I meant did your vendor make the claim on 10mil?

Additionally did you order 132 boards or the yield acheived from the panels?

The realities with any process is that as you approach its limits, you will
get higher fallout; edges of the bell curve and all that.

If your supplier is telling you that parts have failed then it tends to
suggest that they have a reasonable quality system in place. They know the
process and its limits and are therefore testing for those failures. It's
an old but true saying that you can't test in quality, you can only design
for it.
 
W

Wingle

Jan 1, 1970
0
Sure, I can use bigger holes. But I can't use bigger pads. It was
hard enough to make the layout work with 10 mil holes and 24 mil
pads. This board is very small and defined by the customer's
requirements. It is a daughter card on an existing product so I have
no flexibility in size except for extending one end which I have
already done as much as possible. Even that does not do a lot for the
density issue since the board is over 5 times longer than it is wide.
Extending the length more just means I have longer lines to try to
squeeze through the same bottlenecks around the chips and
connectors.

I guess I am confused about "process limits". I have seen vendors
that claim to have capability for hole sizes down to 6 mil. They just
say that they can't guarantee that the hole will not be plated closed
which is fine with me. So I don't see where 10 mil holes should be a
real issue. Did I pick a poor PCB maker? Am I just not grasping the
realities of PCB manufacturing?

I am looking at a fab right now that is a mix of 10 and 7 mil drilled
vias. Board has 8 BGA and is 2x7" so your process is not in any way
pushing the envelope. If you are getting bad plating in 10mil vias
then the most likely cause is insufficient agitation during the
plating and air bubbles were trapped in the vias. You will need to
section (slice & dice) the failing fabs to confirm whether the plating
is actually thick enough across the whole of the fab. If it is air
bubbles you are probably okay as that usually is batch related. If it
is a function of the vendor skimping on the plating, you are screwed.

That being said, I have no empirical data but there does seem to have
been an increase in the failure rate of commercial fabs in the last
year or two. Usually in the plating of the vias. This is across
several vendors US & Asian.
 
Q

qrk

Jan 1, 1970
0
I had some PCBs made with 22 boards per panel (small boards). I
wanted a single panel for prototypes, but it turned out I could get 6
panels for only $500 more. This would get me through the first round
of production if I didn't need any changes. The day the maker was
supposed to ship them, I got an email saying they had a poor yield and
only got 116 good boards out of 7 panels vs the 132 I ordered.

So now I have a concern about the quality of the boards. I was told
the failed boards had problems with the plating in the 10 mil holes I
used for vias. They claim that the "good" boards have no quality
issues. My concern is that the vias may be marginal and open once
they are temperature cycled a bit.

I am not sure how to handle this with the vendor. I guess I could
just flat out tell them that I am concerned with investing some
$18,000 building up over 100 boards only to have my customer see
failures in the field. I don't feel like they have done 100% on this
since they did not provide the quantity I requested.

They have offered to rebuild the entire set of panels if I am not
happy with the result, but that would be a week delay. I also don't
know if they are willing to let me use one of the current panels and
remake the rest.

Anyone have experience with 10 mil via holes and reliability issues?
If you have a problem with an order like this, is it reasonable to use
one panel and reject the rest?

At least they have a good enough quality control that they can spot
this problem. You can have them do a cross section of a good board to
see if the vias look healthy.

Plating systems have to be top-notch to handle small via sizes. If the
board house hasn't kept up on updating their equipment, they will have
problems with small features.

I routinely use 8mil drill with 15mil pads. The pad size is marginal,
but the four board houses I have used never had problems with that via
size for the past 5 to 8 years.

There is one case back in the early 90s where the plated through holes
would disconnect when moderate current (apx 1 amp) passed thru the
plated hole after soldering. Before soldering, the PTH handled 10A,
after soldering it would blow around 1A. Most of the bypass caps
disconnected at power up.
 
T

TheM

Jan 1, 1970
0
rickman said:
Anyone have experience with 10 mil via holes and reliability issues?
If you have a problem with an order like this, is it reasonable to use
one panel and reject the rest?

I had problems with a vendor once, it was "weak" vias. They were 20mils
though, done on early ROHS process. And yes, baking boards twice
for smd and through-hole did create new broken vias, some immediately
and some later. If I knew about this, I'd toss entire batch right away.
Caused quite a big of grief. I ask my vendor now to leave them a bit
longer in the metalization "soup" and he had to compensate for part of the
damage (tarnished name can't be restored so easily).

You can try baking boards without components and than passing them
through tester again, make sure testing current is set to high"ish" level.

Mark
 
R

rickman

Jan 1, 1970
0
I had problems with a vendor once, it was "weak" vias. They were 20mils
though, done on early ROHS process. And yes, baking boards twice
for smd and through-hole did create new broken vias, some immediately
and some later. If I knew about this, I'd toss entire batch right away.
Caused quite a big of grief. I ask my vendor now to leave them a bit
longer in the metalization "soup" and he had to compensate for part of the
damage (tarnished name can't be restored so easily).

You can try baking boards without components and than passing them
through tester again, make sure testing current is set to high"ish" level.

Mark

Thanks for your suggestion. I thought of that, but I don't have a way
to test the bare boards. Turns out I have four more weeks to order
the panels, so I have some time to evaluate the boards in the
prototypes.

I'm waiting to hear back from the board vendor. But I expect I will
have to bite the bullet on this one and reorder the production panels
from a better supplier. The whole reason I bought so many was that
they were not much more than just buying prototype quantities. So I
knew it was a bit of a risk. Not a big deal now that I have more time
to deal with it. I was mainly worried about the schedule.
 
T

TheM

Jan 1, 1970
0
rickman said:
On Apr 10, 1:41 pm, "TheM" <[email protected]> wrote:
Thanks for your suggestion. I thought of that, but I don't have a way
to test the bare boards. Turns out I have four more weeks to order
the panels, so I have some time to evaluate the boards in the
prototypes.

PCB vendor surely has a machine to check for continuity, even the cheap
vendors do. Ask them.

Mark
 
Q

qrk

Jan 1, 1970
0
Hi Mark,
Have you done any PTH vias (0.012"D) that are in SMT solder pads that are
filled either with a non conductive material before the solder is added? I
have done this on a couple of jobs recently and it simplifies layout and the
vias used for thermal flow, let's say six under a DD Pac work great.
What say you?
Harry

We have used filled vias for a different reason, to get more space in
a tight layout. Really strange to see pads with no visible drill hole!
I normally avoid filled vias due to extra cost. When I put thermal
vias under a Dpak, I make sure there's enough solder paste to fill the
via. The pad, or Cu pour, on the opposite side of the board is mostly
covered with soldermask, but the via drill hole isn't tented so the
via can burp. I usually use around 50 to 70% pad coverage for
solderpaste, depending on the part and/or if I use thermal vias in the
body pad.

Harry, I've been having fun making switching supplies recently. Made a
50W forward converter and, something we chatted about briefly a few
years ago, a SEPIC switcher to charge up a capacitor bank with
constant current for a pulse amplifier. Both run at 600kHz. The new
controllers sure make life easy. Both these supplies used the
technique above for the power components thermal vias.
 
R

rickman

Jan 1, 1970
0
PCB vendor surely has a machine to check for continuity, even the cheap
vendors do. Ask them.

You are suggesting that I temperature cycle the boards a few times and
send the blank boards back to the vendor for retest? I guess that is
an idea. So far they have been a bit difficult to communicate with.
I shouldn't say "difficult", just very slow getting answers from
them. I ask a question and it seems to require a lot of research to
get an answer. Then I hear back after a day or so. It is like they
don't seem to feel like they screwed up and are not making any real
effort to help me deal with the resulting repercussions.

I'll give them until tomorrow (Friday) to get back to me with
something substantial. If we don't have some sort of dialog going
that is likely to result in an improvement in my satisfaction, I will
just cut my losses and move on. I need to keep my customer happy and
I can't do that with an unresponsive vendor.
 
J

JosephKK

Jan 1, 1970
0
You are suggesting that I temperature cycle the boards a few times and
send the blank boards back to the vendor for retest? I guess that is
an idea. So far they have been a bit difficult to communicate with.
I shouldn't say "difficult", just very slow getting answers from
them. I ask a question and it seems to require a lot of research to
get an answer. Then I hear back after a day or so. It is like they
don't seem to feel like they screwed up and are not making any real
effort to help me deal with the resulting repercussions.

I'll give them until tomorrow (Friday) to get back to me with
something substantial. If we don't have some sort of dialog going
that is likely to result in an improvement in my satisfaction, I will
just cut my losses and move on. I need to keep my customer happy and
I can't do that with an unresponsive vendor.

Just be sure that you tell them that. There are a lot of native
English speaking "Front ends" for Chinese fabs that are several time
zones away. It could explain the lag and the poor information
transmission quality.
 
R

rickman

Jan 1, 1970
0
Just be sure that you tell them that. There are a lot of native
English speaking "Front ends" for Chinese fabs that are several time
zones away. It could explain the lag and the poor information
transmission quality.

These guys are in the US. I did finally get someone who could at
least try to get a little info, but I didn't get a lot. I was told
they checked the chemistry and didn't find anything out of whack. He
offered to do a destructive test, but never gave me a RMA. Finally
someone called as a general follow up and I told her what had
happened. It was a bit surprising that she didn't know ahead of time
that there was a problem. She also didn't have access to any
information on the problem or the contacts I had already had about
this. She asked me to send her the last email about what they had
found and promised to get back to me on Monday.

At this point I am ready to release the test fixture to be made and I
am looking for someplace else to do it. It is 8" x 10", 4 layers and
I only need a small number, say 4. Any suggestions?
 
D

David L. Jones

Jan 1, 1970
0
On production boards I usually order electrical testing of the PCB blanks.
If you spend enough time hammering the online quote system you can get the
best balance of qty vs. cost. For example, one of my boards jumps from
$50/order to $250/order additional for electrical testing when I order over
38 boards. I've always thought electrical testing should be included in the
price (what if I charged my customers extra to verify the product I sell
them works?), but I'm not aware of anyone who doesn't charge an additional
fee.

www.pcbcart.com do electrical testing as standard, no additional fee.

Dave.
 
A

Anton Erasmus

Jan 1, 1970
0
[Snipped]
These guys are in the US. I did finally get someone who could at
least try to get a little info, but I didn't get a lot. I was told
they checked the chemistry and didn't find anything out of whack. He
offered to do a destructive test, but never gave me a RMA. Finally
someone called as a general follow up and I told her what had
happened. It was a bit surprising that she didn't know ahead of time
that there was a problem. She also didn't have access to any
information on the problem or the contacts I had already had about
this. She asked me to send her the last email about what they had
found and promised to get back to me on Monday.

At this point I am ready to release the test fixture to be made and I
am looking for someplace else to do it. It is 8" x 10", 4 layers and
I only need a small number, say 4. Any suggestions?

I have had very goods results from http://www.pcbcart.com. They are
based in china, but I have had no problems with their product. The
quality is excellent, the price is very good and you can get a direct
quote on their web site. I normally pay about US$60 to get the boards
couriered to South Africa, which takes about 36 hours. They have Fedex
and DHL as an option.
The only problem I have had is that the status on their web site are
sometimes not updated. To get the latest status it is best to email
them.

Regards
Anton Erasmus
 
R

rickman

Jan 1, 1970
0
Out of curiosity, can you identify the PCB house you were using? I've used
PCBExpress/ECD/Sunstone (all the same company) since 1998 with mostly good
results. Generally speaking I've been happy, though they've pulled a few
boners over the years with respect to quality. Things have really improved
in the last 6 months or so, and they've always been willing to fix their
mistakes.

You got it in one! I ordered from Sunstone. I finally got a proper
reply from the last person I spoke to and she has given me answers
that sound like maybe they weren't just pulled out of somebody's...
well, you know. They said there was a problem with air bubbles and
that the good boards really should be good. I will be bake cycling
these boards before I build the production units, but I expect I will
be able to use them if I don't have to make any changes. They have
offered to make up the 16 board shortfall or give me credit for the
missing boards. Plus they are offering 15% off my next order.

On production boards I usually order electrical testing of the PCB blanks.
If you spend enough time hammering the online quote system you can get the
best balance of qty vs. cost. For example, one of my boards jumps from
$50/order to $250/order additional for electrical testing when I order over
38 boards. I've always thought electrical testing should be included in the
price (what if I charged my customers extra to verify the product I sell
them works?), but I'm not aware of anyone who doesn't charge an additional
fee.

I got electrical testing. Good thing, huh? I assume that otherwise I
would have gotten untested panels and found the problems myself.

Anyway, IMO they offer the best balance of price vs. quality vs. speed. It
doesn't hurt that they are about 100 miles away which makes the free UPS
ground essentially overnight for me.

I can't argue with the price. The reason I ordered from them was that
they offered 6 panels at the price of one panel from the other shops.
I think I am going to give them the order for the test fixture. That
should go out today.
 
Top