Searching \ for '[EE]: Your thoughts on PCBs from design to product' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: www.piclist.com/techref/pcbs.htm?key=pcb
Search entire site for: 'Your thoughts on PCBs from design to product'.

Exact match. Not showing close matches.
PICList Thread
'[EE]: Your thoughts on PCBs from design to product'
2002\05\07@140123 by Byron A Jeff

face picon face
I'm contemplating my first real PCB production run. I know that the topic
has been beaten to death in the forum. I realized though that the problem isn't
a lack of information, but instead a overflowing wealth of info. I wanted to
get your experiences of a wholistic view of the process from design to
production.

The situation: I have a prototype design done in wire wrap. For production
it will need a few items added, so the design isn't yet airtight. In the
end I'd like to get a moderate production run of say 100 boards. The board
size is going to be somewhere in the 3 in x 3 in to 4 in x 4 in range.

I envision the process in three stages:

1) Design: finish adding the goodies to the prototype, layout a PCB, then
test and tweak until a rock solid design and board is complete.

2) Prototype production run where a handful of boards are done with the final
design from the board house, which are then tested.

3) Final run. The actual production run.

The variables are turnaround time (TT), limiting cost (LC), and quality (Q).
Each of these vary at each stage. Here are my roundabout guesses on a
0-10 scale.

Design: TT:10 LC:10 Q:4. This needs to be a quick dirty phase because it
       may iterate over several versions. It needs to be relatively
       inexpensive due to revisions. The quality only needs to be good
       enough to test.

Prototype: TT:10 LC:5 Q:10. The prototypes should be the same quality as
          the production boards. Quick turnaround time in order to verify
          the results. Since this step is done once, cost isn't a significant
          issue.

Final: TT:3 LC:9 Q:10. For the final run I'd like to see top quality at the
      best price. Since everything has been tested, turnaround time is no
      longer critical.

What I wanted to see was folks' experiences at each phase. What tools did you
use? Which house did you choose? Why?

There are numerous choices at every stage. Any assistance in narrowing down
the field to fit the criteria outlined above would be helpful.

Thanks,

BAJ

--
http://www.piclist.com hint: PICList Posts must start with ONE topic:
[PIC]:,[SX]:,[AVR]: ->uP ONLY! [EE]:,[OT]: ->Other [BUY]:,[AD]: ->Ads


2002\05\07@144444 by James Paul

picon face
Byron,

I can add the following info....

1) For better price, go with longer turn times.  Logical right?
   Since TT is no longer critical, go for the longest time you
   can achieve vs the price you want to pay for the finished boards.

2) The tools we (I) use is OrCad Layout Plus.  This is what I started
   out on at TI, and is also what we have at Applied MEMS.  Some people
   don't like OrCad, but to me, it seems just fine.  It is sort of
   buggy and quarky though.   But I've learned to workaround these
   difficulties.

3) Find a board house that you like that is close to you geographically.
   This makes communication between you and the board house much easier.
   Also, you can hand deliver and pick up rush items.

4) Take as much time as you can on the initial layout.  And don't try
   to do it all in one sitting.   I have found that if I do a small part
   of it, leave it for awhile, and think about it for awhile, I usually
   come up with the answet to a puzzling question I had about routing,
   or I envision a different (and better) way of routing (or rerouting)
   a portion of the board.   Several times this has save adding an extra
   layer or two. To me, this is the most critical part of the design.

5) Don't sweat it if you screw up.   Just fix the problem and go on.

6) Don't be afraid to ask for help or advice from someone more experienced
   in layout than you.

This is what I have to add to your request for insight.  I hope it helps.
And good luck on your endeavor.


                                                      Regards,

                                                        Jim






{Quote hidden}

--
http://www.piclist.com hint: PICList Posts must start with ONE topic:
[PIC]:,[SX]:,[AVR]: ->uP ONLY! [EE]:,[OT]: ->Other [BUY]:,[AD]: ->Ads


2002\05\07@200409 by Chris Loiacono

flavicon
face
I think your logic is sound.

I have a slightly different perspective that may or may not add some
insight:


1. I like to proto on a breadboard. If I can get the thing to run without
objectionable noise on a breadboard, there will generally be very few of
such surprises in the final design. I always make sure I am using the same
parts I will be using in the final design before proceeding.

Assuming that you have all the obvious areas covered, such as number of
layers, minimum trace widths and copper weight for (especially) power and
ground nets; decoupling scheme w/ cap leads close to Vcc pins, mechanical
design considerations and component selections with alternate footprints for
less-common parts, etc... etc....then

2. I like to fly through the schematic and layout of proto's. I like to
trust my tools, but also to check the result minimally at this stage. Send
out the gerbers and deal with the one or two problems that may come up in a
two or three pc order.

3. Fix the proto bugs and implement any new ideas that have come up since
the time the proto design was frozen. Check mechanicals and mounting holes,
etc,..and move as needed. Then run the gerbers again and check the results
with a good viewer several times. I do this with a list of characteristics
that the tool's DRC won't look for. When I feel 100% confident in the
updated board, then it's ready for a production run. (In other words, just
do it!)
You'll know if it's ready or not, and you'll decide accordingly.

ps: I still like Advanced Circuits because their proto qty prices are OK,
and their production pricing starts at some pretty low quantities...

Have fun,
Chris


> {Original Message removed}

2002\05\07@230241 by Shawn Mulligan

picon face
Sounds like you have a pretty good idea of the process already. Without
knowing the nature of your design -- surface mount, thru-hole, frequency,
size/temperature/environmental restrictions, etc -- here are a few tips on
my watch list. Hope they help.

Drill sizes: Many board houses offer several "standard" drill sizes. If your
design uses drills that are not on this list, you will incur an additional
charge. Check with the board house.

Clearance constraints: Board houses guarantee a minimum clearance between
separate copper. If their guananteed minimum is 0.008 and you've designed
traces that are just 0.007 apart, your board's production may be held for
intervention, or these traces may be 'bridged' on the final board. Usually
not a big deal -- you can often just cut them apart with an X-acto knife.

Footprints: Confirm that you have used the correct footprints on your
design. For example: you may prototype with a sample chip in an SOIC-20
package and design your board with that footprint. When it comes time for
production, you might realize that the SOIC-20 package is scarce with large
lead times, while the same chip in a SSOP package is readily available.
Basically, check price and availability before settling on a footprint.

Test points: When designing the prototype board, make room for testpoints on
any signal that you may want to monitor when debugging your design (as long
as they don't affect circuit performance}. I've designed footprints for
every microcontroller that I use, with dual-row headers bordering each edge,
accessing every pin. This took some extra work, but it is a real help when
debugging a MSP430 series microcontroller in a 64-TQFP package.

Mechanicals: Make sure everything fits on the board, and the board fits in
the case (in every dimension). Sounds trivial, but it's not.

Have a friend double-check your design. Are your tantalum/electrolytic caps
in the right way on +/- voltage rails? Did you accidentally connect the
power backwards?(Throw a diode inline with power, just in case) Are the
diodes in correctly? Did you specify 200K when you meant 200R? All simple
mistakes, yet hard to find when you have your pride-and-joy, newly-populated
board in your hands.

Ask for help: Call your board house of choice, plead ignorance and tap any
knowledge that comes your way. Also, do a web search for board houses, and
search their websites for design tips. You'll find articles on decoupling
caps, sheilding, capacitance issues, etc.

Hope this helps -- not that I have made any of these mistakes!

Shawn

{Quote hidden}

> > {Original Message removed}

2002\05\08@040406 by Alan B. Pearce

face picon face
>I envision the process in three stages:
>
>1) Design: finish adding the goodies to the prototype, layout a PCB, then
>test and tweak until a rock solid design and board is complete.
>
>2) Prototype production run where a handful of boards are done with the
final
>design from the board house, which are then tested.
>
>3) Final run. The actual production run.

I would forget about "finishing the design" on the wire wrap circuit. Go
straight to designing the PCB adding the rest of the parts required to
finish the design to the PCB as you go. I would strongly recommend putting
as many pad sets for extra chips as you can on otherwise spare area if at
all possible, without increasing the size of the board.

Then get a panel of boards made at a 24 hr turn round house. This will give
you several PCB's at a good price, and back in your hands rapidly. Attend to
parts ordering/documentation and any other menial chores that normally get
put aside while you wait.

Now debug your layout and remainder of your design using one of these boards
you get back. If necessary build a second board with neat modifications to
it as a "shippable sample" to verify each and every mod you think you have
made to the first PCB you built up. Having verified that you have correctly
enumerated every mod on this second PCB, modify the PCB masters, adding
silkscreen and solder mask if necessary/desirable and get a production batch
of PCB's made.

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@070820 by Byron A Jeff

face picon face
On Wed, May 08, 2002 at 09:03:28AM +0100, Alan B. Pearce wrote:
> >I envision the process in three stages:
> >
> >1) Design: finish adding the goodies to the prototype, layout a PCB, then
> >test and tweak until a rock solid design and board is complete.
> >
> >2) Prototype production run where a handful of boards are done with the
> final
> >design from the board house, which are then tested.
> >
> >3) Final run. The actual production run.
>
> I would forget about "finishing the design" on the wire wrap circuit. Go
> straight to designing the PCB adding the rest of the parts required to
> finish the design to the PCB as you go. I would strongly recommend putting
> as many pad sets for extra chips as you can on otherwise spare area if at
> all possible, without increasing the size of the board.
>
> Then get a panel of boards made at a 24 hr turn round house. This will give
> you several PCB's at a good price, and back in your hands rapidly.

What I'm reading here is to essientially skip the design PCB and go straight
to step 2.

But that has sirens going off in my conservative little pea brain.

That design won't be right. That design can't be right. And even after I fix
it, the resulting design won't be right either.

And with those few boards adding up to $100 an iteration, that's a very scary
prospect. Kind of like programming to a mask ROM where any error makes the
batch useless, and where a batch is going to run a chunk of change.

I guess I'm asking what's the PCB equivalent of a PROM? Something that you can
have done in singles, can be done quickly, and is cost effective.

Honestly I'm not a pro at this, just a hobbyist taking a shot. As a software
guy, I know that there will be errors in the first few iterations. I find
the thought of running those iterations at step 2 above somewhat daunting.

{Quote hidden}

Thanks for the insight. I certainly will think about it.

BAJ

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@075239 by Alan B. Pearce

face picon face
>What I'm reading here is to essientially skip the
>design PCB and go straight to step 2.

The way I read your original post was that as step 1 you were going to add
the remaining goodies to your wirewrap prototype which currently works. I am
saying that you should do a PCB layout of the currently working prototype,
and add the remaining undeveloped goodies to that layout, maybe a step 1.5
if you like.

>But that has sirens going off in my conservative little pea brain.

>That design won't be right. That design can't be right. And even
>after I fix it, the resulting design won't be right either.

Well fair enough, but would it be any more right if you had the total design
working satisfactorily on the wirewrap and made a PCB for that? I would
certainly be making a sample batch of PCB's first and building probably a
couple of boards to make sure before committing to a full production run. I
envisage only one run through the 24 hour turn round facility, and that
without silkscreen and soldermask, so it is real cheap.

>And with those few boards adding up to $100 an iteration,
>that's a very scary prospect. Kind of like programming to
>a mask ROM where any error makes the batch useless, and
>where a batch is going to run a chunk of change.

Well you have not said just how large your expected production run is, but
somewhere along the line you will need to commit a sum about this size to a
preproduction run to ensure there are no bugs. I am suggesting only one
iteration, and then you should be able to go straight to the production
layout with all faults fixed. It is all to easy to make a board with the
power lines to one chip swapped over, or a polarised capacitor the wrong way
round. :)

What is the cost of your labour on the production run if you have to do one
track cut/wire patch? I suspect it would rapidly come to the cost of a run
of minimal cost boards like I am suggesting.

>Thanks for the insight. I certainly will think about it.

Your welcome. I'm just remembering the design cycle of a colleague who was
doing a complete VHF land mobile transceiver. I lost track of how many board
revisions he went through in development to get the whole machine settled
down.

Yours should not be that bad, but if you are using A/D conversion it would
be well to commit to a PCB as early as you can, even just double sided, to
get your grounding well sorted early on.

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@093917 by Byron A Jeff

face picon face
On Wed, May 08, 2002 at 12:51:47PM +0100, Alan B. Pearce wrote:
> >What I'm reading here is to essientially skip the
> >design PCB and go straight to step 2.
>
> The way I read your original post was that as step 1 you were going to add
> the remaining goodies to your wirewrap prototype which currently works.

My intent was switching to prototype PCB's. I guess I was just looking for
some validation to the idea of prototyping with a homemade setup because
it would take some iterations to do, and both cost and turnaround time
were important.

{Quote hidden}

Nope. It would still need fixing.

>I would
> certainly be making a sample batch of PCB's first and building probably a
> couple of boards to make sure before committing to a full production run. I
> envisage only one run through the 24 hour turn round facility, and that
> without silkscreen and soldermask, so it is real cheap.

I'm still learning how to price this stuff. A lot of what I read, say at
http://www.apcircuits.com for example, doesn't seem to even offer runs without the
soldermask.

Might you have a specific example of a place that has quick turnaround time,
no silkscreen or soldermask, and is 'real cheap'?

>
> >And with those few boards adding up to $100 an iteration,
> >that's a very scary prospect. Kind of like programming to
> >a mask ROM where any error makes the batch useless, and
> >where a batch is going to run a chunk of change.
>
> Well you have not said just how large your expected production run is, but
> somewhere along the line you will need to commit a sum about this size to a
> preproduction run to ensure there are no bugs.

That was my step two in my original list.

> I am suggesting only one
> iteration,

As was I.

> and then you should be able to go straight to the production
> layout with all faults fixed.

My leery meter is going off again. I wouldn't dare commit to a production run
unless the sample batch was already perfect. That's why I was hoping to
iterate completely in the design phase, so that I could get one perfect
preproduction sample batch (quickly I hope), verify that they look and work
perfectly, and then go to the production run unchanged. That's the key in my
mind: the production run has to be exactly the same as the last preproduction
sample run, with no changes. Any change that goes untested has the potential
of ruining the production run.

> It is all to easy to make a board with the
> power lines to one chip swapped over, or a polarised capacitor the wrong way
> round. :)

Exactly. That's why I would unfortunately iterate over a preproduction run
before committing to the final PCB.

Am I off the mark here? I'm a completely newbie to the entire process.

>
> What is the cost of your labour on the production run if you have to do one
> track cut/wire patch? I suspect it would rapidly come to the cost of a run
> of minimal cost boards like I am suggesting.

You have no disagreement from me here. What I'm trying to do is limit that
perproduction run to one iteration. So the 1st and only preproduction run that
goes to the board house is already perfect.

But what I got from your previous message is that there's the possibility of
having to iterate with the quick turnaround boards too, each with mounting
setup costs. This is what I'd like to avoid.

Also am I correct in assuming that if there is absolutely no change between the
preproduction run and the production run, that there isn't an addition setup
cost at the board house?

{Quote hidden}

I'm not. It's a really simple circuit. However I'm trying to get a handle on
the process so that the first submission to the board house is perfect.

If anyone would care to outline PCB techniques or board houses that are:

1) The fastest
2) The cheapest
3) The highest quality

Then maybe I can settle to how to navigate through this minefield. I'll do
me design development with the cheapest route, my preproduction with the
fastest, and the final run with the highest quality, with the caveat that
the preproduction and production runs needs to be in the same board house.

I'm searching for personal recommendations and I'd appreciate any that are
offered.

BAJ

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@094616 by Byron A Jeff

face picon face
On Tue, May 07, 2002 at 01:42:38PM +0500, James Paul wrote:
>
>  Byron,
>
>  I can add the following info....
>
>  1) For better price, go with longer turn times.  Logical right?
>     Since TT is no longer critical, go for the longest time you
>     can achieve vs the price you want to pay for the finished boards.

Agreed. But for the preproduction run, I'd need the same board house to
turn around quick prototypes for validation.

>
>  2) The tools we (I) use is OrCad Layout Plus.  This is what I started
>     out on at TI, and is also what we have at Applied MEMS.  Some people
>     don't like OrCad, but to me, it seems just fine.  It is sort of
>     buggy and quarky though.   But I've learned to workaround these
>     difficulties.

Well tools are an animal of a completely different stripe. I'm in the process
of evaluating those now.

>
>  3) Find a board house that you like that is close to you geographically.
>     This makes communication between you and the board house much easier.
>     Also, you can hand deliver and pick up rush items.

Hmmm. hadn't thought of that. I think that I had limited my options to
the internet based board houses that accepts their info over the internet.
Overnight or two day would certainly be fast enough turnaround on the
preproduction prototypes.

>
>  4) Take as much time as you can on the initial layout.  And don't try
>     to do it all in one sitting.   I have found that if I do a small part
>     of it, leave it for awhile, and think about it for awhile, I usually
>     come up with the answet to a puzzling question I had about routing,
>     or I envision a different (and better) way of routing (or rerouting)
>     a portion of the board.   Several times this has save adding an extra
>     layer or two. To me, this is the most critical part of the design.

Good advise. I do this with most all of my software and firmware projects.

Fortunately this is a simple board. It'll be single layer, through hole. I'm
less concerened about routing screwups than I am about leaving off desired
features off the final product.

>
>  5) Don't sweat it if you screw up.   Just fix the problem and go on.

I'm a programmer. That a mantra of life!

>
>  6) Don't be afraid to ask for help or advice from someone more experienced
>     in layout than you.

Check.

>
>  This is what I have to add to your request for insight.  I hope it helps.
>  And good luck on your endeavor.

Thanks for the help. I really appreciate it.

BAJ

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@102711 by John Dammeyer

flavicon
face
Hi Baj,

I can understand your concern.  I used to wirewrap everything too.

You are right.  The design won't be right.  I've had things go wrong
like SOT-23 pinout backwards, pull up resistors forgotten, opto-couplers
with the wrong pinouts or a circuit that just doesn't plain work the way
I expected.  I must admit,  where there is uncertainty,  I do try and
breadboard some things but short of an etch resist pen and a local acid
bath on a pc board,  some things just don't work well on a breadboard.
Both RF and High Power DC come to mind.

So when I get a new board back from the proto house (solder mask but no
silk screen for boards that use surface mounted devices) I expect that
it may have a lot of jumpers.  When I do software for customers I've
even received first run boards with major bugs and jumpers and that's
from very experienced designers.

But the software often ends up being the bottleneck and better to have
working hardware with jumpers and chips glued upside down and the
programmers hard at work than idle programmers waiting for that first
board.

To demonstrate I'll air some dirty laundry in public.  Check out.

http://www.pacificsun.ca/~john/photos/rf-rev1.jpg

The end product looks a lot different but the proto allowed me to do
detailed testing for both software and hardware.  And yet problems with
layout did creep into the final product.  I keep an itemized list, and
write what needs to be changed onto the list as I discover the problems.
Right away.  Not in 10 minutes when I've forgotten.  Then when I do the
new boards I work through the list fixing the little things.  If I have
multiple lists from previous iterations I also go through those again
too,  just in case.

And the problem with software people doing board design?  It's easy.
The board is never done and can always have one more feature.  ;-)

John




Wireless CAN with the CANRF module.
www.autoartisans.com/documents/canrf_prod_announcement.pdf
Automation Artisans Inc.
Ph. 1 250 544 4950

{Quote hidden}

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@105200 by Alan B. Pearce

face picon face
>I'm still learning how to price this stuff. A lot of what I read, say at
>http://www.apcircuits.com for example, doesn't seem to even offer runs without the
>soldermask.
>
>Might you have a specific example of a place that has quick turnaround
time,
>no silkscreen or soldermask, and is 'real cheap'?

well you could try out Olimex http://www.olimex.com/pcb/ which is the PCB
house promoting the contest that James has been listing in this list. He
operates out of Bulgaria, and claims no import taxes into Europe or USA. I
have not personally used him, but others on this list claim to have with
good results. Now I know Bulgaria is not just round the corner from you, but
if a few days can be used on other things while you wait, it may be worth
investigating.

OTOH as this seems to be your first foray into the minefield you may find
that you are better off doing your first project with a PCB house that is
within driving distance, so you can hop in the car and go talk face to face,
or have their rep call on you. If you can build up a raport with them, you
may be able to get your prototypes at a good price anyway.

Best of luck whichever way you go.

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@115708 by gacrowell

flavicon
face
> I guess I'm asking what's the PCB equivalent of a PROM?
> Something that you can
> have done in singles, can be done quickly, and is cost effective.

To answer this specific question, this type of operation is done by a rapid
prototyping board cutting tool, like an LPKF http://www.lpkf.com   Some hobbyists
have built similar tools.  With one, you can literally have a pcb in an
hour.

But, there are a whole list of gotchas.  First, you have to find someone who
has one.  Then there are the limitations; (usually) only two layers,
(usually) no plated vias, (usually) no soldermask or silkscreen, limitations
in tracewidth and routing.  When you're done with the gotchas, it is very
unlikely (unless you are doing a very simple board) that the proto will be
identical to your production board.

Gary Crowell
Micron Technology

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@122930 by Matt Pobursky

flavicon
face
On Wed, 8 May 2002 09:36:33 -0400, Byron A Jeff wrote:
>I'm still learning how to price this stuff. A lot of what I
>read, say at http://www.apcircuits.com for example, doesn't seem to
>even offer runs without the soldermask.

They have an entire production line that does only these types of
boards! From their web site:

"Proto 1 service: Quick turn engineering prototypes.  Orders
received by 11:00 AM Mountain (1 PM  Eastern) any business day
will ship the next business day."

I use AP Circuits for these types of boards at least a dozen
times a year. I rarely build anything more than a handful of
components on a breadboard or perfboard unless I'm looking to
just get a quick look at a single device or very simple circuit.

As an example, I recently built a small adapter board that
converted a 4Mbit static ram with battery backup circuit and
battery holder to mount in a 32 pin PLCC socket FLASH socket for
development work with a Rabbit 2000 CPU design (speeds downloads
and debugging). The total cost of 6 boards was $68 (US) and I
received them 2 days after I placed the order.

Note that the boards are not routed, they are sheared.
Rectangular boards only and you might have to "clean up" the
edges. No soldermask or silkscreen -- just plain tin-lead plated,
2 sided boards. But for most first run boards used to get real
hardware up and running, this is about the cheapest and easiest
route I've found.

If you must have "finished" boards with silkscreen and
soldermask, Advanced Circuits is a very good choice. I use them
almost as much as AP Circuits. They are running a $33/ea. (2
board minimum, 5 day turn) special on 2 sided boards right now.
They are just like finished production boards. They also usually
deliver faster than 5 days in my experience.

http://www.4pcb.com/33each

With resources like these, I find it hard to justify much time at
all hand building anything. In the end, you spend a lot of hours
and end up with something that's NOT what your end product will
be. The "real circuit board" route gets you much closer the first
time and I usually find circuit boards easier to modify than hand
wired prototypes.

Matt Pobursky
Maximum Performance Systems

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@125508 by Pic Dude

flavicon
face
Another datapoint...

Also check out ExpressPCB.com .  Though you have to put the
design in their tool (free download), it's very easy to use,
and if you can fit your design within 3.8" x 2.5", there's a
great deal on 3 PCB's f/$59.  (You can also panelize if your
design is smaller).  The $59 includes 3-day shipping.  I've
used them once, and am very happy with the service and
turnaround.

Only thing I can ask for is better printing options.

Cheers,
-Neil.




{Original Message removed}

2002\05\08@171926 by Olin Lathrop

face picon face
> >  3) Find a board house that you like that is close to you
geographically.
> >     This makes communication between you and the board house much
easier.
> >     Also, you can hand deliver and pick up rush items.
>
> Hmmm. hadn't thought of that. I think that I had limited my options to
> the internet based board houses that accepts their info over the internet.
> Overnight or two day would certainly be fast enough turnaround on the
> preproduction prototypes.

Just my two cents, but I don't think geographic proximity is much of an
issue.  I'm in Massachusetts and I routinely use PCB Express, which ships
from Oregon.  I have never talked to a human there, and hopefully will never
have to.  From my point of view, they are on the other end of the internet
and of a UPS delivery.  The exact geographic location make little
difference, except perhaps to the price of a rush shipment.  Even then, the
cost of a board run drawfs the price of shipment.

Other board houses I have considered but never used were 4PCB, Advanced
Circuits, and Olimex.  If I remember right, 4PCB came out more expensive,
and Advanced Circuits and Olimex only did double sided.  Things may have
changed since I last checked.  I also sorta remember Olimex is in some third
world or former communist country, so shipping to the civilized world may
take a *long* time.


*****************************************************************
Embed Inc, embedded system specialists in Littleton Massachusetts
(978) 742-9014, http://www.embedinc.com

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\08@174454 by Olin Lathrop

face picon face
> With resources like these, I find it hard to justify much time at
> all hand building anything. In the end, you spend a lot of hours
> and end up with something that's NOT what your end product will
> be. The "real circuit board" route gets you much closer the first
> time and I usually find circuit boards easier to modify than hand
> wired prototypes.

I agree.  A hand wired breadboard only tests the circuit itself, but doesn't
test:

- The schematic correctly entered and being what you intended or hand-built.

- The mechanical part definitions being all correct.  Yes, I know most
packages come with libraries you can usually trust, but I find I still
define a bunch of parts myself on every project.

- The layout being sufficient electrically.  Issues of sufficient ground,
EMI, analog section isolation, current capability of all traces, etc.

- Mechanical clearances between parts beyond just the foot print, and
between the board and other objects in the system.

- Proper placement and size of mounting holes, or anything else that has to
interface with the rest of the system mechanically.

A breadboard can be useful for experimenting with a circuit *concept*,
although it is not a substitute for careful up front calculations (neither
is simulation).  I may screw around with something on a breadboard, but
often the first implementation of circuits I design is on a PC board as
close to production as possible.  The cost of a small prototype run of 4
boards is only a few hours of time.  Most of the time the second generation
boards are good enough to be final product, unless features were added after
the first boards were made.  If this is a small volume hobby project, you
should be able to rework the first boards and use them normally unless you
really messed up.


*****************************************************************
Embed Inc, embedded system specialists in Littleton Massachusetts
(978) 742-9014, http://www.embedinc.com

--
http://www.piclist.com hint: The list server can filter out subtopics
(like ads or off topics) for you. See http://www.piclist.com/#topics


2002\05\09@024120 by Dmitriy A. Kiryashov

picon face
Hi Olin.

I guess 4pcb and Advanced Circuits are the same.
http://www.4pcb.com is Advanced Circuits website.

Completely agreed with idea that closeness doesn't mean
quality and lowest cost. I'm buying boards across the
country much more cheaper than the local pcb guys can do.

WBR Dmitry.


{Quote hidden}

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.


2002\05\09@074544 by Olin Lathrop

face picon face
> I guess 4pcb and Advanced Circuits are the same.
> http://www.4pcb.com is Advanced Circuits website.

Then the other name was maybe AP Circuits.  One outfit is in Colorado, the
other in Alberta (Calgary?), but I seem to have their names garbled.  The
one in Colorado was more expensive than PCB Express last time I priced out a
job (I don't bother now, I just go to PCB Express), and the place in Alberta
only did double sided.  Again this may have changed in the last year or so.


*****************************************************************
Embed Inc, embedded system specialists in Littleton Massachusetts
(978) 742-9014, http://www.embedinc.com

--
http://www.piclist.com hint: The PICList is archived three different
ways.  See http://www.piclist.com/#archives for details.


2002\05\09@100752 by SHAWN

picon face
AP Circuits (Alberta Printed Circuits) is located in Calgary Alberta.
Currently, they only do double sided. Their website is: http://www.apcircuits.com

Shawn
{Original Message removed}

More... (looser matching)
- Last day of these posts
- In 2002 , 2003 only
- Today
- New search...