Searching \ for '[EE]: Single Sided Boards - How do you do it?' 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/index.htm?key=single+sided+boards
Search entire site for: 'Single Sided Boards - How do you do it?'.

Exact match. Not showing close matches.
PICList Thread
'[EE]: Single Sided Boards - How do you do it?'
2002\11\24@015109 by Josh Koffman

flavicon
face
Well, after much work and some heartache, I have created my first board
in Eagle. Now we'll see if I can transfer it to the Press-n-Peel and
etch and drill properly. Anyway, Since this is my first time with Eagle,
first time with Press-n-Peel, and my first time etching a board at all
in quite a while, I decided to only make a single sided board. Pity
though, since Eagle routed my board perfectly with two layers. So, Eagle
couldn't figure out a way to produce a single sided board with all the
nets routed. Not a problem, I spent many an hour manually rerouting
stuff. My question is this: How do you deal with jumper wires? I dropped
spare pads down and routed to the pad, skipped a section, then dropped
another pad and routed from there. I am left with an airwire across
where the jumper would be. However, is there a better way? I searched
around in the Help and I couldn't seem to find anything. Does anyone
have a better way to do this?

Thanks,

Josh
--
A common mistake that people make when trying to design something
completely foolproof is to underestimate the ingenuity of complete
fools.
       -Douglas Adams

--
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\11\24@020353 by Wagner Lipnharski

flavicon
face
Josh Koffman wrote:
> Well, after much work and some heartache, I have created my first
> board in Eagle. Now we'll see if I can transfer it to the
> Press-n-Peel and etch and drill properly. Anyway, Since this is my
> first time with Eagle, first time with Press-n-Peel, and my first
> time etching a board at all in quite a while, I decided to only make
> a single sided board. Pity though, since Eagle routed my board
> perfectly with two layers. So, Eagle couldn't figure out a way to
> produce a single sided board with all the nets routed. Not a problem,
> I spent many an hour manually rerouting stuff. My question is this:
> How do you deal with jumper wires? I dropped spare pads down and
> routed to the pad, skipped a section, then dropped another pad and
> routed from there. I am left with an airwire across where the jumper
> would be. However, is there a better way? I searched around in the
> Help and I couldn't seem to find anything. Does anyone have a better
> way to do this?
>
> Thanks,
>
> Josh

One way is just change the "cost" of the "non existent" layer's so high
that Eagle will try to do everything possible on the "cheap" side, leaving
less possible tracks on the  "non existent" layer.  You can also first
position manually (manual routing) the wires on the "non existent" layer,
so Eagle will be happy to route the rest on the cheap existent layer.

Just 2 questions:  How many holes do you have in this board? what is the
board size?  You will be amazed that just trying a different components
disposition on board can (sometimes) magically solves it with no jumpers at
all on a single sided board.  Sometimes hard work pays of, sometimes makes
you crazy.  :)

W46NER.

--
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\11\24@035122 by William Chops Westfield

face picon face
> Pity though, since Eagle routed my board perfectly with two layers. So,
> Eagle couldn't figure out a way to produce a single sided board with all
> the nets routed. Not a problem, I spent many an hour manually rerouting
> stuff. My question is this: How do you deal with jumper wires? I dropped
> spare pads down and routed to the pad, skipped a section, then dropped
> another pad and routed from there.

For single sided boards...

If you get ALMOST get there with the autorouter, let it route your bottom,
and then turn back on the top layer and autoroute again.  Then use jumper
wires wherever eagle put a trace on the top.  You may have to do some
rearrangement to get your jumpers to be straight.  If you want straight
jumpers.

For manual routing, I start on the bottom, route to a "conveniet" location
not near to many other traces, then use the middle mouse button to switch
layers.  This creates a via, and then I route my "jumper" on the top layer
until I'm close to the destination, use the middle button again to get back
to the bottom, and finish.  The jumper goes between the vias (make sure your
via drill/pad size is set appropriately!)

There's a big problem with amateur boards, in that your holes aren't plated
through, and you therefore can't count on any connection that goes THROUGH
the board at a component hole unless you can solder that lead on both sides
of the board.  (For some components, this is impossible - you can use
rectangles in tRestrict layer to prevent Eagle from routing to topside pads,
if you want.)  This means that for small number of topside tracks, you'd
rather have (added) vias (where you can solder a wire on both sides) than
connections that go top-to-bottom via a pad.

There is either a ULP or a routing ".ctl" file that's supposed to optimize
things for single-sided boards with jumpers.  I tried it a couple of times,
and it seemed to work pretty well.  (In general, though, I'm not impressed
with Eagle's ability to route single-sided boards, and end up doing mostly
manual routing.)

BillW

--
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\11\24@083842 by Olin Lathrop

face picon face
> Well, after much work and some heartache, I have created my first board
> in Eagle. Now we'll see if I can transfer it to the Press-n-Peel and
> etch and drill properly. Anyway, Since this is my first time with Eagle,
> first time with Press-n-Peel, and my first time etching a board at all
> in quite a while, I decided to only make a single sided board. Pity
> though, since Eagle routed my board perfectly with two layers. So, Eagle
> couldn't figure out a way to produce a single sided board with all the
> nets routed. Not a problem, I spent many an hour manually rerouting
> stuff. My question is this: How do you deal with jumper wires? I dropped
> spare pads down and routed to the pad, skipped a section, then dropped
> another pad and routed from there. I am left with an airwire across
> where the jumper would be. However, is there a better way? I searched
> around in the Help and I couldn't seem to find anything. Does anyone
> have a better way to do this?

Tell Eagle it's a two layer board but make the cost for the top layer very
high.  Set the via size so that you get pads for your jumper wires.  Eagle
will then compute a complete solution with as many tracks on the bottom side
as possible.  I recommend about 8 optimization passes.  Now just etch the
bottom side and solder wires into the via holes to replace the top layer.


*****************************************************************
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\11\24@103604 by Bob Axtell

face picon face
Being an old guy, having worked with commercial
1-sided PCBs in the past, I feel that I need to pass
my 2-cents to people attempting 1-sided PCBs. The
2-cents is: don't waste money on 1-sided boards.

A PCB must perform two, unrelated tasks: (1) it must
interconnect the components, and (2) it must rigidly
MOUNT (hold in place) the components.

A 1-sided board makes a fair attempt at the first requirement,
in that wire jumpers can be installed to eliminate top-side traces,
but it fails miserably to properly mount the components. The leads
of all components are passed through the board and only contact
the bottom copper traces through a small solder blob about 30 mils thick.
That blob has little strength, and the connection can withstand very
little vibration or flexing. Commercially, in years past the board was
dipped in shellac to strengthen the physical resistance to vibration, but
that lessens its ability to accept flexing.

A 2-sided PCB, on the other hand, has an interconnect from a pad on
top to a similar pad on the bottom, with a hole lined with copper at least
1/16" long+ a 1/16" blob. When a component is passed through that and
soldered and the hole filled with solder, the solder connection is 100x
stronger than that of single-sided boards. Vibration tests done at TI in
1960 proved to us that 2-sided boards could sustain 1Khz 5G swings (some
components could
not, though).

These days, the best way to make a prototype is to send it to somebody who
can make a decent 2-sided, 1-oz PCB with good feedthru holes. Its worth the
money, it really is.

--Bob
EDTec LLC



{Original Message removed}

2002\11\24@113018 by Mike Harrison

flavicon
face
Fine as long as you can afford it. Look inside almost any consumer product and you will see the lengths
they go to to avoid using a double sided PCB - loads of wire-links,
ink-printed tracks etc. I'd agree that SS PCBs are nowhere near as
rugged, especially with heavy components, but for a huge number of
applications they are fine, IF carefully designed.
On Sun, 24 Nov 2002 08:28:39 -0700, you wrote:

{Quote hidden}

>{Original Message removed}

2002\11\24@122211 by Wagner Lipnharski

flavicon
face
Mike Harrison wrote:
> Fine as long as you can afford it.
> Look inside almost any consumer product and you will see the lengths
> they go to to avoid using a double sided PCB - loads of wire-links,
> ink-printed tracks etc. I'd agree that SS PCBs are nowhere near as
> rugged, especially with heavy components, but for a huge number of
> applications they are fine, IF carefully designed.


Of course, with the market and price competition for low cost products, it
is amazing how they can produce a PC mouse with switches, electronics,
sensors, rotators, shafts, keys, case, wire, connector, package, etc, for
less than $1.50 at the Taiwan plant.
From the manufacturer cost up to the consumer price, you can think about at
least 600 to 800% price increase. Any 15 cents in cost can means up to 1 or
more dollars at the consumer price, and this can means the product staying
in the market or not.

For this kind of market, one single cent saved from using double side
boards or jumpers on a single side board, will make them go for the single
sided board.  Nobody will complain if a mouse is dropped to the floor and
stop working, it is only a $8 piece of junk anyway, and everyone knows that
dropping electronics to the floor means a high risk to have it not working.

But you will not find single sided boards in expensive products, where
quality and reliability is a must.
Of course you can find single sided boards into cheap $5 multimeters, but
you will not find them on $80 Fluke units.

Suppose you need to produce a 3x4 board, 50 units, just to sell the device
for your friends, or just to start a small gadgets business.  A double
sided PCB will never cost the double of a single side, and in most cases
the board cost is not more than 10% of the whole product, so, suppose you
produce 50 boars for $4 each (single sided), final product cost around $35,
if you move to double sided board, it will increase $2 at the cost, final
product still be possible to be sold by original price without much impact
in profit, but with much better quality.  For low quantity production
without worldwide "dog-eat-dog" competition, I really don't see any strong
reason to not produce in double sided boards.

Even we did it in the past, soon to realize it doesn't make any sense.

VV46NER

--
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\11\24@142018 by Spehro Pefhany

picon face
At 04:29 PM 11/24/02 +0000, you wrote:
>Fine as long as you can afford it.
>Look inside almost any consumer product and you will see the lengths
>they go to to avoid using a double sided PCB - loads of wire-links,
>ink-printed tracks etc. I'd agree that SS PCBs are nowhere near as
>rugged, especially with heavy components, but for a huge number of
>applications they are fine, IF carefully designed.

Horses for courses. If it meets the requirements and is cheaper,
including any stuff you may have to do to make it meet the
requirements (eg. eyelets on some holes), then it's better. A HUGE
number of single-sided boards are made every day. Same with the
laminate- cheap paper phenolic, FR-4, polyimide or Gtek, etc.
Sometimes it's cheaper (or the only way) to go with multilayer,
and swallow the costs. That said, we are doing more 4-layer
designs than single-layer in our market space these days (but the
single-layer designs will have more units built).

High volume designs can use things like injection moldings to
support inexpensive boards and their components mechanically that
would be impractical in a low-quantity product.

Best regards,

Spehro Pefhany --"it's the network..."            "The Journey is the reward"
spam_OUTspeffTakeThisOuTspaminterlog.com             Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog  Info for designers:  http://www.speff.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\11\24@142220 by H. Carl Ott

flavicon
face
 Well, considering that most of the stuff I design these days is SMT, (and
mostly hobby stuff) I'm not sure I see that particular advantage of double
sided pcb manufacture.
 I've seen plenty of TH (through hole) components pop off single and
double sided boards, and I will certainly agree for production boards with
switches, connectors, and higher mass TH components, a double sided board
will do a job better.

 The advantage I do see with single sided prototyping is cost and speed.
Single sided copper clad is cheap. Toner transfer paper is cheap (at least
the stuff I use).
  I can lay out a board in the morning, and have it stuffed and tested by
the evening. And when I find problems in the board, toss it in the garbage
and just cut another one.

 Now, I'm not going to insist that this is a no-brainer process, and it
does take some experimenting to get the process down. But It's not too
difficult for most people, just don't expect perfect results the first time.

  Certainly sending it out to fab house is easier, but when I want it now,
and I want it cheap (we'll not discuss what I pay myself in hourly wages) I
make it myself.

  btw, here is a pdf on my projects page that may help anybody who want's
to experiment with toner transfer pcb fabrication. Learn from my mistakes.
    http://users.rcn.com/carlott/projects.html


-carl


At 08:28 AM 11/24/2002, you wrote:
{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\11\24@143252 by Dominic Stratten

flavicon
face
$1.50 ???????? I pay 0.42 ukp for my mice (through a distributor who make
money on them too !)

Cheaper to buy them and use them for the 9 pin D plugs and cable than to
make my own. The balls are good for putting in your enemies fuel tanks too
;-)


{Original Message removed}

2002\11\24@204744 by James Newton, webmaster

face picon face
source=
http://www.piclist.com/postbot.asp?id=piclist\2002\11\24\142220a

Carl, that is a very nice tutorial you have at
users.rcn.com/carlott/toner_transfer_exp.pdf
I'd like your permission to convert it to HTML and post it on
piclist.com.

---
James Newton: PICList.com webmaster, former Admin #3
.....jamesnewtonKILLspamspam@spam@piclist.com  1-619-652-0593 phone
http://www.piclist.com/member/JMN-EFP-786
PIC/PICList FAQ: http://www.piclist.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\11\24@233522 by Russell McMahon

face
flavicon
face
I have made a spam filter set that moves suspect messages to a "suspect"
folder for checking prior to deletion. I hate to auto-delete material which
may be valid. The filter criteria get tuned over time to catch as much as
possible without too many false traps.

Nine messages from this thread were in my suspect mailbox just now. Looks
like it's time to revise the filter criteria again :-)


       RM

--
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\11\24@234602 by Josh Koffman

flavicon
face
I wonder what set it off. Could it be the question "How do you" ?

Josh
--
A common mistake that people make when trying to design something
completely foolproof is to underestimate the ingenuity of complete
fools.
       -Douglas Adams

Russell McMahon wrote:
> I have made a spam filter set that moves suspect messages to a "suspect"
> folder for checking prior to deletion. I hate to auto-delete material which
> may be valid. The filter criteria get tuned over time to catch as much as
> possible without too many false traps.
>
> Nine messages from this thread were in my suspect mailbox just now.

--
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\11\25@172341 by H. Carl Ott

flavicon
face
 James,
 Certainly you have my permission. I also have the original as a word
document, If that would be easier to convert to html.
 Let me know if you want it, and where to email it.
 I always meant to go back and add some photos, but I don't see that
happening any time soon.

-carl

At 05:44 PM 11/24/2002, you wrote:
{Quote hidden}

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


2002\11\25@172347 by Peter L. Peres

picon face
On Sun, 24 Nov 2002, Dominic Stratten wrote:

*>$1.50 ???????? I pay 0.42 ukp for my mice (through a distributor who make
*>money on them too !)
*>
*>Cheaper to buy them and use them for the 9 pin D plugs and cable than to
*>make my own. The balls are good for putting in your enemies fuel tanks too
*>;-)

What do they do in a fule tank ? They are easy to remove (magnetic).

Peter

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


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