Searching \ for '[OT] Eagle board layout questions' 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=eagle
Search entire site for: 'Eagle board layout questions'.

Exact match. Not showing close matches.
PICList Thread
'[OT] Eagle board layout questions'
2005\05\29@120853 by jrem

picon face
I am looking for Eagle Light clues for the best way to layout a single
sided board with the minimum number of top side routings and vias.  Are
there any hints as to board layout which can help me accomplish this?
I typically lay out the board then move stuff around, ripup, ratsnest,
and auto to try to minimize the top laer routings, but I never can seem
to get it optimized.  

Thanks, John.

__________________________________________________
Do You Yahoo!?
Tired of spam?  Yahoo! Mail has the best spam protection around
http://mail.yahoo.com

2005\05\29@123104 by Robert Young

picon face
----- Original Message -----
From: "jrem" <spam_OUTjrem123TakeThisOuTspamyahoo.com>
To: <.....piclistKILLspamspam@spam@mit.edu>
Sent: Sunday, May 29, 2005 11:08 AM
Subject: [OT] Eagle board layout questions


> I am looking for Eagle Light clues for the best way to layout a single
> sided board with the minimum number of top side routings and vias.  Are
> there any hints as to board layout which can help me accomplish this?
> I typically lay out the board then move stuff around, ripup, ratsnest,
> and auto to try to minimize the top laer routings, but I never can seem
> to get it optimized.
>
> Thanks, John.
Some very GENERAL suggestions.  Your milage may vary.

1) Don't bother with the auto router for a single layer board.  Do you
yourself.  It is an OK autorouter but sometimes it just isn't worth fooling
with.  This sounds like one of those times.

2) Watch the rats nest when initially placing parts.  Keep in mind that you
can switch back to the schematic and swap gates and if necessary re-connect
pins (ie exchange A for B on 2 input AND gate).

3) When routing, route power and ground first as these are going to be
serpentine traces on single sided boards.  Use wider than normal trace
widths for power and ground.

Item #2 is probably going to pay the biggest dividends.

Rob

2005\05\29@130053 by Bob Blick

face picon face
Hi John,

I don't use Eagle, but in general the advice is to raise the cost of
top layer, and raise the cost of vias. Sometimes it ends up being a
tossup between running the autorouter over and over while adjusting
it, and routing by hand.

Cheers,

Bob


On 29 May 2005 at 9:08, jrem wrote:
> I am looking for Eagle Light clues for the best way to layout a single
> sided board with the minimum number of top side routings and vias.  Are
> there any hints as to board layout which can help me accomplish this?
> I typically lay out the board then move stuff around, ripup, ratsnest,
> and auto to try to minimize the top laer routings, but I never can seem
> to get it optimized.  

2005\05\29@130246 by phil B

picon face
good advice in general.  I've long ago given up on the
autorouter.   In general, I've found that manual
routing isn't that hard and gives you a much better
feel for the board you are making.  After you've done
a couple, you'll get a good sense of how to place
things so they route easily.

If you want a truely single sided board, you may have
to really work at it.  I get good results by making
one side a ground layer and that tends to really
simplify the problem.  It also makes for a quieter
board.

To get good logical component grouping from the start,
I lay out the schematic in such a way that the
components of each subcircuit are near each other.  I
name and lable nets and dont necessarily run actual
nets between connected pins.  This allows the
schematic to be layed out somewhat akin to the board
layout.  Then parts are somewhat logically group on
the board when I create it from the schmatic.  

Pin and gate swap is useful though you may have to
tweak the libraries (74xx libs seem to be deficient
there) - its a good idea to examine the libs 'cause
they aren't always right.  Its pretty suprising how
many libs have all the pins at swap level 0.  You
might also consider changing pin assignments on your
PIC based on simplifying routing.  switch back to
schematic and change them.  Many pins are
interchangable (though not all, take care).

I actually route all the short runs first and then do
power/gnd.  With a ground layer, the power is usually
easy to route.

Phil

shouldn't this be tagged EE rather than OT?


--- Robert Young <rwyoungspamKILLspamieee.org> wrote:
> {Original Message removed}

2005\05\29@170729 by William Chops Westfield

face picon face
On May 29, 2005, at 9:08 AM, jrem wrote:

> I am looking for Eagle Light clues for the best way to layout a single
> sided board with the minimum number of top side routings and vias.

The Eagle autorouter is not very good at single sided boards.  It's big
"trick" for routing seems to involve moving tracks to another layer, and
when it can't do that...  Still, attempting a single sided route can be
a good way of evaluating your placement, orientation, and packaging  
choices.
There is a 1layer.ctl file at

http://www.cadsoft.de/cgi-bin/download.pl?page=/home/cadsoft/
html_public/download.htm.en&dir=pub/userfiles/misc

that sets up the autorouter somewhat appropriately.

Density is the enemy of one-sided routing (and vis versa.)  If you're  
doing
homemade boards, you may find it worthwhile to make modified libraries  
with
extra space between pads (transistors with .15 inch lead spacing instead
of .1, for instance.)  Resistors are your friends; you can fit several
traces underneath a typical 1/4W resistor, and it's a good trick for  
getting
signals to where you want them (although I'm not sure I can explain  
exactly
how that works; you just have to get a feel for it...)

Leave a lot of room between your components for your initial attempts at
routing; you can always move them closer together after you have a good  
idea
where there is room for them.

Be willing to swap pins around, even pins that would not traditionally  
be
considered swappable (like the IO pins on a microcontroller.)  It's  
pretty
easy to change which pin does what in software, and it can be worth it  
if
it makes your board layout easier.  You will need to learn just which  
pins
can and can't be switched: on a 12f675, GP0,1,2,4,5 are swappable if  
you're
doing digital IO, but not if you're using some of their alternate  
functions
(comparator, timer, etc), and GP3 is input only, for instance.

Some chips just seem better designed for single sided PCB layouts.
74x540 vs 74x240 is obvious, but also I find the "end" power pins of a
12f PIC more convenient than the corner pins of an ATtiny11, for  
instance.
Some of the modern chips with multiple GND and Power pins are pretty  
impossible.

People have recommended putting the power traces in first, which makes  
a fair
amount of sense.  However, typical power routing can be very disruptive  
to the
layout of other signals, and you may want to think of this as laying  
out the
power BUSSES first, and worrying about the actual chip connections to  
the
power later; you may get your most "bang for the buck" using jumpers on  
the
power net (and jumpers are nice and heavy compared to the tiny traces  
you can
run signals through.)

BillW

2005\05\30@105522 by olin_piclist

face picon face
jrem wrote:
> I am looking for Eagle Light clues for the best way to layout a single
> sided board with the minimum number of top side routings and vias.

If it's single sided, then there can't be vias.  Something doesn't make
sense.


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

2005\05\30@105930 by olin_piclist

face picon face
Bob Blick wrote:
> I don't use Eagle, but in general the advice is to raise the cost of
> top layer, and raise the cost of vias. Sometimes it ends up being a
> tossup between running the autorouter over and over while adjusting
> it, and routing by hand.

I've never tried doing a single sided board with Eagle.  I guess your method
uses the second layer to have Eagle tell you where the jumpers need to be.
However, I see a problem when using thru hole parts.  Eagle will assume the
holes are plated and connect to both layers.  That will not be valid in
cases when the pins under a component on the top side are inaccessible.
Somehow you need Eagle to think that thru hole pads only connect to the
bottom layer, but I don't know how to do that short of defining new packages
in the libraries.


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

2005\05\30@123519 by Peter

picon face

On Mon, 30 May 2005, Olin Lathrop wrote:

> I've never tried doing a single sided board with Eagle.  I guess your method
> uses the second layer to have Eagle tell you where the jumpers need to be.
> However, I see a problem when using thru hole parts.  Eagle will assume the
> holes are plated and connect to both layers.  That will not be valid in
> cases when the pins under a component on the top side are inaccessible.
> Somehow you need Eagle to think that thru hole pads only connect to the
> bottom layer, but I don't know how to do that short of defining new packages
> in the libraries.

Actually you use keepouts under the parts and pretty strong bias against
anything non-vertical on the top layer and Eagle will get it right most
of the time (with some help). The 'vias' will simply be promoted to pads
where the wire bridges are soldered.

With some coaxing Eagle can make pretty good single sided boards like
that.

Peter

2005\05\30@123637 by phil B

picon face
I've run into this (non-PTH problem) as I often make
my own PCBs.  Its fairly easy to look at a part/pin
and decide if you can solder it on both sides -
resistors, axial caps and diodes, for example.
Sockets, for example, aren't.   I avoid doing it with
ICs because of heating issues.  You do need to take
into account placement/installation order.  So you
form a set of mental design rules for non-PTH boards.
Vias can be made with a simple piece of wire soldered
on both sides.  Its kind of ugly but does work.  I can
turn a board around in hours rather than days and a
board designed with the non-PTH rules still works when
made by a board house.

For the autorouter, you weight the top really costly
and it will route mostly on the bottom.  But you still
need to fix up the board to handle the non-PTH design
rules.  A via will do the trick but I've found its not
that hard to do it "right" and avoid a via.  I don't
bother with the autorouter for a number of reasons
though non-PTH isn't one of them.

Phil


--- Olin Lathrop <.....olin_piclistKILLspamspam.....embedinc.com> wrote:
{Quote hidden}

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

2005\05\30@140319 by PicDude

flavicon
face
For single-sided with Eagle, I turn off the top layer altogether, so it routes
only the bottom layer.  Then with the resulting set of unrouted traces, I
move components around and re-route, or manually route some of those.  The
remaining unrouted traces become jumpers, so for those I just add VIAs in
appropriate locations.

For double-sided boards that are non-PTH, I do something similar, but prior to
routing, I place small circles with the tRestrict layer over the component
pins that are unsolderable on the top.  For any vias that get automatically
created, I do the same (use a wire), but I enlarge the pads first.

Cheers,
-Neil.



On Monday 30 May 2005 11:36 am, phil B scribbled:
{Quote hidden}

2005\05\30@160637 by William Chops Westfield

face picon face

On May 30, 2005, at 7:59 AM, Olin Lathrop wrote:

> Somehow you need Eagle to think that thru hole pads only connect to the
> bottom layer, but I don't know how to do that short of defining new
> packages
> in the libraries.

eg, you don't want your jumpers going through the same holes as
component
pins.  (Hmm.  Probably.  OTOH, it would cut down on drilling, and 30g
Wire
doesn't take up much space.  OTTH, I tried this once and it was a
pain...)
You don't particularly want jumpers that go UNDER other components
either.

I you're trying for a single sided board, hopefully the number of
top-side
traces will be relatively small, whether or they connect through pins.  
In
that case, it is relatively easy to move the jumpers off of the pins to
a
more convenient location...

BillW


'[OT] Eagle board layout questions'
2005\06\01@113731 by alan smith
picon face
WE have a $30,000 autorouter....that makes a good
spagetti dinner.  All our critical routes we do by
hand, especially all of my analog and power supplies.
Autorouters are ok sometimes....but typically needs
cleanup after anyway.



               
__________________________________
Do you Yahoo!?
Make Yahoo! your home page
http://www.yahoo.com/r/hs

2005\06\01@114334 by alan smith

picon face
A long time ago...in a fab house far away.....

I cost extra to do a single sided board vs double.
Talking like 15+ years ago, where boards were done
with mylar tape...

Now days, most fab houses start with double clad board
and so it all gets etched off anyway, and to photo
mask both sides is pretty much in the noise.  Only
additional costs are plating the holes, again, pretty
cheap now.

Before just blindly going down the path of forcing to
single sided board, make sure it warrents the cost.
Of course, if your etching yourself, guess thats a
different story.


--- Olin Lathrop <EraseMEolin_piclistspam_OUTspamTakeThisOuTembedinc.com> wrote:

{Quote hidden}

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

2005\06\01@141421 by Spehro Pefhany

picon face
At 08:43 AM 6/1/2005 -0700, you wrote:
>A long time ago...in a fab house far away.....
>
>I cost extra to do a single sided board vs double.
>Talking like 15+ years ago, where boards were done
>with mylar tape...
>
>Now days, most fab houses start with double clad board
>and so it all gets etched off anyway, and to photo
>mask both sides is pretty much in the noise.  Only
>additional costs are plating the holes, again, pretty
>cheap now.

Yes, the difference is probably more in the photoplotting and setup
rather than the per-board costs with most board houses. It's hardly worth
worrying much about these days. The difference between 2 and 4 layers is
far more.

>Before just blindly going down the path of forcing to
>single sided board, make sure it warrents the cost.
>Of course, if your etching yourself, guess thats a
>different story.

Or if you're buying a stamped single-sided board in *large* quantity.
There, the process is completely different (typically done in a different
factory entirely, even if its the same company) and the cost difference can be
quite impressive. All the holes and the outline created in one quick press
operation. The holes are too rough to plate through, but it's possible to
make double-sided boards of dubious reliability using low-temperature-
cured gunk deposited in the holes (as used in some TV remotes, for example).

But for 1,000 boards or whatever? F'getaboutit.

Best regards,

Spehro Pefhany --"it's the network..."            "The Journey is the reward"
speffspamspam_OUTinterlog.com             Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog  Info for designers:  http://www.speff.com
->> Inexpensive test equipment & parts http://search.ebay.com/_W0QQsassZspeff


2005\06\02@035437 by Alan B. Pearce

face picon face
>>Now days, most fab houses start with double clad board
>>and so it all gets etched off anyway, and to photo
>>mask both sides is pretty much in the noise.  Only
>>additional costs are plating the holes, again, pretty
>>cheap now.
>
>Yes, the difference is probably more in the photoplotting
>and setup rather than the per-board costs with most board
>houses. It's hardly worth worrying much about these days.
>The difference between 2 and 4 layers is far more.

I suspect that for a factory made single sided PCB there is no saving, as
the photo plotting would be done by a step and repeat operation, and the
operators would expect to have 2 photoplots, so having only one will upset
their "normal operating procedure" and become a special case.

>>Before just blindly going down the path of forcing to
>>single sided board, make sure it warrents the cost.
>>Of course, if your etching yourself, guess thats a
>>different story.

Agreed

>Or if you're buying a stamped single-sided board in *large* quantity.

Yeah, just look at the PCB used in your video recorder. I dismantled one
that died recently, and was quite surprised. Single sided punched paxolin
PCB, many wire links, surface mount components except for all electrolytic
caps, some crystals and connectors, and the large components in the power
supply.

More... (looser matching)
- Last day of these posts
- In 2005 , 2006 only
- Today
- New search...