Searching \ for '[EE] Routing SMD boards' 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=routing+smd+boards
Search entire site for: 'Routing SMD boards'.

Exact match. Not showing close matches.
PICList Thread
'[EE] Routing SMD boards'
2010\10\23@123306 by David

flavicon
face
Hi,

I have had some moderate success designing PCBs in Eagle and having them made by BatchPCB.  I currently use a fairly crude method of soldering SMD parts, but it seems to work (info at http://tinyurl.com/2brjyn6). I'm pretty happy with this workflow.

However, the skills I built up manually routing double sided through-hole boards with "huge" components don't translate well to surface mount.

As an example, see the board at http://tinyurl.com/35gdrpx (none of the finishing e.g. silkscreen/ground pours is done yet).  It is a simple breakout for the FT232RL so I can use it with a breadboard, but getting all the wires routed without hundreds of vias is challenging me.

So I would welcome any tips for SMD boards.  Do people use the auto-router?  Would it be more sensible to layout on 2 sides somehow (e.g. Vcc/GND on one, signal on the other).  Do I just need lots more practise at component layout and routing?

And yes, I know you can buy these things.  But I'd rather spend a few weeks reading a datasheet and learning about how things work.

Davi

2010\10\23@124144 by doug metzler

picon face
I put a ground plane on the bottom layer - that way I don't have to route
any of the ground wires, but I can still route on the bottom layer and it
will keep separate from ground.

I never use auto-route - I find it's easier (and somehow very Zen-ful) to
route the thing myself.  Practice is really the key to this.  Once you've
done it a few times it gets easier, then it begins to get tedious, but it
doesn't take that long.

Also spend a little time surfing around and look at how other people have
done it.  Specifically makerbot and arduino board layouts are readily
available and you can even download the Eagle files.

DougM

On Sat, Oct 23, 2010 at 9:33 AM, David <spam_OUTlistsTakeThisOuTspamedeca.net> wrote:

{Quote hidden}

>

2010\10\23@130126 by Mike Harrison

flavicon
face
On Sat, 23 Oct 2010 17:33:02 +0100, you wrote:

>Hi,
>
>I have had some moderate success designing PCBs in Eagle and having them
>made by BatchPCB.  I currently use a fairly crude method of soldering
>SMD parts, but it seems to work (info at http://tinyurl.com/2brjyn6).
>I'm pretty happy with this workflow.
>
>However, the skills I built up manually routing double sided
>through-hole boards with "huge" components don't translate well to
>surface mount.
>
>As an example, see the board at http://tinyurl.com/35gdrpx (none of the
>finishing e.g. silkscreen/ground pours is done yet).  It is a simple
>breakout for the FT232RL so I can use it with a breadboard, but getting
>all the wires routed without hundreds of vias is challenging me.
>
>So I would welcome any tips for SMD boards.  Do people use the
>auto-router?
NO! NO! NO! Don't even think about it!

> Would it be more sensible to layout on 2 sides somehow
>(e.g. Vcc/GND on one, signal on the other).
Yes - normally you'd put a groundplane on  the bottom and do as much routing as possible on top,
using the bottom for occasional jumpers to preserve the  connectivity of the groundplane.
Ground is usually the place that the largest number of connections go  to, so putting it on a plane
instantly means you can pretty much forget about all of these connections.
> Do I just need lots more
>practise at component layout and routing?

Yes. practice is the only way to get better - It can't be taught - you will develop a feel for what
will work.  
The main  thing to  remember is that placement is everything - time   spent getting the placement
right is saved  many times over when routing.  And don't be afraid to rip-up...

Also, take a hard look at existing boards to see how other people have done it. You can learn from
both good and bad examples!

2010\10\23@131059 by Oli Glaser

flavicon
face
On 23/10/2010 17:33, David wrote:
{Quote hidden}

My advice is not to use the autorouter (hardly anyone ever uses them), they never work for anything but the simplest, low speed boards where routing is not critical. Some people use them for selected (non critical) bits on boards which is okay as long as you know what you are doing I suppose. Personally I never use them.
With 2 layer boards often an orthogonal method is used (vertical traces one side, horizontal the other) with a ground plane/fill on one side - if you can route as much on one side as possible and leave the other for a nice (mostly) unbroken ground plane that's good for simple boards. At the very least route power and ground together to minimise loop inductance.
For high speed or mixed signal stuff it's better to use a 4 layer (or above) board and have layers dedicated to ground/power planes, this makes signal integrity/EMI issues much easier to deal with. Vias are a necessary evil with SMD, so get used to having loads of them on your board, if you need a really solid connection you can "stich" a few together..
I would grab a couple of books as it's a complex subject with many differing views on the best way to do things (such as whether to split ground planes between analog and digital or not), there are plenty around - check out some of the documents on this page, they should get you started:
http://search.analog.com/search/default.aspx?query=practical+analog+design+techniques&local=en <http://search.analog.com/search/default.aspx?query=practical+analog+design+techniques&local=en>

Also a couple of books are: High Speed Digital Design (Johnson & Graham) and Real Analog Solutions for Digital Designers. I'm sure there are more PCB specific books around though if you check Amazon..

As you say, practice will help - after making a few boards you should start to get used to what's important.

2010\10\23@132137 by PICdude

flavicon
face
Depends on what the circuit is.  For switching regulators, etc, I  don't use the auto-router, but I do use it regularly for other boards.    I almost always add guard rings first, route the ground trace and  other power traces manually, then I'll route analog traces manually.   The digital traces usually get auto-routed, but if they're interfering  with the analog traces, I'll restrict the appropriate areas.  I  usually add ground and Vdd traces last.

The auto router gets the job done as a first pass, but there are a  number of things that bug me about it, so there's always some tweaking  to do.

Cheers,
-Neil.


Quoting David <.....listsKILLspamspam@spam@edeca.net>:

> Hi,
>
> ...
> So I would welcome any tips for SMD boards.  Do people use the
> auto-router?  Would it be more sensible to layout on 2 sides somehow
> (e.g. Vcc/GND on one, signal on the other).  Do I just need lots more
> practise at component layout and routing?
> ...

2010\10\24@084544 by Olin Lathrop

face picon face
David wrote:
> Do people use the auto-router?

I certainly do.  It's a great tool as long as you undertand it can't take
care of everyting for you, and that you really have to read the manual
several times to understand what all the tweaks do and then how to use them
to achieve what you want.

I usually route a few critical sections manually, then iterate with the auto
router to do the rest.  In the beginning I use just a single route pass to
see what kind of solution it comes up with.  Then I may move some things
around, tweak the net classes, and manually route a few things.  Repeat
until you get a reasonable enough first pass route.  Then crank up the
optimization passes.  I usually use 8 for the final route.  The first pass
is optimized to find a solution.  The remaining passes try to tweak the
solution to minimize via, use of the bottom layer, or whatever is important
in that design.

> Would it be more sensible to layout on 2 sides somehow
> (e.g. Vcc/GND on one, signal on the other).  Do I just need lots more
> practise at component layout and routing?

Good layout is the first step to good routing.  If the layout is a mess, the
route will be too.  Place anything that needs to be in a fixed place first
(external connectors, mounting holes, etc), then try to have the layout
follow the logical structure of the circuit.  That minimizes the impact of
interconnects between subsystems and keeps the connections inside subsystems
small and local.

For two layer boards, I often make the bottom layer a pseudo ground plane.
That means its mostly a ground plane except for short "jumpers" to make the
toplogy work.  Setting the cost of routing inside polygons high helps the
autorouter do this, but it then unfortunately tends to lump the jumpers
together.  In this case the success metric is not the number of islands in
the ground plane but how small their largest dimensions are.  In other
words, a bunch of small islands is better than a big one, as long as the
ground signal can reasonably flow around the small islands.


********************************************************************
Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products
(978) 742-9014.  Gold level PIC consultants since 2000

2010\10\24@085046 by Olin Lathrop

face picon face
Mike Harrison wrote:
>> So I would welcome any tips for SMD boards.  Do people use the
>> auto-router?
>
> NO! NO! NO! Don't even think about it!

That's totally silly, of course.

It's a tool.  It's not perfect, and it requires you to be in the loop, but
so do a hammer and a srew driver.  People who knee jerk say you can't use
the auto router haven't bothered to learn it.  You do have to read the
manual, several times.  It's not free, but it can do the routine stuff with
no errors and a lot faster than you can.


********************************************************************
Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products
(978) 742-9014.  Gold level PIC consultants since 2000

2010\10\25@020235 by Oli Glaser

flavicon
face
On 24/10/2010 13:46, Olin Lathrop wrote:
> David wrote:
>> Do people use the auto-router?
> I certainly do.  It's a great tool as long as you undertand it can't take
> care of everyting for you, and that you really have to read the manual
> several times to understand what all the tweaks do and then how to use them
> to achieve what you want.

I agree with the above actually, I was a bit hasty  with my last post in which I had also meant to say something similar, but rereading it I gave the autorouter what might sound like the thumbs down which is not entirely what I intended.
Of course it's a tool like anything else and if you treat it that way and don't expect it be perfect and to do the whole job for you then it can help.
The reason I don't use them (I have occasionally in the past for small bits of boards) is I haven't found one I like very much, and also possibly as I didn't spend enough time learning how to control them properly.
Bottom line is as long as you know what the end result you want is (very important as the autorouter can't think for you) then you should be able to achieve that whichever way you choose. It depends a lot on the type of board too of course, making a very sensitive mixed signal board is going to be a totally different process to a slowish digital board with non "sensitive" parts, I'm sure some autorouters could do pretty decent jobs on the whole of such boards if set up correctly.
If I ever start using them again I would use them in the way Olin mentioned, and spend some time to learn how to get them to do the things I want easily and quickly (which is the whole point, if I can do it quicker manually or have to spend ages "cleaning" up after the autorouter then it kind of defeats the objective)

2010\10\25@060812 by RussellMc

face picon face
> Yes - normally you'd put a groundplane on  the bottom and do as much routing as possible on top,
> using the bottom for occasional jumpers to preserve the  connectivity of the groundplane.

Y'All - feel free to critique this if any is bad or overdone advice.
(I know that at least one person doesn't need that encouragement :-)
).

Do note that while doing this is usually fine you must be sure that
you are not bisecting a significant current path. A significant path
may be either a large current one almost regardless of context
(almost) or a variably small one in analog circuitry or where
miscellaneous minor voltages count.

If you cut across a return current path from  a track on the top layer
the current will route around the slot on both side and you end up
with a slot radiator This may have effects from essentially zero to
stunningly terrible. Experience will introduce you to the stunningly
terrible cases :-). Very large currents should probably be encouraged
to stay off your groundplane unless unavoidable.

As people have been talking about "short jumpers" in this context the
effects should usually be not too bad. (Murphy loves "should" and
"usually" so keep an eye out for him :-) ).

Another possible effect is local potential rise at a crucial analog
point as currents route around a jumper "slot". This "should usually"
be an issue only for fully analog circuits or for components related
to eg a uP's ADC. If you have eg external pull down resistors on an
ADC pin you "probably don't" want a slot between them and their
desired ground return point. If you use an external ADC voltage
reference the same applies to it's "ground" connection and the
processor's analog ground pin. These should always be tightly adjacent
so not usually an issue. Don't let FET gate pulldowns or clamp diodes
get separated from their drains by a break. In this case the risk is
"interesting" parasitic gate oscillations which can translate into
interesting load excursions and even interesting holes in your FETs.




     Russell McMahon

2010\10\25@110235 by Dave Lagzdin

picon face
I'd get real "tweezers",  useful

media.digikey.com/Photos/Wiha/MFG_44501.jpg
http://media.digikey.com/Photos/Wiha/MFG_44510.jpg

On 23 October 2010 12:33, David <listsspamKILLspamedeca.net> wrote:
> Hi,
>
> I have had some moderate success designing PCBs in Eagle and having them
> made by BatchPCB.  I currently use a fairly crude method of soldering
> SMD parts, but it seems to work (info at http://tinyurl.com/2brjyn6).
> I'm pretty happy with this workflow.

2010\10\25@112408 by Gary Crowell

picon face
On Sun, Oct 24, 2010 at 6:46 AM, Olin Lathrop <.....olin_piclistKILLspamspam.....embedinc.com>wrote:

> David wrote:
> > Do people use the auto-router?
>
> I certainly do.
>

Very good advice follows.


> Good layout is the first step to good routing.  If the layout is a mess,
> the
> route will be too.


The only thing I'd add is that a good layout actually starts with a good
schematic.  Logical organization and signal flow there makes the translation
to a practical layout much easier.  The schematic is also the
most convenient place to assign net classes and most design rules.

PCB designers regularly get flack from managers who want to know "how much
routing is done" on a project.   They don't understand when you say "none -
still in palcement"  (or, "still adjusting rules").  They don't perceive
that as progress.  In fact, when the placement (and rules) is (are) well
done, the routing practically falls out on it's own.  The %routed = work
approach often results in a routing nightmare.  Substitute
planning<>placement, and coding<>routing, and it's the same as writing
software.

Gary

----------------------------------------------
Gary A. Crowell Sr., P.E., CID+
Linkedin <http://www.linkedin.com/in/garyacrowellsr>
Elance<www.linkedin.com/redirect?url=http%3A%2F%2Fgaryacrowellsr%2Eelance%2Ecom&urlhash=kJm9>
 KE7FI

2010\10\25@112600 by alan.b.pearce

face picon face
> I'd get real "tweezers",  useful
>
> media.digikey.com/Photos/Wiha/MFG_44501.jpg
> http://media.digikey.com/Photos/Wiha/MFG_44510.jpg

I find the ones with crossed over tips ("Normally Closed" tips) useful
for handling things like resistors, capacitors and transistors.
-- Scanned by iCritical.

2010\10\25@113258 by Mark E. Skeels

flavicon
face
Gary and all,

This is a great point and as an engineer, don't you find it a constant struggle to explain things like this to management?

It's difficult because we are always doing something for people who don't understand what we do, but have responsibility to evaluate the results.

Mark Skeels
Engineer
Competition Electronics, Inc.
TEL: 815-874-8001
FAX: 815-874-8181
http://www.competitionelectronics.com

[SNIP]

{Quote hidden}

2010\10\25@114134 by Dave Lagzdin

picon face
On 25 October 2010 11:26,  <EraseMEalan.b.pearcespam_OUTspamTakeThisOuTstfc.ac.uk> wrote:
>> I'd get real "tweezers",  useful
>>
>> media.digikey.com/Photos/Wiha/MFG_44501.jpg
>> http://media.digikey.com/Photos/Wiha/MFG_44510.jpg
>
> I find the ones with crossed over tips ("Normally Closed" tips) useful
> for handling things like resistors, capacitors and transistors.
> --

Can you get those in an equally fine tip?

2010\10\25@114831 by William \Chops\ Westfield

face picon face

On Oct 25, 2010, at 8:24 AM, Gary Crowell wrote:

> a good layout actually starts with a good schematic.

When dealing with something like a microcontroller, it is worth  keeping in mind that IO pins may be interchangeable (pin-swappable) in  ways that you might normally overlook.  For example, it's extremely  logical that segments A-G of a display map directly to bits 0-6 of  some IO port, but the firmware won't be any more complex if the  mapping is more random (A=3, B=0, C=6, ...) and it might make the PCB  layout much easier (depending on the actual pinouts of the devices  involved.)

BillW

2010\10\25@115944 by alan.b.pearce

face picon face


> -----Original Message-----
> From: piclist-bouncesspamspam_OUTmit.edu [@spam@piclist-bouncesKILLspamspammit.edu] On Behalf Of Dave
> Lagzdin
> Sent: 25 October 2010 16:42
> To: Microcontroller discussion list - Public.
> Subject: Re: [EE] Routing SMD boards
>
> On 25 October 2010 11:26,  <KILLspamalan.b.pearceKILLspamspamstfc.ac.uk> wrote:
> >> I'd get real "tweezers",  useful
> >>
> >> media.digikey.com/Photos/Wiha/MFG_44501.jpg
> >> media.digikey.com/Photos/Wiha/MFG_44510.jpg
> >
> > I find the ones with crossed over tips ("Normally Closed" tips) useful
> > for handling things like resistors, capacitors and transistors.
> > --
>
> Can you get those in an equally fine tip?

I haven't attempted to get them with an especially fine tip, but I would guess they would be available. The ones I have are ordinary modellers ones, but I am not attempting anything smaller than 0603, and the tips are not the finest grade points on them. I could imagine the very fine needle tips would be required if going smaller.
-- Scanned by iCritical.

2010\10\25@124203 by doug metzler

picon face
of the two tweezers above I strongly recommend the ones with the bent tips,
marked 7A.

I use them both at work and at home all the time.  They are unbeatable.

DougM

On Mon, Oct 25, 2010 at 9:00 AM, <RemoveMEalan.b.pearceTakeThisOuTspamstfc.ac.uk> wrote:

>
>
> > {Original Message removed}

2010\10\25@141131 by Olin Lathrop

face picon face
Mark E. Skeels wrote:
> This is a great point and as an engineer, don't you find it a constant
> struggle to explain things like this to management?

No, at least not to good management.  If they don't get it, then it's your
job as the engineer to dumb it down to their level and explain what they
should expect to see when in terms they can understand.

It's not good enough just to be a techno-weenie.  You have to be able to
explain a technical issue to someone non-technical in terms that are
relevant to them.

> It's difficult because we are always doing something for people who
> don't understand what we do, but have responsibility to evaluate the
> results.

Part of your job is to explain it in terms they can understand and that are
relevant to them.  If a manager doesn't understand layout and routing, just
tell them your in the middle of the design and you expect to send out boards
by the end of next week, or whatever the situation is.


********************************************************************
Embed Inc, Littleton Massachusetts, http://www.embedinc.com/products
(978) 742-9014.  Gold level PIC consultants since 2000

2010\10\25@143833 by Mark E. Skeels

flavicon
face
On 10/25/2010 1:12 PM, Olin Lathrop wrote:
> Mark E. Skeels wrote:
>> This is a great point and as an engineer, don't you find it a constant
>> struggle to explain things like this to management?
> No, at least not to good management.  If they don't get it, then it's your
> job as the engineer to dumb it down to their level and explain what they
> should expect to see when in terms they can understand.
>
> It's not good enough just to be a techno-weenie.  You have to be able to
> explain a technical issue to someone non-technical in terms that are
> relevant to them.
>
Right; I have found that I actually enjoy this process. But as you point out, it is part of the job, Olin. A part some people may not expect.

Mark

2010\10\25@170647 by David

flavicon
face
On 25/10/2010 16:02, Dave Lagzdin wrote:
> I'd get real "tweezers",  useful
>
> media.digikey.com/Photos/Wiha/MFG_44501.jpg
> http://media.digikey.com/Photos/Wiha/MFG_44510.jpg

I agree.  Currently I have a nice pair of locking tweezers and a few pairs of tweezers that are used in surgery.  Very very fine tips, designed for suturing.

It's the applying heat part of my process that is "crude", as it involves an old frying pan and a gas hob.

(Currently working through the other replies on and off-list, thanks!

2010\10\25@171835 by David

flavicon
face
On 25/10/2010 16:24, Gary Crowell wrote:
> On Sun, Oct 24, 2010 at 6:46 AM, Olin Lathrop<spamBeGoneolin_piclistspamBeGonespamembedinc.com>wrote:
> Very good advice follows.
>
>> Good layout is the first step to good routing.  If the layout is a mess,
>> the
>> route will be too.
>
> The only thing I'd add is that a good layout actually starts with a good
> schematic.  Logical organization and signal flow there makes the translation
> to a practical layout much easier.  The schematic is also the
> most convenient place to assign net classes and most design rules.

Well in this case (hijacking my own thread), you can see the original schematic here:

http://tinyurl.com/2wegteq

I haven't finished the connections between signal lines and the pin header (which will just be in whatever order is most convenient for routing) and there are some labels missing.  I also need to check the ^RESET line in the datasheet.

Comments on the schematic layout would be fine, but please don't slate my usage of the FT232 until I've had a chance to check what I'm doing :)

This is a hobby that I have no intention of turning into a career, but unfortunately my OCD side likes to get things as close to "right" as practical.

Davi

2010\10\25@200140 by Jesse Lackey

flavicon
face
Hi - I concur with this and the thread in general, with just a bit to add.

I put a ground pour on top and bottom of all designs, and in one of the two middle layers of a 4-layer.  Of course doing dc/dcs or precision analog etc. changes all this, but for general noncritical stuff a ground pour (solid, not hatched) of usually 16 or 24 mil wide wires and 12 to 24 mil isolate.  If you're going to have boards made without soldermask (say barebonespcb.com) a larger isolate is really helpful.

I spend a lot of time doing parts placement.  A board with parts well placed almost "routes itself".  A really dense board with parts well placed means it is possible to route it vs. just simply impossible.  The better the placement the faster the route goes and the fewer vias and traces on the backside, which leaves more solid ground copper and less electrical noise and more flexibility for changing/adding parts to fix design problems in the next spin etc. etc.

Autorouter.  I don't use it, I found that it was more work to set up net classes and whatnot to get results that I wasn't particularly happy with to be worth doing.  But.  It is great for doing 'test routes', in the sense that if it has a real hard time, you probably will to.  For significant designs (> 100 parts and/or seriously space constrained) this helps to explore overall placement strategies or establish a good pcb size for detailed cost / size analysis (i.e. if it is installed in a space constrained larger system, how much of the available room will it take up?) before doing all the detailed routing work.

I set the via drill to be 16mm, and in the DRC you can change the restring I think it is to get the smallest via that can be made with the cheapest mfgr design rules, which have 15mil or 16mil minimum drills else you pay more.  This definitely helps vs. the Eagle default vias.

If you do use the autorouter, be sure to do (of course) critical routes first - anything needing more than trivial power, traces to xtals, decoupling caps, all of dc/dcs, and other critical analog.  Save your work, then fiddle with the autorouter.  In version 4 of Eagle you can't "undo" the autorouter's work, you can only rip up traces and there could be many, so having a saved state to reopen is essential.

Have fun!
J



doug metzler wrote:
{Quote hidden}

>> -

2010\10\26@030349 by Ruben Jönsson

flavicon
face
>
> On Oct 25, 2010, at 8:24 AM, Gary Crowell wrote:
>
> > a good layout actually starts with a good schematic.
>
> When dealing with something like a microcontroller, it is worth  
> keeping in mind that IO pins may be interchangeable (pin-swappable) in  
> ways that you might normally overlook.  For example, it's extremely  
> logical that segments A-G of a display map directly to bits 0-6 of  
> some IO port, but the firmware won't be any more complex if the  
> mapping is more random (A=3, B=0, C=6, ...) and it might make the PCB  
> layout much easier (depending on the actual pinouts of the devices  
> involved.)
>
> BillW

Yes - and with a lot of microcontrollers you can actually configure at what pin a certain function is going to be placed. By function I mean Serial, pwm, timer IO and so on. This is extreamly useful when optimizing component placement on the layout. I wonder if there are autorouters that considers this?

/Ruben


==============================
Ruben Jönsson
AB Liros Electronic
Box 9124, 200 39 Malmö, Sweden
TEL INT +46 40142078
FAX INT +46 40947388
RemoveMErubenspamTakeThisOuTpp.sbbs.se
==============================

More... (looser matching)
- Last day of these posts
- In 2010 , 2011 only
- Today
- New search...