[EE] Kicad auto-routing

[Zik Saleeba]

I've become frustrated with EAGLE's auto-router. It's really only
usable on the simplest designs - and in those cases hand routing is
easy anyway.

I'm thinking of changing to Kicad. Does anyone have experience with
Kicad's auto-router? How well does it work? Do I have to move to a
more expensive PCB program to get decent auto-routing?

Thanks,
Zik
--
http://www.piclist.com PIC/SX FAQ & list archive
View/change your membership options at
http://mailman.mit.edu/mailman/listinfo/piclist

[Nuno Sucena Almeida]

Hi,

I never used Kicad, but this note seems relevant:

http://kicad.sourceforge.net/wiki/index.php/About_KiCad#MUCS-PCB_Autorouter

On Thursday 27 September 2007 07:25:07 pm Zik Saleeba wrote:
> Kicad

--
http://aeminium.org/slug/

[Morgan Olsson]

Den 2007-09-28 01:25:07 skrev Zik Saleeba <z...@zikzak.net>:

> I've become frustrated with EAGLE's auto-router.

Try http://www.freerouting.net/
You can run it together with Eagle on any modern OS (Java)
It also have nice manual push and shove.

> It's really only
> usable on the simplest designs - and in those cases hand routing is
> easy anyway.

I find the eagle autorouter handy to check routability, mode components arund until itis ood, then clean up everything, add most important connections manually, and let it finish it.

But mostly i hand route anyway...

>
> I'm thinking of changing to Kicad. Does anyone have experience with
> Kicad's auto-router? How well does it work? Do I have to move to a
> more expensive PCB program to get decent auto-routing?

I have tried specctra
Before that Ultiroute.

I always end up hand-routing most...

Bu that said i mostly do 2-sided boards and a handful IC:s plus hundred discretes or so.

--
Morgan Olsson

[Xiaofan Chen]

On 9/28/07, Zik Saleeba <z...@zikzak.net> wrote:
> I've become frustrated with EAGLE's auto-router. It's really only
> usable on the simplest designs - and in those cases hand routing is
> easy anyway.
>
> I'm thinking of changing to Kicad. Does anyone have experience with
> Kicad's auto-router? How well does it work? Do I have to move to a
> more expensive PCB program to get decent auto-routing?
>

I do not have much experiences with PCB layout since I have not
done any PCB layout. I always work with the layout designers.
They all told me the auto-router is basically useless for my designs.
In my previous job, mostly it was simple 2 layer board with some
power supply, analog processing and a PIC and the layout tool
was P-CAD. Space constraints were always a problem for
sensors (liquid level sensor and photoelectric sensors). CE
compliance was also a big concern -- most re-layout modification
was due to CE.

In the current job and this is my first project in the company,
it is relative more complicated with 3 small 8-layer boards
with blind/buried vias and the tool is Expedtion. It is heavily
on the analog side. Even the very experienced
PCB designer called it a very difficult design due to
space constraints. We have to add the plan for 3rd layout
due to function and CE issues on the first prototypes.

In both jobs, the layout designers do not use auto-router.

Maybe auto-router will be ok for part of the work on
relative low speed digital desig with not much space
constraint.

Xiaofan

[Vitaliy]

Zik Saleeba wrote:
> I've become frustrated with EAGLE's auto-router. It's really only
> usable on the simplest designs - and in those cases hand routing is
> easy anyway.

Welcome to the club. :)

> I'm thinking of changing to Kicad. Does anyone have experience with
> Kicad's auto-router? How well does it work? Do I have to move to a
> more expensive PCB program to get decent auto-routing?

It seems that if you want quality, hand routing is the only way to go. I
find myself hand-routing even in situations where I need something
quick-and-dirty (yes, I'm picky).

Last time I checked, ELECTRA does a much better (and quicker) job than
Eagle's built-in autorouter, but it wasn't good enough to justify the price.

http://www.konekt.com/support.htm

Here's a link to the 14-day trial:

http://www.konekt.com/dld/product/setup.exe

Vitaliy

[Zik Saleeba]

Thanks Vitaliy and everyone else who responded. I've decided to try to
learn to love hand-routing.

Cheers,
Zik

[David VanHorn]

> It seems that if you want quality, hand routing is the only way to go. I
> find myself hand-routing even in situations where I need something
> quick-and-dirty (yes, I'm picky).

Picky pays..

I'm working with a PC-104 system now, that has significant EMI issues.
Looking at the layout, it's obviously autorouted, and they did all the
things that I would NEVER do, like dumping crystal cap ground leads
into the ground plane, when it was DEAD EASY to route them properly.
As a result, and absolutely symptomatic of bad layout, there's
significant EMI that gets worse when you plug in any shielded cable.
The "ground" is carrying high frequency currents, which are taking
every possible path home through the plane, instead of being carried
home on a single isolated track.

Smart autorouters seem to be like flying cars or AI. Always just a
few years away.

[Hazelwood Lyle]

> -----Original Message-----
> From: piclist...@mit.edu
> [mailto:piclist...@mit.edu]On Behalf
> Of David VanHorn

> I'm working with a PC-104 system now, that has significant EMI issues.
> Looking at the layout, it's obviously autorouted, and they did all the
> things that I would NEVER do, like dumping crystal cap ground leads
> into the ground plane, when it was DEAD EASY to route them properly.
> As a result, and absolutely symptomatic of bad layout, there's
> significant EMI that gets worse when you plug in any shielded cable.
> The "ground" is carrying high frequency currents, which are taking
> every possible path home through the plane, instead of being carried
> home on a single isolated track.
>
> Smart autorouters seem to be like flying cars or AI. Always just a
> few years away.

Let's assume that I am inexperienced enough to make that exact mistake. (hypothetically, of course!)

Could you suggest a source of documentation to teach me more about
such a silly beginners mistake?

I'm not the smartest person on this list, but I'm learning..

Thanks,
Lyle

[William "Chops" Westfield]

>> It seems that if you want quality, hand routing is the only way to
>> go.

I think part of the problem is that "commercial" autorouting is aimed at
engineers doing many-layer boards with very high density and need for
esoteric features. Those are the people with money. It might be
possible
to write some sort of single-layer autorouter that would do amazing
things,
but who would buy it? (in particular, it seems to me that a really good
single-layer autorouter needs to be able to move and rotate parts...)

BillW

[William "Chops" Westfield]

On Oct 5, 2007, at 6:48 AM, David VanHorn wrote:

> they did all the things that I would NEVER do, like dumping
> crystal cap ground leads into the ground plane

You're not supposed to do that? Sigh.

Anyone want to critique my "Freeduino" PCB design here:
http://www.freeduino.org/freeduino_open_designs.html
(the 1206 version is the one we're most interested in.)
(Arduino is supposed to be a open source hardware/software
Atmel AVR development/education board. But the original
team has stopped releasing CAD files for the hardware, and
"Freeduino" is an attempt at an Nth party correction of that
omission. "our open source hardware is more open than your
open source hardware!")

BillW

[Gerhard Fiedler]

William "Chops" Westfield wrote:

>>> It seems that if you want quality, hand routing is the only way to go.
>
> I think part of the problem is that "commercial" autorouting is aimed at
> engineers doing many-layer boards with very high density and need for
> esoteric features. Those are the people with money.

Not only that. It takes time to set up an autorouter to work well (and to
learn how to properly set it up). For most boards I've done, I think it
would take more time to do that properly than to just route it manually.
(Consequently I did the latter :)

Gerhard

[David VanHorn]

> > they did all the things that I would NEVER do, like dumping
> > crystal cap ground leads into the ground plane
>
> You're not supposed to do that? Sigh.

A ground plane is similar to the infinite plane of resistor problem.
Current injected between any two nodes follows EVERY possible path to
get from one to the other. If you route a specific track, from the
ground side of both caps, to the nearest ground pin on the AVR, and
only then, join the plane, you'll find that it makes the board
significantly quieter.

Same idea should be used in power supply and analog layout.

Just don't tell me you used 22pF crystal caps on a 22pF crystal.. :)

[William "Chops" Westfield]

On Oct 5, 2007, at 2:14 PM, David VanHorn wrote

>
> Just don't tell me you used 22pF crystal caps on a 22pF crystal.. :)

Who can tell? Someone else did schematic entry, and it's one of
those typical hobbyist projects that says "16 MHz crystal" with
no further specifications :-) It does have 22pf caps...

> If you route a specific track, from the
> ground side of both caps, to the nearest ground pin on the AVR, and
> only then, join the plane, you'll find that it makes the board
> significantly quieter.

Hmm. I was happy to get a "ground ring" around the crystal and caps,
and thought that would help. You're saying the ground ring and the
cap grounds should connect to the AVR ground pin separately, even
though they're really close? There's ground plane on the bottom, too.

[David VanHorn]

>
> Let's assume that I am inexperienced enough to make that exact mistake. (hypothetically, of course!)

Purely hypothetically.. :)

> Could you suggest a source of documentation to teach me more about
> such a silly beginners mistake?

Actually, damned few. The analog light is going out in the world it seems.
I have a couple of good books at the office, but I'm not there at the moment.

> I'm not the smartest person on this list, but I'm learning..

Me too

[David VanHorn]

> > Just don't tell me you used 22pF crystal caps on a 22pF crystal.. :)
>
> Who can tell? Someone else did schematic entry, and it's one of
> those typical hobbyist projects that says "16 MHz crystal" with
> no further specifications :-) It does have 22pf caps...

Hmm. Then the appropriate xtal would be about 16pF or so.
Or bring the caps up to 39pF

> Hmm. I was happy to get a "ground ring" around the crystal and caps,

Actually, you are VERY close to right.
The track running around this cluster isolates most of it.
I would just add a small exclusion zone around those three pads to the
left, and one to the right of the gnd pad, so that the processor's
ground pad is the only place that this cluster touches any other
ground.

[Alan B. Pearce]

>> Hmm. I was happy to get a "ground ring" around the crystal and caps,
>
>Actually, you are VERY close to right.
>The track running around this cluster isolates most of it.
>I would just add a small exclusion zone around those three pads to the
>left, and one to the right of the gnd pad, so that the processor's
>ground pad is the only place that this cluster touches any other
>ground.

Personally I would have the two inner ends of the caps as the ground
connection, rather than the outer ends as illustrated, making it closer to a
point ground. Without knowing which pins on the micro are the xtal
connections, I also tend to have the xtal mounted parallel to the ic pins,
and the cap ground connections taking the shortest route to the nearest
ground pin.

However, after thinking about it, the layout illustrated may be fine if the
two capacitors are side by side instead of end on, as the lower cap has its
ground end very close to the ground connection on the DIL holes (I'm
assuming that is the micro). If the other cap was beside it then it would
also have a very short ground connection, but at the moment it has a
'reasonable' path around the ground plane loop that is around the caps and
xtal.

[KPL]

> > Who can tell? Someone else did schematic entry, and it's one of
> > those typical hobbyist projects that says "16 MHz crystal" with
> > no further specifications :-) It does have 22pf caps...
>
> Hmm. Then the appropriate xtal would be about 16pF or so.
> Or bring the caps up to 39pF

Can You explain this a bit more? :)

--
KPL

[David VanHorn]

> > Hmm. Then the appropriate xtal would be about 16pF or so.
> > Or bring the caps up to 39pF
>
> Can You explain this a bit more? :)

Despite any microcontroller data sheets to the contrary, the CRYSTAL
determines the cap values. If a given uC data sheet shows say 22pF
caps, then you're seeing the result of misinformed consumers beating
up the vendor to provide something they shouldn't. A correctly done
app note will not show cap values unless they also show a specific
crystal part number. It's up to you, the engineer, to select the
appropriate crystal, and then the proper caps given that crystal, and
your PCB layout.

A given uC may have a preference for crystals of a given impedance and
drive level, but that's a different issue. The fox application notes
cover this pretty well.

[William "Chops" Westfield]

On Oct 8, 2007, at 12:45 AM, Alan B. Pearce wrote:

>> so that the processor's
>> ground pad is the only place that this cluster touches any other
>> ground.
>
> Personally I would have the two inner ends of the caps as the ground
> connection, rather than the outer ends as illustrated, making it
> closer to a
> point ground.

Ah, I think I'm starting to understand. While a ground plane provides
nice shielding and power distribution, "bypass caps" should be wired
directly across the pins of the IC they are bypassing, rather than
between
a power pin and the ground plane (even if the ground pin of the chip is
relatively close by.) This helps prevent the transients that are
produced
by the chip from being propagated onto the ground plane via the
"infinite
resistor array" effect that Dave mentioned.
In other words, the ground plane is not your ideal power distribution
plane.
Hmmph. That's rather inconvenient. Are there any tricks to
implementing
this using common CAD packages? Even if you directly wire caps to pins,
EAGLE will happily fill in the ground plane as well. I guess it
falls out
nicely on 4-layer boards, where the inner layers are power planes but
the
outer layers (and the caps and their wiring) are on the outside.
How does the tradeoff of wanting separate ground planes and power
connections
go? It's counter-intuitive that I might be able to reduce EMI by
deleting a
component side ground plane, for instance, but taking the concept to
the limit,
that seems to be what is implied...

Are there amateur-level tests that can give you relative EMI info?
Not exact
values, but "it's better if I do THIS than if I did THAT" ? Scope
with a
dipole or something ?

BillW

[David VanHorn]

> Ah, I think I'm starting to understand. While a ground plane provides
> nice shielding and power distribution, "bypass caps" should be wired
> directly across the pins of the IC they are bypassing, rather than
> between
> a power pin and the ground plane (even if the ground pin of the chip is
> relatively close by.) This helps prevent the transients that are
> produced
> by the chip from being propagated onto the ground plane via the
> "infinite
> resistor array" effect that Dave mentioned.

Right. I try to locate my caps at the chip ground pin, and I route
thin to the cap, and thick to the chip.

> Even if you directly wire caps to pins,
> EAGLE will happily fill in the ground plane as well. I guess it
> falls out
> nicely on 4-layer boards, where the inner layers are power planes but
> the
> outer layers (and the caps and their wiring) are on the outside.

I watch where the planing is happening, and either use "no plane"
zones (old dos orcad) or I move the traces around to prevent the plane
from going where I don't want it to.

[William "Chops" Westfield]

On Oct 5, 2007, at 3:25 PM, William Chops Westfield wrote:

> There's ground plane on the bottom, too.

Hmm. It's come up in other discussions that having ground planes on
both top and bottom of a board may not be such a good idea, although
I'm not convinced that the reasons stated are applicable to a small
and relatively low-current board like this (ATmega168 + FTDI USB/
serial bridge.) Any comments from the experienced PCB designers?

Thanks
Bill W

[David VanHorn]

> Hmm. It's come up in other discussions that having ground planes on
> both top and bottom of a board may not be such a good idea, although
> I'm not convinced that the reasons stated are applicable to a small
> and relatively low-current board like this (ATmega168 + FTDI USB/
> serial bridge.) Any comments from the experienced PCB designers?

I plane both sides. But I'm careful about how I plane, and what gets
returned in discrete tracks. I also separate into analog, digital,
supply, and other plane sections.
Selective shoving of tracks keeps max fill area, without letting one
plane touch the other, except exactly where I want them to.

[Alexandre Guimaraes]

Hi, Dave

Can you elaborate a little bit at what drives the decision of what
returns trough the ground plane and what get's a dedicated ground return
track ? Is current the only factor ?

Best regards,
Alexandre Guimaraes

-----Mensagem original-----
De: piclist...@mit.edu [mailto:piclist...@mit.edu] Em nome de
David VanHorn
Enviada em: 22 October 2007 11:10
Para: Microcontroller discussion list - Public.
Assunto: Re: [AVR] Freeduino Board (was kicad autorouting)

[David VanHorn]

On 10/22/07, Alexandre Guimaraes <lis...@logikos.com.br> wrote:
> Hi, Dave
>
> Can you elaborate a little bit at what drives the decision of what
> returns trough the ground plane and what get's a dedicated ground return
> track ? Is current the only factor ?

I don't worry about DC current, but I do about pulsed or high
frequency AC current.
The main rule is "put it back where you got it from".

Oscillator crystal caps should ground ONLY to the uP ground pin,
switching power supplies should be treated as current loops between
the caps and inductor/transformer, through the diode. Try to only
attach ground connections out to the system at points where AC
currents will be near zero, like at bypass cap ground pins. I've been
known to split up a single cap to three, both for ripple current
ratings as well as to keep as much of the HF energy close to the
transformer as possible.

[Alexandre Guimaraes]

Hi,

>Oscillator crystal caps should ground ONLY to the uP ground pin, switching
power supplies should be treated as current >loops between the caps and
inductor/transformer, through the diode. Try to only attach ground
connections out to the system at points where AC currents will be near zero,
like at bypass cap ground pins. I've been known to split up a single cap to
three, both for ripple current ratings as well as to keep as much of the HF
energy close to the transformer as possible.

Makes lot of sense to me... But.. What goes to the ground plane ?

Sorry for asking too much but I have always made most of my boards
without a ground plane or just had one bellow low noise, high gain analog
sections. Most of the things I read in the books is related to very high
speed designs and most of my boards have 4 mhz clocks and consume just a few
miliamps. These techniques seems to me to be quite appropriate to be
discussed here. On dense 2 sided boards the only way to have a mostly
continuous ground plane is to use it to route the ground returns but I am
always afraid to make things worse...

Best regards,
Alexandre Guimaraes