fantastic video of ladyada routing

Eur van Andel wrote on Sat, 19 December 2009 18:42

It is fascinating to watch her work. As most experienced Eagle experts

 

know, routing is the Real Work

If you really think schematic drawing and parts placement aren't important

too, let alone getting the circuit right in the first place, I hope to

never encounter one of your designs.

Quote:

and the autorouter is for sissies, just like vias are.

Then I hope to never have to pay for one of your designs either.  The

autorouter is a tool that has its place.  You certainly can't just fire and

forget, but it can help you get routing done faster.  Vias by themselves

are not inherently bad either.  So a signal switches from one layer to

another.  Big deal.  Most board houses don't charge extra for vias, so if a

few vias makes your design tractable, keeps a ground area less broken up,

or even just saves cost during the design without further penalty, then

they are a tool you should use.  If you are doing a lot of manual routing

only due to a misplaced sense of asthetics, then you are doing your

customer a disservice by making him pay for something he doesn't need.  A

"beautiful" design is one that meets all the criteria for the least cost.

Note that nothing in there says anything about how many vias are used or

how you decided where the tracks go.

I'm not saying the autorouter is the only solution either.  In most

designs, there are factors to consider that usually dictate manually

routing some nets.  For example, you have to consider capacitive coupling

and sometimes leakage to high impedence nets.  You have to keep the loop

area of high currents small, as is often the case in switching power

supplies.  You want to keep loop currents off of planes by making single

feed points, sub-ground planes, and the like.

There are plenty of reasons to manually route, but there are usually also a

lot of nets where it makes no electrical difference whether they go this

way or that, or use a few vias to get between nodes.  Those are good

candidates for the autorouter.

What I usually do with 2 layer boards like the example, is to define the

bottom layer a ground polygon from the start.  Then I find all the ground

SMD pads and use vias right next to them to connect them to the ground on

the bottom layer.  This makes best use of the ground plane to leave as much

routing opportunity on the top layer as possible, which is something the

autorouter doesn't do.  Then I manually route the critical nets, which are

usually the ones carrying the switching power supply AC high loop currents,

crystals connected to PICs, bypass caps, etc.

Once that is done, save a copy of the board and let the autorouter fly.  Of

course you use autorouter parameters appropriate for the board.  In this

case the bottom layer cost is set very high to avoid breaking up the ground

plane.  Using the autorouter is a iterative process.  The first few times I

don't use any optimize passes.  At that point I'm looking for areas it has

a problem finding a solution, nets I forgot to set to a specific net class,

and other things that just don't look right.  This may cause me to move

some parts around, possibly gateswap or pinswap, and manually route a few

more traces to keep the autorouter from making a mess it can't recover from

later.  As you fix things, you allow the autorouter to do a few

optimization passes.  I usually use 8 for the final route with various

costs changing with the different optimize passes.  The first few passes

are more optimized to finding a solution, with the later passes optimized

to criteria such as keeping off the ground plane to the extent possible.

Once that is done in the case of a two layer board with ground polygon on

the bottom, I inspect how the ground got broken up.  What you want here is

lots of small islands with the groud plane flowing around them as apposed

to a few large islands of traces and vias.  Keep the maximum dimension of

each island as small as possible.  Again, there is of course a tradeoff

between how much effort you put into adjusting the route a little to break

up a clump of vias and how much it matters.  In real engineering everything

is a tradeoff.

Quote:

No movement of components either,

I thought I saw a few things get moved around, although there is nothing

wrong with moving parts after discovering some restriction in routing.

Good placement has a lot to do with good routing.  Placement is worth

spending time on because it saves time and uncomfortable tradeoffs later.

What bothered me about when she moved stuff is that there seemed to be no

visible indication of the part outlines at the time.  I use the silkscreen

layer not only as a visual sanity check for assemblers, but also to show me

the part extent during placement.

Quote:

and a very neat schematic.

Yes, neatness counts, a lot.  Good documentation is very important.

Quote:

My schematics are a mess, since they are optimised for routing, so all

 

chip symbols have their pins at the proper sequence.

Yuck.  The schematic is a visual explanation of the circuit.  This not only

helps you during design, but is the primary means of communicating the

circuit to others later.  As such, it should be optimized to do just that.

At that level, the physical location of pins on a IC are usually

irrelevant.  When you want to see the pins, look at the board view.  You

certainly don't want to pessimize the schematic for a one-time minor

convenience during layout.

Quote:

Note the attention to detail when she makes the silkscreen:

Of course.  Once again, neatness and good communication count.  After

routing is done, I routinely clean up the silkscreen and docu layers.  This

means moving the names and values of parts to visible places, making sure

they are clearly visually associated with the right part, and deleting them

when they can't be.  A bad silkscreen label is worse than no label.

Sometimes there is no way to fit all the part names in a dense area.

Delete them instead of making a mess.  The manufacturer will have to rely

on the board drawing in those areas.

Just one screwup later is probably worth more time than you spend on a

clear and accurate silkscreen.

Quote:

this is a board that will primarily be used by others, so she adds lots

of signal names.

I don't remember signal names.  To me it looked like pads being labeled.

In fact I don't like the way she did that at all.  It appeared that she was

making up the labels in the board editor.  There is too much chance of

messing that up.  The right way is to set the VALUE attribute of such parts

in the schematic, then make >VALUE show up on the silkscreen in the

package.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

She did an Ok job on the layout. Sure she used few vias, but here I have

the same opinion as Olin: who cares? I really don't like how the traces

"wiggled" around everywhere, and though this was partly because of the

large number of through-hole parts, it would have been less necessary if

vias were used more. Many experienced engineers I know prefer that

where-ever possible, with 2-layer boards, you use one layer for vertical

and the other for horizontal traces. I admit this is harder to do when

using lots of through-hole parts... which is why I avoid using many of them.

I also find it's easier to ignore the supplys until the routing is done

for most of the board. Then I like to use one side for a gnd plane, and

the other side for a vcc plane, and I usually get good coverage with

both planes, and then optimize traces to decrease the chop-up of the

supply layers. In the end, even with complicated boards, this greatly

helps ease routing.

She didn't move parts much (I noticed twice and only watched the start

and end of the video), but that was because of good positioning before

she began the routing, which is essential for a good design.

I did like her schematic. I do much the same there, though I don't

optimize the symbols for "flow" as I find it annoying when doing the

layout and especially when troubleshooting and when programming if

there's a mcu. Instead I use named nets and carefully placed parts in

the schematic to make it both neat and readable.

My 2cents...

"Eur van Andel" <eur@fiwihex.nl> wrote in message

news:hgjobb$qed$1@cheetah.cadsoft.de...

Hi

 

I'm surprised no one posted this:

 

http://www.adafruit.com/blog/2009/11/19/pcb-routing-with-eagle-video/

 

(via Make)

 

Ladyada is an accomplished PCB publisher. From what I can see, this is a

daughterboard for an SD card, with an SMD card connector and a voltage

level shifter.

 

It is fascinating to watch her work. As most experienced Eagle experts

know, routing is the Real Work, and the autorouter is for sissies, just

like vias are. After all the work is done, she has only three.

 

See how she wriggles the lines through, sometimes changing the layer of

some signals up to four times. She does not hide the GND airwires and

changes the shape (and layer!) of the GND plane several times. I always do

the GND plane dead last and hide behind via's to patch the different

planes together.

 

She doesn't avoid "acid-traps" (90º angles in traces) either, although she

has set the 45º angle in routing.

 

She does go back to the schematic, but mostly for naming signals, and

gateswapping. I often leave signals unconnected, only to attach them to

the most convenient PIC pin after routing the wires.

 

No movement of components either, and a very neat schematic. My schematics

are a mess, since they are optimised for routing, so all chip symbols have

their pins at the proper sequence.

 

Note the attention to detail when she makes the silkscreen: this is a

board that will primarily be used by others, so she adds lots of signal

names.

 

 

A must-see for everyone here.

 

 

--

Eur van Andel  eur@fiwihex.nl

 

Wow... you guys are harsh!  Nevertheless, I may not agree with the way that

everything is done or may have a different way of going about it, but

enjoyed the video.

Thank you for posting... and Happy Holidays!

Terri