element14 Community
element14 Community
    Register Log In
  • Site
  • Search
  • Log In Register
  • Community Hub
    Community Hub
    • What's New on element14
    • Feedback and Support
    • Benefits of Membership
    • Personal Blogs
    • Members Area
    • Achievement Levels
  • Learn
    Learn
    • Ask an Expert
    • eBooks
    • element14 presents
    • Learning Center
    • Tech Spotlight
    • STEM Academy
    • Webinars, Training and Events
    • Learning Groups
  • Technologies
    Technologies
    • 3D Printing
    • FPGA
    • Industrial Automation
    • Internet of Things
    • Power & Energy
    • Sensors
    • Technology Groups
  • Challenges & Projects
    Challenges & Projects
    • Design Challenges
    • element14 presents Projects
    • Project14
    • Arduino Projects
    • Raspberry Pi Projects
    • Project Groups
  • Products
    Products
    • Arduino
    • Avnet Boards Community
    • Dev Tools
    • Manufacturers
    • Multicomp Pro
    • Product Groups
    • Raspberry Pi
    • RoadTests & Reviews
  • Store
    Store
    • Visit Your Store
    • Choose another store...
      • Europe
      •  Austria (German)
      •  Belgium (Dutch, French)
      •  Bulgaria (Bulgarian)
      •  Czech Republic (Czech)
      •  Denmark (Danish)
      •  Estonia (Estonian)
      •  Finland (Finnish)
      •  France (French)
      •  Germany (German)
      •  Hungary (Hungarian)
      •  Ireland
      •  Israel
      •  Italy (Italian)
      •  Latvia (Latvian)
      •  
      •  Lithuania (Lithuanian)
      •  Netherlands (Dutch)
      •  Norway (Norwegian)
      •  Poland (Polish)
      •  Portugal (Portuguese)
      •  Romania (Romanian)
      •  Russia (Russian)
      •  Slovakia (Slovak)
      •  Slovenia (Slovenian)
      •  Spain (Spanish)
      •  Sweden (Swedish)
      •  Switzerland(German, French)
      •  Turkey (Turkish)
      •  United Kingdom
      • Asia Pacific
      •  Australia
      •  China
      •  Hong Kong
      •  India
      •  Korea (Korean)
      •  Malaysia
      •  New Zealand
      •  Philippines
      •  Singapore
      •  Taiwan
      •  Thailand (Thai)
      • Americas
      •  Brazil (Portuguese)
      •  Canada
      •  Mexico (Spanish)
      •  United States
      Can't find the country/region you're looking for? Visit our export site or find a local distributor.
  • Translate
  • Profile
  • Settings
Autodesk EAGLE
  • Products
  • More
Autodesk EAGLE
EAGLE User Chat (English) fantastic video of ladyada routing
  • Blog
  • Forum
  • Documents
  • Events
  • Polls
  • Files
  • Members
  • Mentions
  • Sub-Groups
  • Tags
  • More
  • Cancel
  • New
Join Autodesk EAGLE to participate - click to join for free!
Actions
  • Share
  • More
  • Cancel
Forum Thread Details
  • Replies 3 replies
  • Subscribers 172 subscribers
  • Views 306 views
  • Users 0 members are here
Related

fantastic video of ladyada routing

eur
eur over 15 years ago

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

 

 

  • Sign in to reply
  • Cancel
  • autodeskguest
    autodeskguest over 15 years ago

    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

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Cancel
  • autodeskguest
    autodeskguest over 15 years ago

    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...

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Cancel
  • Former Member
    Former Member over 15 years ago

     

    "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

     

     

     

    • Cancel
    • Vote Up 0 Vote Down
    • Sign in to reply
    • Cancel
element14 Community

element14 is the first online community specifically for engineers. Connect with your peers and get expert answers to your questions.

  • Members
  • Learn
  • Technologies
  • Challenges & Projects
  • Products
  • Store
  • About Us
  • Feedback & Support
  • FAQs
  • Terms of Use
  • Privacy Policy
  • Legal and Copyright Notices
  • Sitemap
  • Cookies

An Avnet Company © 2025 Premier Farnell Limited. All Rights Reserved.

Premier Farnell Ltd, registered in England and Wales (no 00876412), registered office: Farnell House, Forge Lane, Leeds LS12 2NE.

ICP 备案号 10220084.

Follow element14

  • X
  • Facebook
  • linkedin
  • YouTube