SparkFun Forums

[odriew]

Schematic: https://dl.dropbox.com/s/y8nm9584hz4x33 ... pdA-A&dl=1

I have a schematic that I'm trying to create a board layout for. Unfortunately, my attempts at a layout only leave the autorouter at 67%. I'd love it if someone could try making a successful layout, but either way I am in need of advice on how to create a layout that the autorouter can manage.

Edit: Image of schematic: https://www.dropbox.com/s/o6p5b2vr4zk7h ... cImage.png
Image of preliminary board layout: https://www.dropbox.com/s/h8xbk6w6xwppu ... tImage.png

[Ross Robotics]

Have you tried manually routing the board? It is actually better to route it yourself than to autoroute.

How small/big do you want the board?

[leon_heller]

What PCB software are you using? The autorouters provided with the low-cost packages are rubbish!

[n1ist]

Processor is either an QFP or QFN. That looks quite doable on a 2-layer board. As mentioned, skip the autorouter.

Before worrying about routing, you need to fix the schematic...

- Add decoupling caps
- Crystal resonator caps are the wrong value
- Missing grounds on sd-card
- Missing junction dots at negative of C2, U2p4
- Verify power input connector. If phone, it will short supply when plugging in. If coax, do you really have center negative?

[odriew]

Decoupling caps, resonator caps, sd grounded, added junction, center positive; I appreciate the schematic check.

I'm using the autorouter on Eagle, and I dread manual routing. For those with experience in manual routing, is there a method I can follow to minimize trial and error (i.e. "route power lines first" or something like that)? Maybe 0ohm resistors? as the decoupling caps seemed to help the autorouter.

Also I'd like to use a Sparkfun enclosure, so 3.95" by 3.15" SHOULD be more than enough (I think).

[leon_heller]

Route critical tracks, such as power and grounds, and clocks, first. Then route the rest of the connections, starting with the shortest ones and working up to the longest ones.

[lyndon]

And discipline yourself to keeping horizontal traces on one layer and vertical on the other. It makes layout much easier. As soon as you break the rule, you start getting into trouble.

[odriew]

https://www.dropbox.com/s/ri00610jbq5q9 ... dFINAL.png

Here it is, though the DRC failed merely due to the pin spacing on the LPC2138. Maybe it will pass the BatchPCB DRC...
Hand-routed, by the way (as if you couldn't tell).

[odriew]

aaaaaand, https://www.dropbox.com/s/nm2zpfq66rnis9c/FINAL.png

IT PASSED. Thanks all for the help.

[InactiveUser001]

That circuit is very possible to do on 2 layers or simply 1 with a few wire links.

However 75% of getting it right is good placement, by placing the components close to the pins they connect to the rest is easy.

For example, top RH corner - those 2 caps on the regulator.
The bottom one rotate 90 clockwise and move to the RH pin of the regulator.
The top one move to the RH side of the regulator.

Look at it as the circuit flows and it should help, into cap, into reg - out of reg & into cap then off to rest of circuit.

And as for horizontal one side vertical the other - that's an old method that does not always work well with today's components. I can see several instances of unnecessary via to the other side for several tracks to allow a single track through.
It should be the other way around, if you are making the PCB yourself you want to minimise the vias and I would suggest thickening many of the tracks where possible - you have bags of room to do so.

Also retrack those with jagged edges - make 45 degree turns rather than use free routing - it helps with the etching and looks miles better.

[n1ist]

- Vcc and ground traces need to be wider, to reduce impedance.
- Bypass caps should be right next to the pin they are bypassing (ideally, the Vcc trace should hit the cap first, and then the pin).
- Since you have a predominantly SMT design, I would try to keep the traces topside as much as possible. That would leave the back available for a ground pour and improve routing by reducing the number of vias needed. For example, look at the top of the processor. If the one trace going left was on the back side, the other 4 could be kept on the top.
- On the SD socket, I would add pads on the back side of the board behind the two that the shield solders to. Then drop vias between the pads. This will help mechanically anchor the pads so the socket is less likely to rip off the board
- Try to hit pads straight on. Traces ideally should run horizontal or vertical with short 45-degree traces between 45-degree bends.
- Don't forget to add the board name and revision to the top silk

/mike

[Joe5]

There's some good advice here. Experience and tips like you see here are your best teacher but many people either don't want to take the time or don't have the time to learn. Laying out a board is part art and part science. Everybody has slightly different methods getting there but there are some general rules to observe. I've never used Eagle. I use CIRCAD part of the time and DesignSpark for the other. I'm still trying to figure out which one I like the best. You would appreciate the new PC CAD packages because I started out making my own prototypes back when we had to hand "tape" them on mylar film. I guess that tells my age.
My understanding is that DesignSpark program will accept EAGLE footprints and symbols.