Could Someone Review my Routing Job?

[ConnorM]

I was wondering if somebody could have a look at this PCB that I routed. Does it look good? Is there anything that I should change? I'm a beginner so I don't know very much!

The board is 160mm x 63mm with 10mil traces.

[Pack34]

Any reason the board is so big?

You might want to double check the orientation of that battery connector and make sure you have room to connect and disconnect it without hitting nearby components.

[phil from seattle]

Overall, doesn't look too bad. It would be helpful to also post the schematic.

A couple of things:
- You have several long runs that parallel closely - maybe less than 10 mils apart. One pair is by the A12 label. While there is nothing wrong with that, you have lots of space so I would add some separation. See the picture.
- Look at the resistors I've circled: avoid the funky jogs.
- Also, what size are those resistors? the silk is tiny and won't be readable. Plus routing though them seems kind of tight. I've avoid it or move up to a larger resistor size.
- Check the drill size on your DIP pads. They look to be small.
- In general check all your library parts for hole size. I've found several Teensy footprints that were flat out wrong. got calipers? Nothing worse than getting a board back and discovering parts don't fit.
- Have you run a design rules check on your board?
- Know the minimums of the PCB vendor and don't design to those minimums. I'd shoot for 2 to 4 mils bigger (min clearance of 6 mils, use 8 or 10).
- Check your mechanical part (connectors esp) clearances. I do a paper mockup with the real parts.
- I would run wider power traces. 16 mil is my standard.

[hermit]

Any reason the board is so big?

Agreed.  Your cost goes down dramatically if it is 100X100 anyhow so why not see if you can make that size work?

[wraper]

Way too much space wasted and routing is ugly. You should avoid routing under SMT parts and preferably between IC pins too. Also there are many places with very suboptimal routing like this one which I fixed.

[hermit]

I did a layout for someone using the Teensey.  It was made easier by only soldering the pins on that are actually needed.  You might have to add a few just for mechanical stability too.   Just buy the board without pins and do that part yourself.  We mounted the Teensey on header pins so we could stuff a few parts underneath it too.

[phil from seattle]

I have to say I disagree with the "make it super small" theme.  The board is a bit big but it's his first. So what? It's not going into mass production and it's his wallet. Most Chinese PCB fabs charge the same up to 100x100mm. So, I'd recommend fitting it into that envelope but not pushing it very hard.

[phil from seattle]

And, I agree on the ground plane comment. Make ground polygons on top and bottom that cover the entire board.

[Zero999]

Any reason the board is so big?

Agreed.  Your cost goes down dramatically if it is 100X100 anyhow so why not see if you can make that size work?

There might be a valid reason for the board size, such as the requirement for it to be fitted in an enclosure with threaded holes in specific places or on top of another board.

I agree that adding a ground plane is a good idea. I would also be good to have a plane for the positive supply too, even if it's broken with various traces.

That Teensy module would look better if it's flipped by 90^o, but there could be a mechanical reason for it being where it is.

[ConnorM]

The position of the Teensy and board size are based on mechanical requirements. I will have a look at some of the other suggestions and post back with an updated PCB. Thanks!

[mariush]

Here's my suggestions

Since you have a lot of through hole parts, give up on the surface mounted resistors and use axial resistors and maybe even ceramic capacitors with their longer bodies. It would allow you to comfortably route one or two traces between the holes for that resistor and make routing easier in some places.
You're probably not going to pay by the hole made in the pcb and you'd save an extra pass with the hot air gun or whatever you're going to use for soldering resistors... and there's enough circuit board real estate to estate to use 0.125w thin metal film resistors or whatever on your board.

any particular reason why this project requires two different connectors (x1 to x3 with 5566-4 and x4 to x7 as 5566-2) ? Could you maybe save some money buying 5566-4 in bigger volume and using just two wires in those connectors on the right?

i would orient the battery connector in the same direction as the other connectors, like the microusb or whatever that is at the top of the board

You could easily make this board single layer, in the worst case you'd just have to add a few jumper links (or 0 ohm resistors) in some places.

maybe move JP1 more to the bottom edge of the board so that you can easily insert connectors without having your hand over the whole board?

[bson]

I see MOSI and MISO on a header, but no clock.

Add silkscreen labels for the connectors.

Should the battery really be across Vin/GND?

It looks like you route GND like a trace - use a pour on the bottom side and connect to it with vias.  Move signal traces to the top layer and only use the bottom to cross other traces.  This is minimized by reducing the spacing between traces that need to be crossed.  Just shove them together and hop over using the bottom.  This will leave you a large mostly unbroken ground plane.

Route traces in descending order of signal speed.  Power traces last - they can have more vias and snake a bit more, especially if you use wider traces and a top pour for Vcc.

Use a fatter trace for Vcc.  Then pour it on the top copper layer.

In fact, use fatter traces all around.

It's not a big deal, but in general it's a good habit to place dampening resistors closer to their signal sources.

Don't hesitate to run traces underneath parts.  For example, the blue (bottom side) trace from X7 can be routed underneath the part, on the top layer, to the pin it's going to first (pin 9 of MCP6004 U??? if my eyes don't deceive me).

X6 to MCP6004 pin 13 can be routed on the top layer, inside of the one from X7, except maybe for the last few mm.

Add reference designators for your passives, especially the resistors, to reduce the risk of mix-ups and using wrong values.  Or the value itself; either works.

The six pin header in the middle of the board can be moved out of the way of the traces going through it.  Just shove it over closer to the Teensy assuming the latter doesn't need a bunch of courtyard not shown.

[ConnorM]

I've attached two pictures, one with the ground planes on the top and bottom, and another with them removed. I thought it might be easier to look at without the ground planes.

I ran a DRC with OSH Parks design rules and there are no errors.
I removed routing underneath SMT components.
I increased the silk screen font.
Power traces are 16mil now. I'm not sure that I did this properly, I might have missed some!
I tried to fix some of the weird wiring/jogs.
I added a ground plane on the top and bottom by making a polygon, giving it net name GND, and then clicking rats nest. Is this correct?

How does it look now?
Thanks for the help!

[phil from seattle]

Improvement! 

You did miss one power trace by C7. Maybe others. [edit]that's a gnd trace, sorry.[/edit]

You made a ground plane - but still have ground traces. That might be an artifact of not showing ground planes but makes me wonder if you got it right. Ripup any ground traces and hit rats nest. It should still say "nothing to do".

Power traces. I like to route mine around the edge of the board where possible. It tends to keep them out of the way.

Component values on silk screen. You've got plenty of space so it doesn't matter here but if you do more dense boards, you probably will want to drop values. They are of marginal value, IMO. Most designers don't put them on the silk layer. I also don't bother with names on the silk layer for things like connectors - instead I will use more descriptive text (like Motor1 vs J10 or some such) but that's just my style. The goal is to make it easier to use the board with application specific labels rather than part names.

[wraper]

Copper fill apparently is not connected to anything.

[ConnorM]

On my board I am using analog ground, net name is "AGND", and a regular ground, net name is "0". Do I connect the pours to net name "AGND" or "0" ?

[pigrew]

Maybe rotate the battery connector another 180 degrees? Currently, the wires may interfere with the mounting bolt.

The mechanical drills of your X1-X7 seem to be non-plated? You may want to change them to plated through holes to add mechanical support to them. Unless they are plastic? Then the non-plated holes makes sense.

As already mentioned, the ground plane doesn't seem to be connected to ground. There's some "dead copper" that should be dealt with. Either remove the dead copper, or add vias so that it's no longer dead. (For example, the area where the R20 designator is).

Move as many non-GND tracks to the top layer as you can, and if you have tracks on the bottom, keep them short. Avoid long tracks splitting your ground plane.

If you use a GND fill on both top and bottom, add some via stitching. At minimum, I'd add a GND via next to each SMD GND pad.

Double-check the drill diameter of the mounting holes. They seem large.

It's always suggested to avoid acute angles of tracks (acid traps), though my understanding is that it's less necessary these days. You have one on the bottom under MCP6004.

Add some indication of pin-1 for your 100mil pitch connectors: a line/box/arrow on the silkscreen, or a square pad for pin-1.

Even if I don't plan on automatic pick-and-place assembly, I'd tend to add fiducials to the layout.

Add board info to your silkscreen, for example the board name, revision date, and your name.

[pigrew]

On my board I am using analog ground, net name is "AGND", and a regular ground, net name is "0". Do I connect the pours to net name "AGND" or "0" ?

Without a schematic, it's difficult to say for sure. Usually you'll get a good result by shorting them together. If you do have multiple ground nets, they'd need to be shorted together somewhere, and analog components placed in a isolated region of the board. There are a few other guidelines, but in this case it's very likely best to just short them together and only have one GND.

[ConnorM]

Does this help at all?

[phil from seattle]

It's gets a little more complex when you have AGND and GND. Where you have analog components, make an AGND poly. On the rest of the board make a GND poly.  You can use rank to allow nesting of polys.  Eagle is resistant to connecting 2 dissimilar traces but you need to connect those two together.

I've made special components to do the connection between two grounds so eagle doesn't bitch at me. There must be a better way. Maybe look up star ground techniques for eagle.

[pigrew]

After looking at the schematic, I'd still suggest just going with a single ground net, especially since you're using the ADCs of the microcontroller. The additional slight immunity to digital noise is likely not worth the design effort. It looks like the entire board is analog, anyway (except for JP2)? You can put JP2 close to the micro's board, keep analog tracks away from it, surround by ground fill, and I think that'd be pretty good.

Also, double-check your accelerometer voltage dividers. Note that they already have an output impedance of 33 kOhm. Though, you can always just swap component values once you get the board.

[ConnorM]

Sorry I've never done this before! But just so I understand, in my schematic I should go back and just connect all grounds to the teensy's ground, or should I connect all grounds to the teensy's analog ground?

[ConnorM]

I removed AGND from my schematic and redid the pours. I'm not really sure if this is any better, I didn't have time to look over everything but I will later today.

[phil from seattle]

You should connect teensy gnd and agnd together if you are going with a single ground.

[pigrew]

Perhaps ignore my previous advice, then.... I didn't notice that the Teensy has a separate AGND pin. It seems that GND and AGND are connected together on the Teensy through a ferrite bead.

It's now a tough choice about if they should just be shorted together on your PCB. It'll likely give an acceptable result to just short them together still. (but I have no personal experience relating to this)

If you want separate planes:

1) The analog pins are all on one side of the Teensy. Could you move the Teensy so that the digital connector is on one side (the left), and all of the analog components are on the right? This would let you have a nice GND plane separation (have GND on the left and GNDA or the right, with them connected on the Teensy board).
2) Figure out how to provide an analog supply. On the teeny, there is a ferrite bead (EDIT: with decoupling capacitor) for filtering VDDA, but VDDA doesn't have a pin header. Perhaps add a ferrite bead for filtering VDDA on the right-side 3V3_LO? This should reduce ground loops.