Another PCB Design Noob - New Thread for new board

Based on the feedback on my previous layout, and realizing all of the rookie mistakes I made, I’ve restarted from scratch. I also created a new thread so that there wouldn’t be any confusion about which design is being discussed.

On the new board, I’ve removed all of the non-core functionality (Vreg, USB support, LEDs, etc…). I’m focusing on getting to core required components for the MCU to function placed first. Once I get these parts right, I will move on to routing the MCU data lines.

The only components currently on the board are: MCU, crystals (real time, and main), caps, ferrite bead, and a few pull-up resistors (for reset and NMI pins).

I’ve routed almost everything using 90 degree routing, with the idea that I can add Miters later. I’ve kept the ground fill (on the bottom) and the remaining air-wires hidden.

(By the way - I discovered that Sparkfun has published Eagle files for most of their products. I’ve reviewed the BRD files from their products with high pin count MCUs, and got some really good ideas from them.)

Please share your thoughts and feedback, and be specific where possible.

http://farm2.static.flickr.com/1350/472 … 6b2e_b.jpg

I like to add vias at T intersections of thin traces. It helps prevent acid traps. Since you are probably looking a pretty low frequencies the capacitive loading issue probably isn’t a problem.

It really comes down to how much you trust the fab house. If you are planning on using gold phoenix/batch PCB (a cheap fab house), count on acid traps being on your board.

Acid Traps:

http://www.edaboard.com/ftopic94521.html

Remember I mentioned mitering when using right angles. You can click on the miter tool in Eagle (it looks like a cutoff corner) and choose a radius larger than zero. Then you can choose either round or 45 degree miters. Click on a corner to miter it. You can also select a miter radius while routing, so you don’t have to go back and miter everything.

Mitering is neat because you have easy to lay out right angle routing while avoiding acid traps.

Thanks for the tip about adding via’s at the T’s, I’ll definitely add those. I’ll also try to bump my wire size to mitigate the effects of overetching.

I am planning on adding Miters to the 90 degree connections (where I can).

I am undecided about the board house for my initial build. I’m designing it so that it will pass the BatchPCB DRU checks (nothing below 8 mils, etc…), but I may use pcb-pool to get it back a little quicker.

Routing looks solid - so I’m going to get nitpicky:

Why so few 45 degree angles? 90 degree angles make a PCB look like it was designed in the 80s, IMHO.

What is the big inductor for? Is that your ferrite bead? If so, it is more proper to use the prefix E, not L. F is used sometimes too, but the IPC calls for E.

Is the white writing on the PCB your silkscreen? It is way too small - standard board houses cannot print that fine.

I suspect the unconnected pads on X2 should be grounded. All four pin crystal oscillators that I’ve used have called for their other two pins to be grounded.

You should have some sort of silkscreen marking the shape of X1. It’s confusing without it.

None of these are major problems.

Thanks for taking the time to review and make comments; I really appreciate your input. Fortunately, I have good answers or reasons for everything you asked.

NleahciM:
Why so few 45 degree angles?

This is a work in progress and not finalized. I routed everything at 90 degrees to start so I could keep everything lined up (in fact the few angles routes are incorrect and should be at 90). **Once I have the routing done I'm going to use the Miter tool to convert all of the 90 degree corners into 45 degrees or rounded.** (I mentioned this in the original post. But perhaps it wasn't clear enough, as you're the 2nd person to mention it.)

NleahciM:
What is the big inductor for? Is that your ferrite bead?

The inductor is a filter between Vcc and AVcc. It's actually a 10uH inductor, not a ferrite bead as I incorrectly stated earlier. Its from an application note for the MCU. With that said, I noticed the part layout looked abnormally large. Sure enough, when I check it against the real component, it was wrong. I was able to find the correct library part for this, which is the size of a normal 1206 SMT part.

NleahciM:
Is the white writing on the PCB your silkscreen? It is way too small - standard board houses cannot print that fine.

Good catch on the line size. I haven't actually done any of the silk-screening yet. The white that you see in the image is from the part libraries in the placement layer. If I decide to include this in my final board, I'll make sure to upgrade them to a line that will print.

NleahciM:
I suspect the unconnected pads on X2 should be grounded. All four pin crystal oscillators that I’ve used have called for their other two pins to be grounded.

This is interesting. Its the first time I've used an SMD crystal, so I'll check the datasheet and see what I'm supposed to do. In the schematic, the parts only show two connections, which are the ones connected on the board.

NleahciM:
You should have some sort of silkscreen marking the shape of X1. It’s confusing without it.

I agree that its confusing. Also, it doesn't match my crystal very well. I'm going to modify the library for it and I'll add some placement guides.

Thanks again for taking the time to review this.

Cheers,

Rob.

This is a work in progress and not finalized. I routed everything at 90 degrees to start so I could keep everything lined up (in fact the few angles routes are incorrect and should be at 90). Once I have the routing done I’m going to use the Miter tool to convert all of the 90 degree corners into 45 degrees or rounded. (I mentioned this in the original post. But perhaps it wasn’t clear enough, as you’re the 2nd person to mention it.)

The only reason its mentioned frequently (I noticed it aswell to be honest :P) I think is because its more efficient to route with 45’s in the first place, rather than doing twice the work, and this is what most of the folks here do (myself included). Personally I dont like the look of 90’s, but I just use one of the angle tools when I route, and I dont find it any harder to line up parts this way.

Yeah, it is really easy to simply route with 45’s to begin with in EAGLE, everyone here at SFE does that.

Oh and going back to the silk screen thing, GoldPheonix (where SFE gets their boards) seems to be able to handle 40 mil text with a 15% ratio, just FYI.

Supply and ground tracks should be much wider.

AZRobo, I’m not sure which MCU you’re using, but you may want to put a biasing resistor across the leads of X2. You don’t need to populate it, but it may save you some grief in getting the oscillator to run if for some reason the internal biasing resistor doesn’t like your crystal.

I’m assuming X1 is a leaded cylindrical can resistor you’re putting on it’s side and soldering to that large area?

Roko:
You don’t need to populate it, but it may save you some grief in getting the oscillator to run if for some reason the internal biasing resistor doesn’t like your crystal.

If there is only one thing I have learned about getting prototype PCBs, it’s liberally apply footprints. I cannot express how great it is to have a footprint there when you need it.

leon_heller:
Supply and ground tracks should be much wider.

Agreed.

AZRobbo:
Please share your thoughts and feedback

This looks pretty nice.

You did a good job packing the crystals and the bypass capacitors close to the CPU.

I suspect that you’ll be forced to push them a little further apart in order to get room to run the other traces to not-yet-connected pins on the CPU – that will be fine.

I would solder the case of watch crystal X1 to ground – i.e., add a short trace from X1’s biggest pad to a via to GND.

There’s a long discussion of the benefits and drawbacks of soldering crystal cases to ground [at AVRfreaks. (I see someone else has already frowned at the unconnected pins of X2).

I guess I’m getting spoiled by CPUs that have the 2 crystal pins right next to each other, making it easy to keep-out any other traces, because the trace to pin 17 looks like it’s running annoyingly close to the crystal.

Does anyone have any references that discuss this “vias at T intersections” idea?

Otherwise, I’m going to assume it’s just as misguided as the [“OF FLYING ELECTRONS” theory of [90 degree traces.](http://www.edaboard.com/ftopic94521.html)](http://www.edaboard.com/ftopic94521.html)](http://www.avrfreaks.net/index.php?name=PNphpBB2&file=viewtopic&t=20615)

DavidCary:
Does anyone have any references that discuss this “vias at T intersections” idea?

Otherwise, I’m going to assume it’s just as misguided as the [“OF FLYING ELECTRONS” theory of [90 degree traces.[/quote]

They’re not referring directly to degraded signals, which is definitely a myth as far as right angle intersections goes. They’re referring to acid traps, which occur at right angles and on narrow traces can result in a significant percentage of extra etching happening, reducing the width of the trace, which /can/ have an impact on the signal quality.](http://www.edaboard.com/ftopic94521.html)](http://www.edaboard.com/ftopic94521.html)

utoxin:
They’re not referring directly to degraded signals, which is definitely a myth as far as right angle intersections goes. They’re referring to acid traps, which occur at right angles and on narrow traces can result in a significant percentage of extra etching happening, reducing the width of the trace, which /can/ have an impact on the signal quality.

If I am routing at right angles on a PCB using 8 mil traces and being made by a cheap fab, I put a via at the intersection to reduce acid traps. That is what I was driving at.

This “right angle intersection” discussion always seems to creep up every once and a while.