I’ve just designed a breakout for the ATXMega256A3, the second ever board layout i’ve done. I was hoping somebody could take a look at it and yell at me if i’ve done anything exceptionally stupid with the layout. this pdf has a scale factor of 3
http://fs06n1.sendspace.com/dl/03ef4378 … eakout.pdf
I’ve used the DRC for batchpcb in eagle, so it should be good on that front
Generally looks OK, but a few suggestions:
Put more vias to the groundplane. You want as low impedance to groundplane as possible, which means you should have vias as close to the component pins as posisble. For example, capacitor C3 should have its own via to ground close to the pin - it should NOT have that track to share a via with D4 etc.
Suggest beefing up the width of your power tracks.
Not sure what power supply input voltage you’re using but if the regulator has to drop much voltage, I suggest trying to put a decent copper pour connected to the tab of the regulator. Estimate the likely current draw for the board, and then calculate the power dissipation based on the input voltage. The datasheet for the regulator should have some hints on how much copper area you’ll likely need to dissipate the heat. If you’re using a hotplate / oven to solder the board (recommended - see Sparkfun tutorials), than this connection should be a direct pour - you want a low thermal impedance.
Most of the board has a groundplane (which is good), but I sugggest making an effort to minimise the breaks in it. For EMC & noise reasons, you really want to minimise the number and length of breaks in the groundplane. Highly recommended, even if you need to move tracks or components around. I can see a number of instances that you could remove the tracks on the bottom layer, and other instances that you could drastically shorten the length of them.
Post your .sch and .brd file. That pdf is too difficult to interpret.
Why did you decide to pour your 3.3v net rather than ground?
Your caps on the regulator look like 0805; without knowing the regulator type, anything in 0805 size is going to be inadequate.
Make your traces bigger. There’s no reason to make traces small when you have the room. Especially your power traces.
MichaelN:
Generally looks OK, but a few suggestions:
Put more vias to the groundplane. You want as low impedance to groundplane as possible, which means you should have vias as close to the component pins as posisble. For example, capacitor C3 should have its own via to ground close to the pin - it should NOT have that track to share a via with D4 etc.
Suggest beefing up the width of your power tracks.
Not sure what power supply input voltage you’re using but if the regulator has to drop much voltage, I suggest trying to put a decent copper pour connected to the tab of the regulator. Estimate the likely current draw for the board, and then calculate the power dissipation based on the input voltage. The datasheet for the regulator should have some hints on how much copper area you’ll likely need to dissipate the heat. If you’re using a hotplate / oven to solder the board (recommended - see Sparkfun tutorials), than this connection should be a direct pour - you want a low thermal impedance.
Most of the board has a groundplane (which is good), but I sugggest making an effort to minimise the breaks in it. For EMC & noise reasons, you really want to minimise the number and length of breaks in the groundplane. Highly recommended, even if you need to move tracks or components around. I can see a number of instances that you could remove the tracks on the bottom layer, and other instances that you could drastically shorten the length of them.
ok thanks. I reworked the GND vias, now there’s basically one for every connection to ground. power tracks upsized. Would it be a bad idea to use the vcc plane for the heatsink on the regulator?
TheDirty: I poured both of them. Ground on bottom, 3.3V on top… the caps are 0603’s. actually, all the resistors, caps, and leds are 0603. Why won’t they cut it?
I hadn’t even noticed the top plane was 3.3V! I don’t have a problem with this, as it helps ensure a low impedance power supply. Definately connect the tab of the regulator to this! (assuming the regulator has the tab connected to Vout). As stated, it is preferable for thermal reasons to directly connect this to the plane with no thermal reliefs. However, if you’re planning on soldering this by hand, soldering direct to a groundplane is very difficult.
As for the comment about 0805 / 0603 capacitors being inadequate, it will of course depend on the regulator and the power supply input, but if the voltage and capacitance values are sufficient you should be OK. Without seeing your schemtic & knowing what kind of power supply you will use, it is hard to say.
One important point to note is that some low-dropout regulators are not stable with the extremely low ESR values you get with ceramic output caps. Most modern regulators are OK, but it is important to check the datasheet. I refuse to use regulators that aren’t stable with ceramic output caps.
If you do post the schematic, a PDF would be best for me (I use Protel, not Eagle. I tried Eagle, but it was just too annoying).
OK, so now i’ve reduced the interruptions on the ground plane to 3. Minimum trace width is now 12mil instead of 8, power lines are 24mil. Schematic pdf and new board pdf are attached
galed:
TheDirty: I poured both of them. Ground on bottom, 3.3V on top… the caps are 0603’s. actually, all the resistors, caps, and leds are 0603. Why won’t they cut it?
What regulator are you using?TheDirty:
2. Your caps on the regulator look like 0805; without knowing the regulator type, anything in 0805 size is going to be inadequate.
TheDirty:
What regulator are you using?
Oh, it’s the LM317
On the datasheet for the FT232R under bus powered configuration, it has decoupling capacitors, plus a ferrite bead. Never used the ferrite bead myself, but at least use the capacitors. Plus 3v3OOUT is tied to ground through a 100nf cap.
I think your reset button moved, but your text staid in the same place.
galed:
TheDirty:
What regulator are you using?Oh, it’s the LM317
Looking at the board only, I thought it was probably a LM1117. 1uf and 0.1uf are fine then, but I would still put something like a 10uf on the incoming power.
added the necessary caps to the FT232RL and moved the reset label to the switch.
i could spend days doing and re-doing this circuit board until it was absolutely perfect… too bad i have things like class… :roll:
That looks much better. I guess you decided not to connect the tab of the regulator to the 3.3V plane? Hopefully you’re not trying to dissipate too much power in this regulator.