Yup. Another newbie needing review. Please take a look at the attached board design and provide comments.
Just a little background:
This board is destined for a kitchen timer/thermometer/temprature controller. Power is provided by a regulated external power supply, which also contains load control hardware. It contains a type K thermocouple interface and decoder in the shape of a MAX6675. Also on the board are interfaces for a 4x4-type keypad (with decoder) and text LCD.
The whole thing is controlled by a PIC18F4550. A USB interface will provide PC connectivity to enable programming of presets, etc.
1- The USB D+ and D- lines should be short and the two traces need to be keep close together. Ideally they should be routed with impedance control, 90 Ohm differential. Do not put any copper between these two traces.
2- Look up and read layout guide lines for the thermocouple chip and connector. The data sheet and/or an app note should have this information. This issue is that the traces become part of the thermocouple.
3- It looks like you have copper poured on the bottom layer but this copper is not connected. Also you have fairly thin traces to route ground. Instead make to bottom copper pour ground and connect all to this pour.
4- I see three colors indicating that this is a three layer board. Is this correct? Cost of making the PCB does up a lot once you have more than two layers. Also it is more common to have an even number of layer, 2, 4, 6, etc.
These are just what I saw and I’m sure there are more issues that others will point out.
Your Vcc line needs to be a bit wider to reduce inductance
Since you have a ground pour, tie grounds directly to it (or through a via for smt devices)
You need to place one decoupling cap (100n) right next to each power pin of each chip. The ground side should go to the plane. Ideally, the Vcc trace should go to the cap first and then to the chip through a short wide trace.
The caps for the crystal need to be right next to the crystal. On these, it’s best to tie the ground pins directly to the nearest ground pin on the processor with a wide trace rather than going straight to the ground plane.
Something looks a bit odd on J1 - are the pins really not in a straight line?
I’m not a huge fan of autorouters. For small areas and if you have your constraints set correctly they are OK. Just make sure you have proper constraints (width, spacing, differential coupling).
Tried posting this earlier but SparkFun wasn’t responding. This does repeat some of what n1ist said.
Decoupling cap need to be very close to the Vdd & Vss pins pins an IC. I think C4 is the decoupling cap for the PIC and should be on the bottom of the board, under the PIC so that it is close to the Vdd & Vss pins.
If the board is only two layer then why are there three layer colors and routing on those three colors?
Auto-routers that come with a PCB cad program are not great. I do PCB lay-out professionally with some expensive PCB tools and very rarely use the built in auto-router. The auto-routers that are very good cost 10’s of thousand dollars. Manual or inter-active routing on small boards like you have are the best way.
When you post the next revision of your PCB also post the schematic.
It might be a good idea to route most of the spare IO pins on the PIC to through hole pads or 0.1" header. This will allow you easy modifications if you need to use additional PIC pins or wish to use this PCB for other projects.
