Hi, I’m a brand new hobbyist looking for some advice.
I’ve just created my first PCB layout in Eagle and want to actually have this manufactured. This will then be a little test board that I can use try various PIC programs. I wanted to keep this as simple as possible as I eventually want to create a simple IR transmitter that can register a hit on my laser tag gun.
I was going to have a look at your but, frankly, I’m not willing to wait the 60 seconds for the download to start at the website you used to post the files. It takes all of 10 seconds on Google to identify a file hosting service that’s a little less onerous.
For a better response, show images rather than Eagle files, so that people can see them directly. Most people can’t be bothered to download files and open them.
CircuitPeople:
I was going to have a look at your but, frankly, I’m not willing to wait the 60 seconds for the download to start at the website you used to post the files. It takes all of 10 seconds on Google to identify a file hosting service that’s a little less onerous.
The schematic needs redrawing properly. It’s probably OK, but it’s difficult to read.
On the PCB, route the supply and ground first, using wide parallel tracks. Then route the crystal, returning the capacitor grounds direct to the nearest ground pin on the chip.
Missing connection between negative of battery and ground
You can use multiple ground symbols instead of a wire connecting them all on the schematic - it will make it less crowded and easier to read. The same goes with power symbols (vcc)
C1 will likely be a higher voltage rating than 12v
C2 should use a polarized capacitor symbol. Also, 12v is not a common voltage for a 'lytic; 10v or 16v are more common. Either can be used on a 5V rail
PIC1 pin 4 should be MCLR*, not MCRL*
I would add an ICSP (programming) header to the board
PIC1 pin 14 (Vdd) needs to be connected
I would use standard reference designators (Y1 for the crystal, IC1 or U1 for the PIC)
If you are thinking of using the super capacitor, I would add it to the schematic and board. You can always label it as DNI (do not install) for now. You can even put a text note on the schematic that tells you to either load the supercap and charging resistor or the regulator for future reference.
PCB:
As Leon mentioned, the power and ground routing can be improved. You may want to do the ground as a pour instead of a trace
The traces to the crystal and its capacitors should be short and direct. Rotate the crystal and place it next to the two pins it connects to. Put the caps on the other side of the crystal, in line with its pins.
There are traces and components hanging too close (or off) the edge of the board. Keep at least 100mil from the edge
The footprint for C2 is wrong (if it really is a 100u cap)
C1 (the bypass cap for the PIC) should be right next to the power pin of the PIC. Ideally, the trace should connect from the regulator to C1 first, and then to the PIC.
Don’t run traces under the tab of the regulator; it is metal and will short out the trace.
There are no mounting holes. I would also add to the silkscreen the board name, model, revision, etc.
Missing connection between negative of battery and ground
You can use multiple ground symbols instead of a wire connecting them all on the schematic - it will make it less crowded and easier to read. The same goes with power symbols (vcc)
C1 will likely be a higher voltage rating than 12v
C2 should use a polarized capacitor symbol. Also, 12v is not a common voltage for a 'lytic; 10v or 16v are more common. Either can be used on a 5V rail
PIC1 pin 4 should be MCLR*, not MCRL*
I would add an ICSP (programming) header to the board
PIC1 pin 14 (Vdd) needs to be connected
I would use standard reference designators (Y1 for the crystal, IC1 or U1 for the PIC)
If you are thinking of using the super capacitor, I would add it to the schematic and board. You can always label it as DNI (do not install) for now. You can even put a text note on the schematic that tells you to either load the supercap and charging resistor or the regulator for future reference.
PCB:
As Leon mentioned, the power and ground routing can be improved. You may want to do the ground as a pour instead of a trace
The traces to the crystal and its capacitors should be short and direct. Rotate the crystal and place it next to the two pins it connects to. Put the caps on the other side of the crystal, in line with its pins.
There are traces and components hanging too close (or off) the edge of the board. Keep at least 100mil from the edge
The footprint for C2 is wrong (if it really is a 100u cap)
C1 (the bypass cap for the PIC) should be right next to the power pin of the PIC. Ideally, the trace should connect from the regulator to C1 first, and then to the PIC.
Don’t run traces under the tab of the regulator; it is metal and will short out the trace.
There are no mounting holes. I would also add to the silkscreen the board name, model, revision, etc.
/mike
Many thanks for the advice. We’ll endeavour to implement your pointers.
The schematic needs redrawing properly. It’s probably OK, but it’s difficult to read.
On the PCB, route the supply and ground first, using wide parallel tracks. Then route the crystal, returning the capacitor grounds direct to the nearest ground pin on the chip.
Thanks heaps. Any good references to review on good PCB layout?
I did a quick respin of this board to show a better layout. Still not the best (I’m not happy about how the ground pour is split by the VCC trace to the ICSP header, but there’s not much you can do about it on a single-sided board.
If the ICSP header is rotated 90° CW and moved to be off the end of the PIC the three line can be routed from under the PIC to the header. This keeps the three traces close enough together that there won’t be a ground split and also
allows easier access to the two IO pins.
I suggest adding pads and traces from any of the unused PIC IO pins. These don’t need to be to a header but just a pad so it is easy to connect a wire latter. Remember that Microchip keeps the pins-outs of PICs very close from one PIC to the next and even from the 16F to the 18F PICs. This makes it very easy to upgrade to a different PIC in the future without a major PCB change.
That’s the real trick of artwork; trying to visualize everything. I agree about the pads for the unused I/O. They have saved my neck a number of times.
Here’s the board with the connector rotated (and the power supply; doing it this way also cleans up some of the routing). Adding the spare pads is left as an excersize for the reader
If the LEDs do not need to be on that board edge I would make the PCB long to the left and move the LEDs to the left board edge. This will allow lots of room to put pads on the unused IO pins.
That’s the real trick of artwork; trying to visualize everything
Sure is. I currently working on a 10 layer board with fine pitch BGAs and high speed memories. I tend to spend more time thinking of how to route everything than I take to actually do the routing.
It really just practice, the more you do the easier it is.
