SparkFun Forums

[mxguy31]

Hello,

I have lurked around for some time now, but need some help from the vast expeiance available here.

I have designed a board that will allow me to comunicate with the Advantech PCLD-785B and PCLD-782B through an RS485 interface. They are basically isolated IO boards, available on e-bay for cheaper than I can make them. This is my first real PCB design. I did this as a route to have a number of isolated IO available to be contolled through my PC. I am about the send the PCB (Drawn in eagle 6.2) to a fab house (iteadstudio.com). I would appreciate a quick review by anyone who has some free time to see if there are any issues that I should correct before forking out the cash.

Areas that I have the most concern about are the crystal osciallator set, and the ground planes. Also should I add some VIA's between the ground planes in general, or is it really worth while?

If you are willing to spend a few minutes to have a last look for me I can send you the eagle files. I consider this project to be open source, and free.

[mxguy31]

I have converted the top and bottom layers to .png for easy viewing.

Thanks again for any help!

[leon_heller]

The ground connections on the crystal feedback capacitors should be returned directly to the nearest ground pin on the MCU by a track.

[WethaGuy]

Can you reverse the 50-pin connector so the ground pins are not between the signal pins an chip? This would take care of the need for vias between ground planes also. You have a massive VDD feed. Is that much power going through this? There are 2 unlabled pairs coming off your oscillator that appear to be for caps. Caps are usually in series across the oscillator, not parallel to ground. Your clearances look a little too tight. You may end up getting a board back that has bridging or bleeding. Don't use the manufacturer's smallest clearance unless you absolutely must. It's better to size it up 2mils or even more to ensure you have usable boards.

I'd recommend downloading Sparkfun's design rules and running those against this board. It's going to find the clearance problems and other issues that Sparkfun has solved over the years.

The board has a bit of slack space. You could tighten it up and save some $.

[mxguy31]

Wow, thanks for the feedback! this is awsome!

leon, The ground line from the load capacitors:

I avoided running a single trace because I heard that a different length of ground trace to each capacitor should be avoided. I didn't think it would be much of a problem if I ran it the way you suggest, but I didn't know so I just attached them directly to the ground plane so that it would be essentially the same distance. I will make the change and run a separate ground. I assume this would avoid turning the ground plane into a giant antenna?



WethaGuy,

WOW lots of good stuff, thanks!

Unfortunately I can not reverse the 50-pin connector. I designed the board so that I can use an elevated female DIP connector to directly attach it to the advantech board header. If I reversed it, the board would hang over the back of the advantech board and risk being snapped off. I evaluated using a ribbon cable to connect the two, but then I have to mount the board somewhere. Directly mounting it like I have solves both problems. It was an issue I toiled with for some time. The slack space around the 50-pin connector has been left to allow for mounting holes if this idea doesn't work out. Also the studio charges ~$25 for ten 10x10cm boards. making it smaller doesn't save any cash... I was originally going to go with surface mount to save some money on board space, but I figure if there is no gain I will go through hole and make it easier to solder.

The massive VDD feed... yah... I know it is overkill. I sized it to be able to carry the full load current of the power supply for the board (L7805CV at 1.5 Amps). It was an arbitrary decision, considering normal max load current is around 600mA (the max485 uses a lot when transmitting). Is it is bad thing to have it this large, or just odd looking?

I am running 10mil clearances for everything, I will up it to 12mil to be safe. I am using Iteadstudio.com to create the board, they specify 6mil minimum and 8mil reccomended. Good thought on using sparkfuns DRC. I will see what it spits out.

The caps follow what i have seen as normal... unless I have misinterpreted something. I have attached an image of the circuit design. Maybe I missed something. This might explain the clock on my breadboard version running fast...

[mxguy31]

Ok I made the modifications suggested, and checked it with the sparkfun design rules without any errors. I think this might be the final rev before being printed... I will give it a couple days for any other suggestions. Thanks again, I will look for a place to host the source doccuments for all to use (if they want!).

[MichaelN]

It would be nice if one of the layers was a more complete ground plane. Since this would be difficult in your case, I’d suggest “stitching” the top and bottom planes together in a bunch of places with vias. This won’t add to the price, unless you really go overboard. This will minimise the loop area of any signal return currents on the GND plane, which can greatly improve the EMI performance of a board.

[mxguy31]

Sounds good, I added about 30 via's in various places. Mostly at the end of "stagnant" ground lines, around the perimeter, and other spots that looked bare.