I’m working on a board that will take readings from 8 thermocouples using AD595. I haven’t done much work (any) with PCB designs before so if someone could take a quick look and see if there is anything obvious I should be changing on the board, especially the routing, that would be great. This is coming out of the eagle autorouter which I have read is not very good but I need help on figuring out what it might be doing wrong. I will fill in a ground plane on the top and an analog ground plane on the bottom after I get all the routing figured out.
I tried to post this a few days ago but it never showed up. I hope it doesn’t double post.
I really feel bad for saying this, but that looks like a spider web in the corner of my shed. How is anybody supposed to know what components you have? And you want someone to trace and following all those lines and then remember where they went, then tell you if anything’s wrong?
You should really crawl around the net for some good Eagle tutorials that teach organization. Here’s a good one that was on the first page of a Google search, http://electronics.stackexchange.com/qu … schematics.
First thing is you need to place your components where there is the fewest crossing Net lines. Then label your nets. You can also split up your nets by naming the net at both ends.
I did a thermocouple signal conditioner with the 595/594 many years ago. I don’t remember it being at all sensitive to layout, but Analog has a recommended layout [here that emphasizes keeping the thermocouple connection near the chip for best compensation.](http://www.analog.com/static/imported-files/application_notes/AN-369.pdf)
One point I should have mentioned (JimEli reminded me).
Print out your layout full size on paper and put a sheet of styrofoam or similar below it and then populate it with parts. You will immediately see which parts are too close together and which ones can be moved closer. It’s a step I try to always remember to do.
Having the schematic symbol for a component look like an IC is not the best way most of the time
Labeling the pins inside the schematic symbols with their function makes the schematic much easier to read
Using named nets rather than spaghetti lines makes the schematic easier to read. For example, separate each thermocouple connector form the next one by 100-200 mils. Place short net stubs on each pin. Then label the nets TC8_P and TC8_N (or TC8_1 and TC8_2 or anything that make sense). Likewise, do the same for the DG407. That will clean things up
You have text collisions all over the place
You probably will want a ground pin on each of the headers to make them more useful
Avoid 4-way (+) junctions in schematics or boards. Use two T-junctions instead. It’s much easier to find shorts where lines cross if none of them do so intentionally
Add a fuse before D1. Otherwise, connecting the supply backwards will likely vaporize your traces
Look at [this example of a schematic using a mux and AD595 for thermocouples
PCB:
Avoid right angles. Use two 45-degree bends instead
Traces should connect to pads and other traces at 90 degrees. Acute angles can cause acid traps
Allow yourself a little more space between components
Use much wider traces for power and ground; consider a ground plane.
Thanks for all of these tips. I read through the guides you referenced and I revised the schematic which I think is much neater now. Next I’m going to do the styrofoam layout, great idea. There’s a couple comments I was still not clear on.
I doubt the top layer traces running under the DG407 pins will work.
- Why not? I'm not arguing the point, just curious what makes it not work.
I did a thermocouple signal conditioner with the 595/594 many years ago. I don’t remember it being at all sensitive to layout, but Analog has a recommended layout here that emphasizes keeping the thermocouple connection near the chip for best compensation.
- In this case with the DG407 multiplexer I'm assuming the way to apply this rule is to just keep the multiplexer as close to the AD595 as possible rather than the thermocouple connectors?
n1ist, I’m just now reading through your comments but thanks, especially for finding that blogtronix example. I’m going to go over all of that next.
Can’t read JimEli’s mind, but if nothing else I’d suspect you’ve got some trace-to-pad clearance issues. While there’s fabs that can deliver (if their DRU doesn’t give any complaints, at least), it is a bit of an unnecessary gamble; you can easily make the traces go right through the middle between two pins, rather than hugging so closely to one of them.
The only place you can’t do that is where you’ve actually got 2 traces trying to make their way between two pins at the mcu. However, you’ve got plenty of space to the right - between the mcu and the inductors - to which you can move the right trace.
The via under AD595 is also precariously close to one of the AD595 pins - move the trace next to it a bit over to the right, and that via suddenly has a lot more margin to work with.
Just one note on the schematic - though the way you have drawn the crystal and support capacitors is technically fine, there’s a defacto (maybe official, but not that I know of) standard of drawing these in a schematic;
the general arrangement of the capacitors at a 90 degree angle from the crystal, parallel to each other, and equidistant to the crystal, makes it visually very easy to recognize, even in a moderately busy schematic such as that of the Arduino UNO Rev3 (there’s actually two crystal+caps groups in there): http://arduino-info.wikispaces.com/file … ematic.jpg
Unless you are doing something different that I don’t know about, but with the way you have drawn the reset circuit, it would stay in reset the whole time. Did you forget a button?
Have you already prototyped this?
I have to say, you did a fantastic job on the schematic, very easy to read and understand!
