I am a first timer here. I teach electronics to art students at CSU Long Beach (no small task) and am in the process of developing a carrier board for the PICAXE 08M (PIC 12F683). Weve been using the PICAXE because its cheap, easy to program, and has some surprising hardware for such a small chip.
Ive been thinking about the Arduino a lot lately and love Tom Igoe’s concept that “wires are scary”. This is especially true to beginning students who have very little electronics experience. So what Ive been trying to develop is a small Arduino-esque board that would be cheaper and uses the simpler PICAXE 08m instead of the ATmega. At least initially Ive stuck with simple through-hole components so it could be offered in kit form (but maybe someday I could make the whole thing surface mount w/ usb…).
Here’s my board so far. This is the first time for me using Eagle (what a bear of a program to wrap your head around) although I have done numerous PCBs though Express PCB. This time I want to go through BatchPCB and then in the future look into a large order through Gold Phoenix. There is to be a ground plane attaching all gnd pins. Here are some of my questions:
What is the deal with the ‘hatched’ polygon option? Ive seen this hatching on the ground planes in the production Arduino boards but dont understand how this differs from the solid ground plane? When should I use the hatched ground plane?
I have taken the silkscreen for the DB9 and the 2.1mm power jack and converted them to tDocu layer (thanks to some past posts on this subject) so they are not visible on the sillkscreen layer. Am I safe in assuming the final board dimension should be the thin black rectangle that surrounds the board or do I need to do something else to define the board edge?
2b. This black line showed up when I switched to the board from the schematic for the first time along with the crosshairs in the bottom left corner. The cross hairs measure 0,0 but they dont sit on top of the thin black line. So am I to believe the final routing will be inside this black line?
In general is there any other advice that you could offer for this relative n00b?
If in doubt, use a solid ground plane. One reason hatched ground planes are useful is when you want to have an even-ish copper density on both sides of the board [something that if not right, can cause board warp @ high reflow temperatures]. That won’t be a problem for you.
I usually change the cam to create an outline layer gerber files [just a gerber file with only the Dimension layer]. BatchPCB will take an outline file IIRC.
2b. Not 100% sure, but I’m fairly sure that most vendors will route right to the edge of the line. Maybe the line is offset so that a trace drawn on grid coordinates @ 0,0 won’t be too close to the edge?
Increases the spacing from IC1 to R2 - on a bad soldering job / etc, the tab of IC1 might be able to touch the leg of R2. The other option would be to source IC1 with a plastic tab. I’d also make sure that R1/R2 have enough clearance - looks a tiny bit tight in that photo, but I don’t know what wattage of resistors you’re using.
You can also reduce the number of vias a bunch, the one from the back of the barrel jack connector to D1 can be routed on the bottom layer to D1, from C1 to the connector and D1 can also all be done on one layer, In fact, from taking a look at this, the entire thing can be done on the front layer, which lets you have the entire back as a ground plane.
One other note - I always preview my gerber files before going to manufacture, viewmate works well. I’ve caught several stackup / mirroring issues that way.
My old habit has been to keep power and gnd traces on the bottom layer leaving the top layer strictly for signal lines. (Yeah I dont normally do production boards.) But what you suggest does make sense. If I bring the power lines up top that would almost entirely leave the bottom layer for gnd alone. Should I go ahead and do this?
Duly noted on the placement issues there. I will check into that and also I will of course use viewmate to check everything before sending it out.
Ok heres an update. All the power & signal lines are on top. This leaves the bottom for a ground plane (not shown). I will also have a power plane for Vdd on top. Moved resistors to side by side and shifted everything around a little. I think that has helped a lot. Im not entirely so sure about the long signal line from pin3 on the DB9. Its not that big of a deal though.
that long trace shouldn’t be a problem - its only serial right? The board looks fine.
Oh, one other thing - I usually put a 0.1uf capacitor on the output of IC1 along with a 0.1uf cap right near the VDD of a pic. They’re so close in this case probably a single one near the pic would be fine. It most likely would work fine without any at all, but its just one of those things that might cause you problems.
Caps are always a good thing right? So I fixed the long wire thing simply by swapping the two resistors around. (Sometimes its hard to see the forest for the trees!)
Ive got to say this forum has been a huge help! This project of mine keeps looking better. Ive got the ground plane ironed out & have added a vdd plane which elimated some of my traces.
I have a new question now regarding text: What is the practical difference between vectored, proportional, and fixed? Vectored is what Im used to but the proportional font seems nice. Is there any difference post production or is there any advice on this?
alejmrm:
What about SMT? you can gain real state back if you change everything or almost everything to SMT, like caps, res, diodes, linear regulators.
Any way, is just a suggestion!
And a good one at that, but heres an answer:
b_w_:
… to beginning students who have very little electronics experienc … At least initially Ive stuck with simple through-hole components so it could be offered in kit form (but maybe someday I could make the whole thing surface mount w/ usb…) …
Use vectored, during gerberization all text gets rendered as vector. If you use another font, your text will look different on the board [different size too!] than it does in the software.
Vectored… good to know b/c Ive got everything sitting at proportional at the moment. Ill get on that.
This one is meant for kit form so I have to use off the shelf parts, but I am really excited about the FT232RL usb chip and the possibilities that that brings. A micro w/ usb on a credit card thin board .75x1.25" in size would be pretty cool.
(I must say Ive been spending too much free time on eagle lately!)
