Wow! Lots of good info here, I will reply as best as I can, going backwards!
GARTHWILSON wrote:
The main problem with putting vias in SMT pads is that if it's going to be assembled by machine and solderpaste gets squeegeed onto it, it'll get pressed through the holes and make a mess on the other side. I've seen it happen.
I know on this particular project I'm going to hand solder, but I also want to try the paste on a duplicate board and see the results. So I am going to put a bit of room between vias and pads.
GARTHWILSON wrote:
You'll want the thermal reliefs on pads that connect to a plane. If you don't have them, the plane acts as a great heat sink that makes it very difficult to get the temperature up high enough to solder something by hand, and worse, to de-solder it. (Again, been there, done that.)
AH!!! Now THAT makes sense! I was always wondering why "thermal", but now I see it!! Ok, thank you for that explanation Garth.
BigDumbDinosaur wrote:
In my designs, I don’t directly connect the device’s VCC pin to the power plane. Instead I connect it via a short trace to the device’s bypass capacitor, with the latter’s through-hole being the bond to the power plane. This arrangement, promoted by Dr. Howard Johnson, makes the capacitor more effective at preventing switching noise from getting into the power plane. See below illustration for an example.
Excellent reminder BDD. I made mine just like that as well. Make sense to follow those who know better than I do.
BigDumbDinosaur wrote:
Filled planes on the outer layers don’t function in that fashion and as I said, mostly add unwanted parasitic capacitance.
Ah ha, the OUTER layers cause that parasitic capacitance. I see them *so often* though, hm! Still, I wasn't wanting to do any of that anyways, and you helped sway me.
SamCoVT wrote:
The main issue with vias in pads is that they can wick solder down through the via during soldering. If you using a stencil with solderpaste and reflowing the board (using the toaster oven or hot plate/skillet methods, for example), this can result on less solder on that joint than you might want.
I see. Maybe I should get some stencils while getting the boards printed. And maybe a used skillet
SamCoVT wrote:
If you're going to be using an LM3480IM3-3.3, that's a part I use reasonably often for small currents, but it's worth noting that it comes in an SOT-23 package, which generally has quite poor thermal performance. For small loads (like 10 to 20mA), you can usually use it without thinking twice. For larger loads, you need to do the thermal calculations or build and measure (if you are lacking test equipment, the "finger test" works here - if you can hold your finger on it while powered up (less than about 60C), even if it's uncomfortably warm, it's fine (thermally) - if it burns your finger, it may or may not be fine (the regulator can operate at up to 125C junction temperature, but your finger is only good up to 60C)).
And...
SamCoVT wrote:
This, by the way, is one of those places where you might use a small copper pour to enhance the thermals of the device. If you haven't already bought them, you may want to consider switching from an SOT-23 package to SOT-89 package. The L78L33 is available in an SOT89 package. While it is physically bigger, it generally doesn't take up that much more PCB room than an SOT-23 and it has a proper thermal tab (which will benefit from a small copper pour around the device)
I did some research on this this morning. If the SOT-23 package is not a good one for this job, I'm willing to try something else. I went and looked up the L78L33, the main problem I see that it says the minimum voltage would be 5.3V or something, which is not what I'm expecting. Just 5.0V or maybe even a little less. That worries me, so I went searching some more. I found my old friend the LM1117-3.3, which I had used on a project years ago with success. Well, they also have an LD1117-3.3, and it's in a SOT-223 package which is definitely bigger than the SOT-23. Seems easy to work with, plentiful to get, and cheap. So that's my new converter for now. Thank you for that advice Sam!
SamCoVT wrote:
You had mentioned a CPLD and I was going to ask if you're going to be using an SMD PLCC socket, but your post while I was writing this up indicates you will be using one of those. I have not had good luck hand soldering the PLCC sockets with the internal contacts when using the "cheap from ebay" sockets because the plastic melts and the contacts move in the socket. I'd recommend using a stencil (oshstencils.com if you're in the US - they do ship international but it costs more than the stencil) and the skillet method or using a through-hole socket if you're not going to be using a name brand socket.
I was looking into through-hole sockets, but they don't, um, use a compatible footprint with the actual SMD PLCC-32 chip. Here's the thing: I am needing to use a socket for this particular ROM, just because I'm sure I will mess up one or two things while prototyping. But eventually I'd like to just solder the ROM chip permanently to the device because it really won't be changing ever once I'm happy. The SMT sockets have an identical footprint to just soldering the chip directly to the board, so I could simply not use the socket on later models, and only use this socket on my prototyping/first board. So, although you have cautioned me (and I definitely see why!), I will continue forward with the SMT socket and hope for the best. I wouldn't bake/skillet the socket to be sure.
SamCoVT wrote:
Otherwise, you should be able to solder down to about 0.65 or even 0.5mm with some practice and a bit of magnification. If you do this a lot, I'll recommend you get nice tweezers like Excelta ergonomic tweezers with the green foam handles - their "cheaper" versions (at around $20-40 each) will do fine
Oh, so there are professional tweezers out there? Not for just pulling nose hairs?!
Some additional questions:
I am putting both +5V input and +3V3 input options on the connector. Eventually I foresee my (future) 6502 running at 3V3, so I want to be able to bypass the voltage converter. But having that option permanently available would be nice. Could I just leave that +5V input floating, and just directly connect 3V3 to the output of the LM1117-3.3 instead?
Also, coming out of the LM1117 it goes directly to my 100uF cap. From there I use a via to connect it to the 3V3 inner plane. That seems a bit like a bottle-neck. Could ALL of the device's power go through a single via, and still be ok?
Thank you all very much for the advice and help!
Chad