Hey everyone!

I am going to be embarking on a new journey, using +3V3 power, CPLD's, and SMT/SMD parts. More to come later.

I'm asking some related questions here:

1) Nearly every connection is on the top of the board, so it's very difficult to route both +3V3 and GND that way. How do I then reach the bottom of the board efficiently? Can I put vias inside of a SMD pad, so it kinda-sorta acts like a through-hole? What is your recommended trace width for power/ground? Currently I'm using 0.508 mm traces and 0.889/0.381 mm vias, which are HUGE for this kind of work it seems.

2) I see some folks use copper fills, which is cool, but how close can I go with those? What's the deal with "thermal" vs "solid" connections anyways? Why not just fill everything absolutely possible?

3) Using 3V3 is different for me, but I believe I can still use my usual AS6Cxxx SRAM and 74HC' parts. The CPLD I'm planning on using has 5V-tolerant inputs so that's nice. I'm planning on using an LM3480-3.3 to bring 5V to 3V3, do you have other suggestions? Would my board still need a 100uF polarized cap to regulate the 3V3? This first device will be more of a "plug-and-play" device for my 6502 SBC, trying to start small and go from there.

4) These CPLD's have multiple VCC and GND pins. Should each VCC get it's own 0.1uF bypass cap? Or will 1 on the primary power pin be enough?

5) I heard once or twice that the footprints on KiCad for some of these SMD parts are not great. Any personal experiences? I'm using "hand solder" versions on resistors and capacitors, we'll see if that helps.

6) I was honestly just going to solder it by hand, with tweezers/pliers and a soldering iron and all that. The usual pitch on my chips is 1.27 mm which seems pretty do-able for me at this point, my soldering skills have greatly increased over the years. Does anyone recommend the goop + oven technique instead at something like 1.27 mm pitch?

Any links to helpful sources would be nice as well.

I'll be following up on a separate topic in amount a month's time. I'm happy to start learning new stuff! Thank you everyone.

Chad

Edit: Changed the title so that it's a bit more appropriate to the topics at hand.

_________________
x86?  We ain't got no x86.  We don't NEED no stinking x86!

First off, thank you BDD. Very good info!



Ah! I feel pretty stupid now I've been doing big 2-layer boards so long, I forgot how small 4-layer boards are very affordable!



Great, that's what I'll do. On one of the SMT sockets the pins are on the inside going towards the center, so I would then put vias on the OUTSIDE instead I'm guessing.



I know Garth has some info on the difference between copper pours and inner board layers, but I am still confused. KiCad calls them "fills" but they seem identical to me. You told me once that the VCC and GND planes act as one big capacitor that helps out. Perhaps when I say "copper pours" you are thinking I'm using them for signals perhaps, which I would not. IDK.



Uhhh, OH MY. Yep, I've been looking at 5V so much that I've completely ignored those 3V numbers on the datasheet. Until now! So, what family of 74' parts would work better at 3V3? Any suggestions for replacements? Maybe I need to look over my RAM choices again too...



Good to know, thank you.



I've read through it. There is a lot of contradicting stuff in there, and it's hard to find specific information. I think someone told me that I just need to pick someone's advice and roll with it. So, thank you BDD, great advice here!

Chad

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. There are several methods to mitigate this, including using smaller holes (about 12 mil or so or smaller holes generally won't wick solder much, and a lot of board houses can do these tiny holes now), moving the holes to the edge of the pad (like BDD suggested), or asking you board house to cap them (costs extra at most board houses I deal with - if your board house has a question asking about vias in pads, it's generally to know if they need to cap them). I usually use 10 mil vias when doing this - if it's a connection that carries current or heat, I use multiple.

Parasitic capacitance is generally why you don't fill everywhere possible (BDD already touched on this). Places where you DO want copper pours are where parts get hot and you want to use the PCB to manage the thermals somewhat. I do a lot of power converter and high power LED designs, so my boards are generally >90% copper covered solely for heat spreading. For this kind of design you are talking about, however, it's probably best to avoid them.

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)).

I know it says 100mA in the datasheet, but pretty much the ONLY way to get that is to have Vin be very close to Vout (eg. if you are planning on going from 5V to 3.3V, you might be able to get close to the 100mA listed, but not from a 12V or 24V source). The good news is that this device has thermal protection (that works about 90% of the time, in my experience), so if it does end up being overloaded thermally it will just drop it's output (eg. turn off the output) and turn back on a moment later when it has cooled a few degrees. If you see things resetting over and over after running fine for a bit, it could be this protection behavior and it's worth checking that the power is stable.

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)

One last note about voltage regulators in general, is to read the datasheet to see what they want for capacitors to keep the regulator stable. Some are stable even without caps, and some need a minimum amount of capacitance at the inputs and outputs to be stable. TI's datasheet for the LM3480IM3-3.3 says that it requires a minimum of 0.1uF on the input and on the output. More is allowed. The L78L33 is technically stable even without caps, but the example circuit shows 0.33uF on the input and 0.1uF on the output and you should have at least that much.

When using an electrolytic capacitor, you generally want a ceramic (like a 0.1uF) in parallel with it. The ceramic is much "faster" (we're bypassing a whole bunch of electrical theory and totally oversimplifying here) but doesn't hold much charge, while the electrolytic is much slower but holds a lot more charge. Both of them together can handle a wide range of possible voltage disruptions.

BDD nailed #4 so on to:
When unusure, verify or draw the footprints yourself. Most datasheets have a recommended PCB footprint for the part (although they almost always measure distances from the edges of pads, which is annoying because I have to place them by their centers), but some manufacturers will have a separate "package" datasheet that covers all of their parts in that particular package (it's at least referenced in the datasheet when they do this).
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.

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, but just make sure you don't drop them as you'll need to buy a new pair (while you can bend the tips back into alignment, it will be nothing like whey they were new). Also, if you haven't done much SMT soldering before, you'll need to practice. Order extra boards and solder your most expensive parts last. You'll also want some solder wick that has flux in it already.

Good luck and have fun! While its easy to make mistakes, almost everything is repairable if you have the time, patience, and skills. Even those of us who do this for a living make solder bridges once in a while and have to fix them.

Edited to fix grammar mistakes.

_________________
x86?  We ain't got no x86.  We don't NEED no stinking x86!

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?

Wow! Lots of good info here, I will reply as best as I can, going backwards!



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.



AH!!! Now THAT makes sense! I was always wondering why "thermal", but now I see it!! Ok, thank you for that explanation Garth.



Excellent reminder BDD. I made mine just like that as well. Make sense to follow those who know better than I do.



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.



I see. Maybe I should get some stencils while getting the boards printed. And maybe a used skillet



And...



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!



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.



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

Indeed, if you are trying to go from 5 to 3.3 you need an LDO or at least a quasi-LDO regulator. Your LM1117-3.3 looks like it might be reasonable for your application, but do read the datasheet carefully about the caps that it needs. The TI datasheet says the output cap needs an ESR between 0.3 and 22 Ohms and at least 10uF, which rules out a ceramic 10uF cap (ESR will be to low). They suggest tantalum caps for input and output.

Indeed there are, and they are a real pleasure to use. I use 3C-SA-ET at home and I can pick up an 0402 and position it reliably without it pinging out of the tweezers. Digikey carries those, but you may find them cheaper elsewhere. If you do ever get a nice pair, just don't drop them and never, ever, pry with them. As long as you never bend the tips, you will only have to buy them once.

Some regulators don't seem to mind this and others really don't like it - especially if your "provided" 3.3V is a little higher than what the regulator would like it to be. Many datasheets don't describe this scenario and I happen to know from "experience" which ones I commonly use that *don't* like that scenario. Section 8.4.1 in the TI datasheet for the LM1117 seems to say that you normally don't need a protection diode across the regulator, but they do show where it would go and describe when you might need to add it.

Most of the regulators I use will not pull *down* at their output, meaning if you accidentally input a higher voltage directly to the regulator's output node, the regulator will not hold it down to 3.3V and you will likely need to replace the regulator and whatever else in the circuit doesn't like higher voltages.

Sure* (* assuming the via is large enough, and you get to pick the size). I commonly put an amp through single 0.020" (0.5mm) vias. From a DC perspective, the via is like a trace with a trace as wide as its circumference, although it's also worth mentioning that vias are often around 1/2 Oz copper weight if you have 1 oz/ft^2 copper weight on the outside layers. From an AC perspective, it's a tiny inductor and this is one of the reasons you want bypass capacitors next to each IC (so you don't have to calculate anything about this little inductor and can ignore it).

You may be interested in the Saturn PCB Design Toolkit (free software (as in gratis, not libre) for windows) to help calculate the minimum value for such things as traces and vias. If you don't know what a setting does, then leave it at the default and it will usually be reasonable.

Chad,
Hand solder SMT PLCC socket can be quite challenging. You need to worry about 3 issues:
1. Fine tip and awareness of where the hot tip is so not to burn the plastic socket.
2. SMT foot print large enough for solder tip to heat the PCB pads, not the contact fingers of the SMT socket
3. The solder joints are hidden beneath the contact fingers of the socket and the SMT pads, so inspection is difficult and you can have intermittent contacts.

I would not consider via-in-pad for SMT PLCC socket; the extra heat needed and difficulty with inspection make it particularly challenging.

I understand the reason for using SMT PLCC socket, but you may want to wait until the design is proven and you have more experience with SMT soldering.
Bill
BTW, I have two tweezers, one fine, one coarse. Sometimes I use both tweezer at the same time to position and bent wires.

So much learning! Thank you all.

Quoting backwards again:



Good reasons to just go with the through-hole socket for now. 1) I am not ready for simply soldering my ROM directly to the board, and 2) I am not yet experienced enough to do *everything* SMT. Good compromise, thank you Bill.



Attached pictures are from my schematics, and the recommended from the datasheet. Could I add a diode in there, forcing any external 3V3 to not go back into the LD1117? Also, if the LD1117 output is grounded because of a floating V_in, this would also prevent problems there as well, right? If so, what type of diode would work? I am very unfamiliar with power regulation, typically I just use 5V for everything and walk away.



Whoa. Ok, I'll just make my via an appropriate size there, and that should do it. Good points!

Thank you all! This is great info!

Chad

Putting a diode inline with the output will just drop the output 0.7ish volts, and the output cap should be right at the output, so that configuration isn't going to work well.

First of all, there is nothing tricky about 3.3V except that it's not 5. You should be doing all the things you did before to get good regulated 5V, but just with 3.3V parts.

Looking at the part number you've selected and the datasheet diagram, it looks like you've selected an ST part number. ST has a reputation for making good copies of other manufacturer's parts and offering them at a less expensive price point, so as a hobbyist you'll see them a lot (because of the lower price) and they are a good choice for cost savings. Check out the difference in price between a MAX232 IC and an ST232 IC. What ST isn't so good at, in my opinion, is datasheets. Because they are trying to be a second source, they are trying to sell to people who have already designed in a more expensive part and are now either trying to reduce BOM cost or find an alternate part if the original supplier doesn't have any stock available to sell at the moment. This means that their datasheets don't need to be as detailed, and they are often just enough to get an engineer to say "looks good enough based on the specs".

If it's not an ST specific part (ST doesn't just copy - they make their own stuff too), then I'll recommend looking at other datasheets. TI tends to have more how and why application information in them. Specifically, the ST datasheet doesn't even mention anything about the ESR of the output capacitor, while it's spelled out (or in one case has a footnote) in several of the other manufacturers I quickly checked.

To make it slightly more confusing, not all of these clones of other manufacturer's parts are exactly identical. The Diodes AZ1117C-3.3, for example, is compatible with low ESR caps and you could use a ceramic 10uF on the output (but it does still need an ESR less than 20 Ohms and a tantalum would work fine here as well).

Even if you are using the clone parts, it's worth checking out the other data sheets. If you design using the Linear or TI parameters, then any of the others will, indeed, be a drop in replacement. You should check out the Linear or TI datasheet (they are essentially the same as TI bought Linear in 2016). These datasheets also show the protection diode and how it is installed, but it's likely you don't need it unless you have a very large (eg. 1000uF or more) output cap.

_________________
http://WilsonMinesCo.com/ lots of 6502 resources
The "second front page" is http://wilsonminesco.com/links.html .
What's an additional VIA among friends, anyhow?

One point about regulators: you will often see parameters like '200mA' and '17v maximum input voltage' (or similar combinations).

That output current is the one to watch because it is almost *never* available at the maximum supply voltage - and in some cases it is only available when the supply voltage is very close to the minimum. This is - obviously - because the regulator has to dissipate all the power that isn't going to the output, and 200mA at 17 - 3.3v is a lot of watts. Things get hot quickly. One reason for this is that parts like the old 7805 which could cheerfully dissipate into fresh air have mutated over time into physically smaller and smaller parts which *can't*.

This isn't often an issue with static low loads like HC logic, but when things start speeding up or you have something like a processor, ram, or rom in there, then it is important to pay a lot of attention to your power regulation.

Another issue with battery powered circuits is that if you're power saving using processors which spend a lot of time asleep with just a few microamps of supply, there's not a lot of point in using a regulator which has tens of milliamps of standing current! There are a few regulators which have only one or two microamps standing current - MCP170x familiy, and some from Deep Simplicity are good for this, but beware if you need both this and bursts of high current.

Neil

Ah! I never think of these things. Yes, thank you for that.



Of course I knew the first letters are from the manufacturer... but apparently I forgot that here! I went and looked up the TI version, TLV1117LV33, and yep that datasheet has a lot more information. Thank you for telling me about this.



An oscillating power supply is not good for sure. I will follow what they say exactly.



Does it come back to P = V * I, the more voltage the less current?



I really don't want heat. For all of the projects I've done, if anything is above body temperature then something is very very wrong.

Ok, great info here guys, thank you so much.

First, I'm going to use the TI part. It's not expensive, and it's an easy configuration. Second, I'm going to set up some solder jumpers or something to allow for outside 3V3 input, instead of assuming that the regulator will be ok with it. It's not like I'll be changing the power supply much if at all.

Well, I sure have learned a lot here. Thank you again, I appreciate all of the help and personal experiences I'll be giving updates and results as I have them, but at this time I'm just waiting for stuff to arrive in the mail to continue testing.

Chad

You should certainly use the ST parts if they are cheaper - it's their datasheets that are lacking, not the parts themselves. If you design using TI's datasheet, you can drop in the cheaper ST part with virtually identical performance. If you are more comfortable buying a TI part to go with TIs better datasheet, that's also a valid choice.

It looks like the 1117 family should be OK with you powering up the 3.3V side directly as long as you don't short the 5V (input) side to ground. I would expect you would leave the 5V (input) side floating when you are not using it.

--------------------------------------
The TI datasheet does a great job explaining the power dissipation and heat sink requirements (using the PCB design to heat sink, a complicated topic in of itself) but here is the abridged version:

Indeed power is V*I, but there are two different power losses. The first is quiescent current (often denoted as Iq, but called Ig in some places in TI's data sheet for ground current). That's the current just used to power and run the regulator IC. TI specs the quiescent current as 5mA typical and 10mA max, so we will use the worst case of 10mA. The quiescent power is then Vin*Ig so 5V * 0.010A = 0.050W or 50mW. (Note: Make sure you are using Volts and Amps (rather than mA) when calculating power and the result will be in Watts). The regulator will dissipate this much power (or less, as that's worst case) even with no load at all.

The power dissipation from handling the load current will be a lesser voltage, as the regulator will be dropping the voltage from your input voltage down to 3.3V and it only dissipates heat based on the drop. That calculation is (Vin-Vout)*I_L where I_L is the load current. I don't know your load current, but lets go with 200mA for the sake of example. The dissipation due to the load would then be (5V-3.3V)*0.200A = 0.34W or 340mW.

The total dissipation will be the quiescent power + the power due to the load, so 50mW + 340mW = 390mW.

The next step is somewhat sketchy - you need to select an Rθ. Theta is used here to denote this is a thermal resistance. The good news is that the thermal equations are the same as the electrical equations you use with resistors, but in this case a thermal resistance resists the flow of heat and develops a temperature across it instead of resisting current and developing a voltage across it. If you can use V = I*R then you can also use ΔT = P*Rθ where P is your power, Rθ is your thermal resistance, and ΔT will be your temperature rise (eg. the part will be that much hotter than somewhere else, usually the PCB or the air in the room).

In TI's datasheet, in section 7.4, we find RθJA = 61.6°C/W (the JA part means from the Junction (the semiconductor inside the IC) to the Ambient). This means that for every watt you dissipate as heat, the inside of the IC will be 61.6°C hotter than the air in the room. We can now calculate how hot the part will get. At 200mA load current, we calculated 340mW of total power. The temperature rise (above air temperature) will therefore be 0.340W*61.6°C/W = 20.9°C. If we assume the room air is 25°C, then the junction temperature will be 25°C+20.9°C = 45.9°C (this will pass the finger test as warm, but not burning hot). The limit on the junction temperature is 125°C, so the device is capable of higher currents.

The reason why I mentioned that this part is sketchy is because the Rθ in the datasheet is only valid under certain circumstances and some manufacturers don't even tell you what those circumstances are! Other manufacturers will give you 3 or 4 different ones to choose from, with none of them exactly matching your circumstances. Some measure it with the part soldered to "minimum pads", which is just the PCB footprint, while others might have 1 square inch of copper heatsinking with 1oz/ft^2 copper weight. TI is nice enough to show you several thermal configurations and you can see from their data that you need about 1 square inch of copper to get the datasheet thermal resistance.

Because the datasheet thermal resistances almost never line up with what you actually have for circumstances, your calculated value is an estimate. In this case, you have so much thermal overhead (eg. your calcualted Tj is much lower than the 125°C max) that it's going to be fine at 200mA. If your calculations put you close to the max Tj, then you would want to verify by building one and measuring the temperature.

--------------------------------------------------
A quick example to show you where you can't actually have the max current listed in the datasheet:
Same 200mA load, but now with 12V in. Quiescent power will now be 120mW. The voltage drop is much larger so the power due to the load will be (12V-3.3V)*0.200A = 1.74W for a total dissipation of 1.86W. The temperature rise from the ambient to the junction inside the IC (with 1 square inch of heatsinking using copper on the PCB) will be 1.86W*61.6°C/W = 115°C. If the air temperature is 25°C and the junction is 115°C hotter than that, then Tj = 25°C + 115°C = 140°C and you are over the max junction temperature. The regulator is rated for 800mA max, but you can see that at 12V, we can't even have 200mA. You can only get close to that max current when Vin and Vout are very close (which you happen to have as your circumstances). If you really needed 200mA from a 12V source, you'd likely need to pick one of the other packages that has a lower thermal resistance.

Edited to fix grammar