Screaming Circuits: Layout


Passively annoying

Passive components can be kind of offensive sometimes. I can understand them in analog circuits or charge pumps. But the fact that we need to put them all over our digital logic is just rude. Technically, I Common ground 0402s schunderstand why they have to be there, but philosophically, they violate my basic principles of life.

Back in the early days of personal computers, there allegedly was a company that had it's engineers remove bypass caps one by one until the motherboard stopped working. Then they'd add the last one back in and smile about the short-term cost savings. Well, that was a bad idea. The reality is that we need them.

I've written about some of the problems that can show up because of passives (or other small two lead parts like LEDs and other diodes). Like here, here and here. That last example has popped up recently and I have some more thoughts on it. Essentially, I'm talking about multiple two-lead components that have one lead tied together. That's a pretty common scenario with bypass caps or LEDs (or the LED current limit resistor).

There are a couple of ways to do this. Some error prone and some not. First, the general rule of thumb for two lead passives is, if at all possible, to have the same amount of copper going into both sides. That means that if you have one 8 mil trace going to one pad, have one 8 mil trace going to the other. Also make sure that you have solder mask stopping the solder from going off pad.

Passively annoying bad way AMethod A here is bad. It might just barely meet IPC standards, but it still is really not manufacturable. First, there are no thermals. That makes the solder melt much slower on the right side which can lead to unreliable solder joints or tombstoning.

Second, even though the theoretical solder mask openings don't touch and the keep-out (it's not shown but is just a hair narrower than the mask area) areas don't touch, they are close enough that you might not have any mask between the parts on the thermal pad. That can lead to components shorting.

Passively annoying bad way B Passively annoying bad way B1Method B is also bad. You have your thermals in there so that's good, but the parts are still so close together that you might not get any mask between them, leaving a path of bare copper between the parts that can cause them to drift around and mess things up.

Method B1, on the right here has the same issue. Likely no solder mask between the parts and a bare copper path between the parts.

 

Passively annoying bad way CMethod C here is fine. The parts are still at risk of not having mask between them, but there isn't bare copper running straight between them. There will be mask between the parts and the pad so there isn't any way for solder to bridge or the parts to drift.

 

 

 

Passively annoying bad way DMethod D here is also okay. You do need more room to spread the parts apart. That's a bummer, but sometimes "bummer" is the cost of reliability. Here, there will be solder mask between the parts and there are thermals. Everything is happy.

Use method C if you have a little side to side room to play with or method D if you have a little top to bottom spare room.

 

 

Duane Benson
Prevent flanking maneuvers.
Don't be like the Solders at Thermopylae

Electrolytic Ambiguity

I've written about ambiguity a few times before, like this post about fiducials. But I'm not talking about the PC board today. I'm talking parts. More specifically, I'm talking about silk screen markings for your parts on the PCB.

CapacitorsDiodes have a lot of opportunity for ambiguity, as you can read here. There are many ways to mark parts, but fewer ways to clearly mark them. Take a typical electrolytic capacitor. It can be thru-hole, smt metal can, tantalum, or a few other form factors. The capacitor manufacturers aren't doing any of us any favors where markation is concerned.

Check out this image. Yikes! In all cases shown here, I've oriented positive on the left, which, according to IPC is pin 1. This is also the zero degree rotation for the centroid value. But, isn't it nice of those component manufacturers to put the identification bar on the positive side for tantalum capacitors and on the negative side for metal can electrolytics? Not!

So, how should you mark this in the silk screen on your PCB? For an electrolytic capacitor, the best approach is to mark the positive sided with a (+), plus sign. If you mark pin 1, with the number 1, it can easily be mistaken for the minus sign. If you mark the negative side with a minus sign, it can easily be mistaken for pin 1.

For a metal can capacitor, it is also acceptable to put the notched outline in silk screen. We still recommend that you place the (+) plus sign on there too.

Duane Benson
I'm just positive I put the negative right on the left

Counting once, counting twice...

Panel single scLet's say you have two options: First, you could send in your PC boards for assembly as individuals. Second, you could send them in a panel. That's all fine and dandy. For a few, send individuals. For a bunch, panels might make more sense. But, when you do go to quote and order, how do you count the parts?

Let's take this example. As a single, this board has 32 line items on it's bill of materials. That's 32 unique parts. Counting all of the individual part placements, there are 56 total parts: 42 smt and 14 thru-hole. So, naturally, if you quoted the assembly of 20 of this board at Screaming Circuits, you would enter your desired board quantity as 20, Panel 4-up sc32 total unique parts, 42 smt and 14 thru-hole.

But what do you do if you send it in panel form? How do you count? It's actually not as difficult as it seems. In this example, it's in a panel of four. There are still only 32 BOM line items, but there are four times as many placements. That means that if you quoted this, as a panel, you would enter 32 total unique parts, 168 smt and 56 thru-hole parts. If you still need 20 of the final boards assembled, you would enter 5 as your desired board quantity.

In the end, you will have 20 assembled boards. In case you are wondering about the cost, there won't be a difference. As long as the final number of boards (after the panel is broken apart) are the same, your cost will be exactly the same for panel vs. one up. You don't save any money by sending in singles. However, if your board is panelized and all of your parts on on reels, full or partial, you can save money by ordering Short-Run production.

Duane Benson
50 Years ago today
Robert Rushworth flew the X-15 to Mach 5.03 at 100,400 feet altitude

Fiddling with Fiducials again

I recently posted a note about fiducials but I didn't have any images. Here's a couple of examples:

IPC acceptable fiducialsThis first example shows what IPC would like to see. If this is an individual board, this would be it. If it were part of a panel, you would follow the same pattern on the panel rails and also put it on each individual board in the panel.

As I wrote in the earlier post, we don't require these, but it's always a good idea. You'll need them once you go into volume manufacturing anyway.

The next example won't make IPC happy, but it will make Screaming Circuits happy:

Also acceptable fiducialsIt only uses two fiducial dots, but it isn't reversible. Reversibility is okay for jackets, but not for circuit boards. Since one of the dots is offset, it can't be placed on the machine and recognized as correct in any way except in the proper orientation.

The important aspect of both of these examples is that they remove ambiguity. There can't be any uncertainty, which is good because uncertainty is your enemy. It's a subtle enemy. It might not bother you 99.9 times out of a hundred, but then, when you're not looking, it can strike. So, give a hoot and stomp out ambiguity.

Duane Benson
False data can act only as a distraction. Therefore, I shall refuse to perceive.

Is it your fiduciary duty to use fiducials?

We don't require fiducials here. It's not mandatory. That's because we live in a prototype world and in that world, theory doesn't always match up with reality. That being said, there are things we can do and things we would prefer to do. Personally, I would prefer to get some ice cream, but my belt suggests otherwise.

So we do like fudicials, which begs the question: "how do we like them?" Well, the objective of a fiducial is to make machine registration of your PCB easy. That means the pattern should not be reversible. It should only have one correct orientation. Use three of them separated as far apart from each other on the board as you can. But don't put them any closer than 4.75mm from the edge. Ideally, it would be a 1mm copper area centered in a 3mm circle with no solder mask. Oh, and all of the fiducials on the board should look the same and be the same size.

Duane Benson
Over easy, yolk not broken.

Ambiguity

P3281577 smIt's pretty important to have unambiguous polarity markings and pin one markings printed on your PCB. In theory, for SMT parts, it really shouldn't matter; the centroid would take care of the placement orientation. But, you may have noticed that it's not a perfect world. It took me a while to figure that out, but I have finally concluded such.

It's not uncommon for the CAD library part to have the wrong zero degree rotation orientation The IPC specified location for pin one orientation Quad and BGA for square chips like QFPs, QFNs and BGAs is either the upper left or middle top. Check out our Centroid guide for more detail. If it's wrong in CAD, the centroid will be wrong as will everything downstream. That's why markings on the board are still important.

What do you do if your part is ambiguous though? This particular chip has three markings that could be interpreted as pin one indicators. At first glance, I'd assume it's the dot in the center top. It would match with the text. However, there is a white dot in the lower left that could be pin one indicator which would mean, in this case, the CAD library component had the incorrect zero rotation orientation.

Datasheets aren't always easy to find. This one is behind a registration wall. If you have a part like this, it's really helpful if you include some documentation (in electronic form) clarifying. I found the datasheet for this particular part and was able to confirm that it is correct as placed with pin one down in the lower left (90 degrees).

Duane Benson
Via via in the board,
what's the top on my PCB?

More CAD footprint woes

AT this point, I really shouldn't call them "woes." More like business as usual. I'm talking about the need to make custom footprints, or at leas modify footprints. Back in the old days, the only thing needed to make footprints was some copper pds, maybe plated through, maybe not. It was pretty rare to even need to make a custom footprint. Other than the occasional odd switch or relay, it was all done.

I really need to just get over it though. On the one hand, it seems like none-productive time; like I should be able to get right to schematicing and layouting. On the other hand, It's so common, I just need to see it as no different than any other routing task.

Starting at the top of my BOM, I have:

  • An MCU in QFN format - I modified a symbol and added a custom paste layer to the copper land
  • Two SOIC Mosfet drivers - I modified the symbol on an existing footprint
  • Some Mosfets in a PowerQFN package - Made a complete custom footprint
  • A Mosfet in SOT-23 package - Who hoo! I found a workable part in the library
  • Some Power Schottky diodes - custom copper land

Custom footprints

I have another Schottky, some TVS diodes, LEDs and a bunch of passives that came straight out of the library. It's certainly not everything that needs footprint work, but with so many variations of the more complex parts these days, it safe to assume that any SMT project will require a fair amount of library work. It's just the way it is.

Duane Benson
It's a pain but at least it's not as bad as 11811 has it

Shrouded vs. non-shrouded

Notch down bp purpleA connector isn't a connector isn't a connector. In this photo, the original PC board was designed to have an unshrouded break-away header, as shown in the inset on the right. I measured it. The entire header fits within the silkscreen outline.

However, as you can see, a shrouded header was used in that spot. While as designed, there was plenty of clearance between the header and the two capacitors and resister, the shroud for the substituted header covers all of the resistor and half of the capacitors.

You can prototype it this way, but it will never fly in production.

Duane Benson
Find the ghosts of Dawnstar

QFN Solder Paste Layer

LBDCminiI've got the fab order placed with Sunstone.com for my next demo project. The little board is represented here at pretty close to actual size on screen - provided you have a 22" monitor set at 1680 pixel horizontal resolution. Give that, you might want to click on it to pop up a bigger representation of it. That makes it about 4 X life size.

When you do that, take note of the QFN / DFN parts: The processor in the middle, the LiPoly battery charger right between the upper two mounting holes and the RS232 driver in the lower left. I've followed my paste layer advice and segmented the paste stencil layer to reduce the chance for float or major voids.

I found a footprint in the library for the big processor in the middle. I just had to modify the paste layer, as shown here. I made the footprint for the charger and RS232 chips from scratch. Neither had anything close enough in the library.

The DFN has a slightly different approach to segmenting the stencil layer. Little squares like I used on the other two chips work just as well, but this is effective as well.

Another thing to take note of is the markation on the LEDs. The original footprint for the 0402 LEDs does have a polarity mark, but it's one of the types that can easily be misinterpreted or can be difficult to see. The diode symbol put down in silk screen removes any possibility of ambiguity.

Duane Benson
I'm happy I live in a split level head.

 

Particle Update

I've been ignoring my Geiger counter for a while now, but I picked it back up and made some progress again. For some reason, I just wasn't getting the 555 based HV power supply to generate a high enough voltage. In frustration, I bypassed the 555 and fed a PWM signal in from a microcontroller board that PIC SMT geigerI have laying around.

That fixed the problem. I still don't know why I wasn't able to the the 555 doing what it was supposed to do. I'll have to spend some more time on that some other day, but for now, I've prototyped it out and I'm happily detecting particles. I whipped out the new layout and will send off to Sunstone.com com for another set of PCBs.

I've also replaced the Atmel chip with a PIC. I don't have anything against Atmel. I'm just more familiar with PICs. Once I've built a few of these, I'll change to really small packages - QFNs or BGAs for the chips - to make the board a little more fitting with our assembly capabilities. The SOIC chips are fine, but our machines don't even come close to breaking a sweat with things that big.

Duane Benson
We treat agoraphobia for PC boards