SO packages are confusing

[JenniferG]

I've recently learned how to make schematics and PCB's in Kicad.  All the stuff I've done up until now was 2.54mm pitch TTH.

I now want to try out some various DACs.  The DAC8550 is available currently (chip shortage is horrible), and I checked out the TI data sheet and it says "Tiny MSOP-8" package.  What does Tiny here indicate with respect to footprint? Or is just a marketing adjective in this case?

I looked in the SO Package library in Kicad and they have 6 different MSOP-8 footprints.  I put all 6 of them on the same PCB and they have differences in the center bottom of the chip.  They have a version where nothing is under the chip.. I presume this the one the DAC8550 uses but have no way to find out.

All of the Kicad footprints are 0.5mm pitch.  I looked at some MSOP breakout boards on ebay and it's confusing because they offer both 0.5mm pitch as well as 0.65mm pitch.  Kicad doesn't seem to have a 0.65mm pitch footprint.

Ideally I'd like to make little 25mm by 50mm breakout boards which can break out two MSOP 16 ic's per side.

Is there some resource I can read / watch on youtube which discusses all the variations of MSOP (and SOP) packages and how to figure out what to use? I spent a lot of tiem searching youtube and google but I guess I am looking for the wrong thigns.

[JenniferG]

Here is a screenshot I did of the six MSOP footprints Kicad offers.. all 0.5mm pitch (no 0.65mm pitch)

J1 and J3 appear to be the same as well as J2/J4/J5.  What's with those pin holes under the chip lol?  Is J6 the one I need for the DAC8550?  (the DAC8550 is MSOP 8 and this is MSOP 16.. but I want to use MSOP16 for all my breakout boards because they can be used for any size chip I guess. (except those with the pins in the middle bottom)

[Ice-Tea]

J1 through J5 are pretty much the same. Pad 17 is for the thermal pad found on some packages but not all (J6). Some of these thermal pads have the vias "pre-applied" (J2, J4, J5), some don't. The advantage of pre-applying is you don't forget them and they're put nicely on a grid relative to the component, the disadvantage is that you may end up with a lot of different via sizes on your board which is a bit "sloppy".

[sleemanj]

See page 29 of the datasheet for the recommended pattern and stencil openings.  There is no center pad.

[John B]

Also the thermal pad is a bit of a PITA if you're hand soldering. You only need to tin the pad with the tiniest whiff of 0.35-0.4mm solder, then reflow the IC to the pad with a hot air gun and some flux. Very easy to put too much solder on which squishes out and can bridge to the pin pads.

[JenniferG]

J1 through J5 are pretty much the same. Pad 17 is for the thermal pad found on some packages but not all (J6). Some of these thermal pads have the vias "pre-applied" (J2, J4, J5), some don't. The advantage of pre-applying is you don't forget them and they're put nicely on a grid relative to the component, the disadvantage is that you may end up with a lot of different via sizes on your board which is a bit "sloppy".

Oh I see thank you. The vias are so there is a connection to perhaps a large copper plan on the back of the board to distribute heat?  or perhaps a pcb which is entirely a ground plane on the back?   

[JenniferG]

Also the thermal pad is a bit of a PITA if you're hand soldering. You only need to tin the pad with the tiniest whiff of 0.35-0.4mm solder, then reflow the IC to the pad with a hot air gun and some flux. Very easy to put too much solder on which squishes out and can bridge to the pin pads.

I look forward to learning SMD soldering.  This DAC chip will by my first attempt I think.  I think I'll start with a PCB hot plate ? or should I try the air gun approach first?  I have a heat gun here I use for heat shrink tube but guessing that wouldn't work for soldering these?

[JenniferG]

See page 29 of the datasheet for the recommended pattern and stencil openings.  There is no center pad.

Thank you, now I know to look for "pattern & stencil openings" in data sheets for MSOP/SOP packages

EDIT: I just read the data sheet, and it says it's 0.65mm pitch.  But Kicad only offers 0.5mm footprint?  Do most of you use Kicad here? Or Eagle? EasyEDA?  I was turned onto Kicad and it's been fun so far.  I like that I am allowed to make large PCB's and 4 layers without havign to buy an expensive subscription.. it's free   Working on a 11.5" wide, 3" tall PCB , 4 layer for a synthesizer mod project.

[T3sl4co1l]

Are 4 and 5 actually different names/files?  They're essentially pixel-identical:



1 and 2 have square exposed pads, the rest rounded.  Doesn't really matter.  Vias are obviously present or not, and 6 has no exposed pad.

In general, watch out for "MSOP" having 0.5 or 0.65mm pitch (rarely others), body width from 2.8 to 4.6mm (the latter is supposed to be called TSSOP), and various lead lengths.  Most package designations are used haphazardly; beware. Always check the drawing to be sure.

Also, brush up on some IPC-7351 -- a copy can usually be found somewhere online.  The exact dimensions aren't too important, but understanding how they're calculated, and identifying kinds of joints, and how much clearance they need, is good stuff.

Tim

[Ice-Tea]

J1 through J5 are pretty much the same. Pad 17 is for the thermal pad found on some packages but not all (J6). Some of these thermal pads have the vias "pre-applied" (J2, J4, J5), some don't. The advantage of pre-applying is you don't forget them and they're put nicely on a grid relative to the component, the disadvantage is that you may end up with a lot of different via sizes on your board which is a bit "sloppy".

Oh I see thank you. The vias are so there is a connection to perhaps a large copper plan on the back of the board to distribute heat?  or perhaps a pcb which is entirely a ground plane on the back?

The datasheet should contain information what you are supposed to connect it to. Often, it is GND but not always. And yes, the 'idea' is to dissipate or distribute the heat.

[JenniferG]

Okay I see, the MSOP-16 is only offered in 0.5mm pitch.  The MSOP-12 is either 0.65mm or 0.5 pitch.  MSOP-10 are only 0.5mm pitch.  MSOP-8 are only 0.65mm pitch.

[Kleinstein]

The libraries that come with KiCad  are a bit messy. I was also surprized to not directly find a MSOP / SSOP / TSSOP 10 with 0.65 or 0.635  mm pitch.  For the footprints MSOP / SSOP / TSSOP are partially exchangeible.  Chances are there is one hidden somewhere.

There is a good chance to get symbols and maybe footprints from some distributors that offer a footprint service (e.g. Digikey). With many part you can get part definitions, though not sure about the foorprints with all of them and the symbols are often limited (just a box with pin numbers). There are some services for extra part entries.

There are also more parts libraries available in the web. So a google search would help.

Worst case there is the possiblity to draw the footprints yourself. It it a bit messy however as the manuals for Kicad in this area are not allways up to date. For such a relatively simple case, e.g. starting with MSOP14 and just remove some pins it could be reasonable simple.

Without much soldering experience, I would start with a smaller PCB, maybe seprate the project into multiple boards in a more modular way.
Depending on how you solder there are slightly different variants of the footprints that work better: e.g. hand soldering with an iron likes to have foodprints that extend out a little more.
It also depends on personal preference and tools how much space is needed.

[JenniferG]

Without much soldering experience, I would start with a smaller PCB, maybe seprate the project into multiple boards in a more modular way.
Depending on how you solder there are slightly different variants of the footprints that work better: e.g. hand soldering with an iron likes to have foodprints that extend out a little more.
It also depends on personal preference and tools how much space is needed.

Yeah I am gonna start by simply soldering the DAC8550 on a single little 25mm x 50mm pcb.  Onto a breakout board I make.  I want to make a 2 sided breakout board in Kicad which accomodates any MSOP without a heat sink.  I'll use two sides so there are more soldering options.  I'll add 2.54mm pitch headers there on the same PCB.  I'll put round pin female SIP sockets on this PCB so jump from it to the bread board with 22 awg solid core breadboard wire.  The rest of the project will be TTH/breadboard.  Any time I need another IC which is only available in SMD, I'll just solder it to a breakout board I made.

[Kleinstein]

MSOP can be a little challanging to solder, but other SMD parts like 1.27 mm spacing (e.g. SO16) and especially the resistors are rather easy to solder by hand. No real need to get back to THT.

If one takes the effort of getting a special PCB for the DAC chip it should be more than just a direct break out PCB. One should at least include decoupling capacitors. These should be close to the chip, even if a DAC is usually not that critical. It may also be sensible to have a little more function (e.g. the reference) with it.  At many places the smaller PCBs don't get cheaper and one could still cut the ready made PCB.

There are ready made break out PCBs available for the more standard footprints.

[JenniferG]

So I just designed a breakout board to be able to handle any MSOP, either 0.5mm or 065mm pitch.  There was room for two MSOP chips on this breakout board.

What do you think about it?  Any problems with it?



I made my own because I don't like any of the breakout boards out there. They are tiny and not uniform width and they expect you to solder square pins headers on it and insert into the breadboard.  But I dont like doing this as those pins are quite large and destroys the clips in the breadboard, making things too loose in short order. 

I also like my breadboard helpers to all be the same width so they fit neatly on my breadboard system.  More info about my "BLOCKS" breadboard system I use here:

https://www.modwiggler.com/forum/viewtopic.php?t=267893

I use round pin IC/SIP sockets on my little breadboard helper PCB's and jump from there with solid core 22guage wire to the breadboard.

Anyways if all is good I can print up these super cheap at JLCPCB.   

Regarding the decoupling caps, that makes sense, so I'll modify the design above I just shared in the video and add two rows of holes for each side of the IC.

[JenniferG]

Here's a new youtube video I just posted. I added the extra row of pin poles for any local circuitry which might be added.  If I have to I can point to point above it but I figure an extra row of pins should cover most things like decoupling?



Btw little pcb's this size 25x50mm only cost 33 cents each including shipping if you buy 30 from JLCPCB. 

I am thinking about making it so there is just a single MSOP chip on this board with a perfboard area to the side of it on the other half of the board. 

[mariush]

Decoupling capacitors are supposed to be as close as possible to the input voltage pin of the component.

In the video above, they would go right where the 0.5mm or 0.65mm text is.

You could easily make a custom footprint where the 0.5mm pitch part is combined with the 0.65 pitch part ... put half the 0.5mm pitch inside the 0.65mm pitch footprint .. because there's no center pad.

You could also go further and add footprints for capacitors or pull up/down resistors on each pin  ex

Code: [Select]

    (from MSOP)
         |
 [ ]    [ ]    [ ]  <-  to via to ground (bottom layer of pcb)   the pad on the left optional, top fill voltage maybe.
         |
  (to breakout) 

[jpanhalt]

I made my own because I don't like any of the breakout boards out there. They are tiny and not uniform width and they expect you to solder square pins headers on it and insert into the breadboard.  But I dont like doing this as those pins are quite large and destroys the clips in the breadboard, making things too loose in short order. 

The jumper wires provided by 3M (e.g., part # 923351) for its breadboards are 22 AWG (0.025" (0.6438 mm) diameter).  Typical square header pins are 0.025" across the flats.  They do not ruin the contacts when inserted aligned with the holes.  I have never had a problem with them.  The pins on some TH devices are larger and can present a problem.

As for your design, I can't tell much from the rendering, but I see no advantage in putting multiple footprints on the same PCB unless they are aligned.  For example, the smaller footprint inside the larger one.  The disadvantage of your design is that it covers up valuable space on the breadboard that cannot be used for other components or wires.

[JenniferG]

The disadvantage of your design is that it covers up valuable space on the breadboard that cannot be used for other components or wires.

It doesn't though. It's off to the side, see the modwiggler forum link I gave above to show the system I use.

[JenniferG]

Latest version:



I'll have to revise again now after tips above from mariush   I appreciate all the feedback.

[jpanhalt]

Where the outlines cannot be superimposed on the same side, some commercial vendors of BOB's use both sides.  That is, the small chip on one side and the larger chip on the other.  Only one set of headers (i.e., 2 headers) is needed.

[JenniferG]

Where the outlines cannot be superimposed on the same side, some commercial vendors of BOB's use both sides.  That is, the small chip on one side and the larger chip on the other.  Only one set of headers (i.e., 2 headers) is needed.

Yeah originally I had just 1 row of headers for the IC, but then someone suggested putting a decoupling cap close to the chip so I added the extra rows to handle any close up circuitry for any given MSOP chip. I am making this board to be compatible with all MSOP if possible.  All number of pins.  Look at the traces in the above video.. the outer header rows are connecting directly to adjacent header row.. agian it' sjust to all for any up close circuitry like a decoupling cap.

[JenniferG]

This MSOP breakout board I designed is intended for use with any MSOP IC.. at least that's what I want it to be.  If I needed to decouple I'd use the inner rows to do that and put the headers on the outer rows.  e.g.

[mariush]

Man you're thick ...  decoupling capacitors have to be as close as possible to the chip, to the voltage pins.
In the picture below it just happens that those holes have very short traces to the headers.
It just so happen that your DAC8550 has the voltage and ground pins both on one side so it would work if pin one is the top left one in your picture
But if you accidentally rotate the chip 180 degree and you solder it so that pin 1 is at the bottom right, where the "mm" text is, then you have long traces going all the way to the bottom of the headers, so you'd have maybe a couple inches or a few cm of traces. 

Also there's no rule saying that voltage and ground are always on one edge ... a lot of chips have voltage in one corner and ground on the pin diagonally opposite. For example, this ADC has voltage and ground in opposite corners : https://ww1.microchip.com/downloads/aemDocuments/documents/APID/ProductDocuments/DataSheets/21034F.pdf

This MSOP10 microcontroller chip has voltage on pin 4 and ground on pin 2, see page 30 in datasheet. But could easily have been pin 4 and pin 6 and then you'd have a capacitor between two long traces, as it's opposite headers.
Your pcb is big enough that you could have MSOP 10 footprint, or even MSOP16.

Here's what I was thinking with footprints for some capacitor / resistors to ground , showing half of a msop - made it in paint so dimensions aren't exact but you get the idea .. the other pad of the surface mount capacitor / resistor can go through a via to the other side to a ground

[T3sl4co1l]

Man you're thick ...

Great start there...

FYI, bypass caps have to be within some reasonable distance, depending on what kind of logic family the chip is based on.  For example, CD4000 you might not care at all.  74HC and most digital ICs, within 10cm say will be fine.  That's risetime around 5ns, 20mA drive capacity, 3.3-5V supply, that sort of thing.  Stronger chips like bus drivers may need more and closer.  Faster and stronger loads (like 74LVC, most MCUs much faster than 30MHz, gate drivers, etc.) even more.

As or more important, is having a ground plane under everything, so that, when the IC's outputs change state, the sudden change in direction has a firm footing, and doesn't upset the level of other outputs.  Or inputs for that matter.  "Equal and opposite reaction" applies here, just as anything else.  Never ignore the currents through the supply pins, everything that happens at an output has to go through a VDD/VSS pin too!

Not that you'll have that luxury on a breakout board, or breadboard.  Just do your best with enough wide and short ground connections.  If you're breaking out a particular chip, and it's fairly fast/strong, you might arrange grounds on every other pin, say; or more likely just build up whatever partial circuit it needs, fewer signals reaching the breadboard the better.

For a breakout board, at worst, you can glom a cap onto a pin or pad directly, and run a short jumper over to the other side.  Most times, it'll do to put it in the breadboard underneath.

Tim

[jpanhalt]

Hi Tim,

I don't disagree at all, but my advice for Jennifer is to use a commercial BOB for an occasional project.  I bought several sheets of generic BOB's years ago and have use only a few since.  If you need a specific peripheral, say a TC amplifier, strain gauge, accelerometer, etc., buy a ready made BOB.  If you don't like 0.025" sq. pins in your headers, use whatever you want.  Soldier will fill the gaps.

Then, if your are up against a real problem and need/want a specific BOB, design one for that device specifically.  A week's/month's/year's  supply is cheaper than a head of lettuce.

Don't waste your time trying to design a generic BOB so early in your adventure with no plans to commercialize it.

[JenniferG]

Don't waste your time trying to design a generic BOB so early in your adventure with no plans to commercialize it.

For example, this guy wants $10 for an MSOP breakout board on ebay:
https://www.ebay.com/itm/392144981122

For $11 I can get THIRTY of my custom ones from JLCPCB.   Btw, it appears the one above on ebay doesn't have any more features than what I did with my design -- other than a ground in the middle bottom.  There are no extra holes for decoupling cap like I've done with the extra row of pins.    With the extra rows it allows you to put decoupling cap on ANY two pins, very close to the chip.. it's only like a couple mm away..

Not to mention I can't stand the little breakout board available above on ebay because I don't put them directly into my breadboad.. I put them off to the side and use round pin SIP sockets:



See the small module of mine to the right in the middle? -- the one with the Arduino Nano on it.  It's 25mm x 50mm.. the same size as the MSOP "breakout board" I designed earlier today and shared here.   My "BLOCKS" system uses boards that are all the same width: 50mm.  The longer ones are 70mm  (standard size small perf board is 50mmx70mm).   So I have only two pcb sizes I am currently working with in my system:  25x50 and 70x50 mm.

I call them BLOCKS because they are like building blocks.  I can slide in any combination for different projects.  I might be using 3 different MSOP chips in the project at same time.. I can just remove a 50x70mm board and slide in three 50x25mm BLOCKS: MSOP boards.

Btw, I appreciate everyone's help here.

[JenniferG]

I see these MSOP boards here, 25 for $9 or so.  About the same cost as 30 of mine.  But they don't match my system and I made mine with the max number of pins so you can use them with any MSOP chip.  e.g. MSOP-12 for 0.65mm pitch.. I can stick an MSOP-8 on it.    Also I have both 0.5mm and 0.65mm pitches.

https://www.ebay.com/itm/403425727652

[JenniferG]

Man you're thick ...  decoupling capacitors have to be as close as possible to the chip, to the voltage pins.
In the picture below it just happens that those holes have very short traces to the headers.
It just so happen that your DAC8550 has the voltage and ground pins both on one side so it would work if pin one is the top left one in your picture.

You call me thick -- which actually made me feel bad -- but I read differently from the DAC8550 data sheet.  I put the decoupling cap in the right place in my previous photos?  Pins 1 and 8.

I think 2mm from the chip is close enough for the decoupling cap for my breadboarding purposes.  You are talking about making a modification to a board for a particular MSOP chip. I am designing this breakout board to be compatible with ANY MSOP chips.. any number of pins or pitch.



I appreciate your help though, if I was adding the DAC8550 chip or other MSOP chip to a final project PCB I'd do like you say and put it as close as possible.  But right now I am just trying to make universal utility modules, as prototyping building blocks.

[jpanhalt]

So, get your 30 boards and move on.  I'll bet you never use more than a third of them.  BTW, getting that first group of professionally made boards for your own design is worth more than $9.00, even if you don't use a single one.  They have other uses too, such as decorations for Christmas trees and coasters for drinks during the Holidays. 

[JenniferG]

So, get your 30 boards and move on.  I'll bet you never use more than a third of them.  BTW, getting that first group of professionally made boards for your own design is worth more than $9.00, even if you don't use a single one.  They have other uses too, such as decorations for Christmas trees and coasters for drinks during the Holidays. 

Haha, those would be cute ornaments I agree!  I was thinking actually though, as gifts, I might 3D print more of those breadboard stations and include a set of all my BLOCKS utility PCBs with it   Including a couple MSOP boards I make   Of course I am partial to my system and thing it is superior to anything else I've seen   Even though I am a newb

The breadboard stations come in double wide as well. I need to 3D print one.

[JenniferG]

As or more important, is having a ground plane under everything, so that, when the IC's outputs change state, the sudden change in direction has a firm footing, and doesn't upset the level of other outputs.  Or inputs for that matter.  "Equal and opposite reaction" applies here, just as anything else.  Never ignore the currents through the supply pins, everything that happens at an output has to go through a VDD/VSS pin too!

So like this then? -- modified the design.  It now has two ground planes, top and bottom and ability to tie those two ground planes to any MSOP pin with a very short jumper wire.  (Both the top and bottom ground planes are connected together, and so are the two ground pins.. i.e. it's not one ground pin for top and a separate ground pin for bottom.)

[John B]

If I have to use adapter/breakout board I would bodge on an SMD ceramic cap directly to the pins of the IC, using fine wire to bridge the gap. Otherwise the conductor length in your capacitor diagram defeats the point of the bypassing cap. It doesn't have to be pretty or even easy to do by hand, it's only proof of concept until you design the PCB for the complete circuit.

[JenniferG]

If I have to use adapter/breakout board I would bodge on an SMD ceramic cap directly to the pins of the IC, using fine wire to bridge the gap. Otherwise the conductor length in your capacitor diagram defeats the point of the bypassing cap. It doesn't have to be pretty or even easy to do by hand, it's only proof of concept until you design the PCB for the complete circuit.

It's amazing that a couple of mm isn't close enough.. i.e. TTH adjacent pins.  I'm newb so I just don't understand why it has to be 1 mm from chip instead of 2mm.

[JenniferG]

Btw, I just created a Github repository for all my BLOCKS utility module PCB's for my system.  Kicad files and gerbers generated for JLCPCB:

https://github.com/JenniferGDev/Blocks

[John B]

If I have to use adapter/breakout board I would bodge on an SMD ceramic cap directly to the pins of the IC, using fine wire to bridge the gap. Otherwise the conductor length in your capacitor diagram defeats the point of the bypassing cap. It doesn't have to be pretty or even easy to do by hand, it's only proof of concept until you design the PCB for the complete circuit.

It's amazing that a couple of mm isn't close enough.. i.e. TTH adjacent pins.  I'm newb so I just don't understand why it has to be 1 mm from chip instead of 2mm.

You want to look at the total trace distance. Your diagram implied the use of a through hole ceramic cap, so there is lead inductance there too. Your total length will include from the IC pin to the header, then 2x leads on the cap, then header back to the IC.

MLCC SMD caps can actually be much easier to solder directly to a pin, then a tiny bit of wire to the opposite pin in this case

[JenniferG]

You want to look at the total trace distance. Your diagram implied the use of a through hole ceramic cap, so there is lead inductance there too. Your total length will include from the IC pin to the header, then 2x leads on the cap, then header back to the IC.

MLCC SMD caps can actually be much easier to solder directly to a pin, then a tiny bit of wire to the opposite pin in this case

Should I go ahead and put pads on my breakout board to hold smd capacitor?  Like one pair of pads at each 4 corners of the IC? With any luck the power pin will be at on of the four corners on a given chip.  I can have one side of the pad tied to the ground plane.  So all one would have to do is solder on the cap and that's it .. no wire because a little trace will be there as well.

If so, what package / foot print shoudl I use for the SMD cap?

[JenniferG]

Okay so how about this guys?  I added 4 smd cap pads on each side of the pcb around the 4 corners of the IC.  So for example if I hooked up DAC8550 to this I'd put the smd cap in the upper left pair of pads.   And I'd simply connect the two pads in the upper right corner , to connect GND from the IC to the ground plane.

[JenniferG]

I give up.. TI, in its own datasheet says the 8850 is a "Tiny MSOP-8" package.. yet in another part of the document it calls is VSSOP(.

I miss the good ole days when everything was 2.54mm pitch TTH. I don't know why they have to have like a 100 different standards for package footprints on SMD IC's.  Really confusing.

[T3sl4co1l]

If I have to use adapter/breakout board I would bodge on an SMD ceramic cap directly to the pins of the IC, using fine wire to bridge the gap. Otherwise the conductor length in your capacitor diagram defeats the point of the bypassing cap. It doesn't have to be pretty or even easy to do by hand, it's only proof of concept until you design the PCB for the complete circuit.

Dude, it's a fuckin' SPI DAC.  It doesn't need a poured concrete foundation.  A few cm will be more than fine.

It's good practice for when you do need the short length.  But you don't always need it.

It's amazing that a couple of mm isn't close enough.. i.e. TTH adjacent pins.  I'm newb so I just don't understand why it has to be 1 mm from chip instead of 2mm.

The full loop length is what matters, so it's actually more like 20mm.  But like I said, that'll be fine.

You'll have a harder time dealing with signal quality from the SPI source itself, especially if you want to run it near the rating (30MHz).  But ATmega328 doesn't even go that fast.

And by "harder time", I mean in a relative sense.  What's harder than an already solved problem?  A slightly unsolved problem.

Here, it basically amounts to, putting in a 33-100 ohm source termination resistor on SCK, and preferably MOSI and nCS as well.  Read up on "source termination" to see how that works.  That'll cover you, still working up to fairly messy jumper wires.  Preferably, make twisted pairs with a ground dedicated for each signal, and wire them all into GND at both ends -- but it should still be fine up to say 20cm long wires just flying around wherever (loose, not paired).

If you see bit errors or glitches or whatever, spooky stuff like that, especially spooky stuff that seems to depend on where the wires are positioned -- you can always improve it later (by adding the GND twists, or using still better layout).  Or if you're seeing interference in sensitive circuits, or getting glitches due to nearby sources.  EMC (electromagnetic compatibility) is a big whole thing.

As for the new board layout, the ground fill is fine, I would maybe expose SMT pads on the back side, beside the header areas, so you can glom solder directly across for a minimum length (read: from pin to trace to pad) ground connection when needed.  I wouldn't bother with the adjacent bypass caps, but you can if you like -- and it's certainly a minimum length arrangement as shown.  SMT pads beside the headers can also be used this way, for components I mean, not just jumpering stuff.

and I mean like these, note the SMT pads beside the holes: https://www.digikey.com/en/products/detail/schmartboard-inc/202-0010-02/9559360

They don't show a rear view, but it's similar I think to this one, which they don't show the front of for some reason... https://www.digikey.com/en/products/detail/schmartboard-inc/202-0006-01/9559298
Or just read the datasheet.

You could add an exposed pad in the middle (to support MSOPs with that), and some vias nearby to better join top and bottom GNDs together.  Doesn't have to be via-in-pad, but a couple more GND-GND vias spread around would be just a little improvement.  (GND stitching vias every say 1-2cm is good up to pretty high frequencies (low GHz) so it's pretty damn cheap insurance on a small board like this.)

Or if you don't have hot air soldering, some people like to do it this way: you can put one massive via in the middle of the exposed pad, big enough to get a solder iron tip in there.  Then you can solder that pad, and still have some chance to inspect the joint.

Tim

[JenniferG]

You'll have a harder time dealing with signal quality from the SPI source itself, especially if you want to run it near the rating (30MHz).  But ATmega328 doesn't even go that fast.
Tim

Thank you for the very informative reply! I'll study what you've wrote but I want say that I am not planning on using the Arduino with the DAC8550, it will be STM32F103CBT6.  (It's for a Eurorack Braids module which I want to build on the breadboard for learning purposes.. along with reading the C++ code -- Emilee uses the STM32F103CBT6 with a DAC8551.  However that chip isn't available so I am going to try using the DAC85550 with a small modification to the C++ source since it uses two's complement instead.)

Here schematics and code for Braids are here -- schematics are in EAGLE format.
https://github.com/pichenettes/eurorack/tree/master/braids

[JenniferG]

As for the new board layout, the ground fill is fine, I would maybe expose SMT pads on the back side, beside the header areas, so you can glom solder directly across for a minimum length (read: from pin to trace to pad) ground connection when needed.  I wouldn't bother with the adjacent bypass caps, but you can if you like -- and it's certainly a minimum length arrangement as shown.  SMT pads beside the headers can also be used this way, for components I mean, not just jumpering stuff.

and I mean like these, note the SMT pads beside the holes: https://www.digikey.com/en/products/detail/schmartboard-inc/202-0010-02/9559360

They don't show a rear view, but it's similar I think to this one, which they don't show the front of for some reason... https://www.digikey.com/en/products/detail/schmartboard-inc/202-0006-01/9559298
Or just read the datasheet.
Tim

I created a video for you just now, it's just a few seconds long.  I have on one side of the board MSOP 0.65mm pitch and the other is 0.5mm pitch.  Allegedly this board would support any MSOP-8 to MSOP-16 chip -- ones without the ground /heat sink in the middle that is.

[T3sl4co1l]

Hm, I don't really like the idea of a combo breakout; but, I also don't have much justification for why.

I suppose the worst is that, because the traces (and pads) are in roughly the same place, top and bottom, there's no ground plane immediately under either one.  It's a complete void through the board.  Ideally you have traces always over or under ground plane.  But it's also not a big loop, and you'll likely be making far bigger loops through space as you wire up everything else -- and at that, probably only a few signals will be any kind of high speed, not all of them.

So, even at its worst, it's hardly bad.  It's probably more interesting that I feel that way about it in the first place, than why, heh.

So yeah, that's fine.

Tim

[JenniferG]

Hm, I don't really like the idea of a combo breakout; but, I also don't have much justification for why.

I suppose the worst is that, because the traces (and pads) are in roughly the same place, top and bottom, there's no ground plane immediately under either one.  It's a complete void through the board.  Ideally you have traces always over or under ground plane.  But it's also not a big loop, and you'll likely be making far bigger loops through space as you wire up everything else -- and at that, probably only a few signals will be any kind of high speed, not all of them.

So, even at its worst, it's hardly bad.  It's probably more interesting that I feel that way about it in the first place, than why, heh.

So yeah, that's fine.

Tim

Check it out again they are offset, Each has a ground plane under the IC.  EDIT: I see, the traces are above each other with no ground plane.  I'll fix it with 4 layers perhaps
EDIT #2: one would think though since the ground plane is directly below the chip's pins that would pickup all the noise the signal might emit? (or however shielding RF EMF or whatever noise works.. I dont know about that stuff yet, just know it exists and certain precautions need to be made)

[JenniferG]

This is interesting VSSOP-8 0.65mm pitch is almost identical to MSOP-8 0.65mm pitch.  Video below. I wonder if my MSOP breakout board would accommodate the DAC8550 well?  It's interesting in the TI data sheet it says it is in a tiny MSOP-8 package.. but under the package section it lists it as VSSOP-8.

In the video below, J2 is MSOP-8 and J1 is VSSOP-8.

[tooki]

I miss the good ole days when everything was 2.54mm pitch TTH. I don't know why they have to have like a 100 different standards for package footprints on SMD IC's.  Really confusing.

Versions optimized for miniaturization, cost, thermal performance, etc. And in standard parts, interchangeability with competing manufacturers’ packages.

But I really don’t think the packages are that confusing. What is confusing is the nomenclature, with manufacturers using their own names for standard package types…

[Siwastaja]

The only reliable and non-confusing process goes like this:
* Ignore footprint names
* Forget any assumptions
* Never try to reuse any footprints

Instead:
* Just look at the package drawings (and recommended footprint, but take even that with a grain of salt) in the datasheet of that very part.
* Learn to use your CAD drawing tools well so that creating new footprints becomes a habit.

[T3sl4co1l]

This is interesting VSSOP-8 0.65mm pitch is almost identical to MSOP-8 0.65mm pitch.  Video below. I wonder if my MSOP breakout board would accommodate the DAC8550 well?  It's interesting in the TI data sheet it says it is in a tiny MSOP-8 package.. but under the package section it lists it as VSSOP-8.

Like I said. Package designations are all over the place.  Some use internal codes, some reuse/abuse common names, etc. MSOP doesn't really mean much.  VSSOP I think tends to be more consistent but that might just be because mostly TI is using that designation(?).

Other examples: SO(IC) at least is almost always 1.27mm pitch, but body width mostly comes in two flavors; "SOP" is SOIC-like but tends to be "everything else" that's similar; SOJ is pretty much the same packages (plastic molding and lead size) but with the leads curled under ('J' shaped); etc.  (But J-leads aren't very popular anymore; not entirely sure why, maybe gull-wing is actually more reliable?, I don't know the stats.)

Even SOT-23 (TO-236) has a number of variations.  The pitch is (almost?) always 0.95mm, but the body width, and lead width and length, are sometimes a little bit off -- not bad enough the footprint doesn't work, but might have poor yield in production.  Also the frame lead or flat versions (SOT-23F) are generally pretty close, but may vary, particularly the heel dimension.

Mind, I'm mixing meanings here.  The manufacturer might not present their product as "SOT-23", they use some internal designation.  You look at the part and it's a small three-lead staggered component of about that size.  It passes the duck test.  You'd call it that if you saw it on a board.  But it might not technically be SOT-23 as such.

Hence:

The only reliable and non-confusing process goes like this:
* Ignore footprint names
* Forget any assumptions
* Never try to reuse any footprints

Be careful like this!

Tim

[JenniferG]

Has anyone used these round pin headers for breadboarding? If so how does the diameter of these round pins compare to the square pin headers? I'd like to keep the pin size down to 22 guage if possible.. it's the guage of solid core breadboard wire I use on my breadboard.

If these work well, I mgiht as well just buy the little square breakout boards sold for SOP/SSOOP/etc.. and use directly on my breadboard.

https://www.aliexpress.us/item/2255800155034595.html

[Kleinstein]

The diameters are given in the drawing: 0.5 mm one side and 0.6 mm for the other.  So this should be perfectly OK and not stressing the bread board.

[tooki]

I only use the round headers on breadboards. The solder end is the side with the flat shoulder, and that pin is usually 0.6mm diameter. The plug side with the taper usually has 0.4 or 0.5mm pins, which are great for breadboards.

The only downside to the round pin headers is that they’re significantly easier to damage than the square pin ones, and being brass, you can only bend them a few times before they break off. So be careful when removing them from a breadboard so you don’t bend the pins.

Another breadboard tip: for TO-220 packages, use flat nose pliers to grasp each pin from the tip to just below where it widens, and twist 90°. This way, rather than forcing the breadboard contacts apart by the width of the pin, the contacts now only have to spread apart by the thickness of the pins.

[JenniferG]

I only use the round headers on breadboards. The solder end is the side with the flat shoulder, and that pin is usually 0.6mm diameter. The plug side with the taper usually has 0.4 or 0.5mm pins, which are great for breadboards.

The only downside to the round pin headers is that they’re significantly easier to damage than the square pin ones, and being brass, you can only bend them a few times before they break off. So be careful when removing them from a breadboard so you don’t bend the pins.

Another breadboard tip: for TO-220 packages, use flat nose pliers to grasp each pin from the tip to just below where it widens, and twist 90°. This way, rather than forcing the breadboard contacts apart by the width of the pin, the contacts now only have to spread apart by the thickness of the pins.

Thanks for the wonderful tips!   Journaling this.

[dolbeau]

I give up.. TI, in its own datasheet says the 8850 is a "Tiny MSOP-8" package.. yet in another part of the document it calls is VSSOP(

The "features" block at the beginning of a datasheet is basically a marketing blurb. Helps figure out chips from one another but not for finer details. The table with part numbers/package/body size is the more reliable bit, combined with the drawings and other technical details (pinouts, ...) is what you can rely on.

Having started to do PCBs with SMD components a couple of years ago as a hobbyist, I would advise from my experience:

(a) double-check the pinouts for the symbols in the schematic, no matter what the source
(b) double-check the land patterns in your footprint, no matter what the source
(c) double-check that the signals you see on the footprint from (b) on the PCB matches the pinouts from (a), geographically speaking, and which one is pin 1
(d) the 'check DRC' command should be used liberally

As for the footprints, as other mentioned, pre-defined footprints (even for 'standards') aren't always reliable, and some manufacturers have recommendations that slightly differ from one another or from Kicad's idea. When using a pre-defined footprint or symbols (from Kicad or from e.g. SnapEDA or similar), always double-check it against the manufacturer's datasheet. For 'standard' chip in 'standard' package, there's usually multiple packages options; when selecting one, check for availability of this specific variant, and check the datasheet/land patterns of more than one manufacturer, just in case. When in doubt, make sure the PCB as enough room to accommodate the largest 'viable' package option (both the package itself and the land patterns of the various manufacturers) - but also that you don't route so many traces underneath it that it won't accept the smallest one. For hobbyist stuff, you may find yourself redesigning the PCB and/or BoM to use a different package or manufacturer because of the chip shortage, and it's easier when there's enough room from day 1.

If you're going to solder yourself, then obviously you need to pick packages you're comfortable soldering. If you're going to pay the PCB manufacturer to solder some components, then go fairly small - smaller PCBs are cheaper, and the cost of assembly for SMD isn't higher for smaller packages as far as I can tell (up to the minimum size supported). 0603 and 0402 are perfectly fine for the cheapest PCB assembly options from the likes of SeeedStudio of JLCPCB, and so are .5mm pitch packages and even many BGAs.

[Siwastaja]

It's also totally normal to have up to 4-5 different names for the same footprint even within the same datasheet!

If the part is available in 5 different packages, each with 3 different names, all this in the same datasheet, you easily get mentally overloaded, but in principle, the only task to do is mentally map from order number to the drawing, this is all that matters: find the right drawing for the part you are going to order. Forget everything else, like trying to relate to other products with same or similar footprint name. It doesn't matter.