Purpose-built Boominator PCB project

[gmarsh]

Well, didn't get it done last night... and lots of stuff going on today so I don't think it'll be done tonight, sunday perhaps. I moved around a bunch of stuff, somehow cramming the design even tighter now, to make room for configuration switches. Going to attempt to wire up a 4-way "SOIC switch".

Snapshot attached of where it sits.

Saturnus: Thanks for the info. If I manage to squeeze in 4 switches, it might become 8 configurations yet. I'll worry about that stuff later when "production board time" rolls around. It'd be nice to get some frequency sweeps of Boominator boxes, in various configurations, to set up the default EQ curves.

Edit: Pricing... for a bare PCB and parts, I'd say $75 to $100 in reasonable quantities (say, 10+). For a prebuilt PCB I have absolutely no idea at this point, I haven't spoken to any manufacturers.

[gmarsh]

And parts availability on a couple of the DC/DC bits has forced me to rip up part of the design. It'll be done soon, I promise

[marce]

My only comment would be move the thermal vias apart a bit to allow solder between them, and to size the pads so that you can get a solder mask dam between the pins, this is critical for these devices to avoid shorts between the pads. Beware though most PCB manufacturers will cry and try and remove these solder mask dams when they front end engineer your Gerber data.
If you can find it IPC-7093 is an excellent spec covering all aspects of these type of components.
The picture shows the footprint I use for 7x7,mm QFNs' the yellow squares are where the solder paste is deposited, the thermal vias used are 0.25mm finished drill size with a 0.6mm land (IPC-class 3 compliant). This allows us to get the recommended 50-70% solder coverage of the thermal pad, and minimises the amount of solder that disappears down the vias.
Marc

[gmarsh]

Cool - thanks for that info.

Right now my smallest drill is 0.508mm, limited by the board house I planned to use. After reading your post, and talking to the PCB guy at my workplace, I think I might jump board houses.

[marce]

Glad to help, I've layed out loads of boards with these type of devices, they are fast becoming the only choice with some devices. They are excellent for getting the heat out of the actual chip, they fix them to the thermal pad. But from an assembly point of view they are a pain, but having an x-ray ATE system helps. With the power devices getting a good joint between the thermal pad and the board can be critical for heat dissipation. The thermal pad to case works well, even though they are expensive, also allows you to have a totaly enclosed product to IP67, very waterproof. If you have a look at engine ECUs and similar, the cases are now being moulded with heat fins as an integrill part of the enclosure, free heatsinking and easy assembly, the pads also have some give so you dont stress the board. I always add mounting hole near any devices that require the heatsinking and where the pads are, you dont want the board to bend with theses components, the lack of any legs means the solder joints can be easily stressed if the board bows.
It a nice looking design.

[marce]

A bit more info...sorry
by coincident someone asked a question about thermal design on a Electronics/PCB forum I frequent, so I thought the links I put up there will illustrate what I have said in more detail. The last link is specifically for QFN's and is a good read.

Thermal Vias – A Packaging Engineer’s Best Friend Electronics Cooling Magazine – Focused on Thermal Management, TIMs, Fans, Heat Sinks, CFD Software, LEDs/Lighting
http://www.gendreaumicrosystems.com/...ermal-vias.JPG
http://powerelectronics.com/mag/602PET22.pdf
http://www.ti.com/lit/an/snva183a/snva183a.pdf
http://www.cirrus.com/en/pubs/appNote/AN315REV1.pdf

Thermal data for some vias...
0.5mm finished 0.025mm Cu plating min 176 degC/W
0.7mm " " " " " 102 degC/W

[gmarsh]

Whew. Layout almost there. Things left to do:

- Figure out QFN/MSOP-EP thermals
- Silkscreen. The thing's so densely packed that it's going to be a headache
- Pick a cheap but suitable board house to get the PCB made
- Probably start pouring some top side planes (power/ground/etc)
- Add some ESD protection to the control inputs/status outputs
- Clean up the schematic to make it 'shareable'

I upgraded my Eagle install to 6.1, using the freeware license. Turns out that the freeware tools only let you edit the first schematic sheet, and this project has two schematic sheets. Dunno if it's a bug, but you can actually edit the 2nd sheet via cloning and copy/pasting from the first page - pain in the *** to do, but it works. Hopefully Cadsoft leaves this 'feature' in there, otherwise I gotta find a way to move everything onto the first sheet.

[PressureFM]

Looks great!

So if I understand correctly you are able to bridge the amp for 2 x 30 Watt, right?

[gmarsh]

You won't be able to parallel a pair of outputs to drive 30W into 2 ohms.

But, you'll be able to make pairs of outputs drive the same signal, and drive a pair of 4 ohm speakers in the same airspace, with the same end result. Unless you've got specific 2 ohm speakers you want to use, you should be OK.

[gmarsh]

Latest update:

I'm adding a header to allow plugging in an ADI "USBi" interface, allowing realtime adjustment/tuning of speaker parameters. I might also try to sneak an I2C EEPROM into the design for the SigmaDSP to boot from, allowing retuning without reprogramming the Atmel, though space is tight for that.

Still not sure what to do about QFN heatsinking. Vendors are recommending 0.3mm holes for heatsinking, minimum drill on the board is 0.5mm which is a limitation of most "hobby sized" board houses I normally deal with. I'm even contemplating moving that up to 0.6mm so I can get Olimex to build the board and save a few bucks. I'll probably swiss-cheese under the QFN and just fill the whole mess with solder by hand, and when/if volume manufacturing of this board happens, I'll work out a 'proper' QFN footprint then.

As for volume manufacturing, I really couldn't be bothered to invest time/money in taking orders, ordering parts, finding an assembly shop, etc - I'd sooner let someone else handle all that. If I can get enough interest from people, I might even pitch the idea to Sparkfun:

Pitching Your Product - SparkFun Electronics

I think there's a few other companies around that do the same sort of thing. We'll see, I'm more concerned with getting a prototype built/working at this point.