Main Site Documentation

DAC Board for Gadgeteer


I’m designing a Gadgeteer board for 2 channale 12bit DAC (MCP4922 chip).
May be someone is interested.
This very easy board uses the Microchip MCP4922 that has good performance and it’s interfaced via SPI S socket. The board supply 5V and has the MCP1541 reference voltage regulator to supply 4.096V to the DAC chip, so it can used with 1mV 12 bit resolution. I’ve prototyped on the Fez-Hydra board and works with no issue.
I avoided, for first release, the SMD components, so the board is bigger than smd version, obviously.
Dimensions are 1.6x1.3 inches ( 40x33 mm).
I will do a driver as soon as I get some spare time in the next days.


Excellent, great to see more people starting to deliver their own boards !

I’m far from an expert, but if you’re steering clear of SMD then you might want to increase the pad sizes around the PTH components, to help “novice” soldering. Some of those pads, particularly those on IC1 and IC2 look a tlittle small to me (but then again it is still a small board - maybe not tiny, but still small ! :slight_smile: )


This layout is still rough, need a bit of reworking, so I’ll get your suggestion although the real problem is the soldering of the SHF smd connector (I really hate them!!)


Do not forget the holes, rounded edges, marking.

Read the design guide.


You should consider to change from through-hole to SMD. It really isn’t that hard, even for a hobyist.


Nice! Check out the NET Gadgeteer Module Builder’s Guide version 1.7 at


Not less than 0805 SMD, please :hand: Do think at old hobbyists :wink:


Connector needs to be rotated 180 degrees.


@ Architect: Good catch … I didn’t realize that …

I will finish the board tomorrow evening (I hope …).


This looks like it could be a fun board to play with :slight_smile:

A few comments:

Connector needs to be rotated 180 degrees and should (not must) be centered and must have an “S” near it. Also need the mounting holes on 5mm centers (if you designed the board in inches, you’ll need to do a conversion) Here’s the module design guide:

I agree with the comment about making the resistor through holes larger. Same for the IC2 holes. You also have some signal traces which seem to be a bit too close to the pads on IC2 and C1. I’m not sure if they’ll check-out, but to help avoid shorted boards, increase the spacing anyway.

Have you considered removing all those individual ground lines and just going with a ground plane on the bottom, especially since this is an audio device? If you go with a plane, and try and route most of your signal on a single side, you can remove the giant ground pad on J2 and tighten up the board a bit to make room for those mounting holes. If you prototype with Seeed, for example, 5cm by 5cm is 40% of the cost of the next step up size-wise.

What is JP1?

To broaden your audience, you may consider putting in a set of pin headers to enable non-gadgeteer devices to connect. Up to you, but I prefer to do this on my own stuff to make it possible to use with other boards.

Something messy near pin 1 on IC2. Maybe just s small label?

Does SPI require a resistor or anything to help protect the main board? I don’t recall. Anyone?

On the gadgeteer connector: for my latest board, I modified the connector footprint to pull the pads out a little from the center. There should be plenty of room for a good connection, but now there’s room to get an iron on the pad, especially if you use the ones from Gus rather than the ones from Samtec. Pic attached.

Larger question:
Are you intending to create audio samples on the fly with this? I found this to be a problem with NETMF in the past in that it simply couldn’t crank out the samples fast enough to avoid zippering on the generated audio signal.

The Hydra may be fast enough for an easy signal (wave table lookup, for example, as opposed to math on the fly), but I bet the Spider will not.



Ok most of board is coming out.
The JP1 is for Vref : VCC (5V) or 4.096V from IC1 MCP1541.


:o that’s a large board!! (judging by the size of the person standing in the back off to the corner :D)


Yea she’s there to show dimensions …

The layout:


Not to nitpick, but those clearance areas around the mounting holes don’t appear to meet Gadgeteer size standards.

This can be important because the gadgeteer mounts are well-sized to clear nuts and screw heads.

Also, if you happen to use Seeed studio or Itead, use round pads, not hex ones. They have had some issues where the solder pads are rotated compared to their solder mask.

You can also extend the ground plane much closer to the edges if you want.



@ Pete: Uau what an eye !! I will check !!
I’ve worked with hex pads and I didn’t get problems, but it’s not a problem, I will change to round ones…

Thanks for suggestions… :smiley:

Now the board is coming to the finish …


@ dobova

Not sure if the red color is just in the program, but if you were considering a red solder mask, be aware that the Gadgeteer spec calls for only power modules to be red. For other modules, the recommended solder mask color is black, though that’s not required.


I see a lot of unused real estate.
You can move components a little bit to make the board smaller (=cheaper).


@ Architect
you are right, but for this first run I need more space on board. I will make smd version soon.

@ devhammer
Ahaha, it will not be red! But was beautiful for rendering. I’ll try to get the brown silk like other modules.


It is black actually.


Yes black …