UBB stands for Universal Breakout Board, is a tiny PCB exposing the 8:10 card slot connectors to allow Ben Nanonote to connect to other electronic devices, DIY things, Arduino, SPI interfaces ... without need of soldering the BNN itself like the UART Approach.
It has three operation modes:
- 6 GPIO + 3.3. V power on/off;
- 5 GPIO + 3.3 V power on/off + clock output (frequency is configurable, up to at least 56 MHz);
The motivation for making it is:
- because something like it is needed for the atusb project
- because we're seeing only little use of the Ben's 8:10 card slot.
A bit of background on the latter point. Back when Rikard "discovered" the 8:10 card slot, there was a lot of discussion about how access to it could be made convenient.
One idea was to make an extension cable that would end in a 100 mil header that could then plug into a development board. Wolfgang had a few of these made in China as a "street job". This picture shows one, minus the 100 mil header:
Alas, not much happened beyond this. Part of the problem may be that there are many different ways in which one may want to connect something to the Ben, and a 100 mil header, although popular and versatile, may not always be desirable.
Another issue is that, while the extension cable is simple, turning this into a proper product that can be made in quantity at a reasonable price and with good quality would be more time-consuming and more expensive than one may expect.
UBB dodges the issue of how to connect at the other end (more about this below), and addresses only the problem of getting the signals out of the Ben. Specifically,
- UBB provides the non-trivial electromechanical interface to the Ben's 8:10 slot, but
- it is the user/customer's responsibility to design a connection suitable for their needs, and
- it is also the user's responsibility to implement that connection and to verify its function.
UBB should be easy to manufacture and "productize" in general. (More about this later, too.)
 For whom ?
Use of UBB is expected mainly in three areas: first, to make the Ben more popular as a "master" for circuit development, be this for hobbyists or professionally. The master would typically be a placeholder for some other device that connects in the final design or that may even be embedded in it, but the master may also perform temporary tasks, such as in-system programming and acting as a debugging aid.
Second, similar to the "master" role, aid in experiments where only a partial circuit is made, with the objective of examining certain properties or acting as a tool with a limited lifetime, but where this circuit is not intended to become part of a "finished" device. For such experiments, it's important to have a flexible "master" device. A small Linux system that can connect directly into the circuit while providing all the usual tools and infrastructure is ideal.
Third, lower the bar for experiments with extension circuits designed for the Ben. Such circuits could later become proper 8:10 cards or they could even be integrated into future NanoNote products.
 Current Outcomes
There are already great outcomes from the UBB including:
- Ben WPAN, inspired by UBB, a project that has produced working 6LoWPAN personal area wireless networking.
- UBB-VGA is a way to connect a VGA plug with UBB plugged into a Ben Nanonote and get, at present, 1024x768@50 Hz, video.
 The ribbon cable
A ribbon cable was chosen, because these cable are easy to obtain anywhere and they are quite versatile. Here are a few examples that illustrate possible uses in combination with ribbon cables:
First of all, there are convenient press-fit connectors for them like the ones used for old (PATA) IDE cables. The picture shows a connector with ten contacts. UBB has only eight,but while connectors and even cables of this shape with only eight contacts do exist 1, 2, they are not very common. It is easier to use a cable with ten signals and just cut off the two unused ones after the connector. (And to reserve a bit of extra space where the connector attaches.)
And so on.
 The anatomy of UBB
The drawing shows the various zones of the UBB board. From right to left:
- Permanently inserted: when the board is in use, this area remains permanently inside the Ben's 8:10 card slot.
- Temporarily inserted: when pushing the card to insert or remove it, this part of the card is pushed into the Ben. While the card is inserted, this area stays outside the case and forms a small gap. This 1.4 mm gap can be seen on cards that have an outside part that's wider than the inserted part, e.g., the UART board,The gap is marked in UBB with a small indentations at each end.These indentations only serve as markers and have no other function.
- Coating overshoot: when coating the contacts with silicone or some other isolating material, the coating has to terminate within this 1.5 mm wide area. Transparent coatings can seen in the "yet another PCB" picture above.
- Cable contacts: this is where the bare wire ends get soldered to the exposed contact pads.
- Cable landing: this is a 5 mm wide space to which the cable can be glued. Attaching the cable with glue ensure that the wires and the pads remain in a fixed position relative to each other and makes it easy to solder them.For the best soldering results, one should first tin the wires and then gently bend them down, towards the pads. The following kind of tool works great for removing the isolation from the ribbon cable ends:
 Industrially producing UBB
The following areas need to be considered when taking UBB to a PCB fab:
- the board material,
- the Gerbers that define what goes onto the boards (copper, solder mask, silk screen),
- the cutting of the board,
- and panelization.
Below are a few explanations that should help to obtain the desired results.
Disclaimer: I haven't interacted with a PCB house myself yet, so all this is based on theory and on second hand knowledge.
Disclaimer2:I have interacted with a a PCB house my self and this is too much information for the manufacturer :) , give this page as reference but give them just a sumarized part of the Industrially producing UBB, and the gervers in a more private_software-friendly format like zip files instead of tar.gz, as available here :P
 Board material
The PCB is 0.8 mm (1/32") FR4 with 1 oz copper on each side. The surface finish would ideally be gold (ENIG), but tin-plating may be acceptable. Note that gold-plating, while sounding like something expensive, may not add significantly to the overall board cost.
There is one plated through-hole (PTH) via. The via hole has a diameter of 10 mil, but this can be changed to larger or smaller values if necessary.
Solder mask can and should be applied for appearance and to make it easier to solder the ribbon cable. (It's okay if the solder mask is scratched during use.) A silk screen should be applied.
 Gerber files
When generating Gerbers, at least the following layers are needed to produce the board: Front, Back, Mask_Front, and PCB_Edges.
SilkS_Front (front silk screen) is strongly recommended - it contains labels, the project name, "qi-hw.com", and the license (CC-BY-SA).
The Comments layer is optional and probably best avoided. It has meaningful content if merged into the silk screen, but makes the board look a little crowded. Note that it also contains a drawing that's outside the board.
Mask_Back is optional (it's empty - the back is just one large ground plane).
There are two potential pitfalls when generating Gerbers with KiCad's pcbnew:
- the ground zone at the back may not be filled. To make sure it's up to date, either run the DRC or "Fill or Refill All Zones"
- make sure to check "Exclude pcb edge layer" in the plot dialog. Otherwise, the board outline is placed on all layers, including the copper layers, leaving a ~2.5 mil path of thin copper around the edge. This may not only look odd, but could also cause trouble if shorn off.
For reference, I've uploaded the latest Gerbers as http://downloads.qi-hardware.com/people/werner/ubb/ubb-gerbers-20110207.tar.gz
I recommend using "gerbv" to view Gerber files.
 Cutting of the board
The board geometry has to be fairly precise. Tolerances of up to +/- 0.1 mm are probably acceptable, but more accuracy is better. Here are the general dimensions of an 8:10 card (all in millimeters):
The board outline is specified in the PCB_Edges layer with a 5 mil line whose center (!) is where the physical board edge should be. The following drawing illustrates this:
The yellow line is the board outline as drawn in the layout. The expected actual board surface is shown with black stripes. Here is a side view showing how the cutting tool has to be offset to obtain the desired result (not to scale):
In case the PCB house is unable to generate correct toolpaths with the data provided, I can also perform the offset calculation according to their tool specification.
The board needs an edge that falls off sharply. V-scoring would almost certainly yield undesirable mechanical properties and/or require extensive manual post-processing.
Since the UBB board is small, multiple UBBs should be made from a single board. For this, the UBBs have to be arranged in an array, according to the specifications provided by the PCB factory. If the PCB fab can do this themselves, even better.
If the PCB fab cannot produce a cut that goes all around the UBB board, it needs to remain attached at some point to the original PCB. This is often done with a perforated bridge that is later broken off. The following drawing shows which areas of UBB are more or less suitable for placing such bridges:
The red zone should be avoided, because it would be difficult to remove any remains of the bridge. The yellow zone is easier to handle. The green zone does not need cleaning.
Production final caracteristics:
- double-sided printed circuit foil
- Material: FR4 0.8 mm 35/35 micron
- Mask sensitive antisolder
- Screen printing one side per component
- Tin chemical
- Milling and panel ci
- Electrical Test
- Ci Measures: 11.0 x 25.3 mm
- Actions panel: 181.8 x 161.0mm in pattern: 66
- metallic Drills: 1
Gerber files generated from KiCAD