the Universal Breakout Board (UBB)

Werner Almesberger werner at
Mon Feb 7 10:08:55 EST 2011

Here are a few more thoughts about the Universal Breakout Board:

Since several people have expressed interest in manufacturing UBBs,
I discuss the industrial production process at the end.


My motivation for making it was a) because I needed something like
it for the atusb project, and b) because I think we're not seeing
enough use of the Ben's 8:10 card slot.

Let me give a bit of background one the latter point. Back when
Rikard "discovered" the 8:10 card slot, we talked a lot about how
access to it could be made convenient. 

One idea was to make a 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. I think part of the problem is
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 ?

I see the use of UBB 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 of 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

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.

The ribbon cable

I picked a ribbon cable, 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.)

One can also solder the wires individually, e.g., in this type of
connector (for 100 mil headers):

It's of course possible to solder the cable directly to a circuit,
like I've done with the atusb I'm currently working on:

Or maybe to an adapter board:

Or with a custom-made PCB like one of these, which allows to apply at
both ends the approach of directly attaching the ribbon cable to the

For the nostalgically inclined, there are also press-fit connectors
in the shape of DIP IC packages:

Another non-permanent way of connecting things is with probe clips:

And so on.

The anatomy of UBB

The following 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

- 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 this picture:

- 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

Industrially producing UBB

The following areas need to be considered when taking UBB to a PCB

- 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

Disclaimer: I haven't interacted with a PCB house myself yet, so all
this is based on theory and on second hand knowledge.

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.

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, "", 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

There are two potential pitfalls when generating Gerbers with KiCad's

- 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

I recommend using "gerbv" to view Gerber files.

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.


- Werner

More information about the discussion mailing list