Re: MicropendousX-1343 refresh

[Opendous Support]

I'm surprised you managed to get Freeroute to route the entire
board. Really cool how you got the 3D view to work.

USB signals are differential so I strongly suggest you place a wide
GND trace under them. It isn't practical to meet proper USB impedance
guidelines on a 2-layer PCB since the tracks would be too thick but
you should attempt something.

Similarly for the crystal load capacitors, place GND vias next to
each load capacitor and connect them with thick GND traces or GND
fill. Right now you have a very long trace for one of the caps which
may cause problems.

To comply with USB suspend requirements, the 1117 regulator should
be replaced with a low quiescent current LDO such as SP6205EM5-L-3-3,
or XC6222B331MR-G, or LD3985M33R. Choose a 500mA+ LDO to ensure it
can handle 250mA across the full temperature range since the copper
heatsink area will likely be very small. These are compatible SOT23-5
parts which are easily DIY'able.
http://uk.rs-online.com/web/p/linear-regulator/6865774/
http://uk.rs-online.com/web/p/linear-regulator/6868802/

If you plan on having these boards manufactured I recommend putting
all components on the top layer. If the JTAG header is to be
thru-hole then you can place the GND-GNDPWR cap+resistor in its
plastic casing area. If there isn't enough room you should consider
making the board slightly longer and adding GND pins to the headers.
Unless it must be 50mm long more pins won't hurt.

>during construction found a few things difficult to solder

If referring to the ESD zeners then unfortunately I haven't been
able to find anything suitable larger than 0603 size. The USB
standard requires line capacitance to be <5pF. The CG0603MLC-05LE has
0.5pF while 0805 parts are in the 500pF+ range. I have successfully
used the PRTR5V0U2AX which is SOT143 and DIY'able.
http://uk.rs-online.com/web/p/varistor/6909938/
http://uk.rs-online.com/web/p/varistor/6840854/
http://uk.rs-online.com/web/p/tvs/7258726/

I have switched to the DM3D-SF microSD connector for newer projects
since its pins are all exposed on one end and it survives reflow well.
http://uk.rs-online.com/web/p/memory-card/7388809/

>I discovered that some parts are hard to source in the UK

The B3S-1002P switch is a SMT part but the via-in-pad footprint you
use won't reflow well. Try the EVQ11U05R which appears to be the
cheapest TH SPST-NO at RS and is compatible with the TL59AF footprint.
A 2-terminal TH switch is better than a 4-terminal since it occludes
less routing area and is quicker to solder. Overlapping the B3S-1002P
and EVQ11U05R is a good idea but using any TH switch will occlude the
bottom area to any microSD connector or other components.
http://uk.rs-online.com/web/p/push-button-switches/7561549/

The Wurth 65100516121 appears to be compatible aside from the
location of the positioning posts which you can break off. In fact,
from my experience it appears all companies have different ideas of
where the positioning posts on USB miniB connectors should be.
Consider a switch to USB-microB or full size USB-B which at least are
well defined in the USB2.0 standard.
http://uk.rs-online.com/web/p/audio-video/7480885/
http://uk.rs-online.com/web/p/audio-video/6850961/
http://uk.rs-online.com/web/p/audio-video/7025475/
http://uk.rs-online.com/web/p/audio-video/7480866/

You reuse most of my schematic so I appreciate you leaving my
copyright notice but the board layout has most components changed and
has been rerouted so it is more your work than mine. You may as well
take full credit and don't feel you need to keep the MicropendousX
name. As you mentioned, there are plenty of LPC1343 boards out there
and my focus right now is on the High Speed USB LPC18xx/LPC43xx ICs so
I don't have the wherewithal to support the LPC1343 and LPC17xx
designs. If you plan on moving forward with this sort of
breadboard'able LPC1343 design I will link to your site.

Good Luck!

On Jun 14, 5:27 pm, BobC <bobc...@...com> wrote:
> Hi all,
>
> I recently needed a 1343 board, so I got some MicropendousX-1343 boards
> made from batchpcb. I discovered that some parts are hard to source in the
> UK (mainly the USB connector), and also during construction found a few
> things difficult to solder, e.g. the SD card holder, and the buttons.
>
> So I did a minor refresh to use some different parts, I have put the
> project herehttps://github.com/bobc/bobc_hardware. For the moment, I
> removed the SD card holder. I am afraid I have lost some of the quality of
> Matt's original work, I have not had any new boards made yet. I trimmed the
> size to 50mm, so that I can get it made through Seeedstudio or Iteadstudio
> service.
>
> There is also a sample firmware project based on the Microbuilder.eu code
> base.
>
> There are a couple of other LPC1343 designs out there, notably USBug, but I
> still like the MicropendousX-1343 design.

[Casainho]

Hello Matt :-)

How are you? how are things going?

Let me tell you that at our company we go now on V2.0 -- now we got 2
new partners, more experienced, from economy. One partner are funding
the company - we made a business plan for 400K + 400K + 200K (1, 2 and
3rd year). Our main project is to make a 3D printer and online
services for it :-)

I am looking to the 20€ IMX233 board from Olimex :-) :-) -- I am
planning to buy it, using the Linux and a pen flash wifi to add wifi
to our board. Also the IMX233 may have some other heavy tasks...

[BobC]

Hi Matt,

Thanks for your detailed notes! I will be sure to check them carefully, there are so many considerations that I am not even aware of.

My main goal was to get the simplest possible ARM "breakout", with the minimum added cost. For simple applications the board could be used as is, I figure for anything more complicated I would create a new board anyway with whatever peripherals are required.

I have been using seeedstudio which are very cheap for small Q's but have an arbitrary cost break at 5cm by 5cm, so I want to keep the length 5cm. I also need to source components from RS/Farnell, which have a smaller range than the likes of Digikey.

At work we have used this chip http://uk.rs-online.com/web/p/emi-filter/0250640/ for USB suppression, it reduces component count and is not too hard to solder by hand, I was thinking of putting it in the next iteration.

Freeroute works ok, but needs a little help. Often moving a component slightly will cause it to fail, overall though I find it saves me effort.

Cheers

[Opendous Support]

>My main goal was to get the simplest possible ARM "breakout",

>with the minimum added cost ... need to source from RS/Farnell

Then consider USB-B or USB-microB connectors as it is easier to find
cheap footprint-compatible substitutes to distributor-stocked parts.
USB-miniB is sturdier than microB but harder to find direct
replacements. USB-microB is set to be the standard for charging
adapters so using it as a power supply will be easy. Solar and other
USB-microB chargers will allow for a variety of power supply options.

If USB isn't critical then have you heard of the LPC1114FN28? It is
a DIP part which solves the breakout issue. Supposedly it will be
available later this year.
http://www.eciaauthorized.com/search?pn=LPC1114FN28

>ESD

The USBUF01W6 is a great choice if you don't mind the fine pitch. I
have previously researched similar USB ESD+Filter ICs and as far as I
can tell they are compliant to USB2.0 Full Speed if compliant to
USB1.1 Full Speed. I use discrete ESD zeners by default since they
are compatible with High Speed USB and are cheaper.

Take a look at the USB 2.0 Compliance Checklist for Peripherals, Pg.
4 outlines the routing requirements. The differential impedance
requirement isn't practical on standard 2-layer FR4 and isn't critical
if the mismatch is very short. However, the capacitance is very
important or else you can end up filtering out the signal. Test your
board using a USB2.0 5m cable to see how reliable your design is.
http://www.usb.org/developers/compliance/check_list/peripheral_checklist.pdf
http://www.usb.org/developers/compliance/check_list/

>cost break at 5cm by 5cm

If you don't break out the GPIO-only pins it should fit the 5cm
limit. I understand what you are getting at. Having USB on the board
prevents problems. I fried an LPCxpresso trying to add USB to it.

On Jun 16, 6:05 am, BobC <bobcousin...@googlemail.com> wrote:
> Hi Matt,
>
> Thanks for your detailed notes! I will be sure to check them carefully,
> there are so many considerations that I am not even aware of.
>
> My main goal was to get the simplest possible ARM "breakout", with the
> minimum added cost. For simple applications the board could be used as is,
> I figure for anything more complicated I would create a new board anyway
> with whatever peripherals are required.
>
> I have been using seeedstudio which are very cheap for small Q's but have
> an arbitrary cost break at 5cm by 5cm, so I want to keep the length 5cm. I
> also need to source components from RS/Farnell, which have a smaller range
> than the likes of Digikey.
>

> At work we have used this chiphttp://uk.rs-online.com/web/p/emi-filter/0250640/for USB suppression, it