Jump to content
Sign in to follow this  
spirilis

FTDI FT230X USB-Serial BoosterPack

Recommended Posts

Here's a boosterpack breaking out the FTDI FT230X, a simple USB-UART adapter chip (similar to the FT232RL but with less crap, also less cost). Should allow custom UART speeds and good driver support to have your MSP430 talk to any computer.

 

Compatible with 20-pin or 40-pin XL LaunchPads, for 20-pin LP's just ignore the 21-30/31-40 headers. Uses a Mini-B USB port. Includes 250mA Voltage Regulator for powering the project completely off this board's USB connection.

 

The RTS, CTS, CBUS0-3 lines are all broken out to a header and breakout pads are there for all 40 pins of an XL-size LaunchPad.

 

Breakout pads for RX, TX are there plus jumpers to connect/disconnect the UART lines--plus these can be installed transverse like the v1.5 launchpad, enabling Software UART pinout like the pre-1.5 launchpad chips instead.

 

TX, RX LEDs attached to CBUS1 & 2 by default.

 

All references to "TX" and "RX" are from the standpoint of the MCU, not the FTDI chip FYI. So the "TX" pad goes to the RXD pin on the FT230X, the "RX" pad goes to the TXD pin. Likewise CBUS2 defaults to TXLED# but it routes to the "RX" LED, vice versa for TX.

 

Datasheet for the FT230X: http://www.ftdichip....s/DS_FT230X.pdf

 

Bill of Materials:

USB port - Wurth 651005136521 Mouser link

R1, R2 - 1K 0603 SMD resistors

R3, R4 - 22R 0603 SMD resistors

TX, RX LED - 0603 SMD LEDs

C3, C4, C5, C6 - 0603 0.1uF SMD ceramic capacitors

C1 - 1206 4.7uF SMD ceramic capacitor

C2 - 1206 10uF SMD ceramic capacitor

C7, C8 - 47pF 0603 SMD ceramic capacitors

RG1 - TI LDO voltage regulator, TPS77301

U3 - FTDI FT230XS (SSOP-16)

F1 - nanoSMD fuse, PTC resettable 0.5A 13.2V - Mouser link

 

First, pics (OSHpark mockup):

Top-

post-15991-0-98374800-1354027261_thumb.png

Bottom-

post-15991-0-36072200-1354027269_thumb.png

 

Second, schematic:

DipTrace Schematic - FTDI_FT230X_BoosterPak_draft2.pdf

 

And last but not least, gerbers:

OSHpark gerbers: OSH_FT230X_BPak.zip

Seeed/ITeadStudio gerbers: Seeed_FT230X_BPak_5x5.zip

 

 

This is a 5cmx5cm board (49x49mm) FYI.

 

I am going to have a short run of these made, probably as an order-stuffer with my next Seeed order, then assemble them for the 43oh store.

Share this post


Link to post
Share on other sites

Guess that FT232RL bpak I made will be good for something then.

 

---

Well then again mouser lists early Jan for first deliveries so it'll take almost as long to get PCBs anyhow. I'm planning to make a Seeed order Dec 1 or so.

 

Rob- Do you already have a bpak in the works for this?

 

Sent from my C3PO via Tapatalk

Share this post


Link to post
Share on other sites

Ah k, gotcha... Well this will be a low-priority project for me, probably take until mid-late January to get them built if the parts are hard to come by. Mainly hurried to get the board ready for the Seeed order I'm doing.

Share this post


Link to post
Share on other sites

Hey look at that, apparently I missed the requirement for the series resistors on the USB DM/DP lines too... Updated gerbers/schematic/pics coming. I don't think I'm going to bother with the 47pF caps they mention though. (As someone on the parallax thread mentions, USB cable's capacitance eclipses that easily).

 

I may change the 5V VBUS big cap from 10uF to 4.7uF too since I've read USB inrush current should be limited...

 

edit: Although, I could probably guess why the 47pF's are there, probably for impedance matching (reducing reflections on the main USB line before the signals hit those resistors)... So I'll put them in.

Share this post


Link to post
Share on other sites

Original post updated, flipped the position of LDO_EN/LDO_RST jumpers, added two 22R resistors (I don't have any 27's in my stash but I'd read that 22R is typically used with USB) and two 47pF ceramic caps on the USB port-side of the lines.

Share this post


Link to post
Share on other sites

With this board as well.  There's lots of room to put all the components on a single side.  Unless there's a reason I don't see here, populating just one side makes it easier to produce these and debug them if anything goes wrong.

 

Your decoupling capacitors should be as close to the pin on the chip as is reasonable.  I'm having trouble tracing your power path as well, but it looks like C3, which I assume is a decoupling cap for the FTDI chip is on the other side of the chip from the power via.

Share this post


Link to post
Share on other sites

Hmm well, using both sides has just been my approach... I guess moving from single-sided DIY boards to double-sided fab-built has me spoiled and looking to use the 2nd side as much as possible.  I personally don't mind populating both sides by hand, it doesn't bother me one bit, but I know single-sided components is necessary for mass production (pick & place + reflow soldering).

 

Will keep that in mind for the next design.

Share this post


Link to post
Share on other sites

They're already produced and shipped (waiting on their arrival).  Shame too, that was pure laziness on my part... Don't know what I was thinking!  I found some more mistakes on my F5172 LP board, and while the FT232RL redo is already in production I am making changes to the FT230X-based F5172 board to clean up some of these mistakes.  (Still keeping that one with 2-sided components though)

Share this post


Link to post
Share on other sites

Alright so I'm going to scrap the boards I have, as they use the hideously expensive PTH USB connector, there are obvious decoupling cap layout issues, and I think there's some cash to be saved on the LDO too. (Seems like it's easier to cut my losses on the boards IMO)  I also have a ton of cheap SMD USB mini-B connectors now...

 

But I redesigned it, and I like this a lot better-

Top:

post-15991-0-08116800-1357923267_thumb.png

Bottom:

post-15991-0-67664300-1357923273_thumb.png

 

OSHpark gerbers: OSH_FT230X_BPak.zip

Seeed/ITead gerbers: Seeed_FT230X_BPak_5x5.zip

Schematic: DipTrace Schematic - FTDI_FT230X_BoosterPak_draft3.pdf

 

Using the TI TPS78233, which is around $0.50/pc instead of $1+ like the TPS77333, only catch is it outputs 150mA instead of 250mA and doesn't have a RST output to hold the MCU suspended.  Plus the bottom has been chopped a bit so it doesn't cover the buttons as much.  Sounds like SugarAddict has a board in the works though, so I'll hold off on these unless folks are interested.

Share this post


Link to post
Share on other sites

Hi all,

 

Those are some pretty awesome boards! I'm interested in how oPossum made the usb stick plugin part? I'd like to do the same with a FTDI but with a SMD MSP430G2553 attached to it, so I can use an app running on the computer (like Noduino) to individually control  the leds.  Is there a schematic anywhere for the usb stick version that would be ok to share? I'll happily contribute mine back of course :-)

 

Richard

Share this post


Link to post
Share on other sites

http://www.compendiumarcana.com/forumpics/ftdi_43oh_r1.zip

 

The USB connector is drawn to the official spec. A plastic shim is required with common 1.6 mm boards for proper fit and insulation of the mini-b pads.

 

The shim stock I use is 0.015" for glue or 0.0125" for adhesive tape. McMaster Carr 9513K22 & 9513K21.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

Sign in to follow this  

×