Month: February 2016

In the summer of 2013, I decided that I needed to design a printed circuit board.  I had worked on sections of chips but no PCBs.  I didnt really know which tool to use, but after looking around a bit it seemed like Eagle was a good simple choice as it had wide adoption in the Maker community.  At that point in time the Elkhorn Creek Measuring System was being run off a Raspberry PI and a PSoC5LP but Cypress had just released a new family of chips called the PSoC4200.  I thought that it would be a cool idea to have a PSoC to Raspberry PI bridge board.  So this is what I did.

On the bottom of the board I wanted female pins that matched the Raspberry PI, and on the top I wanted an Arduino pins.  Bottom line, I decided to build a board that was very similar to the CY8CKIT-042 except for having Raspberry PI GPIOs on the bottom of the board.

My board has:

• Power System: Both 3.3v and 5.0v for the PSoC as well as 5.0v@1.0A for the Raspberry PI.
• Reset System: A RPi connection to the PSoC and Arduino XRES.
• An I2C connection between the RPi and the PSoC including the pullup resistors
• A 3-Color LED
• Arduino pins that match the pinout of the CY8CKIT-042

The overall schematic

I used the same RGB 3 Color LED (CLV1A-FKB- CJ1M1F1BB7R4S3) as exists on the CY8CKIT-042.

I wanted to be able to reset PSoC and Arduino from the Raspberry Pi so I attached the RPi GPIO 1_11 to a pulldown transistor that is connected to the XRES of the Arduino and PSoC.  I also attached a small pushbutton to enable a user reset.

I copied the Arduino pin out of the CY8CKIT-042.  This would allow me to easily use all of the projects that I had already developed that that development kit.

This section of the schematic has the required power supply decoupling capacitors.  It also has the ARM standard 10 Pin programming header which allows me to program the PSoC using a MiniProg-3.

I provided pull up resistors on the PSoC P4[0] and P4[1] to easily enable the PSoC to serve as an I2C Master for the Arduino shield.

The connection to get data between the RPi and the PSoC is I2C.  The PSoC is setup as an I2C slave and the RPi is the master.  The connection on the RPi uses the RPI1_3 and RPI1_4 GPIOs.  On the PSoC it is connected to P3[0] and P3[1].

The power supply turned out to be by far the most difficult part of the project.  In the first version of the board I chose a regulator that was to small to supply the Raspberry PI.  When the RPi was plugged in, the regulator immediately went into thermal shutdown.  In general this sucked as the PSoC Applications Manager warned me to pick a big enough regulator.  Oh well.  In the final version of the board I used a 7805 to supply the RPi, this regulator has a giant tab which allows you to sink heat into the ground plane of the board.  On the board I also provide a 5.0V supply and a 3.3V supply for the PSoC using a 1117 regulator.

Here is a picture of the final layout

And here is a picture of the first version of the board.

On thing that you might notice on this board is that the vias are exposed.  What I didnt know is that you need to tell Eagle to “tent” the vias so that they are covered with solder mask.

There is a lot going on in the layout and it is probably easiest to review the layout using eagle.  You can get the design from github at https://github.com/iotexpert/cypi

At my company Cypress, “RCCA” is an abbreviation for “Root Cause Corrective Action”.  It is a formal process for changing the way that you work to prevent an error from happening again.

Unfortunately the title of this post is “Creek Board 1.0 – RCCA”.  What that means is that the first time I sent the Creek Board to be manufactured I made an error, in fact a really stupid error.  Specifically,  the error that I made was a fundamental failure of not having an LVS (Layout versus Schematic) clean design.  If you google “blue wire pcb” the first search result you will find is “Printed Circuit Board Repair and Rework Guides”,  I had no idea why blue wires were used to fix printed circuit boards so I called my friend Dave Van Ness.  He is an old grey beard type of guy.  He told me that the blue wire was traditionally an “official fix” to a circuit board.  It was used because other colors were already assigned (Red to power, Black to ground) etc.  I guess that I thumbed my nose at tradition by fixing my PCB with a red wire.

After laying out a printed circuit board, the last step is to surround the board with a ground plane on the top and bottom of the board.  Then you press the “ratsnest” button on Eagle.  Then Eagle does a “pour” which fills in the empty space of the board with a ground plane.  It then will update the bottom of the screen with the message “Ratsnet: Nothing to do!” which means all of the schematic and layout connections are complete.  Or, if there are connections that still need to be made, it will update the layout with yellow “air wires” and it will give you a message like “Ratsnest: 1 airwires.”  If you send the board to be made with an airwire, that is exactly what you will get.  I will tell you that air doesn’t conduct electricity very well and you will end up needing your soldering iron.

In this case I missed seeing the tiny little airwire.  See if you can see it:

It is hard to see, eh?  In the next picture I turned off the ground layer and zoomed in so you can see that I am missing a power connection between the top and the bottom of the board.  I highlighted this issue by clicking on the “Show Objects” at the top of the toolbar, then clicking on yellow wire.  When I do that, Eagle tells me what the net is that is unconnected and it highlights every object that is attached to that net.

So now what?

What I ended up doing is the normal Cypress thing.  I created a “tapeout checklist”.  The checklist contains a list of all of the things that I double check before I send a PCB to be manufactured.  Here is my current (and short) checklist:

• No remaining airwires
• Vias tented (or not)
• Silkscreen on all connections
• Test points on key nets
• No DRC errors

In the previous post I described the entire system architecture.  In this post, I am going to describe the Arduino shield that I unfortunately call “Elkhorn Creek Water Level 1.1”.  It is unfortunate because in version 1.0 I made a really stupid error which ruined the first run of printed circuit boards.  You can read more about how I made the error and what I am doing in the future in the post Creek Board 1.0 RCCA.

To make this system work I need to be able to interface the PSoC4200 with two sensors:

• The US381-000005-015PG pressure sensor
• A TMP036 temperature sensor

Both of these sensors are subject to environmental noise so they both have capacitive or RC filters connected to them.  I originally built a prototype of this board using a proto board.  However, it was a PITA because the wires would come loose and the system would stop working.

So I decided to make a real PCB.  To do the design, I used the Eagle 7.2 PCB editor as it seemed like it had the most support from the maker community.  The schematic for the system is fairly simple.  It has

• Pressure Sensor
  • X1: A Molex Microfit 3.0 Connector to attach the two wires from the pressure sensor
  • R1: A 51.1 Ohm resistor to group to convert the 4-20mA –>  0.204mV to 1.022V
  • C1/R2: A low pass filter
  • TVS1: A ESD diode to clamp any ESD event to ground to prevent it from blowing up the PSoC4A or the Sensor
• Temperature Sensor
  • TMP36: A sensor that turns temperature into a voltage.  The equation for temperature is T=0.5V+10mV/degreeC.  For 25 degrees C the Voltage = 750mV
  • C2 + C3: Two decoupling capacitors to filter power supply noise
• Arduino Interface
  • A standard Arduino interface set of pins + the additional Cypress CY8CKIT-042 pins.  I only used the A0 and A1 pins for signals and the Vin pin (which is 12v) to drive the current loop
• Measurement Test Points
  • Keystone 5000 test points.  These test points are a little loop of wire that sticks up from the surface of the PCB to make  it easy to probe a voltage with your DMM.  

Here is the final Eagle Schematic for the board.

And the layout:

Once I completed the layout I sent the board to OSH Park to be manufactured.  I have shared the project on their website.  OSH Park is an excellent company that is easy to do business with.  They charged me $22.55 for three of the boards.  The fit and finish of the boards is very nice.  Here is the board:

Here is the assembled board:

 

I have posted all of the project files at github.  You can “git” them from https://github.com/iotexpert/TheCreek  The Eagle project is in the CreekBoard directory.