Wrapping up the Timed LED Lighting Controller Project


I have written about the Timed LED Lighting Controller in previous posts. Starting with the original entry “Stairwell Foot Lighting System. In this entry I will be wrapping up the project and describing the change of direction from the initial design and layout. There may be a bit of overlap but it will be minimal as the project took a small deviation along the way.

Continue reading Wrapping up the Timed LED Lighting Controller Project


A Look into Integrated Light Sources

For a while now I have been intrigued with Integrated Light Sources i.e. NeoPixels. I knew nothing about them and with the coming of Christmas, I was inspired to take a closer look. I knew I would not have anything in place before Christmas 2017. But there is always next year.

Continue reading A Look into Integrated Light Sources

An Encounter with XBee

It has always been on my list to try a project with some wireless communication. I now have a project in mind but there are a few things to sort out first. I have not worked with any wireless at the embedded hardware level. This is not inteded to be any instructional post but my usual style of describing how I have approached this topic, what I encountered and how I worked around any issues I discovered. Maybe this might be of some help to others like me, starting at zero. Continue reading An Encounter with XBee

From Proof of Concept to Prototype

In the last entry for the Timed LED Lighting Controller, I realised that there are no working examples of an I²C driver for the ATtiny20. I then had to work through the data sheet to implement my own. With that done, I could then start on the application firmware and get the board really working. So this is where my proof of concept becomes the prototype.

Continue reading From Proof of Concept to Prototype

“Mocking” – Minimising Risk

In the last post  for the Timed LED Lighting Controller, I had figured out the circuit and a basic layout and approach that I was happy with. That is to separate the hazardous voltage from the control circuitry by putting it on a separate board. But still, this was not enough. I need to assemble this in a case. No hazardous voltage is allowed to be exposed. The idea of printing a case is attractive but I don’t really want to loose focus of this project. I can always reserve the printed case for revision 2.

Reviewing Samples

I found myself feeling like I as facing a bit of a chicken and egg. Needing a housing to fit the board and having to make the board fit the housing. I also needed sort out a set of terminal blocks and ensure that they are in specification. The only way forward was simply have a look around and order some terminal blocks and cases and just to see what is out there. Photos and technical diagrams are great but to have the actual items in hand is much better. I decided to use Reichelt this time. I had not used them before but they had a good range of terminal blocks of various dimensions and configurations and I could purchase single units which was important for a look-and-see. I settled to take a look at a small selection

Manufacturer Pole Spacing Voltage / Current
Springcon 6 2.5mm 150V / 8A
Springcon 2 2.5mm 150V / 8A
Metz Connect vertical 2 5mm 300V/ 10A
Metz Connect angled 2 5mm 300V/ 10A

The smaller units are not suitable for the hazardous voltages but I will still use them for the connections to the motion detectors (PIR13).

img_0352sWithout wasting too much time, I ordered two housings manufactured by Bopla. When they arrived, it was clear that I could use the smaller of the two (BOPLA KS 430) that I had ordered. There are undoubtedly other housing that would suite but this will do for the moment. I will, of course, have to modify the casing to expose the terminal blocks.

Now that the decision was made for the terminals and housing, I could look back at the layout with more confidence. This also meant a bit of a rehash. I had to add the footprints for the terminal blocks and their outlines to make sure they will fit on the board.

Revisiting the Layout

The next was the housing. This was a little more involved since I am going to stack the boards. I ended up making use of the dimensioning tool in KiCad so I could correctly line up the joining pin-header and the mounting holes.The outcome of this was that I needed to extend the respective boards so that they could get past the “assembly posts” for the housing and also that the terminal blocks will reach the ends of the housing.


The larger board has given me space to reorganise a few things. I have now collected all indicator LEDs into a single bank of LEDs. This will look a lot neater when they are exposed to the housing surface compared to LEDs that are placed simply where it is convenient on the PCB. The LEDs are to help with bringing the board up and there is nothing to say they need to be populated for the final version.

Going back on the question of Clearance and Creepage, the dimensioning tool as was also useful to verify the distance between the traces where they look a bit close. At the moment, according the the on-line calculators (Creepage.com and ANSI PCB Trace Width Calculator) I have checked, seems to be in specification – further verification is required.

Mocking the Board

On the screen, it was all looking good, but I was still not confident I had covered all the possible issues. It was then I decided to “mock” the board. Simply print it out and paste the images to some card board and cut them out. I could then use a real pin-header to assemble the two parts to see how they would fit.

Of course, I could not stop there. I had to then also punch through the other through-holes and set the terminal blocks that I now had in my possession. At first this was just for a bit of fun, but as it turns out, I discovered some issues with the layout that would have normally gone unnoticed.


The first issue was that I did not realise the mounting holes for the board at each end are spaced differently. From the perspective of the photo above, the mounting holes on the left are set narrower than the mounting holes on the right.

The second issue was that I had not calculated the “Y” location of the mounting holes correctly and they were 1.7mm out.That was easily sorted out since it did not affect any other parts on the board.

measuredboard-terminalspacingThe third issue was with the terminal blocks for the motion detectors.I was trying to get away with the terminal blocks I had received. I need provision for 12 wires. Three for the I²C Bus and nine for the connections to the motion detectors.I was thinking I could butt two six-pole terminal blocks together. However with the way they are modelled in KiCad and the respective footprints, this was not possible as these terminal blocks have a nominal 2.5mm spacing and a 3mm spacing when butted together. So solve the issue,  I went back to KiCad and remodelled the connections to the motion controllers as three sets of three. In the layout I only needed ensure that there is a minimum 3mm spacing between the three-pole terminal blocks.

The Timed LED Lighting Controller is another step forward. This will be one of the more expensive boards I will send off for fabrication so I am very pleased to have spotted those issues with the layout. The goal is to have as few “spins” of the board as possible and the process of mocking the board was a huge help. Just a few more checks and I can send this off to OSH Park!


Timed LED Lighting Control – Design

From Logical to Physical

Before I could start to translate the block diagram into KiCad, I needed to be sure about some of the parts I will be using. I want to reuse what I already have installed, so the motion detection module is already a given, along with the LED drivers. The micro controller needs three output pins, three input pins, I2C support as well as the pins for a program header. Since I have worked with Atmel in the clock project and therefore have the tool set I need, I decided for the ATTiny20. The only part I needed to look around for was the relays. As per the block diagram, I decided that the coil would be 12V and the switching contact should be for 240V AC RMS. For the moment I have settled on the JW1AFSN12F from Panasonic.

Translating the block diagrams to KiCad was fairly straight forward. The resulting KiCad diagram pretty much matches the block diagram in so much as the power system, relay driver and the PIR13 interface are modelled in their own sheet. In order to help to keep the 240VAC side separated from the Extra Low Voltage control section as much as possible, I opted to try for a stacked board layout. The two boards will be connected via a pin header and socket (P105 and P107). To simplify this layout I opted to utilise the different notations for the Ground plains. GND for the Extra Low Voltage board and GNDA for the Low Voltage Board.


tl2c-sheet2-powersystemThe Power System comprises of two LDO regulators. One for 12Volt and the other for the 3.3Volt supply. It is expected that the plug pack adapter will probably deliver about 14V – if not, I can always drop the 12V regulator out of the design. It is only provided for extra regulation. As already indicated in the previous post, the 12Volt supply is for the PIR13 modules and relays. The PIR13 modules can handle from 5 to 24Volts as a supply. Because of the distance of the cabling, any voltage drop should be within tolerance. The Micro Controller and therefore the signal lines such as for the I²C bus will be at 3V3 which is compatible with the Raspberry Pi removing the need for any level shifting. The ATTiny20 shares the pins for the I²C bus and SPI bus. At the moment, I have separated these with a couple of resistors as recommended in another article. I have my reservations about this and may yet change this over to a set of jumpers or even a double pole switch.


The signal from the PIR13 is open collector. To avoid having a direct connection between the ATTiny20 and the PIR13 modules, I will be installing some MOSFETs I already have from another project.


I am using the same MOSFETs to drive the relays. As a part of this initial design and a lesson learned in previous projects and Contextual Electronics, I will be including test points and indicator LEDs. An additional lesson learned is to not leave any spare GPIO pins unconnected. These can come in handy and for that reason I have even broken them out onto a pin header. I don’t have to populated the pull-down resistors nor the pin headers for these. But they are provided for if I need it.

Laying it out

I originally envisage the layout as a two piece board that will be separated after assembly. The first attempt was a two layer board and was not nice at all, so I shifted the design to a four layer board. This has pushed the price up enormously. The tip came from Chris Gammell to separate the two sections into their own layouts. One as a two layer board (the 240Volt AC section) and the other as four layer. This has reduced the overall cost significantly and now enables to be enlarge them enough for mounting holes and still be cheaper than the original full layout. The trick with this is how to model this in KiCad. I have tried out my own workflow for this:

  • Model the two boards as needed in the Master Layout PCB as 4-layer. This enables matching the mounting holes and pin-headers without having to swap between layouts
  • At the command prompt, copy the Master Layout PCB twice. Once for the 240V board and the other for the Extra Low Voltage (ELV) board.
  • In each new layout file, delete the section that is not needed and re-adjust, if needed the board layout graphics.
    • Adjust the layers for the 240V board from 4-layers to 2-layers.
“Master Layout” Both boards side by side

Design considerations and constraints

I am reasonable happy with this initial cut of the layout. However, I am not quite ready to send this off to OSH Park. This project and board contains an element I have not worked with before – Hazardous Voltage. This can not be under estimated. One aspect to this is to separate the Low Voltage (LV to ELV boards onto their own. There is still the question of Clearance and Creepage to consider on the LV board. There are a number of very good essays written some with calculators

Trace Width
PCB Trace Spacing
Creepage and Clearance
Clearance and Creepage Rules for PCB Assembly

So I have a bit of a quandary. I don’t want to send off the board for manufacturing before I have sorted out the safety aspects of the design first. I could send it off as-is but if there is a specific requirement I need to meet, I will have to request another. I can, however, make a compromise. With the tip for splitting out the boards as separate PCB files, I can send off the order for the four layer part and leave the two layer, LV board for further consideration. In the mean time, I can bring up and test the control board since the relays either are not needed for the proof of concept or can be simply wired in for basic testing.

At the moment, I have a small uncertainty about the housing and the terminal blocks. It is much easier for me to choose or to know what to look for when I have some actual samples in my hand. So I have ordered a couple of samples to get a better idea of these parts. It is tempting to consider to print the case. However, this would push out the project and shift the focus to a 3d Printing project. I would prefer to keep on track with the Timed LED Lighting Control hardware and firmware.

In the next post, I hope to have the casing and terminal blocks worked out which means that the board will be ready for fabrication. So hopefully then I will be able to talk about bringing the board up.