New Gyro’Clock boards!

Here are the new Gyro’clock boards! They arrived a couple of weeks ago but I haven’t had time to write about it until now. They look fantastic! I can’t wait to put parts on to them and see how they work.

Gyro'clock boards fabricated by OSH Park.

Gyro’clock boards fabricated by OSH Park.

The boards are 6cm X 3cm

The boards are 6cm X 3cm and have two copper layers.

I am very happy to have found OSH Park, a community PCB manufacturing service that makes this possible. So hobbyists like me don’t have to spend a fortune to get a professionally made PCB.

The next step is building a reflow oven, so I can assemble the components on to these boards. While waiting for these boards to arrive, I had begun construction of the reflow oven. I will put up a series of posts about how it is made next. Stay tuned!

Manufacturing PCB layouts made in KiCad

Up to this point I have made all my printed circuit boards at home, which is great fun and comes with a great sense of satisfaction when your circuit finally works. But it also takes a lot of time, expensive, and you have to deal with messy corrosive chemicals. But if you really like to print your circuit layout at home, check out how I did it here.

But now I am ready to outsource the manufacturing of my PCB layouts. One of my colleagues told me about this awesome community PCB manufacturing site called OSH Park, where you can get your layout printed at a very reasonable price. And they don’t require you to order a massive number of boards.

I finally finished laying out the component footprints and traces for my new and improved Gyro’clock circuit. Before doing this I ordered all the parts so that I can check them for reference while I am creating some of the custom footprints, and also I don’t run the risk of using obsolete parts after I have manufactured the boards. Here is what my finished design (all layers) looks like in KiCad

New and improved Gyro'clock layout in KiCad

New and improved Gyro’clock layout in KiCad

The 2-layer board is 6.2 cm by 2.9 cm. Not the ideal size I wanted, but I like how everything fits nicely. I chose the following design rules before doing the layout as per specifications on the OSH Park website:

  • minimum trace width: 0.1524 mm (6 mil)
  • minimum via diameter: 0.6858 mm (27 mil)

My default net class values used for all the connections are the following:

  • trace width: 0.2032 mm (8 mil)
  • trace clearance: 0.2540 mm (10 mil)
  • via diameter: 0.6858 mm (27 mil)
  • via drill: 0.3302 mm (13 mil)

I placed all the component on the top plane and made the bottom side into a ground plane, but had to route some traces through the ground plane. Altogether there are 41 vias on the board. A high number of vias, but most of them are ground connections.

In my 2-layer board there are seven layers that are important for getting the board manufactured:

  • top copper layer – contains component pads and traces on the top layer
  • top solder mask – contains regions in the top layer that will be exposed for soldering components
  • top silk screen – contains component references and texts on the top layer
  • bottom copper layer – contains component pads and traces on the bottom layer
  • bottom solder mask – contains regions in the bottom layer that will be exposed for soldering components
  • bottom silk screen – contains component references and texts on the bottom layer
  • PCB edges layer – contains the outline of the PCB board

To manufacture the PCB, OSH Park requires Gerber files for all the layers above plus a drill file. The following steps will explain how to create Gerber files in KiCad for OSH Park. I got these information from this blog, but changed a few options to suit my design.

Step 1: Verify DRC (Design Rules Check) with OSH Park specifications.

  • select DRC from the Tools menu or click the ladybug icon in the top bar. Fix any errors in the DRC before proceeding to next step

Step 2: Open the plot dialog box by selecting plot in the File menu or by clicking the printer with a P icon

Step 3: Select the following options in the plot dialog box

Plot dialog box options in KiCad

Plot dialog box options in KiCad

I used the ‘Subtract soldermask from silkscreen’ option to remove the silkscreen from areas where the holes in the solder mask will be. However, even if you didn’t do that OSH Park and most PCB manufacturers will remove the overlapping areas of the silkscreen. But it is better to check for yourself which parts of the silkscreen will be removed.

Step 4: Click the Plot button in the plot dialog box to generate the Gerber files.

Step 5: To open the drill file option box click Generate Drill File from the plot dialog box

Step 6: Select the following drill file options

Generate Drill File dialog box and options in KiCad

Generate Drill File dialog box and options in KiCad

Here, OSH Park requires you to ‘Keep zeros’, use ‘2:4 precision’ and use a ‘Minimal header’.

Step 7: After selecting the correct options in Step 6, click the OK button to generate the drill file which will be in Excellon format.

Step 8: Finally examine each Gerber file and the drill file for errors using the GerbView tool in KiCad.

Here are what my top and bottom side Gerber files look like in GerbView:

Top side copper, solder mask, and silkscreen Gerbers

Top side copper (green), solder mask (blue), silkscreen (white) Gerbers and the drills (purple)

The bottom side copper (green), solder mask (blue) and silkscreen (white) Gerbers

That’s it! I have submitted my board for fabrication to OSH Park, and it cost me $14.35 for three copies. I will add another post when the boards arrive. Meanwhile I have started work on my other spin-off project, which is to create a reflow oven to assemble the surface mount components into the Gyro’clock boards.

Fixing Keypad door entry – The solution

In my last post I talked about a problem I am having with an electronic keypad door entry unit. I have narrowed down the problem to the keypad interface, which is either worn out or in some other way not doing its job. The conductive traces in the keypad interface is laminated, making it very difficult to fix any broken traces.

So I decided to create my own keypad for this unit with a solid PCB and real push buttons. In making this PCB, the biggest challenge I am facing is reducing the overall height of the keypad so that it will neatly fit inside the original housing. To achieve a thickness close to the thickness of the original keypad I have made two design choices,

  1. Use surface mount push buttons instead of through hole push buttons.
  2. Remove the spacers from the original keypad membrane, which will go on top of the new PCB.

Instead of buying surface mount push buttons I decided to modify a bunch of through hole push buttons I already had. Converting the push buttons from through hole to surface mount was easy with a needle nose plier and a wire cutter. Afterwards, I took measurements of a transformed push button and made a footprint for it in KiCad.

Push buttons transformed from through hole to surface mount

Push buttons transformed from through hole to surface mount

The surface mount push buttons have a thickness of 3 mm, which is 1 mm shorter than the thickness of the buttons on the original keypad membrane. This means the push buttons should be able to fit inside the membrane buttons. However, I will have to carve out the insides of the membrane buttons to get the push buttons inside.

Spacers of the original keypad membrane, which will be removed in the new keypad to make room for the PCB

The membrane has spacers around it to fit the original keypad tightly inside the housing. With the spacers, the thickness of the original keypad (without the buttons) is 4 mm. With the spacers removed, the thickness of the PCB (without the buttons) with the membrane placed on top is 3 mm. This means that the new keypad should fit easily inside the housing.

Having figured out all the details I set out to make the PCB. First I made a simple schematic for the button connections in KiCad, followed by the layout. Since I will be using surface mount push buttons, I kept the components and traces all on the top layer.

Layout of the new keypad

Layout of the new keypad

The layout is very similar to the layout of the laminated traces of the original keypad, except I avoided a via since I didn’t want to go into a second layer. Three hours of work developing, etching, drilling and trimming later I had the PCB ready for soldering.

The new keypad PCB is ready to solder

The new keypad PCB is ready for soldering

Although I have had a bit of practice soldering  surface mount components before, this is my first time trying it on one of my own PCBs. I have stayed away from surface mount components before mostly because I didn’t have a soldering iron designed for surface mount devices. Also I didn’t have flux, which is the secret sauce to soldering SMT components properly.

I still don’t have these equipment, but decided to give it a go anyway since I didn’t really have a choice but to use surface mount push buttons. One of the biggest difficulties with soldering SMT components is holding it in place while trying to solder since you only have two hands to hold the soldering iron, solder and the component! Yes, I did consider melting the solder on the iron first and then bringing it to the component pad, but in the time it takes to do that, the flux inside the solder smokes away making it very difficult to make a good connection.

Thankfully, I had bought this PCB holder with alligator clips and it did a really good job of holding the push buttons in place while I soldered.

The alligator clip holding the push button in place while soldering

The alligator clip holding the push button in place while soldering

As it turned out soldering the surface mount push buttons wasn’t too bad. I found this more satisfying than soldering through hole. The solder did spread a little bit along the track since I don’t have a solder mask on my home made PCB.

The push buttons neatly fit inside the housing where the holes for the buttons are located

The push buttons fit inside the housing where the holes for the buttons are located

The next step is to solder a connector from the keypad PCB to the control PCB, where the processor is located. For the connecting wire I chose an old ribbon wire I found in my  collection of scrap wire, which had six wires – exactly what I needed! I soldered a female header to one end and soldered the other end to the keypad PCB.

Ribbon wire that connects the keypad PCB to the header of the main control PCB

Ribbon wire that connects the keypad PCB to the header of the main control PCB

After soldering all the components it was time to test the device. As expected it worked without any issues and with that satisfying feel of a real button press.

The final step is to put everything back inside the housing. In order to fit the membrane of the original keypad on top of the new keypad push buttons the insides of the membrane buttons need to be carved out. However, this task turned out to be rather difficult since the membrane buttons are strechy and didn’t flake off very easily.

After a few unsuccessful attempts, I managed to poke through one of the buttons with an X-Acto knife, partly removing it from the membrane. And then I had the idea to remove the membrane buttons from the membrane and then glue it on top of the push buttons. Removing the membrane buttons from the membrane was easy since the buttons were connected to the rest of the membrane with a very thin layer.

So I placed the new keypad PCB inside the housing using the rest of the membrane (without the buttons) and white electrical tape to insulate the traces from the metal housing.

The new keypad for the door entry unit installed

The new keypad for the door entry unit installed

My attempts to attach the membrane buttons on top of the push buttons were fruitless. I tried several different types of super glue and even double tape, but nothing would make the membrane stick to anything! May be it needs some special type of glue to make it stick, but at this point it is not worth it to try and find it.

After all the new keypad works better than the original, which is the main problem I set out to fix. Sure the buttons aren’t labeled, but that will make it that much harder for burglars to try to figure out the correct password.

How reliable is this new keypad? Only time will tell. But for now, it is fixed!

 

Music and Lights – the PCB!

After that fun-but-this-is-too-much-work making of the PCB, and over 200 solder joints later, I am finally done with the construction phase of the Music and Lights system.

Music and Lights PCB assembled.

Music and Lights PCB assembled.

One difficulty I had with soldering components on to this board is that certain components like the screw terminals and the audio connector could not be made flush with the PCB surface. This is because in order to solder the pins I had to reach in between the component and the board surface with the soldering iron. So when you look at the board from certain angles you can see the gaps, and it doesn’t look that neat. Next time I will make sure to put the traces for these components on the bottom side so they can be easily soldered.

I put all of the components on the top side of the PCB except for the LM1875 audio amplifiers, which were placed on the bottom side, so that I can heat sink them directly to the ground plane and avoid those bulky heat sinks.

The LM1875 audio amplifiers were placed on the bottom side of the PCB so that they can be heat sunk directly to the ground plane.

The LM1875 audio amplifiers were placed on the bottom side of the PCB so that they can be heat sunk directly to the ground plane.

The next step is to test it and see if all that hard work in designing and making the PCB has payed off. First I decided to try just the Speakers with no lights. The first time you power up a circuit board is always both exciting and dreadful. So it turned out that one of the speakers worked, and one of them didn’t.

Now it’s time to troubleshoot. First thing I did is to check if the amplifier for the speaker that didn’t work has power. Turned out that it didn’t, and this is good news. Close inspection of the solder joints of the amplifier found that I had forgotten to solder the power pin. Thankfully it is an easy fix. After soldering the power pin, both speakers are now happily working.

So far so good. What about the lights? After connecting the RGB strip to the PCB I turned on the lights switch and there was…. no flashing lights. Time to troubleshoot again. As before, I checked to make sure that power is available to all the components of the RGB driver portion of the circuit. This includes the RGB strip, the ATmega328p and the active filters. All the components had power. This means I have to dig a bit deeper to find the problem.

I decided to re-program the ATmega328p first. Surprise surprise! After re-programming the MCU the lights started flashing. Most likely what happened was that sometime in between removing the MCU from the breadboard and putting it on the PCB and soldering it, the program on the chip got corrupted. This could be due to ESD since I didn’t take any protective measures for ESD.

The best part however, is that now there is none of the interference that I observed before when the setup was on the breadboard. The audio is crystal clear even when the RGB strip is running. This means that the interference observed before is due to imperfections of the breadboard. Good layout technique and having a ground plane eliminated the interference problem.

Finally, let’s enjoy a show to celebrate this

So what’s next? This project is not done yet. One of the reasons I build this is to have a platform where I can test and implement different ways of syncing lights to music. So I will be trying out different algorithms and doing a bit of programming for the next little while to get the maximum use out of the Music and Lights system. And I will keep you up to date on that as well. Stay tuned and Thanks for reading!

PCB making at home – Etching

This post continues from my previous post, where I developed the Music and Lights PCB using the UV exposure method. Once an etch resistant image of the layout is successfully placed on the Copper board it is time to do the etching. Etching is the process of removing unwanted Copper from a Copper clad board.

Ferric Chloride used for etching

Ferric Chloride used for etching

 

The etching solution I am using is called Ferric Chloride, a corrosive chemical that will dissolve exposed Cu and pretty much any metal. It also leaves a stain on pretty much anything it touches. When working with Ferric Chloride, it is very important to be in an area with good ventilation as it tends to produce a strong fume (specially when you just open the bottle or container used to store it)

Compared to the photoresist developing process, the etching process is slow. The amount of time taken to etch the board depends on the board size, temperature, amount of etchant and circulation. I finished etching my board in about 40 minutes.

And these are the steps, continuing from the previous post

Warning: Ferric Chloride is corrosive. Wear safety gloves when handling. Work in a well ventilated area.

Step 20: Pick a plastic container and place the Cu board with the etch resistant layout image inside.

Step 21: Pour Ferric chloride into the container until the board is completely covered. Do not dilute with water.

Fill the plastic container with Ferric Chloride until the board inside is completely covered

Fill the plastic container with Ferric Chloride until the board inside is completely covered

Step 22: To increase the etching rate agitate the solution every few minutes by tilting the container back and forth.  Examine the board and flip the board every 5 minutes for the first 20 minutes or so.

The exposed Cu will start to disappear from the edges first. When the exposed Cu has disappeared from about half of the board start monitoring the process more frequently. If left for too long in the etching solution it will start eating through the etch resist as well.

Step 23: When exposed Cu from both sides of the boards is etched away remove the board from the container and rinse with plenty of cold running tap water. Dry the board with tissue or soft cloth.

 

The back side of the PCB after etching

The back side of the PCB after etching. Notice on the right side how the etchant has started to eat away through the etch resist. This side was slightly overexposed during the development process.

As you may notice in the image above, the right side of the bottom PCB layout got a bit eaten away by the etchant. This is because this side was over exposed during the photo development process. Fortunately it is not too bad as the affected area is mostly the ground plane. However, I will have to take extra care when soldering components to ensure that good connections are made.

Top side of the board after etching

Top side of the board after etching. Notice how the top side component pads line up perfectly with the bottom side component pads

Step 24: Use tissue paper and nail polish remover to wipe off photoresist from the board and expose the Copper.

Use nail polish remover to wipe away photo resist to expose the Cu after etching

Use nail polish remover to wipe away photo resist to expose the Cu after etching

Step 25: If necessary, trim the edges of the board with a fretsaw.

If necessary, trim the edges of the board with a fretsaw

If necessary, trim the edges of the board with a fretsaw

Step 26: If you have through-hole components, drill the holes with a PCB drill.

Tip: I used a 1 mm drill bit for larger components like switches and power connector, and a 0.8 mm drill bit for other components.

Drill component holes with a PCB drill. I used 1mm and 0.8mm drill bits

Drill component holes with a PCB drill. I used 1mm and 0.8mm drill bits

That’s it! Now in my hands I have a home made PCB for the Music and Lights system.

Now you might be wondering why in the world go through all that trouble to make your own PCB at home when you can get a better one manufactured professionally. I totally agree that it makes more sense nowadays to get your PCB manufactured, plus you will have a solder mask and a nice silk screen too. But making your PCB at home is fun, and you get to control and see the whole process. It is a path with many challenges and finding ways to overcome them is the best part.

Now to the final note about making PCBs at home,

What to do with all the chemicals when you are done with them

You shouldn’t dump used chemicals down the drain, nor flush it down the toilet nor throw in the dumpster. They will destroy your plumbing and could do terrible damage to the ground water and environment.

Safe and easy way to dispose of them is to contact your local hazardous waste disposal company. I store my used Ferric Chloride and photo developer solution in plastic containers, usually the ones they came in, until a sizable portion is ready for disposal.

PCB making at home – UV exposure

This is the second post in a series of posts I am planing to write about making printed circuit boards at home. The first post explains all the things you will need to make a PCB at home using the UV exposure method.

The purpose of the UV exposure is to get the PCB layout image onto the Copper board. The pre-sensitized board we are using has a thin layer of photoresist coated on top of the Copper layer. When exposed to light (near the UV region) photoresist becomes soluble by a positive photoresist developer. If unexposed, photoresist becomes insoluble to photoresist developer and forms a strong bond with the Cu layer.

As you will see in the steps below this property of the photoresist  is used to put an etch-resistant image of the PCB layout onto the Cu board.

So let’s begin!

Printing the layout onto a transparency sheet

For a double sided PCB, either the top side or the bottom side needs to be mirrored when printing. When the PCB is exposed the layout will get mirrored again. Since most of my components are on the top side I will mirror that side so when the board is developed the components will go on the top side. Otherwise some components, where orientation matter, will have to go on the bottom side.

Tip: The layout editor has a setting where you can mirror the layout when printing. Use the transparency setting on the printer for better results.

Step 1: Print a mirrored image of the top side layout onto a transparency sheet.

Chances are, if you are using an inkjet printer like I am, when you print your layout on the transparency the traces and component pads won’t be completely opaque. So I usually print two copies and align one on top of the other to increase the opacity.

Step 2: Print another mirrored copy of the top side and align it with the previous copy. Use pieces of clear tape at the edges to hold the two transparencies together

Top side of the layout printed on transparency. Top side is mirrored.

Top side of the layout printed on transparency film. Top side is mirrored.

Step 3: Print two copies (not mirrored) of the bottom layout on transparencies and align them as in Step 2.

Bottom side of the layout printed on transparency film. Bottom side is not mirrored.

Bottom side of the layout printed on transparency film. Bottom side is not mirrored.

Step 4: Carefully align the top side on top of the bottom side (with the printed sides facing each other) by hand such that the component pads on the top side perfectly lines up with the corresponding component pads on the bottom side. This is possible only if one side is mirrored as in Step 1.

Step 5: Secure the aligned top and bottom transparencies with a piece of clear tape on one side such that the board can be slid in between the two transparencies making a sandwich.

Carefully align the top and bottom side transparencies.

Carefully align the top and bottom side transparencies.

Preparing the pre-sensitized board

Now is a good time to remove the pre-sensitized board from the wrapper (but don’t remove the white cover yet). The white cover sheet on the board is there to prevent accidental exposure. Chances are the board you got is not the correct size for the PCB you want to build. The 150 mm x 250 mm board I already had at home is a bit larger for my 100 mm x 160 mm layout. So I want to break a piece off the board to make it close to the size I want. That way I can use the extra piece for another PCB.

The pre-sensitized board has a white cover sheet to prevent accidental exposure.

The pre-sensitized board has a white cover sheet to prevent accidental exposure.

If you don’t need to break a piece off your board then you can skip to Step 9. To break a piece off the board,

Step 6: Draw a line across the board on both sides where you want to break it.

Step 7: Use a knife and a straight edge to make a groove (about half a mm) along the line on both sides of the board.

Step 8: Use a table edge to bend the board along the groove until it snaps clean.

Setting up the exposure table

A couch table with a sheet of glass in the center hacked as an exposure table

A couch table with a sheet of glass in the center hacked as an exposure table

Since I didn’t want to spend money on an expensive exposure kit, I found a way to hack a couch table to do the exposure. The table has a sheet of glass in the center where I can place the transparencies and the board. This allows me to expose both sides of the board at the same time.

The exposure table should be setup on a relatively dark room with no direct sunlight or a light source. It doesn’t have to be pitch black (basement is perfect!). But darker the better. If it is too dark to see anything you can use a red light source. Photoresist is only sensitive to wavelengths near the UV region.

Step 9: Place two desk lamps (with fluorescent light bulbs) on either side of the glass sheet facing each other as in the image above. The light bulbs should be 5″ to 6″ away from the glass surface.

Tip: To turn on both lamps at the same time, connect them to a power bar with the switches turned on and then plug the power bar to the wall.

Step 10: Place the transparency stack assembled in Step 5 on the glass sheet centered between the lamps, and secure with clear tape on one side such that you can slide the board in between the top and bottom transparencies.

Place the transparency stack in between the lamps

Place the transparency stack in between the lamps

Exposing the board

Steps in this section are time sensitive, and they must be done in one sitting. The exposure time depends on the power of your lamps and how far away they are from the board during exposure. I am using 13 W bulbs 6″ away from the board and a 8 minute exposure time is enough. I have found previously that a 10 minute exposure is a bit too much for my setup.

You may also want to gather the following items beforehand and keep them in a easy to find location,

  • A second sheet of glass (I took mine from a photoframe)
  • Positive photoresist developer
  • Plastic container large enough to place your board
  • Water
  • Tissue paper or soft cloth
  • Safety gloves and safety glasses

Before you begin, ensure both lamps are off and the room is relatively dark. You can use a red light source.

Step 11: Carefully remove the white protective covering from both sides of the pre-sensitized board taking care not to touch the board surface (hold from the edges).

Step 12: Slide the board in between the top and bottom transparencies and ensure the complete layout falls within the board edges.

Step 13: Place the second sheet of glass on top of the transparency-board sandwich and apply weight to press it down as in the image below.

Exposing the pre-sensitized board

Exposing the pre-sensitized board

Step 14: Turn both lamps on at the same time and set the timer for 8 minutes.

Meanwhile, prepare the developer solution.

Warning: Positive developer is corrosive. Wear safety gloves and safety glasses when handling chemicals.

Step 15: Add 10 parts water to 1 part positive developer solution to the plastic container. Ensure you have enough depth so when you put the board inside, the solution will completely cover it.

Mix one part positive developer to ten parts water in a plastic container.

Mix one part positive developer to ten parts water in a plastic container.

Step 16: When 8 minute exposure is done, turn off both lamps. Carefully remove board from the setup and place in the plastic container with the developer solution.

Step 17: Tilt the container back and forth to move the solution around the board. After a few seconds you will start to see the image of the layout appear (like magic!). Keep agitating the solution until all the excess photoresist is removed from the board and only the image of the layout remains. The board should be in the solution no more than 30-40 seconds. If you keep the board in the solution for too long it will start eating away at the layout image as well.

Step 18: Once all the excess photoresist is dissolved, remove the board and rinse with plenty of cold running tap water.

Step 19: Dry the board with tissue paper or a piece of soft cloth.

Image of the top layout on Cu board after UV exposure and development

Image of the top layout on Cu board after UV exposure and development

 

The image of the bottom side layout after UV exposure and development

The image of the bottom side layout after UV exposure and development

So the UV exposure and development of Music and Lights board turned out not too bad. However, if you notice closely, the left side of the top layout got a bit over exposed. This happens because the glass sheet on top of the board wasn’t pressing hard on this side of the board. When the transparency is not pressing tightly on to the board during exposure, light could seep through.

This is bad because the faint traces on the left side will not be able to completely protect the Cu during the etching process. Fortunately, it can be fixed by going over the traces and pads with a ultra fine tip sharpie (or permanent marker).

The over-exposed traces and pads can be fixed by an ultra fine tip sharpie before the etching process

The over-exposed traces and pads can be fixed by an ultra fine tip sharpie before the etching process

Finally, the board is ready for etching! Etching is easier than the UV exposure part but it takes a bit longer. So I will leave that to the next post. Stay tuned and Thanks for reading!

PCB making at home – getting started

After making a few of my circuits on perfboards I decided it was time to move on to printed circuit boards. Perfboards are probably the best choice for smaller circuits, but as my circuits got bigger and more complex it was difficult to wire everything and make it look neat. Also I really wanted to learn how to design printed circuit boards since PCBs are used in almost all electronic devices these days.

Of course, after you design your PCB you can get it manufactured by a PCB manufacturer, but making your PCB at home is fun and has many challenges to work through. There are many ways to make your own PCB at home. The method I am using is commonly called the UV-exposure method. And I will show you the process I use and how I solved certain hurdles along the way.

Before you decide to make your PCBs at home, there are a few things to consider.

  • You will be working with chemicals and will need to take the necessary safety precautions.
  • After you are done with the chemicals you need to find a proper way to dispose them. No you can’t flush them down the toilet! (This will cost more down the road)
  • You may have to purchase additional equipment (see the list of things needed below)

When I was making my first PCB at home, I had to find alternative ways of doing certain steps since I didn’t want to spend a lot of money on expensive equipment like UV exposure kits. My first step is to look around the house and find a way to hack something to get what I want.

Equipment and materials needed

  1. A PCB layout – I am going to make my Music and Lights PCB.
  2. Transparency film – The type of transparency film will depend on whether you have a laser printer or a inkjet printer. Transparencies made for laser printers won’t work with inkjet printers and vice versa. I have an inkjet printer, and I found inkjet transparencies at Staples.
  3. Printer – A laser printer or an inkjet printer will do.
  4. Pre-sensitized Copper clad board – These boards have a photosensitive coating on top of the Cu layers. And they are either positive or negative acting. You will need a board that is positive acting. You can get them double-sided or single-sided. I will be using a double-sided board for my Music and Lights PCB. The boards come wrapped and you should keep it that way until ready to use.
  5. Two desk lamps with fluorescent light bulbs – For a double-sided PCB you need two lamps, one for each side. Regular light bulbs won’t work well (or take a really long time) since the photosensitive coating needs shorter wavelength light (near UV) to change its chemical properties.
  6. Photoresist Developer – These come in two flavors (but don’t even think about drinking them!) positive or negative. Since I am using a positive acting pre-sensitized board I need a positive developer. You can find these at your local electronics store.
  7.  Etching solution – There are a few etchants you can use, but the one I am using is Ferric Chloride.
  8.  Nail polish remover – This is used to remove the photoresist after etching is completed. If you don’t already  have this your mom or sister will.
  9.  Drill and drill bits – A hand drill won’t work unless it is a small one designed for PCBs. I use a small drill kit I found at Jameco (Part no. 2113252), which came with two drill bits and a stand. The size of drill bit you need will depend on the components on your circuit. But I find that a 1 mm drill bit works for most components.
  10. Plastic containers – large enough to put your board inside flat with the solutions. Metal containers will react with the solutions and should not be used.
  11. Sheet of glass – From a picture frame. To put over the pre-sensitized board during exposure. I will explain why this is necessary when I get to that step. Also since I have to expose both sides of the board at the same time I am using a couch table that has a glass plane in the middle. This is a hack I will explain later.

Since you are gonna be working with chemicals you also need the following safety equipment and a well ventilated area to work with

Safety Equipment

  1.  Safety gloves – The photoresist developer (NaOH) and the etchant (FeCl3) are corrosive.
  2.  Eye protection
  3.  Respiratory mask – The photoresist developer produces a white powder when dried up, and the fumes of Ferric  Chloride is toxic and can cause burns.

Once all the equipment is gathered, it is time to develop the PCB. This is where the fun begins, and it deserves its own post. Stay tuned!