Building Circuits for Stripboard using EAGLE – Mike Perks


This is a great webpage, written by Mike Perks in 2005, which I came across whilst reading Stripboard. Unfortunately, the link therein was dead and it took me a while to locate it. I have taken the liberty to reproduce it here, as it may get lost again, in the sands of time, that is the web. The zip file is here:


Building Circuits for Stripboard using EAGLE

This article, first published on 13 June, 2005 describes the process I use for building circuits on stripboard (aka Veroboard in Europe). I use EAGLE to draw the schematic and help design the circuit layout on stripboard. Some of this article may be useful even if you use other techniques for building circuits. As an example I build a simple audio signal generator and a mono audio amplifier.


Comparing Stripboard to other Techniques

Breadboarding the Design

Draw the Schematic

Create the Stripboard Design

Preparing the Stripboard

Solder the Components

Testing the Circuit

Completed Circuit

Parts List


Please read and understand the following paragraph before continuing.

The contents of this article are for personal, educational and non-commercial uses only. The information is provided “as is”, without any warranty of any kind, and without any guarantee as to fitness for purpose. The content of this article is copyrighted Mike Perks, 2005.

Comparing Stripboard to other Techniques

In general people tend to use a range of different techniques to build circuits from the �dead bug� style to a custom PCB. Each technique has different advantages and disadvantages and here is a good article that compares the various techniques. I have some specific tips and techniques in this article that improve the �ease to copy� and �smallness� criteria.


For one-off circuits (as most hobby projects are), then I have found stripboard to be a good tradeoff between a perfboard which provides no help for circuit connections and a custom PCB which can be expensive to make and is hard to change. In fact perfboard can also be harder to change unless you use wire-wrapping and of course breadboarding is the easiest to change but the least permanent. Therefore stripboard in my view provides a happy medium as summarized by the website:


Advantages of Stripboard:

�        Low Cost – no expensive PCBs to send for.

�        No Mess – no chemical hazard, no slop, no photography or plotting.

�        Fast – take a piece of stripboard off the shelf and start building (although good planning is always helpful).

�        Adaptable – modify the layout to suit the components locally available.

�        Versatile – add more functions or circuits on the same piece of board.

�        Compact – unlike Wire Wrap stripboard can be built into small enclosures.

�        Widespread – universally available in all parts of the World.

Disadvantages of Stripboard:

  • Labor Intensive – if building more than one or two units.
  • Non-optimal – less component density than a well laid out PCB (although I have been able to get some quite compact layouts)


To be fair I should also mention that I have not used all of the different techniques myself and I am also somewhat biased towards stripboard as that is what I cut my teeth with as a teenager playing with electronics. The best source I have found for buying stripboard in the USA is AllElectronics. The part number is ECS-4 and costs $6.25 for a stripboard that is 38 strips by 55 holes as shown in the picture below.


Just before publishing I found this link that describes a similar technique to the one described in this article but with much less detail and only for single hole Veroboard.

Breadboarding the Design

I always breadboard the circuit before transferring it to stripboard. Even for pre-designed circuits I usually end up either playing with the values or adding features to the circuit and so I like to be sure that it all works correctly. Personally I do not have the level of sophistication to go straight to building before I have prototyped first and in any case I think it is a good practice to always try things out before committing to something more permanent


For the purposes of this article and because I needed the circuit, I have chosen to build a simple audio frequency generator and mono audio amplifier. The audio frequency generator uses a quad op-amp package to create square, triangle or sine waves and is documented several places on the Internet such as here. The generated waveforms do have some distortion and there are better and more complex circuits to generate these waveforms but that is a whole other subject. The audio amplifier circuit is based on the LM386 1W audio amplifier chip and is documented here.


I did make a few changes to the circuit as follows:

  • Replaced the standard LM348 quad op amp with a low voltage LM324 so that I could run the circuit off a 5V supply. The 5V also does limit the output of the audio amplifier to much less than 1W but that is not a problem.
  • Replaced feedback resistor with 4.7K instead of 8.2K
  • Swapped the two op-amps A and B for a cleaner stripboard layout (see Create the Stripboard Design below)


Here is a picture of the completed circuit on my breadboard. On the right is the LM324-based signal generator and on the left is the LM386-based audio amplifier. At the bottom are two wires leading to an 8 Ohm speaker. At the top of the breadboard you can see my breadboard interface circuit that is described elsewhere on my projects page.



After successfully breadboarding the design it is time to transfer the circuit to a more permanent version on stripboard. That is what the rest of this article is about. This process consists of following five steps:

�        Draw the schematic

�        Create the stripboard design

�        Prepare the stripboard

�        Solder the components

�        Testing the circuit

Draw the Schematic

Drawing the schematic using the CadSoft EAGLE tool is the first step. If you are creating a new design or even modifying an existing one, then documenting the final (and even intermediate) circuit is essential. Even if you are building a circuit designed by someone else then perhaps the EAGLE schematic is already available. If not, then you should draw the schematic yourself using EAGLE as this is pre-requisite for the other steps.


I use EAGLE for drawing schematics and laying out circuit boards because it quite powerful and there is a free version that I have found suits my needs. The only two things missing from the free version is the ability to lay out larger boards (bigger than 100mm by 80 mm) and multiple layers. I have used Eagle enough now that I intend to buy the non-profit version for $125 because it relaxes some of these restrictions.


The circuit schematic for the audio frequency generator and amplifier circuit is shown below and is available for download. Note that I had to create my own circuit symbol for the LM386 because I couldn�t find one on the EAGLE library download page. The library file for this part is included in the download package of the EAGLE files.


I added a 10 pin connector for the various signals. Note that four of these are for ground but I decided to have multiple pins just in case there isn�t room on the breadboard to have all the grounds running off of one pin. For this connector I�m using male square pins mounted upside down so that the circuit can be inserted horizontally into a breadboard. I usually buy these pins in 40-pin lengths and break off what I need. An alterative is to use a SIL sockets that so a wire can be pushed into the socket hole to connect a hole in the breadboard. Note that the schematic also shows 2 mounting holes and 2 pads that are used to help mount the small rotary potentiometer used for the volume control.


One trick with EAGLE that took me some time to figure out is how to move more than one component or net at a time. The way to do is to do a click on the group select menu �to highlight a group of items. Then click on the Move menu item on the right hand-side menu and select the group to move by right-clicking on one of the highlighted items. Now you can move the group around until you release the right mouse button.

Create the Stripboard Design

There are several methods for creating the layout for the stripboard including:

�        Design as you go meaning the simply add the components and connect them up but this is error prone.

�        Use the stripboard designer tool which doesn�t seem to be maintained anymore.

�        Use another tool such as Paint or Visio to layout the components. I used a multi-layer Visio diagram for laying out my BasicX/AVR development board which is the largest circuit I have built to date.

The problem with these methods is that you have to double check that the circuit matches the original schematic and it is very easy to make mistakes.


As an alternative I recommend using the board layout tool that comes with EAGLE. Although this tool is really meant for PCB layout it can be used for stripboard (or perfboard for that matter). Once you are happy with the schematic you can create a board layout using EAGLE. In fact unless you go out of your way with part renaming or deleting EAGLE will keep the schematic and the board in sync for you. There are 3 steps to creating a stripboard design in EAGLE:

�        Layout the components

�        Draw in the tracks and wire links

�        Add the track breaks

The first thing to do after creating a blank board is to setup a 0.1� grid with a 0.025� alternate grid and display it. Now components can be moved from their default position to one that makes sense for a stripboard layout. I try to position components so they connect horizontally using strips on the stripboard. Inevitably you will need to cut strips and add vertical links to complete all of the connections. The screen capture shows this component positioning. By pressing the Alt key at the same time at positioning an item with the mouse allows positioning of items on the alternate grid or moving them to line up with the 0.1� grid.


Note that these components are shown with their final package format. With resistors you can choose if they are mounted horizontally or vertically and how much space they take up. For example a resistor can be in a 207/5V package which means it is mounted vertically and takes up 5mm (approx 0.2�). A resistor might be in a 207/12 package which takes up 0.5�. By changing this packaging you can choose which horizontal tracks the component is connected to. The same is true for many capacitors especially electrolytics in that you can choose the diameter and pin spacing. For example C3 is 5mm diameter with 2.54mm (0.1�) pin spacing.


In EAGLE the way to change the package is to the select Change from the right-hand menu and then package from the drop-down list. A list of available packages should now be displayed and the most appropriate one selected. You may need to play around with the component sizes to get exactly the layout you want.


With other components either the size cannot be changed e.g. DIPs or you have to carefully choose the component as the package is fixed. For example the trimmer potentiometer R5 is in the B25P package. In this case you need to go back to the schematic and replace the existing part with one that has the package you want. It helps to look back at the breadboard to the actual components you used and try to pick the best part at that time.


In the end you may need to iterate a few times on the board layout and the components. Part of what helps finally nail the layout is the additional of the actual routes which in this case is either stripboard tracks or wire links. I try to make as many of the wire links straight and not crossing other components.� The decision to have IC2 upside down for easier connectivity of components was part of the process of iterating on the board layout.


In the diagram on the right is the final board layout with layer 16 (blue) representing the tracks under the board and layer 1 (red) representing the wire links on top of the board. Notice that I carefully change colors between tracks (blue) and links (red). This is a bit more work and takes practice to get right but is worth it later when deciding where to put track breaks and for wiring the actual circuit. I also use the View menu to view just layer 19 to make sure I did in fact route all the nets.


There are 16 straight wire links shown in solid red and 7 wire links that will need routing around other components shown as a dashed red line. Note that the volume control potentiometer R12 takes up more room than the frequency trimmer R5 and that two extra pads have been added that are holes to take the retaining clips of the potentiometer. At this point it may be worth printing the board layout, taping it to a board and doing a trial fit to make sure all the components and wiring will have enough room. In the board above everything looks very reasonable except for the area around R12, C4 and C5 that needs a little attention.


You can check for ground or power loops in the board layout by clicking on the show button �and then selecting the net you are interested in. The screen capture to the right shows the output when ground net was selected.


In the board layout shown above there are a couple of tricks that are worth noting. I usually run wire links inside a DIP chip as well as outside it. These �internal� wires are normally for power and ground. I then solder the socket over the top. So far I have never had a problem where I needed to unsolder the socket because a link underneath it was wrong. Also shown are two wire links going into the same hole. I use thin copper wire for links (I think it is 24 AWG) and this is thin enough to just squeeze two wires into one hole. The method saves quite a bit of space but is obviously not appropriate for wires carrying larger currents. I also sometimes reuse clipped component leads for wire links instead of the copper wire.


The final step is to indicate where the breaks in the strips are needed. The most convenient break is one that occurs over a hole. In this case it is simply a matter of drilling out the copper on the back until the track is broken. I describe more about how to do this in the section on preparing the stripboard. In some cases a break is needed on a strip between two holes. This is much harder to make and ensure that the two sides do not have connectivity but it does allow for close component positioning. I also add track breaks around mounting holes to protect against any hardware inadvertently shorting two tracks.


To indicate track breaks I use layer 45 (holes) and add holes where I want the track breaks to be. I use different hole sizes to indicate a hole break or a between hole break. It is useful to just display layers 16 to 20 and layer 45 to get an instant picture of where track breaks need to be. This view is also helpful later when the track breaks actually need to be made. Here is a snapshot of just that view with 38 X�s to represent track breaks over a hole and 4 diamonds to represent the breaks between holes. The different symbol is displayed in EAGLE by choosing a different hole size from the Change menu and selecting Drill.


Before moving on to preparing the stripboard, there is a user language program (ULP) for EAGLE that provides a 3D rendering of the board. This ULP called Eagle3D was written by Matthias Wei�er creates a 3D description and then a program called POVRay is used to render that 3D description. Below is the result for the top and bottom of the board. Note that the two potentiometers are not rendered quite right but the rest of the circuit is extremely realistic. The bottom of the board is less interesting except to note that the male pin connector for inserting into a breadboard.



At this point it would be nice to wave a magic wand and make the circuit become a reality. But that isn�t possible so the next step is to get the stripboard ready for soldering.

Preparing the Stripboard

The board design described in the previous section requires a piece of stripboard that has 18 strips of 20 holes i.e. roughly 2� by 2�. The first step is to take a piece of stripboard and cut it to the correct size. Don�t forget to sand the edge to remove any sharp metal from the cut tracks.


The next step is to drill any additional or larger holes that are needed. In the case of the circuit for this article, two 7/64� mounting holes for #4 size mounting hardware and two 5/64� holes for the audio volume control potentiometer tabs are needed. One way to do this is to print out the board layout and tape it to the top of the board. Then it is simply a matter of using a drill (or a vertical drill press if you have one) to drill out the holes through the paper. Pilot holes may or may not be useful and are of course not needed if you are merely making an existing hole bigger for a fatter lead or mounting hardware.


The next step is to cut the tracks in the appropriate places. It helps to print the board from EAGLE with just the layers 16 through 20 as shown above. When printing from EAGLE you can select to reverse the image. Then you can use a permanent marker to mark the spots for the track cuts and compare back to the original. It may be useful to produce a transparency and lay it on top of the board to compare the marks with the required track cuts � just be sure that you have the transparency in the correct orientation.


After marking the bottom of the board, use a small drill such as a Dremel with a 7/64� bit to make a shallow hole wherever there is a mark. If you drill too shallow the track will not be completely cut and if you drill too deep then you may end up with a broken board especially where there is a line of cuts. I don�t bother using a vertical drill press for this because it needs a light touch to drill just a little and I clamp the board while drilling these track cuts. Then I verify the track cuts using a continuity tester. Any cuts not made properly can be cleaned up with a utility knife to remove the copper threads at the sides of a cut.


I use the same knife to make the between hole track cuts and carefully scrape out a line of copper to break the track. I then test these cuts using the continuity tester. Before putting away these tools I do one more complete test of the board just to be sure. Even for this circuit I found one incomplete track cut during this second test. This type of problem would be much harder to find once the board is completely soldered. The picture below left shows a side by side with the board and the template. If you look carefully you can still see some small residue of the blue permanent marker I used. This is easily removed using acetone or similar solvent.



The final step in preparing the board before soldering is to mark the top of the board with the component positions using a permanent marker. This is a poor man�s silk screen but it saves a little time during assembly. Blue permanent marker on a green board doesn�t have a lot of contrast but I think you can get the idea from the picture above right.


All of the preparation work is now complete and this is a good time to take a break. The actual soldering of the board is actually very easy as it is just a matter of placing the links or components in their correct position. Apart from soldering in some extra wire links, this is as easy to solder as a PCB.

Solder the Components

I always solder the components starting with the lowest height ones first and then building up. This makes it easy to ensure that the components are all flat against the board. Even when the circuit is broken up into testable submodules I follow this procedure and then separately test each submodule in order to narrow down any problems. Most of the time these submodules do have interconnections and if these are via wire links then I may not make these final connections until I have done some testing of the submodules.


For the circuit in this article, a possible order of construction is as follows:

�        16 straight wire links

�        Pin header � JP2

�        Small capacitor � C7

�        Resistors � R1, R4, R6, R7, R8, R11, R13

�        Diodes D1, D2, D3, D4

�        IC Sockets and trimmer � R5, IC1, IC2

�        Taller capacitors � C1, C2, C6

�        Vertical resistors � R2, R3, R9, R10

�        Jumper � JP1

�        Electrolytic capacitors � C3, C4, C5

�        7 remaining wire links

�        Potentiometer � R12


Because the pin header JP2 is being mounted on the solder side of the board, I push the pins all the way through so I get the longest pin possible for inserting into a breadboard. The picture on the right shows the before and after of the pin header strip.


As you solder in components I suggest you test for continuity or lack of it especially in places where you may believe there is a solder bridge � just in case. One area that needs vigilance is the between hole track breaks that can be easily bridged.

Testing the Circuit

The circuit needs testing once it has been completely built. Here is the procedure I used to test this circuit:

�        Without any chips installed in sockets, test continuity of the power nets (in this case 5V and ground). Also ensure there isn�t a short between 5V and ground. Test any other nets that are critical or might be suspect.

�        Apply power and test with a voltmeter for the correct voltages at different parts of the circuit. Normally this comes down to verifying the appropriate power pins on the IC sockets.

�        Insert the chip(s) for the submodule you are testing with the power off. Then apply power and check for warmness or smoke. Power off if either of these conditions exists and recheck the circuit. I sometimes use an ammeter to check for excessive power drain.

�        Depending on the test equipment at hand, you can test either the audio frequency generator first or the audio amplifier. For the frequency generator check the output voltage first and then hook up to a frequency counter or an oscilloscope. For the amplifier you can feed it a known signal such as from a microcontroller sound function or the frequency generator just tested.


If you are lucky it all works first time. I say lucky because minor or even major problems are possible. Here are some things to watch out for:

�        Schematic didn�t match actual breadboarded circuit

�        Changes to the circuit after it was breadboarded without testing them

�        Forgetting to cut a track or wire a link

�        Solder bridges either across cut tracks or between tracks

�        Inserting chips upside down

�        Incorrect positioning of components (although the EAGLE design step should avoid this)


In my case I did have a couple of solder bridges. There was one between pins 2 and 3 of IC1 that meant the sine wave output didn�t work and one between pins 5 and 6 of IC2 that caused the amplifier to feedback and use excessive power. Luckily I did not smoke any components as most modern chips have built in protection against such problems.


One trick I have used in the past for stripboard is to run a knife along the gap between every track. This removes the flux that gets built up in this area and can also cut any inadvertent solder bridges between tracks. I would recommend following this practice for your circuits.

Completed Circuit

The pictures below show the top and bottom of completed stripboard circuit in comparison with the 3D rendering from EAGLE. The bottom of the board is very clean and flat � all the wire links are on the top of the board, insulated as appropriate. It is also quite easy to make a change by using a desoldering pump to remove solder around the hole and then simply pulling the component or wire from the board.


Here we are back where we started on a breadboard but this time we have a completed circuit plugged into the breadboard and wired up to 5V power and a speaker. The square wave from the frequency generator is hooked up to the audio amplifier. In addition you can see two 3/4″ standoffs attached to the mounting holes and a label to indicate the function of the pins on the connector.


Parts List

I have included a complete parts list if you want to build this circuit yourself. The parts list also includes the order numbers and prices from Mouser for those people who live in the USA. The total cost is $4.33 not including the stripboard, sales tax and shipping. Personally I like Mouser because there is no minimum order, the prices are very competitive and I because of where I live I get overnight delivery using Fedex ground delivery.


Part Value Description Mouser Part #



C1, C2, C6 47nF multi-layer film capacitor 581-BF014D0104J



C3 10uF electrolytic capacitor 35V 140-XRL35V10



C4 2.2uF electrolytic capacitor 25V 140-XRL25V2.2



C5 470uF electrolytic capacitor 140-XRL25V470



C7 0.1uF ceramic capacitor 581-SR205E104M



D1, D2, D3, D4 IN4002 625-1N4002



IC1 LM324N 512-LM324AN



14 pin DIP socket 517-ICO-143-S8A-T



IC2 LM386N 513-NJM386BD



8 pin DIP socket 517-ICO-083-S8A-T



JP1, JP2 12 off Male 0.1� post 517-2312-6111TG



Jumper 151-8010



R1, R2 100K 1/8 watt resistor Parts Box



R3 15K 1/8 watt resistor Parts Box



R4 470R 1/8 watt resistor Parts Box



R5 1M trimmer Trimmer potentiometer 72-T70YE-1M



R6 10K 1/8 watt resistor Parts Box



R7 820R 1/8 watt resistor Parts Box



R8 1K 1/8 watt resistor Parts Box



R9 470K 1/8 watt resistor Parts Box



R10 1M 1/8 watt resistor Parts Box



R11 4.7K 1/8 watt resistor Parts Box



R12 10K audio Miniature log potentiometer 317-2080-10K



R13 10R 1/8 watt resistor Parts Box




Last Updated: 16 June 2005 to include updated EAGLE library part for LM386.


Mike Perks 2005 � All views expressed in this document are my own and have been derived from Internet research and/or personal discovery. Please let me know if I have unintentionally infringed any copyrights or patents. All copyrights and trademarks belong to their respective owners and are not explicitly marked. BasicX website visited StatCounter - Free Web Tracker and Counter times.


Leave a Reply

Fill in your details below or click an icon to log in: Logo

You are commenting using your account. Log Out /  Change )

Google photo

You are commenting using your Google account. Log Out /  Change )

Twitter picture

You are commenting using your Twitter account. Log Out /  Change )

Facebook photo

You are commenting using your Facebook account. Log Out /  Change )

Connecting to %s