Hi Mk1_Oz, Good attempt for a first time design. However, don't rush to get this made yet, there are some changes you need to make. **First, please read:** https://easyeda.com/editor#id=a0cf7282b35140928ab93bc65c4b9cfb https://easyeda.com/forum/topic/The_best_way_to_design_a_PCB_in_EasyEDA-ThR3pwqIC and: https://docs.google.com/document/d/1CU7RuPyFlSZPzWBN-YZ0x87xeAB4xpLdLaIsUwhLj_M/edit?usp=sharing (I am in the process of writing this detailed tutorial on how to create a schematic and then do a PCB design. It is a work-in-progress and will eventually make it onto the EasyEDA site but it is useful as it is right now and you can see the current draft at the above url.) **Notes about your circuit:** If you choose parts from the LCSC library then they will all be pulled into the PCBn with the right PCB footprints and they will have all the right info from which to create the Bill of Materials (BoM) from which you can then order them from LCSC (EasyEDA and LCSC are the same company: one is the EDA side the other the components and PCB supply side) when you order the PCB and save on the component and shipping costs. You have changed all the component prefixes in the PCB: be aware that these will be reset if you update the PCB from the schematic (see below). This is going into a very (electrically) noisy environment so you need at least a 100nF decouping capacitor across the supply pins of U1. You should also have a 10uF bulk decoupling cap across where the supply comes into the board. See: https://easyeda.com/andyfierman/Power_supply_decoupling_and_why_it_matters_-451e18a0d36b4f208394b2a2ff7642c9 See also online info about opamps etc. You do not need to use such thin traces. Use 10mil or 20mil wide. Move the traces for VIN_12V and D1_1 onto the bottom (blue) layer. They do not need to be on the top. I would advise using copper areas to make one side a ground plane and the other a 5V plane just to reduce the supply and ground track impedances. If you put the ground plane on the component side then it can make probing the components with an oscilloscope (if you have access to one) a little easier. Move D1_1 below the pads so that it is away from the PCB edge. Find yourself a suitable L7805 from the LCSC library. Then choose a suitable vertical mount package (PCB footprint which will include the yellow silkscreen outline). I don't know what software you have used to simulate this design or exactly under what conditions that you have tested in, but you need to be aware that you are using the LM741 as a comparator. It will work as you have set it up but it is not designed to be used that way. You may also using be using it at way too low a power supply voltage. Compare **Recommended operating conditions** in: http://www.ti.com/lit/ds/symlink/lm741.pdf and: http://www.st.com/content/ccc/resource/technical/document/datasheet/group1/d6/9e/4e/8a/fa/65/4c/d0/CD00001252/files/CD00001252.pdf/jcr:content/translations/en.CD00001252.pdf You may be better choosing a dedicated comparator chip that is designed to operate from a 5V single rail supply for example the LM311. * Note that you can do simulation in EasyEDA but please read this first: https://easyeda.com/forum/topic/How_to_find_simulatable_parts_and_run_a_simulation_in_EasyEDA-1YgasK2kC **Holes etc;** Holes for component leads are part of the PCB footprint. you do not need to do anything extra about them. You have no PCB mounting holes but if you do need them, see my tutorial abouve about why they need to go in the schematic. Post back if you need more help. :)

Wow what a reply! Thanks. I will digest and make necessary changes.

Forgot to add, for the life of me I could not find a simple part. A metal film 0.5W 11K resistor (also need a 1K1 and 110 ohm) hence I just left a generic item in order to just get the correct footprint.

None of your resistors as shown in the schematic dissipate anywhere near 0.5W (just check the V across each resistor and do P=V^2/R). You can use 0.25W or probably even 0.125W parts. What's the 110R for?

OTOH, you can always fit physically smaller (i.e. lower power resistor) parts onto the 0.5W footprints youve chosen. :)

Andy, I have thoroughly read your comments and tutorial links and have digested it the best I can. I don't think I quite understood some of it. Attached is my updated PCB incorporating your suggested changes. I am very confused by the copper area. It was set to work with the grounds yet the copper area is linked to the bottom layer but the ground tracks are on the upper. https://easyeda.com/editor#id=a6d22732ae7b462187fd9cdcc24be726|8f33ef781b084f03935fb56ab0d88a68|75984d6a597c4c2092411137c41c9f4f I have not changed from an LM741 to the LM311 that you suggested as I have not yet looked into that component (but will). I have updated the parts and used the LCSC website to assist. However, I could not locate the exact resistor ohms required so used the closest I could find. Not sure why one resistor is physically bigger than the others. Also I took a guess that ceramic caps were teh ones to use. Can you eyeball if this is now more appropriate for manufacture? I would like to have a couple of additional labels (such as indicating 12v +ve and -ve, which Sig_Out terminal is used and maybe labelling of the voltage reg pins). Not sure if I am allowed to add anything in the silk layer or not? PS - I don't know what the 110R resistor is for other than it existed on teh schmitt trigger example circuits I copied and that the actual value provides the output I require)

Something else I just realised: You have used 2 back to back 10V zener diodes: http://www.onsemi.com/PowerSolutions/product.do?id=1N4740A to limit the input swing from your inductive pickup to the 741. That means that even though there is a 10k (was 11k?) resistor in series between the pickup and the 741 inputs which will limit the current through the inverting input pin, they are being pulled about 5.6V above the 5V rail (10V zener voltage + approx 0.6V forward drop of the other zener - 5V supply) and about 10.6V below ground. This exceeds the Absolute Maximum operating conditions in: http://www.ti.com/lit/ds/symlink/lm741.pdf and: http://www.st.com/content/ccc/resource/technical/document/datasheet/group1/d6/9e/4e/8a/fa/65/4c/d0/CD00001252/files/CD00001252.pdf/jcr:content/translations/en.CD00001252.pdf Using an LM311 would avoid this problem: http://www.ti.com/lit/ds/symlink/lm311.pdf http://www.st.com/content/ccc/resource/technical/document/datasheet/2d/22/50/0e/7e/39/43/64/CD00001072.pdf/files/CD00001072.pdf/jcr:content/translations/en.CD00001072.pdf although limiting the input swing to no more than +/-5V (say, 3.9V zeners) would be a good plan. A better solution is to use a single 4.7V zener would limit the input swing to between approx -0.7V to +4.7V but that may distort the duty cycle of the signal out of the pickup by asymmetrically loading it. You could try this on your PCB simply by replacing one zener with a wire link. * Note that the LM311 has an open collector output and not push-pull like the LM741. For reference: more info about decoupling can be found in the datasheets for 7805 type regulators.

It has taken me quite some time but I have taken all of the above advice and reconfigured my schematic and PCB. I have tested this with a breadboard and it appears to work OK on the test bench. The only part that did not get tested is the addition of the 2 capacitors. I believe these align with previous advice but I didn't have any when I did the testing. I created a 'copper' area (by drawing this on the bottom level using the 'copper' tool by surrounding the entire PCB outline) but to be honest I have no idea what this actually did. To my untrained eye it didn't look to do anything when I hit the auto-router button. I just don't yet know enough about PCB design to work out if there are still issues. Perhaps somebody would be kind enough to take a look? https://easyeda.com/editor#id=2e376c1b28194155bc01958420e7740f|b503e320fe394ec390ec9f4d65a06934

Autorouting will trash the copper area. If you must use the Autorouter, do that first then do the for area afterwards.

For info, there are two slightly different TI datasheets for the LM311 comparator: http://www.ti.com/lit/ds/symlink/lm311.pdf http://www.ti.com/lit/ds/symlink/lm311-n.pdf Worth reading both as they cover slightly different applications. :)

You're getting there but it takes too long to write all this stuff down. It's quicker to show than to tell... Here's one I prepared earlier. https://easyeda.com/andyfierman/SineWaveMod_copy-6aca5276122744a981bdc4104413ef9d No cheating! Make yours look like mine then you'll know how to do it next time. :)

Cheers mate. No idea how you got it looking like that but I will start playing!!

1. Rearrange the schematic to make it more readable; 2. Add netlabels and a GND symbol to help make the schematic and therefore the PCB more readable; 3. Run the (Schematic) **Design** manager in the left hand panel to check components, pins and nets; 4. Click on **Update PCB...** in the Schematic Editor or **Import Changes...** in the PCB Editor to bring the netlabels into the PCB. 5. Do **Tools > Global Delete... > Tracks** to remove the existing tracks and start routing from just the Ratlines; 6. Do **Tools > Set Board Outline...** and set corners to 100mil radius; 7. Push the PCB components around until they give you short tracks to sensitive places such as the FB net (easier to do once the nelabels are added!); 8. Route everything *except* the V5V and GND nets by hand on the bottom layer using 20mil tracks. 9. At this point keep in mind that the V5V and GND nets have to have good copper around and between the other tracks and pads to maintain continuity. This may require moving some components achieve. It gets easier with more experience and is something the Autorouter cannot do; 10. In the canvas attributes in the right hand panel (just click anywhere on the empty PCB canvas to see them), set **Copper Zone = Visible**; 11. Draw a rectangular Copper area a bit bigger than the board outline on the top layer and assigned it to GND. Then, with the outline of the rectangle selected, click **Rebuild copper area** in the right hand panel; 12. Draw a second rectangular Copper area a bit bigger than the board outline on the bottom layer, offset it a bit from the GND area to make it easy to select each of the two areas and assigned it to GND (you could also do this by copying and pasting the top layer rectangle then swapping it to the bottom layer and offsetting it). Then, with the outline of the rectangle selected, click **Rebuild copper area** in the right hand panel; 13. Revisit (9) as required; 14. Run the (PCB) **Design** manager in the left hand panel to check components, pins, nets and DRC errors (there should be no DRC errors). For more help, dig into the Tutorial. :)