Hi Perigalacticon, Welcome to EasyEDA. No problem however, for us to look at your project, you must either make it public and then post the url to the public project here or you can share it privately via Access Control: https://easyeda.com/Doc/Tutorial/share.htm#Sharing I can review it privately if you would prefer not to make it public. Just share it with me ![enter image description here][1] via Access Control. :) [1]: /editor/20160904/57cc04e111218.png

I added you to the project. Basically where I'm at is I made a schematic, and I made a PCB layout and ran the autorouter. It looks ok to me but I don't know if it's good. I don't know what the next steps are. I think I need to add soldermask? Thanks!

The circuit outputs are a .25W LED and audio to a .5W speaker. The input is a capacitive-touch antenna. It is powered by a 6V 2CR1/3n battery. I didn't find this battery in the part search do you know how I can put it in?

Um, I'm guessing that the battery fits into a holder of some sort and is not soldered directly into the board (bad plan!). I'm struggling to find any sort of holder for the 2CR1/3n battery. Do you have a link to a suitable holder, not the battery itself - from a supplier?

Reviewing your design: #### Schematic. 1) In addition to C4 you also need to add 4 off 100nF ceramic local decoupling caps as close as possible across the supply pins for U1, U2 and U3 plus another one from the anode of the LED to the emitter of Q1. Without these U1 - U3 may not work correctly. 2) You need a resistor in series with the LED otherwise it will draw an uncontrolled current from VCC when Q1 is turned on. The value of the resistor is roughly `Rseries = (VCC-Vfwd)/Iled` Where `VCC` is the battery voltage (6V?) `Vfwd` is the forward drop of the LED when it is drawing the required (or maximum allowed) LED current. `Iled` is the required (or maximum allowed) forward LED current. 3) Make sure you specify the right version of the LM386. The LM386-1 is rated as 250mW into 8R The LM386-3 is rated as 500mW into 8R. Do not use the LM386-4. See https://en.wikipedia.org/wiki/LM386 for more. 4) Save yourself a load of battery current and replace Q1 with a 2N7002 N channel MOSFET. It has a low ON resistance (compared to Rseries) with a gate drive of even only 4V (i.e. a low battery) and - unlike a bipolar transistor - draws no DC gate current through the 1k resistor (do not omit R6: it prevents the gate capacitance of Q1 excessively loading pin 6 of U1 during turn on and off edges. Without R6, U1 may behave erratically). Make sure you get the pinout of Q1 in the schematic to match the real device on the footprint that you select in the schematic for the PCB (press the `i` key to check the schematic symbol and make the pins the same on the schematic symbol and the PCB footprint). 5) Swap C1 from pin pin 3 of U3 and slider of trimpot, R5, into between the top end of R5 and the junction of R3 and C2. See `INPUT BIASING` in http://www.ti.com/lit/ds/symlink/lm386.pdf 6) If the trimpot is a log taper then check orientation of ends to ensure proper log volume adjustment. Do you really need a pot? Do you want to have to adjust a pot on each PCB you make? Could you not just fix the gain of the LM386 or use a fixed pair of resistor values in place of R5? 7) Add more BoM information to the devices in the schematic to simplify procurement? For examples of this, see: https://easyeda.com/example/Tesseract_Guitar_Practice_Amp-MjP71jBni https://easyeda.com/example/Uberclamp_Schematic_PCB_and_BoM-r4YgysK2k #### PCB layout. 1) Your auto routed layout may be OK but it would be wise to use wider traces (as wide as possible) for power supplies. Better still, place a copper area (plane) on the bottom of the PCB assigned to the ground net and another on the top layer assigned to the VCC net. Run thin traces between the ground pins to connect them and between VCC pins to connect them and so remove the ratlines that otherwise can be a bit confusing. (In fact these traces are not needed because they are connected by the copper areas but if the copper area is made invisible for any reason, then the ratlines appear which can be a bit confusing if you're new to EasyEDA). Then route carefully to give as much copper as possible connecting all the ground pins together through the plane and the same for the VCC pins through the VCC plane. To see examples of this have a look at the PCBs for: https://easyeda.com/example/Tesseract_Guitar_Practice_Amp-MjP71jBni https://easyeda.com/example/Uberclamp_Schematic_PCB_and_BoM-r4YgysK2k https://easyeda.com/example/The_EasyEDA_Commodore_64_Computer_Saver_PSU_overvoltage_protection_circuit-bS4ECcMXV https://easyeda.com/example/The_EasyEDA_Precision_Commodore_64_Computer_Saver_PSU_overvoltage_protection_circuit-G3pLJ5Paw 2) Consider making more of the devices SMD to reduce the PCB size? 3) A nice touch might be to add rounded corners to PCB.

Thank you very much! I will be working on this all weekend. In response to the corresponding points you made: Schematic: 0. I am testing with a 6V 2CR1/3n battery it seems to work well, they are made with PCB pins for mounting horizontally. Could you explain why this is not a good choice? Is there a better 6V option? I'd rather not have the expense of a holder, since the toy is an inexpensive halloween item I expect it will be discarded after a while. The issue is my BOM cost estimate is already ~$7 for a quantity of 100. I was hoping to get that below $5, ideally much lower. 1. Just one capacitor across the battery is really not enough? I have been testing on soldered perfboard with only one, it seems ok. 2. The LED is actually cut from a strip-reel that has a resistor for each LED and it is specified to drive it at 5V. I will be routing wires from the PCB pads to place the LED in another location. 3. I have been testing with the n-4 version of lm386. I had trouble getting good quality sound at high volume unless all the extra capacitors were added, I have it set to 50 gain, but it does pick up some low frequency noise and clicks slightly when the LED flashes. I didn't know I had ordered the n-4 version until a few days ago. However I'm afraid if I use a different one I won't get as good performance? Or should I expect it to be better? Could you explain why not to use the n-4? I see it is for 32 ohm speaker, that is probably the cause of my sound problems as my speaker is 8 ohms? 4. I tested with a 2N7000 mosfet and found that the Drain-Source voltage drop was higher than the PN2222 interestingly, I was disappointed! I will try the 2N7002. 5. Ok. 6. I was planning to replace the pot with a single resistor instead of a voltage divider, do you think this could work, I know the current is very minute but I don't know how much, haven't tested it yet. 7. Yes I will fill in the BOM, it was just a start. PCB Layout: 1. I haven't made a copper area before, this sounds like a non-trivial task, is there a good set of instructions for how to do this? Does this affect the price much? 2. I have been working with solderless breadboard until recently, I don't have a SMD mounting station. I may just have the whole board assembled maybe I'll check the cost. I was going to actually use IC DIP sockets so I can reprogram the chips until all is right, do you think the sockets should fit in their place? 3. I designed the board to fit in a 2"x2" square that has sharp corners but they are not necessary, this is a good idea mainly to avoid handling pain? A last question for you, have you worked with capacitive touch inputs before, do you have any advice for using this technique? Thank you very much! There are many more parts than I expected to make this work, do you think the # of capacitors is normal?

I'm sure you caught that my list numbers got rearranged somehow, I thought I had it right, sorry about that, I don't see an edit post option!

I am pretty unclear about the copper fill / plane design process - could you possibly point out what the different symbols mean at at various pads and vias in: https://easyeda.com/normal/The_EasyEDA_C64_Overvoltage_Protection_Circuit_PCB-bYuM4mEyQ.png?

#### Battery: If you have a battery with wire ends already attached then soldering it to the PCB is fine. It's just that soldering wires to a normal battery terminals can be very dangerous. To make a suitable PC footprint for that is easy. Just open a New PCB Lib page, draw an oultine on the top silk layer for just grateer than the max quoted external dimensions of the battery (include tolerances), add a marker for the `+` (and if you like the `-` end too) and then place two `Round`, `All layers` pads with hole sizes a bit bigger than the battery pin diameter. Job done. You could try looking for `battery` in the SHIFT+F search. That may turn up an outline that is close enough that you can edit and save as your own. #### Schematic: 1) It is good electronics practice to individually decouple each chip. You said yourself about the LM386: `but it does pick up some low frequency noise and clicks slightly when the LED flashes.`. Some of that may be bad layout due to the use of perfboard but some of it may well be poor supply decoupling. The LM386 is actually quite touchy about decoupling and layout anyway. At least put the parts into the schematic so they end up in the PCB then if you can get away without them you can just not fit them. Far better that way round that finding you need them with no place to fit them on the PCB. 2) OK with the LED if it has an internal resistor. 3) LM386-4 is for a 5V to 18V supply. You have a 6V battery so you have very little margin before the battery gets so low it starves the 386-4 of supply voltage. The 386-2 is rated at 500mW into 8 Ohms and runs off 4V to 12V so will carry on at lower battery voltages. You need to read device datasheet very carefully! :) The 386-2 should do better in your app. 4) Really? How much current does this LED draw? 0.25W at 6V implies a bit over 40mA. 50mA at 5V. A 2N7002 should have no problem supplying that with a 4.5V gate drive: https://www.nxp.com/documents/data_sheet/2N7002.pdf Essentially you need a logic level input MOSFET. There are better devices than the humble 2N7002 but they may cost more and be harder to source. I suppose if the device is essentially disposable then maybe the 5mA base current for a 2N2222 isn't an issue. 5) Use R3 and replace pot R5 with a single resistor then use whatever value you find you need for C2 (I don't know what your low pass filotering criterion is so I can say what value). Keep the total series resistance of R3+R5 to no more than 10k. (Refer to LM386 datasheet again). #### PCB 1) Copper area is easy. Set which layer you want to put the copper area onto then go to the `PCB tools` pallette, click on `Copper Area` then drag a rectangle around your PCB. It can be a little in from the board outline but in fact EasyEDA will crop it to suit even if you draw it to extend outside the PCB outline. Then assign it to your ground net or to `VCC` as required. Then click on `Rebuild copper area` (in the right hand panel as you have the copper area tool open) To see it you need to set `Copper Zone` = Visible in the PCB canvas properties (Right hand panel again). You just need to ensure that the copper area has continuity to reach all the gound or VCC pins without being piched off or so thin it might as well be. Hence the advice to manually route any traces as required to achieve this. Copper areas do not affect price. :) 2) As long as you have a good soldering iron with a small (3mm or less) tip and a good quality pair of tweezers, you may find it faster to assemble using say 0805 resistors and 100nF cap parts. You only need to spot solder onto the pads for one end of each part, offer it up with the tweezers and then remelt the solder at one end then spot solde on the other and it's doen. No messing about with bending and pushing wires then renbending them to stay in place as you turn the PCB upside down and solder them then crop them off... :) It takes a bit or practice and do buy spares as some parts will inevitably ping off the tweezers into space! Don't be afraid of using vias to route traces since you have fewer through holes to use instead. Again, on a board like this, via count has no effect on price. Sockets for parts where necessary: up to you. With DIP parts it's a good plan until you have sorted out programming anyway. 3) Rounded corners are a nicety and look a bit more professional. Attention to detail and all that. I don't have a lot of experience with touch switches and the like. I couldn't make out where that is on your schematic anyway. Does this help? https://easyeda.com/forum/topic/making_a_touch_pad-tlUu42Cc9 #### On the number of caps. Don't skimp on decoupling. It can come back to bite you and usually does. If you are set on using the LM386 then you are stuck with the number of caps as it must have an input, an output, one in a Zobel network (C5) and one in the gain setting path (C6). What waveform is the LM386 amplifying? If it's just a series pof pluses than maybe you just need a simpler way of driving the speaker. If it's more complex audio then the LM386 is good enough as it's cheap and readily available. You could look at Element14 to see what else is available. RS: http://www.rs-components.com/index.html offer free delivery even for silly small quantities in the UK (no idea about elsewhere) and for your 100 off may be a good choice for good quality parts. #### About Copper Areas. See above and please look carefully at the schematics and PCB layouts for the projects I linked to. Clone them then play with them to see how the areas work. The `gun sight` thingys by the way are mounting holes (see the `PCB Tools` pallette) but note that they are in the schematic too as otherwise you have to add them back in every time you make a change to the schematic and then update the PCB!

Thanks again very much for all of the help. The LED does draw 40mA. I didn't see a -2 lm386 on the datasheet but I ordered the -1 and -3 to test. When I measured the voltage across the LED I{ found with transistors (I tested 6 of them) the collector voltage was around .4 to .5V when the transistor was on. With the 2N7000 the drain voltage minimum was 2.4V. My notes say the LED was dimmer but I may not have been testing with gate/base resistors, I'll retest. I have a lot of work to do, thanks.

`The LED does draw 40mA.` So that should drop < 200mV across the Rds_on max of 5R of a 2N7002 with a Vgs of 4.5V. Compared to maybe 100mV for the Vce_sat of a 2N2222. Negligible difference for a 5mA saving in battery current by using the MOSFET. `When I measured the voltage across the LED I{ found with transistors (I tested 6 of them) the collector voltage was around .4 to .5V when the transistor was on. With the 2N7000 the drain voltage minimum was 2.4V.` The figures for drain source voltage at different gate voltages and drain currents in this datasheet give a bit more insight into why that might be: https://www.fairchildsemi.com/datasheets/2N/2N7000.pdf Looks like the 2N7000 is a better option than the 2N7002 but overall a version of the 2N2222 might simply be cheaper. `I didn't see a -2 lm386 on the datasheet` Sorry, my bad. I meant LM386-3. FWIW: To see how to get the best out of the LM386, you can play with simulations of it by cloning: https://easyeda.com/example/Demonstrating_the_EasyEDA_LM386_spice_subckt_model-pgoiAgM4m * One thought: as I'm sure you're aware, if you go SMD then you can make the PCB smaller and that does affect PCB cost. Smaller = lower cost. Have you checked the PCB cost through EasyEDA? :)

Thanks for your continued support. I have an updated schematic and PCB now with many changes, it is halloween_toy1_4. Questions: 1. How should I handle the decoupling capacitors; with the VCC and GND planes they just attach to the plains when using the autorouter. What do you recommend? 2. Is it possible to route some traces then have them saved and not changed when the autorouter runs? 3. How do you widen some track widths when there is a copper area surrounding them? Can the widths be saved if the autorouter is re-run? 4. What do you think about the overall design? Thanks!

1) You have assigned both the top and bottom copper areas to GHD. a) Assign the top to GND and the bottom to VCC. b) Move the all GND traces to the top layer and all VCC traces onto the bottom layer. c) route VCC and GND traces so that they enter and leave pads at 0, 90, 180, 270 deg points so that they align with and are covered over - with the heat shunts in the copper areas. Use 6 mil traces for VCC and GND if they are wider than the heat shunts. Thin supply taces used in this way are OK because the copper area actually supplies all the grunt copper. d) then rebuild both copper areas. This will get rid of lots of unnecessary tracks to supply pins. A handy trick is to assign GND on the top layer so that you have a large ground are on which to place some dummy pads to create you some small solder mask free areas to put meter and scope ground probes onto. 2) The autorouter offers you the chance to mark nets to be left unchanged by the autorouter run using the `Skip Nets` dialogue. It also allows you to mark traces as `Special Nets` and to then define particular widths and clearances when they are autorouted. That said, I very rarely use the autorouter so I'm not absolutely sure how the features work. Autorouters are OK but even in simple circuits they can lead to some serious problems that can easily be avoided by learning some good PCB layout skills and practice. OK, it may take longer to route a bourd by hand but you can avoid a lot of potential issues due to an autorouter making poor routing choices and maybe even a PCB respin... :) 3) Change the widths then rebuild the copper areas. If the copper areas get pinched off then reroute. (You begin to see why it is largely a waste of time autorouting?). 4) The layout is getting there, you just need to refine your layou skills a bit. There are other things to tidy such as optimising track routing. For example, look at the routing to R2. If you simply rotate R2 by 180deg the routing tidies up quite a bit. Also look at how the autorouter has routed tracks out of pads that then blocks free copper around pins that connect to the planes; e.g. the ground pins of C8 and Q1. An autorouter doesn't teach these skills, so you can't tell when it has done something silly or that is just bad practice. These articles are quite helpful: http://michaelhleonard.com/how-to-design-the-perfect-pcb-part1/ http://michaelhleonard.com/how-to-design-the-perfect-pcb-part2/

There seems to be a lot of problems with the website today. I{ could not load the webpage for several hours, now it won't run the autorouter it says there is a network error. Can you please fix this?

The site is working now. Is there a way to prevent the autorouter from routing certain portions of a multiple-track net? Specifically I would like to prevent connections between certain pads and prefer others. Thanks.

Andyfierman - I hope you are still available. I would like to place a new component onto the schematic and PCB without remaking the entire PCB. Is this possible?

`Is there a way to prevent the autorouter from routing certain portions of a multiple-track net?` I don't think you can do that directly in the AR. You could try renaming parts of a trace before you run the AR then setting the names back again. Risky because you have to rememebr to reset the names but it might work. I used this trick of temporarily renaming parts of traces to get the Kelvin connection to the current sense resistor (R5) in the Uberclamp PCB without the Rebuild Copper Area just flooding all over them.

Ok thanks. I need to add a switch to the PCB. I added it to the schematic but I don't see it on the PCB, and I can't add the part by clicking the switch icon when in the PCB view. Can you tell me how to do this?

` I would like to place a new component onto the schematic and PCB without remaking the entire PCB. Is this possible?` That's easy. :) Do your schematic editing - including assigning a package to the new part(s) - then go back onto the PCB page and click the `Import Changes...` icon (immediately to the left of the AR icon): ![enter image description here][1] * Be careful though: once you accept the changes you cannot undo them. Save a copy of your PCB before you import the changes and give it a different name (add a suffix or a version number or a snapshot date and time) so that you have a simple way to go back if you get into any trouble. [1]: /editor/20160907/57cf3d4cc13c8.png

FYI the most up to date PCB design is actually halloween_toy_1_5.

The later **halloween_toy_1_6** is looking good but there are some things that need to be fixed. * Have you added the switch by hand? The +ve end of the battery is still labelled as VCC which is bypassing the switch in the PCB whereas your schematic **halloween_toy_1_1** shows the correct connectivity. Note that for Import Changes to work, the PCB to be forward annotated (updated) from the schematic must be the one that was originally created from that schematic (ideally they should have the same name). So whilst saving snapshots with different names is OK, forward annotating a PCB from a schematic can only be done when they have exactly the same name. Ah. I just took a copy of your schematic **halloween_toy_1_1** and your PCB **halloween_toy_1_6**, put them in a new project, renamed the schematic to **halloween_toy_1_6** and then did an `Import Changes...`. Big problems because the schematic does not have all the right package names in it compared to the PCB so it shreds the layout. For instance, the switch and the battery packages in the schematic do not match what is in the PCB so when you do `Import changes...` what is in the PCB gets replaced with what is called up in the schematic. You need to go back to the schematic and update all the package info so that they now match what you have already put into the PCB so that those elements are no longer seen as changes (i.e. differences) between the schematic and PCB. ### In the schematic: Update the battery package from `BATTERY` to `2CR1/3n 6V Battery`; Update the switch package from `TACTILE-PTH` to `slide_switch_1`. ### Edit your PCB Footprints: Update the prefix for `2CR1/3n 6V Battery` from `U?` to `V?`; Update the prefix for `slide_switch_1` from `U?` to `S?`. If you do that and then rename the schematic and the PCB to, say, **halloween_toy_1_7**, when you next do `Import Changes...` everything should be OK and very little will get trashed (the battery footprint shifts maybe because you have edited the package origin since you first placed it on the PCB?). Then, set the power traces as I described earlier so that they line up with the heat shunt spokes then redraw and reapply the VCC copper area (it's gone from halloween_toy_1_7 and the GND copper area is on the bottom).

How do I modify the package type and BOM? Sorry I have been working on a difficult problem related to this project that was top priority. I have heard conflicting opinions about the copper areas, some say only a ground plane on the bottom side and no VCC plane, what is the difference in functionality/performance/safety/reliability for using different planes on different sides of the board? I was able to import the changes without any problem to ver6.

`How do I modify the package type and BOM?` 1) Find the packages you want by doing a SEARCH+F library search; 2) Click on the little heart icon for each one to add them to your `Favorite Parts` list; 3) Highlight the part for which you want to update the package in the schematic; 4) Click in the `package` field; 5) Filter for the package you want in the `Update the symbol's package` dialogue that opens (scroll up the dialogue box if the Filter box is not visible); 6) Click on the package you want; 7) Click `Update` at the bottom of the dialogue. This tells you how to add additional information that appears in the BOM: https://easyeda.com/forum/topic/How_to_add_extra_information_to_the_Bill_of_Materials_BOM-Hp9rJCUcu `what is the difference in functionality/performance/safety/reliability for using different planes on different sides of the board?` For your PCB, which side the copper areas are on makes little difference. I suggested ground on the top simply as a convenience for being able to make uncoated, tinned ground pads readily available for meter and scope probe grounding points. As I said before, copper areas can help balance top and bottom copper distribution to minimise warping in manufacture. On a small, 2 layer PCB it probably makes little difference. More importantly, adding copper areas instead of tracks reduces the resistance of the supply and ground paths. Where decisions about the placing of ground and power planes makes more difference is on boards carrying high speed data and switch mode power signals. This is even more important for 4 layer and up PCBs. Making the right choices in those circumstances makes a big difference to EMC, Signal and Power Integrity but this is a much more complex area and much of it is beyond the scope of what we can provide free of charge in the forum. Signal and Power Integrity should not be too much of an issue for your design but since you are making these boards in some quantity and I'm guessing you may want to sell them, if you are concerned about meeting EMC requirements then please contact support or there is a lot of useful information on the web.

Thanks. I won't sell the initial version but I hope to have another version that I will offer for sale. As far as the frequencies utilized, an audio signal is produced from u1 as a PWM signal running at 250MHz but it is low pass filtered directly out of the MCU. The audio itself is sampled at 8kHz. The LED has a minimum on or off duration of 1ms. There is I2C communication between u1 and u2 running at 400kHz attached to 2 pull up resistors to VCC = 6V. Would you change any of your recommendations based on this information?

1) `an audio signal is produced from u1 as a PWM signal running at 250MHz but it is low pass filtered directly out of the MCU.` 250MHz? Are you sure? That seems a bit high. 250kHz is more what I'd expect. Put R3 and C2 as close as possible to pin 3 of U1 and make sure C2 is firmly grounded with a short ground return path directly back to U1 pin 4. 2) Increase R3 to 1k and reduce C2 to 10nF to reduce current drawn from U1 during rise and falling edges of PWM signal This will slightly reduce that maximum volume from the LM386 (because it is roughly 1k rather than 100R in series with the 10k pot) but reduces the risk of radiating edge noise at the PWM frequency. 3) Increase width of VCC track U3 pin 6 to C4 +ve pin (have you given up on having a VCC copper area?) 4) Keep U1 and U2 as close as possible, minimise the length of the I2C traces and keep the pullups close to U1/U2. 5) Return the VCC end of R1 and R2 directly to C7 or C8 to minimise the ground return path for edge currents of I2C signals. Note that the falling edges of I2C are orders of magnitude faster than the rising edges. 6) Keep Q1 and D1 close and connect C9 directly across D1 anode and Q1 emitter. I probably don't need to but I'll point out anyway that you can minimise all these signal path lengths and get everything closer together using SMD.

Oops that's supposed to be 250kHz, and it is generated by an internal phase-locked-loop clock that runs at 64MHz the way I have it set up, and is a special feature of the ATtiny85 as I understand it.

Andy, 1. I noticed my PN2222 BJT was wired incorrectly. I had the emitter and base switched. When I switch them correctly, so from left to right the pins are E-B-C, the emitter pad is not rectangular, should they all be round? Is there any reason for it to be rectangular? Thanks. 2. Someone mentioned that the heat shunt copper areas on the ground plane were large and it might be hard to solder. Can the size of the connected areas be changed? 3. For S1, I attached the unused pins to GND. So now when the switch is turned off, the VCC side of the circuit is immediately connected to ground. Is this something you would recommend or do you think it have the potential to cause harm? Thanks, Stephen

1) First check the pinout of PN2222 here: http://www.onsemi.com/pub_link/Collateral/PN2222-D.PDF The PCB footprint has pin 1 as a square pad: ![enter image description here][1] Next, in the schematic, select Q1 then press the `i` key. Edit the PCB pin numbering in the pin map as shown below: ![enter image description here][2] Then click `OK`. That sets the pin numbering of the schematic symbol so that it matches the (correct) pin numbering of the PCB footprint. The square pad has no significance other than as a visible reminder that - in this case as it obviously may be different for other TO-92 packaged devices - this is the emitter pin. The silk screen serves as the package orientation guide. FYI: to give room to route between the pins I created a TO92_TRIPOD PCB footprint for a few devices: https://easyeda.com/example/component/2N3906_TO92_TRIPOD-O08ExrlDV?from=editor https://easyeda.com/example/component/BC547_TO92_TRIPOD-NLvNBCA60?from=editor https://easyeda.com/example/component/BC557_TO92_TRIPOD-iSoUqkewN?from=editor https://easyeda.com/example/component/TL431AILP_TO92_TRIPOD-dRnFXR9rI?from=editor https://easyeda.com/example/component/TL431AILP_TO92_TRIPOD2-irN9vfAWG?from=editor 2) Good question. I had vaguely noticed that the width of the shunts appears to be proportional to the size of the pads but I am not sure. I will try to find out if that can be fixed to limit heat shunting. 3) The risk is that you change the switch supplier which unbeknown to you instead of being break before make, is make before break and you short the battery to ground when you turn the board off. and that welds the switch contacts shut and detroys the switch, the PCB traces and the battery. There's no need to connect the unused switch pins anyway. [1]: /editor/20160916/57db0b7227dad.png [2]: /editor/20160916/57db0c5df27f0.png

Thanks Andy. What is your recommendation as far as soldering SMD capacitors and resistors, for a sort of 1st time PCB assembler? For example I was looking at the 1206 package for the .1uF decoupling capacitors. Stephen

Andy can I use the tripod footprint? if I click on it nothing happens if I click on place or edit. Or could you tell me the dimensions you used for it ?

One more question, I saw that in another design the transistor solder pads were oval to give more clearance, they spoke about solder mask swell, and that there needs to be enough soldermask between the pads. is there a way to see this in EasyEDA?

About soldering SMD, from a post about 2 weeks ago: > 2) As long as you have a good soldering iron with a small (3mm or > less) tip and a good quality pair of tweezers, you may find it faster > to assemble using say 0805 resistors and 100nF cap parts. You only > need to spot solder onto the pads for one end of each part, offer it > up with the tweezers and then remelt the solder at one end then spot > solder on the other and it's done.

I will order some with and some without and let you know. Is there a tripod transistor foot print I can use or do I have to draw it? Do you think the soldermask is sufficient between the transistor pads?

EasyEDA automatically defines the solder mask so you don't need to worry about that. For a simple PCB like this the default solder mask will be fine. Oval pads are usually just to give a good solder land whilst still giving enough space between pins. Same for rectangular pads. If you get into the details of pad design you'll find that there's a lot depends on the soldering/assembly process as much as the device package and the PCB fab house rules. Are you hand soldering the later PCBs? Did you know you can ask EasyEDA to kit them and assemble them for you? Email support for more info on this. I dare say we might even be able to include actual PCB design for a 100 off sort of quantity. :? Not sure why you can't place my tripod footprints. Looking into that.

I got a quote for assembly at another supplier and it was way way too expensive but I'll give EasyEDA a shot. I'm finding that my design (component selection) is leading to high costs.

If you want to discuss target costs and ways to cost reduce the design we be able to help out there too. Things like the choice of battery and LED and a few more things. Probably best done via support rather than on the forum.

Andy thanks I contacted the support email and we are in communications now. The LED BTW is not costly by the reel, ~$0.15. My 5 highest cost items so far in descending order: battery, speaker, MCU, PCB, and EEPROM. As you mentioned I imagine an entirely different design is required for higher volume production if the opportunity becomes available.

@Perigalacticon have you get our email about the quote?

Yes I did, the assembly prices are favorable, however I am hesitant to order until I have tested the prototypes which I hope will arrive soon. Thanks

Hello, I just wanted to thank everyone for your support, I received the boards and they worked flawlessly! They look great [see photo attached][1], are high quality and I am very happy for my first PCB to be a successful design with your help. Thanks again! Perigalacticon [1]: /editor/20161001/57ef4e525df24.jpg

Glad we could help you to a successful design and that you are happy with our tools and PCB quality. **:)**