Hi , Welcome to EasyEDA. For a first project in electronics this is a bit ambitious. It looks simple enough: convert a 13V to 15V input to a constant current drive to an LED using a dedicated chip. In practice however it is way more complex than that because you are using a switch mode power supply (SMPS) to do it. Designing an SMPS is a lot easier than it used to be but there are still a lot of rules that must be followed to get a working design at the end of it. There are two key things to understand about SMPS. They operate using very fast switching edges so they generate very fast voltage transitions (dv/dt) and they switch large currents at the same time so they also generate very large and fast current transitions too (di/dt). Combine the two and you have one of the worst possible design challenges in electronics. Large dv/dt means that there's huge potential for crosstalk from input and output signals to small reference and feedback signals. Large di/dt means that any inductance in the wiring, (i.e. PCB traces and component leads) will result in large voltage spikes and ringing that can not just disrupt how the circuit operates but can easily destroy devices. If the circuit operates incorrectly you are very likely to destroy the chip in a few us just because if it tries to switch a large current with any appreciable voltage across the switching transistor then the power dissipation in it will skyrocket and the die will either melt or just vapourise. Here are a few of the rules (but by no means all!). * Read and understand the manufacturer's design procedures. Do not rely on 3rd party design tools unless you can be sure of their validity; * Never try to prototype an SMP on "perf board". The tracks are nowhere near low enough resistance or inductance and they cannot handle currents that are encountered in SMPS circuits (even modest average output currents may require switching currents in the region of amps); * Always read, understand and follow the manufacturer's layout guidelines in their datasheets and apps notes (hint: start here: [http://www.ti.com/product/LM3404#](http://www.ti.com/product/LM3404#)). There are exceptions to this but your project is not one of them;  * Never omit any input or (unless explicitly allowed by the manufacturer's design guidelines) output smoothing or decoupling capacitors;  * Pay close attention to the manufacturer's guidelines on the different variants of device package that are available and any requirements for electrical and thermal connections to any pads that may be used for grounding and heatsinking;  * Ensure that the PCB footprint you have assigned to the schematic symbol matches that of the physical package that you have chosendevice that the and that the pins map onto it correctly. For more about footprints and symbols please read (2.3) in: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f) For more on the importance of decoupling capacitors please see: [https://easyeda\.com/andyfierman/Power\_supply\_decoupling\_and\_why\_it\_matters\_\-451e18a0d36b4f208394b2a2ff7642c9](https://easyeda.com/andyfierman/Power_supply_decoupling_and_why_it_matters_-451e18a0d36b4f208394b2a2ff7642c9) In your design you appear to have specified a chip with a central thermal pad and then chosen a footprint that does not accommodate it properly: your centre pad is not properly part of the footprint you have created, is not grounded and has no additional thermal vias. Similarly, the symbol you have chosen or created has no pin 9 and so has no way to assign a centre pad to ground. If you modify the footprint to add the centre ground pad, assign it as pin 4 rather than 9 (and yes, you are allowed to do this!) then it will be connected to ground in the PCB in the same way as GND on pin 4 of the device and you just have to track or flood ground into it. You then do not need to add the extra GND pin to the schematic symbol (the datasheet only shows the symbol as an 8 pin device). Your layout is some way off that recommended in section 10, Layout Guidelines in: [http://www.ti.com/lit/ds/symlink/lm3404.pdf](http://www.ti.com/lit/ds/symlink/lm3404.pdf) I recommend that you read the following as a starting point for learning about SMPS basics, then have a search for other stuff to get some different perspectives on it: [https://www.onsemi.com/pub/Collateral/SMPSRM-D.PDF](https://www.onsemi.com/pub/Collateral/SMPSRM-D.PDF)

Note also that: 1. your PCB has net names that do not exist in the schematic. It is better practice to put the net labels into the schematic so that they are carried across into the PCB when you first press the **Create PCB...** button;  2. You have changed the footprint for J1 and J2 in the PCB but not in the schematic. This is back to front. The footprint should be changed by changing the assignment of the footprint to the schematic symbol and then doing **Update PCB...** or **Import Changes...** If you change the footprint in the PCB and not the schematic then when you do **Update PCB...** or **Import Changes...** then the footprint in the PCB will be replaced by whatever the symbol has assigned to it. To help understand this, please see Design Flow in the Tutorial and (2.2), (4) and (6) in: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f)

This is a helpful site: [https://www.smps.us/](https://www.smps.us/)

And: [https://www.ibiblio.org/kuphaldt/electricCircuits/](https://www.ibiblio.org/kuphaldt/electricCircuits/)

Thank's for helping! I now see i should have referred to the LM3404 datasheet and that i've tried to my best ability to read and understand it. It evidently didn't go that well  lol... I'll try to be more specific and clear. Let me respond to what i think might be of value in regard this project and add a little more info: (keep in mind i'm no electronic wizard and much of the launguage used in datasheets like the LM3404's sounds almost like Greek to me. If i describe things with wrong therms try your best to decipher it) > In practice however it is way more complex than that because you are using a switch mode power supply (SMPS) to do it. For testing purposes i planned to use my bench power supply and didn't reflected on the consequences it might have driving electronic with a lot of feedback noise before i actually tried to hock up my constant current regulator to power the LED. Having experience with car electronics as an auto technician i realized this could be a problem and therefor i decided to test my circuit on a well charged car battery. This didn't work at first but i noticed that i occasionally got the LM3404 to switch on if i intermittently applied power to the input. To clear things up: This circuit is planned to be mounted in self fabricated lamps to my cabin. The lamps are going to be powered from a large lead-acid battery that is resupplied with electric power from a solar-panel control panel and a large Ctek battery charger. This means a typical voltage at 13,5volt and around 15volt when charging system kicks in (relay). I might need to ad a cap between voltage source and the constant current regulator circuit to smooth out the voltage spikes but since the LM3404 series is designed to be used in automotive applications i not sure if it's necessary? > Read and understand the manufacturer's design procedures. Do not rely on 3rd party design tools unless you can be sure of their validity Yes. I have looked trough the datasheet for the LM3404 and have a vage understanding of how it works and how to pick and place components. I tried my best to cross check between values given by the LM3404 calculator and the values given in the datasheet before placing my order. It's seems to me that the calculator give legit values but i'm in no position to say this for sure. > Never try to prototype an SMP on "perf board". The tracks are nowhere near low enough resistance or inductance and they cannot handle currents that are encountered in SMPS circuits (even modest average output currents may require switching currents in the region of amps); I had that in mind so i added strains of copper wire to the perf board and components to reduce resistance and tried to mimic the layout i have on the ordered pcb design > Never omit any input or (unless explicitly allowed by the manufacturer's design guidelines) output smoothing or decoupling capacitors; Hmmm. Yes probably here it went wrong. Thinking of it in hindsight i realize that was a pretty stupid move. lol. I better wait for the PCB's and the last ceramic cap to arrive before anything else... > Pay close attention to the manufacturer's guidelines on the different variants of device package that are available and any requirements for electrical and thermal connections to any pads that may be used for grounding and heatsinking; Also a significant problem yes! Didn't notice pad nr. 9. I think i'll manage to save the pcb's by slightly modify the boards. > Ensure that the PCB footprint you have assigned to the schematic symbol matches that of the physical package that you have chosendevice that the and that the pins map onto it correctly. I'm fairly sure that the rest of the solder pads are of correct package size in regard to the components i've ordered. > Similarly, the symbol you have chosen or created has no pin 9 and so has no way to assign a centre pad to ground. I have now fixed this problem. Have a look at pcb version 1.4 > Your layout is some way off that recommended in section 10, Layout Guidelines in: > [http://www.ti.com/lit/ds/symlink/lm3404.pdf](http://www.ti.com/lit/ds/symlink/lm3404.pdf) > I recommend that you read the following as a starting point for learning about SMPS basics, then have a search for other stuff to get some different perspectives on it: > [https://www.onsemi.com/pub/Collateral/SMPSRM-D.PDF](https://www.onsemi.com/pub/Collateral/SMPSRM-D.PDF) Thanks for the tip. I will need to have a look at this more closely. Appreciate your help! Thanks a lot!

> @andyfierman Note also that: > > > 1. your PCB has net names that do not exist in the schematic. It is better practice to put the net labels into the schematic so that they are carried across into the PCB when you first press the **Create PCB...** button; > 2. You have changed the footprint for J1 and J2 in the PCB but not in the schematic. This is back to front. The footprint should be changed by changing the assignment of the footprint to the schematic symbol and then doing **Update PCB...** or **Import Changes...** If you change the footprint in the PCB and not the schematic then when you do **Update PCB...** or **Import Changes...** then the footprint in the PCB will be replaced by whatever the symbol has assigned to it. > > > To help understand this, please see Design Flow in the Tutorial and (2.2), (4) and (6) in: > [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f) Yes i became aware of this functions late in the prosess and forgot to return to the schematics to fix the problem the correct way. Thanks for the tips and links!

Just realized that the project i've linked to was from an older project folder. I use the Easyeda in my Chrome browser and have by a mistake deleted the latest folder where a few design changes was made. This was done after i've ordered the pcb's from JLCPCB. Only thing left on my pc is the gerber files. I guess i should start all over again an redo everything but it would be neat if i somehow could import the gerber files back into the Easyeda tool. Is this doable?

Well i did some more reading in the forum and that option is not available it seems. I will redo everything manually with the sugested improvements by  andyfierman

Whoa! Check out: [https://docs.easyeda.com/en/Introduction/Basic-Skill/index.html#Histories-Record](https://docs.easyeda.com/en/Introduction/Basic-Skill/index.html#Histories-Record) and: [https://docs.easyeda.com/en/Introduction/Basic-Skill/index.html#Document-Recovery](https://docs.easyeda.com/en/Introduction/Basic-Skill/index.html#Document-Recovery) in: [https://docs.easyeda.com/en/Introduction/Basic-Skill/index.html](https://docs.easyeda.com/en/Introduction/Basic-Skill/index.html)

Great! Had to go to the recycle bin in: [https://easyeda.com/account/user/recycles/personal](https://easyeda.com/account/user/recycles/personal) Btw. Noticed that while opening files within different projects the Project folder and files in the left menu bar suddenly swaps places. That's probably the reason i managed to delete the wrong files. In my opinion a design flaw. A behavior by the browser-app that probably should've been adjusted.

More reading of the Tutorials needed... You can select how you want the projects listed:  and choose to pin any selected project to the top: 

Schematics looks weird but correct (mind not connected wires) to me. What I think is not correct is inductance of L1. You chose it to be 2.7uH. According to datasheet 8.2.1.2.1 and 8.2.1.2.2 with RON of 220k you would have around several hundreds Hz frequency and 2.7uH is too low for that. What values you entered into calculator exactly?

@egaistek I know. Looks weird because i started editing the shared schematics and should've made a copy of it instead and edit the copy instead. Haven't had time finishing what i started. Will have a look at it now. I will update this thread one's i'm done. Here's the numbers i used: Input voltage - 13 V Input voltage regulation (+-)  - 15 % LED forward voltage - 12 V LED current - 1 A LED current ripple - 0.1 A Switching frequency - 400 kHz

@firebird.formula.400, Having posted that information, please have a read through **If you are asking for help about a Project** in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) and then copy it into your Project Description section. :)

Take it easy now pal.I surely didn't come here to waste anyone's time.I asked for a bit of patient since i felt utside my comfort sone using this editor software and dealing with electronic terms i for the most part has to read up on. Not fully understand the complexity of this circuitry was one of my first mistakes and i've tried to my best ability to take in all of the above advice's. I just need time to go back and fix the errors i've made. Keep in mind i also have a life apart from this. I probably need a few days to go trough and read up on the things mentioned earlier. I can come back if you like and update this thread I fully comprehend the need for a bit of structure and rules in a forum and the moderators daily struggle with newcomers like me. I've moderated in an pc-support forum myself in the early 2k and know how frustrating this can be. What went wrong here is two sided of course and i've tried admitting my flaws and will hopefully correct some of it giving the time. On the other side we have this moderator clearly indicating to me what a pain in the ass i am for not figuring everything out beforehand and for not complying to rules and guidelines he probably expect me to have looked up myself. Can i now please ask for a bit of slack. I will have a look at this and correct stuff when life away from keyboard allows me to...

@firebird.formula.400, Sorry, if it came over that way but I wasn't having a go at you. I thought your post with what amounts to a basic design requirements spec was a good lead in to suggesting that you could capture some information that could help anyone else who came across your project. I certainly didn't mean to sound all moderately and school marmish. :)

Updated my project description! A direct quote from it: > _30.04-2019 All parts have finaly arrived and i've finished two LED driver sircuits. Solderjob have been veryfied with magnifying lens and multimeter._ > _Results are pretty much the same as before. Seems to me that the power MOSFET inside the LM3403 briefly swithes on and then turns off._ > > _04.05-2019 Found that Texas Instrument has this neat web tool for choosing and designing driver circuits: [Webench Power Designer](%5Bhttp://www.ti.com/tools-software/design-center/webench-power-designer.html%5D(http://www.ti.com/tools-software/design-center/webench-power-designer.html))_ > _I put in the same values in this tool and out come a totally different values on the passives controlling on and off time of the MOSFET. I'm not to confident in the vallues i've initially set for this sircuit. I might have misunderstood a thing or two in regard to LED forward voltage and how this value is used in the calculation of the passives._ > > \*08\.05\-2019 Using TI's web tool i played around with different inputs \(Vf\, Vin\, If \) and did some more reading\. I then realized what got me stuck\. An LED's voltage forward has been described all around on the internet as the voltage needed to start letting current flow trough the diode matterial\. This was the voltage i previously used for calculating the circuit\. I now realize that the LED Vf needs to be picked from an IV curve diagram \(or by testing\) and must always be used in relation to the LED If\. Figuring this out I have now printed out a graph paper and plotted the IV\-curve\. A reasonable If and Vf could be set at 0\.8A @ 11\.6V\. Putting in these numbers in the TI's Webench i was no longer able to choose the LM3404 as controll unit in my sircuit\. However lowering the If to 500mA @ 11\.2V finally let me pick the LM3404\. Seems like my initial pick of the LM3404 was a bit hasty and it's not capable driving full effect on the LED with only 2 Volts or so in headroom\.\* > > \*I'm currently considering bying other high power LED's with lower Vf to make use of my prototype PCB's\* If anyone is interested and uses the TI Webench i have made the 500mA design public at this link: [Design # 6 LED driver 500mA](https://webench.ti.com/appinfo/webench/scripts/SDP.cgi?ID=06CAC4FAA264FE7D) I realize this ended in a massive failure but i know i've learned a ton these past weeks. And what do i know maybe i will have a working version of this one day. If anyone have any thoughts and suggestions please leave a comment