Hi Bizit524, Welcome to EasyEDA. Small problem: the link you have given is to a private project so no-one else can see it. Please see **Sharing** in the Tutorial to see how to make it public. If you can also provide a spec describing what your circuit is intended to do and a "How it works" circuit description, that would be great. Thanks.

sorry about that I have now made it public. and added as much detail as I could in it on what things do. I am in the middle of updating the silk screen

my main area of concern is if I hooked up the relays correctly. I want to make sure they will trigger when the GPIO 2 abe 0 go high. I followed this schematic to the best of my ability http://i.stack.imgur.com/owR7U.jpg

Please helpnus to help you. A bit more detail about the individual components and modules/blocks would help. Please don't just assume that everyone else knows all about the parts you're using or that they have the time to go searching the web for data. :)

fair enough so put more labels in the silk screen?

I have added as many silk screen labels as I can and the pcb has a description as much on what every component is supposed to do

Here's an example of what I mean about providing more details about the parts you are using. You have asked if the relay can be driven OK by the circuit you are using. You have not given a link to a datasheet or to the relay. It is therefore not possible to give an informed assessment of whether that part of the circuit will work.

ahh ok. I will get all this information ASAP. I really appreciate you working with me on this.

In the meanwhile, you might like to have a look at this thread: https://easyeda.com/forum/topic/first_time_PCB_maker_project_advice_-SUO60izRL It will give you some pointers in how to deal with ground and supply planes. Don't worry that you can't see the project it is discussing: the other references should be enough to make sense of the basic ideas.

## Caution!! One very important point to bear in mind is that you appear to be carrying mains voltages on your PCB. **Mains voltages can kill.** Before attempting to design anything carrying these voltages you **must** make sure that you fully understand what you are doing. You must design the PCB with sufficient creepage and clearance distances for the voltages and sufficient trace widths to carry the respective currents. If you are in **any** doubt about this part of the design then you should stop at least until you have thoroughly researched the necessary design rules and standards.

Andy yes you are correct there are mains voltages on this. I understand the risks, while I am no means a professional electrician I have taken a few classes, helped my dad wire his house he was building a while ago and always use the proper safety equipment and tools as I have a lot of hand me downs from my grandpa which was an electrician for GE :) :) thanks This is why I am asking for help when it comes to mains voltages on PCB because since I am not a pro I do not know the proper clearances on a PCB so any input would be great Based on the link you submitted I am guessing I would need to add ceramic caps next to the PSU? I have updated the public description with as many datasheets I could find with the corresponding devices I use. I left the diodes (d1,d2 ) blank because I am not sure which one to use. suggestion appreciated

First, for more on creepage and clearance, try searching for: `creepage and clearance distances iec` and `creepage and clearance distances pcb` `Based on the link you submitted I am guessing I would need to add ceramic caps next to the PSU?` In your case no because you are buying a ready made PSU module that will have any necessary output (DC) decoupling.

Thanks for this. I will research this. For the diodes what do you suggest? Honestly I haven't a clue as I was just following a schematic online that did not specify what it was . It was actually this https://www.google.co.uk/search?q=SRD-05VDC&num=100&source=lnms&tbm=isch&sa=X&ved=0ahUKEwjlg9eGqYrPAhWDDcAKHVWzAM0Q_AUICSgC&biw=1309&bih=653#imgrc=S_WF0kGiEPWecM%3A also based on the diagram I linked the the components I have since linked do you think the relays will trigger correctly when pins are high? / did I even wire it up correctly?

The flyback diodes for the relay (D1 in http://i.stack.imgur.com/owR7U.jpg) can be low power parts such as the 1N4148. It's made by lots of people. Here's an example: https://www.nxp.com/documents/data_sheet/1N4148_1N4448.pdf * Sorry but there's a fundamental problem in your project which makes it really hard to comment on the design. You have two PCBs and one schematic. You also have this relay and driver circuit comprising the circuit shown in http://i.stack.imgur.com/owR7U.jpg but those components do not appear in the schematic in the project. The idea of a schematic is that it shows all the components that are physically going on to a PCB. Ideally the schematic contains all the information necessary from which to launch the PCB design using the `Convert Project to PCB...` button. As a minimum it must have: 1) All the components that go on that PCB (including mounting holes as described in some of the examples referred to in the thread I pointed you to earlier); 2) Part numbers for each part; 3) Correct package types for each part. Can you do a complete schematic for each PCB that shows everything that is on each PCB. If it plugs into the PCB then it does not need to be in the schematic for that PCB but if the stuff that plugs in is on *another* pcb then there need to be a *seperate* project for that schematic and PCB too.

Been looking a bit more at your description and links to parts data. There's a problem with your choice of the Hi-Link HLK PM01 100-230 Vac to 5 Vdc 600 mA converter. As stated in: https://skippy.org.uk/quick-look-at-the-hlk-pm01/ The First line looks impressive, ... how many people know that that sentence is meaningless! how do you know what the UL, CE requirements it meets if they don’t tell you which standards they applied! Looking at the unit, ... wire it into the mains and off we go? NO. for starts looking at the GA drawing we can see a problem... ...the AC input pins are 5 mm apart center to center, which means that it will be difficult to get the required 3 mm clearance between Live and Neutral required for BS EN 60335 – “Household and similar electrical appliances. Safety. General requirements” or any similar standard we wish to use. If you are only ever going to use this design on 120Vrms US mains then the input supply pin clearance *may* be enough. Otherwise it is not and extra circuitry is required to make the AC input pins safe at EU mains voltages (230Vrms nominal). Remember that the peak voltage is sqrt(2) (approximately 1.414) times the rms and that the tolerance on the mains voltage can allow it to increase to about 127.2V rms. **I would strongly recommend that you revise your choice of mains PSU adapter and/or input protection and fusing for this design.** **You must consider that you are making this design public and therefore you have a responsibility to make it safe for anyone to reproduce even if it is at their own risk.** BTW last time I looked at the schematic, it showed that the 5V and 0V outputs of the mains PSU were shorted together.

Thanks for the very detailed analysis of everything. to answer a few questions of yours *You have two PCBs and one schematic.* - I did not know this. Ha I thought people could only see one I made a different one just to mess around with. Please only pay attention to the one ESP not ESP DHT Mini. Apparently I share the whole project not just one PCB *1N4148* - Thank you for the suggestion of the diodes I will use that. I delved a little deeper into those as well and found a very similar one if not the same one your suggesting today a few hours ago. *Ideally the schematic contains all the information necessary from which to launch the PCB design using the Convert Project to PCB... button.* - yeah sorry about that I know its probably wrecking your brain just looking at it. I tried to do a schematic and would actually like to as that helps with auto routing however it didn't have all the components that I needed such as the HLKPM01 and the ESP8266-01 - They had a foot print for them but not a circuit made. Unfortunately I am not advanced enough make my own components it took me an hour to figure out how to make a footprint of a DC to DC buck converter *Can you do a complete schematic for each PCB that shows everything that is on each PCB.* - i will try my best but as I said it didn't have all the components :( :( *I would strongly recommend that you revise your choice of mains PSU adapter and/or input protection and fusing for this design*. - I will look for a replacement I saw another company that did a similar package that I think met the requirements youre stating but they were 5x more expensive that is why I went with this before knowing what you just told me :) *BTW last time I looked at the schematic, it showed that the 5V and 0V outputs of the mains PSU were shorted together.*- Would this happen to be on the 5t3bp jumper? that you're talking about? I know you can't tell that from just the PCB but that would have been just in case I switched from a 5v psu to a 3.3 PSU which would mean I wouldn't need the step down circuit (5t3). So I created a jumper which would automatically bypass the that and automatically feed into the rest of the unit. It is only active if you physically jump it across

`Unfortunately I am not advanced enough make my own components...` https://easyeda.com/Doc/Tutorial/creatingtheSchematicLibs.htm#Creating-the-Schematic-Libs https://easyeda.com/Doc/Tutorial/PCBLib.htm#Creating-The-PCB-Libs 1) You need to spend some time just playing about outside the project (start another) to learn how to do this; 2) To start with, pick a simple component such as a resistor, diode, LED or a bipolar transistor in the EasyEDA Libs; 3) Double click on it (in the left hand panel: do not place it in a schematic) to open it for editing; 4) Select the component parts of it to see how it is built up including pin lengths and styles, line colours and stroke widths etc; 5) Play with the `Grid size` and `Snap size` to get things aligned on (i.e. pins) or off (things like the wavy lines on the LED and the emitter arrows of bjts) the grid. Carefully document (add urls to datasheets, supplier and supplier part numbers etc., etc.) and save your edited parts. These will automatically be added to **My Parts** and to the **SHIFT+F** library. You can do the same thing with PCB footprints and, by clicking the `Edit` button, parts from the **SHIFT+F** search. `BTW last time I looked at the schematic, it showed that the 5V and 0V outputs of the mains PSU were shorted together.` ![enter image description here][1] [1]: /editor/20160914/57d8fef04b5af.png

OK thank you. What I am going to do, is stop sharing the project so no one downloads it as you said it was dangerous. I will try and teach myself the links you sent and get a schematic going. then I will get back to you on this thread when I'm done. (this’ll take a while) For the 3mm clearance that you mentioned with /linked to. does this only refer to each side of the board?. what I mean by this is the main terminals are on one side of the board and they need 3mm clearance all around can I add copper to the other side that is not part of the mains or does the 3mm clearance have to be both sides of the board?

`For the 3mm clearance that you mentioned with /linked to. does this only refer to each side of the board?.` You will need to read up on the required clearances for: (a) the mains voltage range in your application (and put HV warning labelling on it and a warning if it is not to be used above a certain voltage); (b) the IEC classification of the materials you are using (FR4 fibreglass); (c) the level of insulation you require (basic, supplementary, reinforced etc.). You only have 2 layers so that clearance **must** be applied to top and bottom layers around **any and all** tracks carrying these voltages (i.e. Live **and** Neutral before and after any connectors, fuses, overvoltage protection diodes etc.). The clearance must be applied to each track to all other tracks and not just to each other. If you cannot get sufficient creepage distance across the board, consider adding slots or cutouts in the PCB: http://www.pcbtechguide.com/2009/02/creepage-vs-clearance.html#.V9kW8ZgrI-U http://www.smps.us/pcbtracespacing.html but note that slots and cutouts do not increase clearance.

`I would strongly recommend that you revise your choice of mains PSU adapter and/or input protection and fusing for this design.` Seen these? http://uk.farnell.com/myrra/47152/power-supply-4-5w-5vdc-reg/dp/1825779 http://uk.rs-online.com/web/c/power-supplies-transformers/transformers/switch-mode-power-supply-smps-transformers/?applied-dimensions=4294965525#esid=4294956957&applied-dimensions=,4293260232,4294498886,4294965525 https://www.soselectronic.com/pcb-mount-ac-dc-converters?brand=MYRRA&sorter=param%3A80%3Adesc