my first pcb any mistake - Page 1
Forum section: electronics / beginners

author: pomme
author_rank: Contributor
timestamp: April 13, 2022, 02:10:05 pm
content: hello I made my first pcb and would like to know if I made any big mistakeit's a pcb for a soldering station based on this schematicI used lines of 2mm because the pcb will be powered with 24V 6A from the red square, but because it's not constant I think 2mm is enoughthe other line is 0.2mmthe blue square is a buck converter and the orange is for earth connection because I use a one side pcbthanks for your replies

author: free_electron
author_rank: Super Contributor
timestamp: April 13, 2022, 02:57:15 pm
content: electrons in = electrons out. so both lines need to be wide !the to92 transistor footprint is garbage. you'll have immense trouble soldering and or drilling that. the pads will peel off the bord.

author: eugene
author_rank: Frequent Contributor
timestamp: April 13, 2022, 03:01:46 pm
content: Without checking many details, I can see immediately that current return paths are too narrow. For example, look at J2 where the power enters the PCB. The 24VDC trace is a fat 2mm, but the ground return trace is only 0.2mm, yet the same magnitude current must travel through both traces.You need to consider current paths (often loops) not just voltage levels.

author: tepalia02
author_rank: Regular Contributor
timestamp: April 13, 2022, 03:07:14 pm
content: I agree with the above answerers.

author: pomme
author_rank: Contributor
timestamp: April 13, 2022, 03:20:58 pm
content: Quote from: free_electron on April 13, 2022, 02:57:15 pmis widening the line until the seconde capacitor enough ?for the to92 transistor should I widen the outer circle or narrow the inner circleand thanks for the "electrons in = electrons out" I didn't know that

author: free_electron
author_rank: Super Contributor
timestamp: April 13, 2022, 03:32:43 pm
content: and your buck converter has an unconnected pin.you need to widen the entire path through the power mosfet , through the inductor all the way to the output connector and back to the input connector.

author: mariush
author_rank: Super Contributor
timestamp: April 13, 2022, 04:25:15 pm
content: I would say don't use TO-92 transistors at all ... use surface mount footprints ... the pads are big and you'll have no problem soldering it to the PCB. The PCB is big enough you have lots of space even to use a DPAK / TO-252 version of the mosfet.You could have J2 on the same side with J1 and have shorter thick traces.You could orient the resistors the same way and route better to make it look prettier.What's R3 doing? does it have to be 3w/5w rated or whatever size that is? I don't see R3 in the schematic.3v zener ? I suspect it will be kinda harder to source a good one.I assume you're gonna have the whole back side copper fill ground otherwise use thicker traces on top for ground.

author: golden_labels
author_rank: Super Contributor
timestamp: April 13, 2022, 04:33:35 pm
content: The pictures show traces on the same side as components are. Is that for illustration only or is that the actual design? If it’s really like that: you will have nothing to solder the components to. That would be a major mistake, though you wouldn’t be the first — uncountable facepalms happened in the past for that reason.

author: eugene
author_rank: Frequent Contributor
timestamp: April 13, 2022, 05:04:02 pm
content: Quote from: pomme on April 13, 2022, 03:20:58 pmCurrent must follow closed loops. If it goes out the positive terminal of a power supply (battery, voltage regulator, whatever) then the same amount of current must go in the negative terminal.I've highlighted the current loop in magenta. (Sorry it's hard to see. I am using a simple tool to edit your drawing.)The current starts from pin 2 of the 5mm connector 24V_FROM_POWER_SUPPLY (or BUCK_CONV_IN), travels through Q1, L1, and out pin 1 on the SOLDERING_IRON_CONNECTOR.The same current then comes back in through pin 2 of the SOLDERING_IRON_CONNECTOR, through the current sense resistor R9, then returns to pin 1 of 24V_FROM_POWER_SUPPLYthrough ground. The traces along all of those paths must be able to handle the full current, not just the +24V node between the power supply and Q1.Study the edited schematic until you see the current loop.

author: free_electron
author_rank: Super Contributor
timestamp: April 13, 2022, 05:49:42 pm
content: the fact that there is an inductor and recirculation diode lets me believe this thing will be driven with PWM . the reciculation diode current is large. so there too you need wide traces.overall part placement and routing is a very bad in this.

author: strawberry
author_rank: Super Contributor
timestamp: April 13, 2022, 07:47:58 pm
content: 1...2mm signal tracessolder pads diameter enough to solderneed to think ahead on how it will come together

author: pomme
author_rank: Contributor
timestamp: April 13, 2022, 11:44:15 pm
content: Quote from: mariush on April 13, 2022, 04:25:15 pmfor now I have purchased all the component so I would like to build this one first because I don't have a good soldering station (I have an iron that you plug to main)R3 is R9 on the schematic Kicad attribut different R than the one on the pdffor the zener I brought from china I hope it going to worki'm gonna use thicker tracesQuote from: golden_labels on April 13, 2022, 04:33:35 pmyes it's for illustration only, Kicad did it this wayQuote from: eugene on April 13, 2022, 05:04:02 pmthanks a lot I understand a little bit more how it works nowand magenta was perfectQuote from: free_electron on April 13, 2022, 05:49:42 pmindeed it's PWM but to be clear it's not me who desinged this it's a youtuber named sasiskas and since I need a soldering station I said way not make this onefor the part with recirculation diode is what I did in the edited schematic good ?I will also put the complet schematic

author: golden_labels
author_rank: Super Contributor
timestamp: April 14, 2022, 03:54:56 am
content: No, it is not good. Forget for a moment about track thickness. Draw loops for the current through the soldering iron. Keep in mind loops are closed.

author: free_electron
author_rank: Super Contributor
timestamp: April 14, 2022, 04:03:32 am
content: I took some time to draw a proper schematic to show you.Schematics need to be clean , readable and convey the design in a clear fashion. the key parameters of components need to be show( voltage, tolerance , value )Nets need to be labeled so they are easy to find during layout.Layout the parts in such a way as to minimize the connections.Junctions only happen a T-splits. Crossing wires NEVER junctionNetnames are used to name nets , not to infer connection ! Wires are for connections.

author: mariush
author_rank: Super Contributor
timestamp: April 14, 2022, 06:16:35 am
content: QuoteIf all you want is a soldering station, maybe it would make more sense to use a schematic from an existing soldering station.For example, it would probably be cheaper to use the ancient Hakko 936 schematic. You can buy compatible hand pieces for a few dollars on eBay, and 24v AC transformers are easy to find and you could replace some components with alternatives (like for example replace the 5.1v zener diodes that are used to produce the reference voltage with 7805 and 7905 linear regulators.Here's the schematic and circuit board layout :http://dalincom.ru/datasheet/HAKKO_936_schematic.pdfExample of handpieces :https://www.ebay.com/itm/224544111810You could also get the whole circuit board and faceplate with potentiometers and handpiece connectors for 8-9$ :https://www.ebay.com/itm/381997375434- you just need to add a 24v / 2x12v 60VA (or more) transformer and the handpiece and you're good to go.

author: strawberry
author_rank: Super Contributor
timestamp: April 14, 2022, 07:46:51 am
content: R1 without divider, clamping diode D3 will limit output voltage range to 0..3.3V

author: nvmR
author_rank: Regular Contributor
timestamp: April 14, 2022, 09:09:13 am
content: OP, add some mounting holes and a revision number, and a place for a serial number. Very useful for the future

author: golden_labels
author_rank: Super Contributor
timestamp: April 15, 2022, 06:22:31 pm
content: pomme:you weren’t responding for some time now. I hope you didn’t get discouraged. Don’t be worried about making mistakes: as long as you try to understand and work it out yourself, not one will think bad of you.Even if you go for mariush’s suggestion to use Hakko-compatible board, try solving your original problem. This will teach you, how to choose trace width appropriately. At the same time this circuit has a properties(1)that makes it possible to make a very neat layout on the PCB. And from that point you may also think about making it more compact without that much effort. A good exercise that will be much harder for other circuits.(1)Namely: it’s nearly a planar graph and it can be laid out almost as it appears on a cleanly drawn schematic. Only a single track must cross another one (one of the resistors may be used as a bridge) and the TO-220 package pin order does not correspond exactly to how it’s seen in the schematic.

author: DavidAlfa
author_rank: Super Contributor
timestamp: April 16, 2022, 12:57:01 am
content: These hair-like traces will be hotter than the soldering iron

author: ThermallyFrigid
author_rank: Frequent Contributor
timestamp: April 16, 2022, 11:09:10 am
content: The trained eye can quickly spot potential problems with some of these very small traces.Some of these small traces probably have more resistance than the component they serve / connect.For beginners,When designing small boards like this would there be a problem with generally making all traces wider or even as wide as comfortable or practically possible?Especially between components where current flow has the potential to be higher.The smaller the trace, the more copper that has actually been removed from the board.Why not leave as much copper as feasible / practical / possible ....generally speaking?When I'm working on boards (even complex boards that I'm re-creating) I sometimes make tracks wider simply because there is no reason to have them that small and increasing the track width simply increases the traces current carrying capacity, PCB adherence and overall solder-ability..Granted, there could be many issues such as noise introduction that I'm not advanced enough to be aware of.It's just a general question.I've done it with some more complex boards so far with no issues.

author: pomme
author_rank: Contributor
timestamp: April 16, 2022, 03:17:29 pm
content: golden_labelstkanks for your encouragement, for a beginners like me it cheers me up. I was a little bit discouraged but i don't intend to give upfree_electronthanks a lots for your schematic it really helped me a lot I think I'm going to make schematics like that in the futur it's much more cleareven if I don't understand why in certain case like (see the picture) why the current that passes is not strong enough that you need thicker traces I'll google it and see what I can findedit : i searched a little bit and I think maybe it has some thing to do with resistancefor example : the resistance generated by R1 and D3 is strong enough that it won't allow a current strong enough that we need to thicken the traceI would like to know if the example is correctQuote from: DavidAlfa on April 16, 2022, 12:57:01 amI'm still learning

author: pigrew
author_rank: Frequent Contributor
timestamp: April 16, 2022, 03:52:17 pm
content: Quote from: ThermallyFrigid on April 16, 2022, 11:09:10 amFor boards that I work on, there are a few reasons not to make the traces super wide:Parasitic capacitance to a ground plane. The traces become parallel plate capacitors. The extra capacitance is GOOD for tracks that are DC or low current. With high frequencies (like digital signals), it will create an extra load on the I/O driver. In this PCB, the area of the SW node should be minimized to reduce losses.Characteristic impedance target. Sometimes you need a particular RF characteristic impedance (like 50 ohms), which will dictate the geometry of the trackHarder to solder. It's more difficult to solder to a big chunk of copper, than a small pad.(maybe)Introduce waveguide modes close to your operating frequency, creating resonances or turning your track into an antenna.For this design, the rules of thumb I'd use are:Use a ground plane (on the back of the PCB).Minimize the area and length of the SW node (and preferably GATE).Make the P24 and HANDLEP track wide, >0.25 mm/A should be safe. For the 6A, the 2mm should be plenty, but I'd likely make it a bit more just because you can. The Saturn PCB Toolkit software suggests 4.25mm tracks for 6A.Maybe I'm missing something, but shouldn't there be a capacitor from HANDLEP to GND, close to the inductor?

author: pomme
author_rank: Contributor
timestamp: April 16, 2022, 04:40:49 pm
content: Quote from: pigrew on April 16, 2022, 03:52:17 pmyou mean this one ?

author: pigrew
author_rank: Frequent Contributor
timestamp: April 16, 2022, 04:43:57 pm
content: Quote from: pomme on April 16, 2022, 04:40:49 pmNo, that's a zener diode, to limit the voltage going to an ADC (so that the ADC/MCU is not fried).I'm talking about a capacitor, likely two or three of them... Maybe 47uF next to the inductor and 100nF ceramic next to the heater connector. The circuit would work without them, but they should reduce the EMI produced.

author: golden_labels
author_rank: Super Contributor
timestamp: April 16, 2022, 05:58:17 pm
content: Quote from: DavidAlfa on April 16, 2022, 12:57:01 amJust make them thinner. If resistance is high enough, large current can’t happen, right?Quote from: ThermallyFrigid on April 16, 2022, 11:09:10 amFrom current handling perspective, you would like to use copper zones. But they become a problem for soldering, acting as heatsink that sucks out all the heat. There is no silver bullet. One may limit that factor by connecting a pin to the zone with only a few spokes, but this is just finding the middle ground between two bad situations.Quote from: pomme on April 16, 2022, 03:17:29 pmIndeed. That fragment does not deliver any significant power. It’s there only to pass signal.

author: pomme
author_rank: Contributor
timestamp: April 16, 2022, 07:37:30 pm
content: Quote from: golden_labels on April 16, 2022, 05:58:17 pmif the traces are thin enough electrons won't have place to pass throughQuote from: golden_labels on April 16, 2022, 05:58:17 pmI'm really happy I understood it.does the resistance of diode or transistor play a big role in preventing big amount of current to pass through ? and if yeshow do we determine the resistance ? is it in the datasheet or do we calculate itQuote from: pigrew on April 16, 2022, 04:43:57 pmdo you recommend me puting them ?

author: pigrew
author_rank: Frequent Contributor
timestamp: April 16, 2022, 08:09:17 pm
content: Quote from: pomme on April 16, 2022, 07:37:30 pmI do recommend adding places to mount capacitors on the output, however you might not need them. It's always better to add places to put a component, in case you need them (at least for initial designs).You may also want a capacitor in parallel to your Zener diode (where you had circled). As it is, you'll see a triangle-wave on the voltage-output pin. If that's your intention, great. If you want the average voltage, then you'll need to add a capacitor in parallel to the Zener, to form a lowpass filter.

author: pomme
author_rank: Contributor
timestamp: April 16, 2022, 11:36:34 pm
content: Quote from: pigrew on April 16, 2022, 08:09:17 pmI didn't understand every thing but I'll keep that in mind and make some research

author: golden_labels
author_rank: Super Contributor
timestamp: April 17, 2022, 07:05:07 am
content: Quote from: pomme on April 16, 2022, 07:37:30 pmFor resistor: Ohm’s law.For diodes: diodes do not exhibit resistance understood in that manner. While each real-world diode has some ohmic resistance, in this case it’s negligible and you may assume in this circuit the diode has no resistance above 3V and does not conduct at all below 3V.

author: pomme
author_rank: Contributor
timestamp: April 17, 2022, 07:31:04 pm
content: okey thanksfor example in the case of R1 and D3 I know that R1 is 10kΩ so ohm's law : I = 24V/10kΩ = 0.0024Aso I know that I don't need thick traces right ?

author: golden_labels
author_rank: Super Contributor
timestamp: April 17, 2022, 08:39:13 pm
content: The short answer: yes. 2.4mA is very low current.A longer answer: it’s even less than 2.4mA: the voltage drop on the resistor is around 21V, as the rest is taken by the diode. ATMega328P inputs in practice take no current. And even without calculating the current, you have a 10kΩ resistor there. With such a huge resistance and low voltages, track width becomes irrelevant, as it will always be orders of magnitudes smaller.The proper answer: judging by this thread, you are at the very beginning of the adventure with electronics. While being a newbie is not a problem, not doing one’s homework will be. You are embarking at a project that can’t be easily designed or understood by an EE student halfway through their first semester. But so far it is clear you miss any knowledge in the topic. Like, literally, any. Nothing wrong with trying things out and learning by experimentation, but there is an enormous gap between what you know and what you try to do. Perhaps try with something simpler first? Something that will let you grasp the basic principles.

author: pomme
author_rank: Contributor
timestamp: April 18, 2022, 12:05:41 am
content: I understand what you mean and I agree with you but this is how my brain understand things (with a project) I tried a classical path but it was so boring that I give upbut with this project I have really learned so much from your feedbackssorry if my questions were too simple and I appreciate your help until now

author: pigrew
author_rank: Frequent Contributor
timestamp: April 18, 2022, 12:19:31 am
content: The zener D1 (protecting the gate) might overheat.When the pFET switch is ON, DRIVE will be about 0.7 V. If the input is a little high (25 V), D1 may have 18.5 V on it, so GATE is 6.5 V. The Zener's current is (6.5 - 0.7 volts )/(100 ohm) = 58 mA.The Zener's power would then be I*V = 58 mA * 18.5 V = 1.1 watts. This seems to be too much, since the max power is about 0.35 watts.You may want to run a simulation of this circuit (such as in LTSpice), and verify that all the components are within their power envelopes and that the circuit functions as desired.

author: pomme
author_rank: Contributor
timestamp: April 18, 2022, 01:03:32 am
content: this schematic is not from me it's from a youtuber called sasiskas and from what I have seen his soldering station worksI don't know if I can put a the link of his video or if it's against the rules of the forum

author: pigrew
author_rank: Frequent Contributor
timestamp: April 18, 2022, 01:18:36 am
content: Quote from: pomme on April 18, 2022, 01:03:32 amMy understanding is that it's perfectly fine to post links to YouTube videos (unless it's done as advertising).andthese are the design files.I'm not saying it wouldn't work. I'm not even saying that it must be changed. I'm saying that there are design issues that should be considered as you are working on the design, and I hope that my comments will help you understand the design.With this overheating issue, in particular, the PWM duty cycle might be low enough that the part will never overheat. Or maybe, it'll cause moderate overheating, and only cause failure after 10,000 hours. It is a design issue that should be considered. It may also point you into investigating other issues, like how V_gs=-18.5 V is probably bad for the MOSFET (its max rating is Vgs = 20 V, and only shows data down to Vgs=-15). A zener closer to 15 V would be safer.

author: pomme
author_rank: Contributor
timestamp: April 18, 2022, 02:50:32 am
content: Quote from: pigrew on April 18, 2022, 01:18:36 amI'll keep that in mindQuote from: pigrew on April 18, 2022, 01:18:36 amOh I see I'll try doing like you suggested and check out the issue you pinpointedI'll take my time to understand an search, I'm not in a hurry anywaythanks

author: golden_labels
author_rank: Super Contributor
timestamp: April 19, 2022, 12:33:44 am
content: Quote from: pomme on April 18, 2022, 12:05:41 amIt’s not that they are “too simple”. The problem is: no one is going to explain you the most absolute basics in a project, that requires a decent grasp of them.What I meant is that you may try something simpler first. To get the feel of how stuff works. Play with some trivial circuits to learn the fundamental concepts before combining many of them in a single project.Quote from: pigrew on April 18, 2022, 12:19:31 amI believe it’s not.Notice that, using free_electron’s schematic version, both Q4 and Q3 operate as voltage followers. So DRIVE will see about the same voltage as PWMDRIVE. That gives additional 5V of margin. 23V is needed for R2 and D1 to even see any current. At 24V and above they would see about 10mA/V increase, with theoretical 180mW/V power on D1. But there is negative feedback from the power supply line: R3.Of course you noticing a potential issue there is still a good thing! 👍

author: pigrew
author_rank: Frequent Contributor
timestamp: April 19, 2022, 02:29:47 am
content: Quote from: golden_labels on April 19, 2022, 12:33:44 amI completely missed R6. With it in mind, the design is fine.With 5V digital IO, SINK goes between 4V and 24V (not 0V and 24V as I mistakenly thought). With 3.3V logic levels, SINK would alternate between ~11V and 24V.I threw together a LTspice simulation, assuming nominal parameters. I believe it's a 5V Arduino being used. When the PWMDRIVE is active, the Zener is at 180 mW, so within the safe range. Even with 25V input and 5.5V I/O, it's within the power limit of the zener.(I couldn't find the RF107 diode model, so I arbitrarily choose the RF071 model... it's an anagram, so maybe it's close?)