my first pcb any mistake

[pomme]

hello I made my first pcb and would like to know if I made any big mistake
it's a pcb for a soldering station based on this schematic
I 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 enough
the other line is 0.2mm
the blue square is a buck converter and the orange is for earth connection because I use a one side pcb

thanks for your replies

[free_electron]

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.

[eugene]

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.

[tepalia02]

I agree with the above answerers.

[pomme]

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.

is widening the line until the seconde capacitor enough ?
for the to92 transistor should I widen the outer circle or narrow the inner circle
and thanks for the "electrons in = electrons out" I didn't know that

[free_electron]

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.

[mariush]

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.

[golden_labels]

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.

[eugene]

is widening the line until the seconde capacitor enough ?

Current 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_SUPPLY through 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.

[free_electron]

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.

[strawberry]

1...2mm signal traces
solder pads diameter enough to solder
need to think ahead on how it will come together

[pomme]

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.

for 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 pdf
for the zener I brought from china I hope it going to work
i'm gonna use thicker traces

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.

yes it's for illustration only, Kicad did it this way

is widening the line until the seconde capacitor enough ?

Current 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_SUPPLY through 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.

thanks a lot I understand a little bit more how it works now
and magenta was perfect 

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.

indeed 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 one
for the part with recirculation diode is what I did in the edited schematic good  ?
I will also put the complet schematic

[golden_labels]

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.

[free_electron]

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 junction
Netnames are used to name nets , not to infer connection ! Wires are for connections.

[mariush]

indeed 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 one

If 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.pdf

Example of handpieces : https://www.ebay.com/itm/224544111810

You 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.

 

[strawberry]

R1 without divider, clamping diode D3 will limit output voltage range to 0..3.3V

[nvmR]

OP, add some mounting holes and a revision number, and a place for a serial number. Very useful for the future

[golden_labels]

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.

[DavidAlfa]

These hair-like traces will be hotter than the soldering iron

[ThermallyFrigid]

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.

[pomme]

golden_labels tkanks 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 up

free_electron thanks 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 clear
even 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 find
edit : i searched a little bit and I think maybe it has some thing to do with resistance
for 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 trace
I would like to know if the example is correct

These hair-like traces will be hotter than the soldering iron

I'm still learning

[pigrew]

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.

Granted, there could be many issues such as noise introduction that I'm not advanced enough to be aware of.

For 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 track
• Harder 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?

[pomme]

Maybe I'm missing something, but shouldn't there be a capacitor from HANDLEP to GND, close to the inductor?

you mean this one ?

[pigrew]

Maybe I'm missing something, but shouldn't there be a capacitor from HANDLEP to GND, close to the inductor?

you mean this one ?

No, 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.

[golden_labels]

These hair-like traces will be hotter than the soldering iron

Just make them thinner. If resistance is high enough, large current can’t happen, right?

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.

From 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.

for 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 trace

Indeed. That fragment does not deliver any significant power. It’s there only to pass signal.