Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

can you check my pcb for acdc converter?

alex_beer

Newbie
Joined
Oct 13, 2021
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
30
Hi, I've designed a trivial pcb to use a 3 watts acdc converter: essentially two wire (in kicad sense) going from screwed terminal to the acdc carrying 220v alternate current and other two wire carrying the output to a usb female port . Where can I have it checked? I mean if after I send it to pcb producer it will come out properly and if I'll assemble it properly it'll work?
In case someone would like to help I've attached the gerbers files and schematic pdf: my first experience with pcb design, and viewing it on tracespace seems a bit odd in top/bottom view.
Thank you
 

Attachments

  • gerbers.zip
    10 KB · Views: 5
  • acdc3w.pdf
    8.8 KB · Views: 22
Last edited:
Solution
Hi,

trace width:
depends on the current it has to carry
So higher current bigger trace width.

--> your design is the opposite.
At 250V you have low current thus you need only small trace width.
at 5V you have much higher current thus you need bigger trace width

****

isolation distance:
depends on the isolation voltage. It also depends on whether it is functional isolation or safety isolation and other parameters.

So the largest distance you need for safety isolation between mains and DC voltage (Safety first). Use 6mm at least.
The next is functional isolation beween mains and mains. Use 1.5mm at least. 2mm won´t hurt.
The lowest is between 5V DC (functional) (here you have the biggest). 0.25mm should be well enough...

betwixt

Super Moderator
Staff member
Joined
Jul 4, 2009
Messages
15,160
Helped
4,946
Reputation
9,913
Reaction score
4,758
Trophy points
1,393
Location
Aberdyfi, West Wales, UK
Activity points
128,764
From the PDF I would say that layout is horrible. It looks like the tracks are far thinner than they could be so you introduce resistance and potentially too much voltage drop or even the tracks fusing. Fatten them up, space them out more to give more clearance around the holes and flood fill the rest of the board with ground.

Brian.
 

alex_beer

Newbie
Joined
Oct 13, 2021
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
30
Well, I've tried to keep the 220v tracks 4 mm apart and enlarged it a bit, hope not too much.
I've connected the filled layer to pad 2, the central one in screwed terminal, which is ground: I'm wondering if I should connect it to ground, and if I should use thermal or solid connection.
 

Attachments

  • acdc3w2.0.pdf
    11.6 KB · Views: 3

SunnySkyguy

Advanced Member level 5
Joined
Sep 26, 2007
Messages
6,988
Helped
1,709
Reputation
3,416
Reaction score
1,697
Trophy points
1,413
Location
Richmond Hill, ON, Canada
Activity points
51,565
This is a case of shoot first, ask questions later type of design and what seems trivial might not be if you triggered a short across the grid. It's usually best to learn the basics then advance by reverse engineering. This layout looks like a primitive autobot layout.

Are you aware of safety requirements for ACDC design with contamination and creepage, leakage , PLT and hipot? How do you know it will be dust and humidity free on the PCB when air gaps are normally used for safety.

Asking for a design review must also include all the design specs. requirements and expectations.

For example, look at all the specs just for a simple 2W power resistor.

My point being is you should learn how to read specs then write them before trying to design, unless you are just doing a hobby activity of copy fabrication.

BTW KiCad has a Gerber viewer. Search for gerbview.exe in the bin path
 
Last edited:

KlausST

Super Moderator
Staff member
Joined
Apr 17, 2014
Messages
20,531
Helped
4,463
Reputation
8,935
Reaction score
4,496
Trophy points
1,393
Activity points
135,752
Hi,

trace width:
depends on the current it has to carry
So higher current bigger trace width.

--> your design is the opposite.
At 250V you have low current thus you need only small trace width.
at 5V you have much higher current thus you need bigger trace width

****

isolation distance:
depends on the isolation voltage. It also depends on whether it is functional isolation or safety isolation and other parameters.

So the largest distance you need for safety isolation between mains and DC voltage (Safety first). Use 6mm at least.
The next is functional isolation beween mains and mains. Use 1.5mm at least. 2mm won´t hurt.
The lowest is between 5V DC (functional) (here you have the biggest). 0.25mm should be well enough.

****

Don´t use a GND plane here.
I even don´t recommend to use a hard wired connection between EARTH_GND and USB_Shield, because it may cause GND loops. I´d use a 100R resistor for example. And in case of wrong connection it should break_OPEN. I recommend a resistor rated for mains voltage (safety).

****

Hint:
swap the two mains connections at the connector. Then you get yeasier routing with short, almost straight traces.

****

I agree with SunnySkyguy.
Read through safety standards.
Don´t risk any others health. Mains voltage is dangerous.


Klaus
 
Solution

alex_beer

Newbie
Joined
Oct 13, 2021
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
30
@KlausST: ops, you're right, the input of AC-05-3 is 100-240 VAC, 40mA, 50/60 Hz, the output 5V, 600 mA. The original arrangement was in fact really stupid; there are side effects in using bottom layer for high tension and/or low tension connections?
Thanks for your guide.
@SunnySkyguy: I'm aware of Dunning-Kruger effect less of pcb design. I'm using creepage.com to get an idea of minimum distances
 

SunnySkyguy

Advanced Member level 5
Joined
Sep 26, 2007
Messages
6,988
Helped
1,709
Reputation
3,416
Reaction score
1,697
Trophy points
1,413
Location
Richmond Hill, ON, Canada
Activity points
51,565
@KlausST: ops, you're right, the input of AC-05-3 is 100-240 VAC, 40mA, 50/60 Hz, the output 5V, 600 mA. The original arrangement was in fact really stupid; there are side effects in using bottom layer for high tension and/or low tension connections?
Thanks for your guide.
@SunnySkyguy: I'm aware of Dunning-Kruger effect less of pcb design. I'm using creepage.com to get an idea of minimum distances
Ha. Note that Pollution Degree = 2 is an assumption of dust and humidity reduction in BDV from 3kV/mm for air (smooth surface) to 150V/mm sine rms and may not protect against 4kV / 1us transients unless you used fuse with MOV. This is why often you see air gap slot in PCB between primary and secondary to reduce degradation of breakdown voltage from surface creepage. so I recall a 2mm air slot about the same as 10 mm surface gap between primary circuit and grounded SELV.

Also , Grounding reduces noise and adds human protection to transients but also lowers immunity to transient self damage. HIPOT is often only tested with secondary DC ungrounded and I have seen major factories fail in HIPOT due to this. ( i.e. transfer product to Mexico then gap changes resulted in HIPOT pass isolated and catastrophic fail secondary grounded.
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
48,930
Helped
14,335
Reputation
28,934
Reaction score
13,083
Trophy points
1,393
Location
Bochum, Germany
Activity points
282,330
The SMPS is designed for overvoltage category II, reinforced insulation, 3000 VAC test voltage. The related PCB creepage distance is 3 mm for pollution degree 2. It's o.k. to increase creepage above these minimal requirements, but I won't expect isolation failure as long as the standard requirements are fulfilled.
 

LaTeX Commands Quick-Menu:

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top