Low Cost PCB's Low Cost Components

Author Topic: [review] PCB layout review  (Read 819 times)

0 Members and 1 Guest are viewing this topic.

Offline info

  • Contributor
  • Posts: 5
  • Country: de
[review] PCB layout review
« on: August 30, 2017, 08:26:36 AM »
Hello there! I am trying to get a grasp at laying out pcb's using eagle. Yeah, I've been reading the negative remarks about it but it's what I started learning with and I don't want to jump ship every time I read a bad review. Anyways, as a beginner I thought I would make a PWM controller for my air pump (aquarium) and I have a reel of 50 555 timers. So I quickly drew the schematic and laid the board out as best as I could. Somehow I locked myself out on the ground plane such that I can't do it without using a jumper but the simplicity of this board makes me think "...you can do better!.."

So if you have any pointers on how to optimize this layout for home etching (either toner transfer or negative film) then please do give your feedback. I don't mind harsh tones and prefer blunt opinions.

The board size is 50mmx70mm but can be smaller as I have halved a 100mmx70mm board. I wasn't sure I could make it smaller and still retain enough clearance for the horizontal mosfet since I would like to try the making the whole board somewhat flat.

p.s. How do you guys make another plane for the mosfet's tab since it's connected to drain?

edit: attached schematic as image
« Last Edit: September 02, 2017, 04:21:11 AM by info »
 

Offline latigid on

  • Contributor
  • Posts: 15
  • Country: de
Re: [review] PCB layout review
« Reply #1 on: September 01, 2017, 05:43:30 AM »
Looks okay. Especially for self-etching you could remove some of the bends, e.g. on C3, above D3 etc.

If you don't want to draw a new symbol/package for the MOSFET, you could draw a line or polygon fill (set to a "higher" priority than the 0V/ground plane) and named as the same signal.

The ground plane won't be doing much anyway, so I suggest rotating C3 and the PWR header 180 degrees. Then run the power trace around the edge of the board. In fact, the power header might be better placed near the MOSFET so the return current has a smaller path back to the PSU.
 
The following users thanked this post: info

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 2946
  • Country: au
  • Question Everything... Except This Statement
Re: [review] PCB layout review
« Reply #2 on: September 01, 2017, 06:28:04 AM »
C1 connects to a ground island. Equally you may want to shift the trace connecting to p1 so the mosfets ground has a straight run to the input connector
« Last Edit: September 01, 2017, 06:33:28 AM by Rerouter »
 
The following users thanked this post: info

Offline mc172

  • Regular Contributor
  • *
  • Posts: 107
  • Country: gb
Re: [review] PCB layout review
« Reply #3 on: September 01, 2017, 06:50:52 AM »
Pin 2/tab of the FET will short to ground if you screw the FET down. You're probably better off just leaving it standing vertical unless there's something in the way, and ignoring the tab in the layout.

Try to get C3 as close to P+ as possible.
Place an additional capacitor (47 nF or something like that, 10 nF, whatever you've got laying around) as close to pin 8 of the 555 as possible.
Place D3 as close to the pump terminals as possible. It will fit between them - this is the best place for it.

Run the track from P- to Drain horizontal out of P-, rather than down at 45 degrees, for a continuous ground plane.

You could also make a lot of the tracks thicker, then if you leave it in the etching tank for a few seconds too long they're not as thin as your arm hairs.

The ground side of C1 is isolated from the main ground - you need a jumper, wire or zero Ohm resistor between the island of ground plane in the middle  to the rest of the board ground. The little yellow line between C3 and C1 indicates that it is not connected. Pin 1 of IC1 is also not connected to ground for the same reason. You might be able to change the layout to prevent an additional component being needed.

 ^-^
 
The following users thanked this post: info

Offline info

  • Contributor
  • Posts: 5
  • Country: de
Re: [review] PCB layout review
« Reply #4 on: September 02, 2017, 12:23:41 AM »
Looks okay. Especially for self-etching you could remove some of the bends, e.g. on C3, above D3 etc....

Okay removed the bendy bends. May I ask why I should avoid bends? I tried keeping away from 90° bends since I hear they are the devils whirlpool during etching but those were just wavy bends


C1 connects to a ground island. Equally you may want to shift the trace connecting to p1 so the mosfets ground has a straight run to the input connector

Thanks for that. Kinda fixed


Pin 2/tab of the FET will short to ground if you screw the FET down. You're probably better off just leaving it standing vertical unless there's something in the way, and ignoring the tab in the layout.

Try to get C3 as close to P+ as possible.
Place an additional capacitor (47 nF or something like that, 10 nF, whatever you've got laying around) as close to pin 8 of the 555 as possible.
Place D3 as close to the pump terminals as possible. It will fit between them - this is the best place for it.

Run the track from P- to Drain horizontal out of P-, rather than down at 45 degrees, for a continuous ground plane.

You could also make a lot of the tracks thicker, then if you leave it in the etching tank for a few seconds too long they're not as thin as your arm hairs.

The ground side of C1 is isolated from the main ground - you need a jumper, wire or zero Ohm resistor between the island of ground plane in the middle  to the rest of the board ground. The little yellow line between C3 and C1 indicates that it is not connected. Pin 1 of IC1 is also not connected to ground for the same reason. You might be able to change the layout to prevent an additional component being needed.

 ^-^

Okay, I fixed the tab issue. C3 is for filtering, I guess? So I just placed it next to the power inputs. P+ & P- are the pump wires soldered directly to the board so theoretically I could move those far away from each other, or am I wrong?
Also tried to increase the widths of the tracks without killing the ground plane but I still can't do this simple board without a jumper :D Seems I need more practice! I have done some test boards with 12 mils using toner transfer and that is repeatable. I guess with uv I can go down to 8 but I haven't really tried although I have all the materials (lazy since toner transfer works fine for my needs)

Thank you all for your input, will update with an etched pcb (both toner and UV) once done

p.s. here is what I have now
« Last Edit: September 02, 2017, 12:25:29 AM by info »
 

Offline StillTrying

  • Frequent Contributor
  • **
  • Posts: 903
  • Country: gb
  • 100% Brand New and High Quality, in theory.
Re: [review] PCB layout review
« Reply #5 on: September 02, 2017, 01:14:08 AM »
The PCB looks OK to me, - couldn't find any obvious errors.
What is the supply voltage, the 100R seems a very low value for an indicator LED on the supply.
 
The following users thanked this post: info

Offline info

  • Contributor
  • Posts: 5
  • Country: de
Re: [review] PCB layout review
« Reply #6 on: September 02, 2017, 03:33:36 AM »
Ah yes, the 100R was just an arbitrary value. I will use a 1K ohm, the supply is 12V. Never really got the "lust" of calculating the actual value so I usually throw something along 1/10th of the supply voltage and I don't mind the brightness. Yes, before I get stoned, I know how to but as time goes by you get lazy when that is just an indicator and there are more pressing matters on your project than the blinky lights, although I think some of us got into electronics because of the blinky lights  :-DD
 

Offline wraper

  • Supporter
  • ****
  • Posts: 6068
  • Country: lv
Re: [review] PCB layout review
« Reply #7 on: September 02, 2017, 05:23:07 AM »
Why do you use SMT version of LM555? It's strange to mix through hole and SMT technologies just for presence of one part which is available in DIP package anyway? Or if you want to use SMT IC, then why not use SMT versions of other parts as well.
 

Online mariush

  • Super Contributor
  • ***
  • Posts: 3025
  • Country: ro
  • .
Re: [review] PCB layout review
« Reply #8 on: September 02, 2017, 05:52:28 AM »
Flip C3 so that the negative side is on the left on the big ground fill.

Align C4 and C2 leads with the diodes D1 and D2. Move the 555 chip UP and a bit to the right.

ADD a zero ohm resistor (jumper wire) from the third pin at the top of the 555 chip then make a trace from the left of the chip to the center pin of that potentiometer. C1 can be squeezed between the diodes, going to the ground fill above the N$6 trace or to the ground fill on the left of the first trace on the trimpot.
This way you don't need such a long Vcc trace.

The Vcc trace can go from under the trimpot, to the right, then nicely fill some area to the left of the 555 chip.  The R3 resistor can probably be placed between D1 and C4

I was even going to suggest rotating the mosfet 90 degrees and placing it UNDER the 555 which should now be a bit higher.  R2 can go straight down to the first pin of the mosfet without jumping traces. D3 could be placed vertically closer to the power connector in all that space that would be freed by C1
and you could get  P+ and P- terminals closer together

I would seriously consider adding a couple more zero ohm resistors (jumper links) just to make my life easier.

PS. and in this circuit probably doesn't matter, but small capacitors (for decoupling) should be as close as possible to ICs... not gonna matter in this circuit but it's good to make a habit of it.

and i think it's a good idea to try to have as few "islands or "peninsulas" in your layout as possible .. like you have in your layout under the D1 and D2 diodes, between the P+ and R2, between R2 and P- , at the trimpot between the diodes...

 

Offline info

  • Contributor
  • Posts: 5
  • Country: de
Re: [review] PCB layout review
« Reply #9 on: September 02, 2017, 08:40:31 PM »
Why do you use SMT version of LM555? It's strange to mix through hole and SMT technologies just for presence of one part which is available in DIP package anyway? Or if you want to use SMT IC, then why not use SMT versions of other parts as well.

I am using what I have in my parts bin. I have a cut reel of ~50 pieces, thats why I used SMT. I don't have any through hole ones at the moment but that would have been my preferred choice anyways. Is it wrong or strange to mix through hole and SMT devices on one build? I see devices (e.g. my late DVD-Player) using a combo of a blob, SMT and through hole devices. Was strange but worked until I opened it up. As a hobbyist I try to keep my costs down while not losing on the functionality intended.
 

Offline wraper

  • Supporter
  • ****
  • Posts: 6068
  • Country: lv
Re: [review] PCB layout review
« Reply #10 on: September 03, 2017, 07:30:56 AM »
Is it wrong or strange to mix through hole and SMT devices on one build?
Of course you can hand solder SMT parts, especially if there is only one such part. But normally you apply solder paste through a stencil, put SMT parts, then reflow. Mixing 2 technologies means doing 2 different processes. Especially true for real production. But if you mix, you want to use as many SMT parts as possible.
Quote
I see devices (e.g. my late DVD-Player) using a combo of a blob, SMT and through hole devices.
Blob is to reduce cost. SMT and through hole were mixed because there was no way around it.
« Last Edit: September 03, 2017, 07:32:42 AM by wraper »
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf