Author Topic: Critique my first PCB  (Read 5296 times)

0 Members and 1 Guest are viewing this topic.

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Critique my first PCB
« on: May 19, 2018, 12:05:47 pm »
Hi. I'm looking for opinions or advice on my PCB layout.

It's simply an adapter for the STM32L4R9I-DISCOVERY board to allow me to use a large round Panasys MIPI LCD display. It is to go in place of the supplied MB1314 AMOLED smartwatch daughterboard.

So it has a backlight LED driver, basically following the datasheet circuit diagram, and then just tracks between the connectors. Both clock and DSI are high speed differentials. Annoyingly the P/N of the differential pairs always seemed to need to cross over each other! On the big connector they are side by side, but as the LCD panel's connector is double row, they are opposite each other instead!

Things I thought about:
  • I could have made use of the bottom layer for more than just one big ground fill. That could have made it much easier to route the tracks. I was trying to keep it simple though and wasn't sure if that was a good or bad idea.
  • Number of vias to the ground layer.. too many? not enough?

I suppose once I have one in my hand I will have a better idea of size and where I could have gone bigger or smaller. I will do a print out as well.

I started with the ST schematics, just so I could get the big Samtec connector. That's why it still has their logo on it, and is named 'copy of mb1314' :-)

Here's a PDF: http://www.internetsomething.com/lcd/pcb/PDF.pdf
The rest (gerbers etc) can be downloaded from this directory: http://www.internetsomething.com/lcd/pcb/

and here's 3D pictures:






Any obvious total fails? Other suggestions?
« Last Edit: May 19, 2018, 06:36:50 pm by carl0s »
--
Carl
 

Online ataradov

  • Super Contributor
  • ***
  • Posts: 5851
  • Country: us
    • Personal site
Re: Critique my first PCB
« Reply #1 on: May 19, 2018, 06:43:44 pm »
1. It is probably better to have some of the traces go on the bottom layer rather than have them snake around between the pins of the connector like this.
2. Purely aesthetic: I'd use only 45 degree traces.
3. Pour solid ground on the top layer as well. And more ground stitching can't hurt. Especially close to those ground pins next to the differential lines
Alex
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #2 on: May 19, 2018, 06:59:05 pm »
1. It is probably better to have some of the traces go on the bottom layer rather than have them snake around between the pins of the connector like this.
2. Purely aesthetic: I'd use only 45 degree traces.
3. Pour solid ground on the top layer as well. And more ground stitching can't hurt. Especially close to those ground pins next to the differential lines

Thanks. I have to admit, it was a lot harder than I expected. I started along merrily and then one track would be unroutable and I'd have to un-do it all and move components. One minute the LCD socket was below and the next it was above. Turning the backlight driver chip around multiple times, etc.

I suppose I just thought that routing on both layers would be too much for me to try to deal with for my first time. Plus I was battling with not knowing how to use the program (Altium) that I borrowed. I think I might want to look at KiCad or Allegro as I have found a few things frustrating (length tuning being awkward, moving objects with tracks connected, erm, highlighted/unhighlighted toggle not actually reflecting what's on screen.. ).
--
Carl
 

Online ataradov

  • Super Contributor
  • ***
  • Posts: 5851
  • Country: us
    • Personal site
Re: Critique my first PCB
« Reply #3 on: May 19, 2018, 07:03:03 pm »
Sometimes it is easier to go back and redo the whole board with your new knowledge after you've struggled though the first one.

I would try to route all differential signals on one layer and actually keep the traces parallel for as long as possible. Then route remaining pins that can be routed cleanly on one side. A then move the rest on the other side. Right now there is not a whole lot of point in your length matching, for example.
Alex
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #4 on: May 19, 2018, 07:05:45 pm »
Sometimes it is easier to go back and redo the whole board with your new knowledge after you've struggled though the first one.

I would try to route all differential signals on one layer and actually keep the traces parallel for as long as possible. Then route remaining pins that can be routed cleanly on one side. A then move the rest on the other side. Right now there is not a whole lot of point in your length matching, for example.

Hmm but the differential pairs are side by side on one connector, and top and bottom on the other. Unless I was to put the smaller LCD connector on sideways?

How come there's not much point to the length matching? Is it not about time delay?
--
Carl
 

Online ataradov

  • Super Contributor
  • ***
  • Posts: 5851
  • Country: us
    • Personal site
Re: Critique my first PCB
« Reply #5 on: May 19, 2018, 07:10:21 pm »
Nevermind, I thought there was much more going on with them. What you have is fine. Well the trace on the right can be made a bit more parallel to the other pair, but really on that distance it is all cosmetic and won't make much difference in real life.
Alex
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #6 on: May 19, 2018, 07:14:30 pm »
Nevermind, I thought there was much more going on with them. What you have is fine. Well the trace on the right can be made a bit more parallel to the other pair, but really on that distance it is all cosmetic and won't make much difference in real life.

Yes I was just thinking about how that could be pulled in and kept parallel. No need for the odd shape.

Thanks for your help!
--
Carl
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #7 on: May 19, 2018, 07:24:08 pm »
I made it more parallel:







Altium is really annoying with that length tuning. For example it wouldn't move that extension piece higher. It will only allow it where it is - beneath the connector outline silkscreen.
It's like it refuses to go anywhere near corners or something.
« Last Edit: May 19, 2018, 07:30:19 pm by carl0s »
--
Carl
 

Online ataradov

  • Super Contributor
  • ***
  • Posts: 5851
  • Country: us
    • Personal site
Re: Critique my first PCB
« Reply #8 on: May 19, 2018, 07:26:19 pm »
Add the ground pour on the top layer. And add more vias to connect the two. That's probably the best thing you can do on this board for signal integrity.
Alex
 
The following users thanked this post: carl0s

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #9 on: May 19, 2018, 07:31:05 pm »
Add the ground pour on the top layer. And add more vias to connect the two. That's probably the best thing you can do on this board for signal integrity.

OK I shall have a go! Thanks.
--
Carl
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #10 on: May 19, 2018, 08:08:17 pm »
Right, I have had a go!

I had the clearance rules turned off before because.. well because I didn't know better. I didn't realise they actually directed things like polygon pour to clear themselves around tracks. I thought they were just there to nag you about things!

So I have done it, and.. well two things. Firstly, it's left a stray bit of copper, and as it's part of the overall polygon i don't know how to remove it. Just ignore it? I suppose it looks nice.. adds balance.

Secondly, the clearance rules have highlighted to me that those tracks coming in beween the pads, are 3.89mils next to the connector pads. Do you think this is too close for el-cheapo PCB manufacturers? Please say it'll be fine..

(I know, I need to put in some more vias)

--
Carl
 

Online ataradov

  • Super Contributor
  • ***
  • Posts: 5851
  • Country: us
    • Personal site
Re: Critique my first PCB
« Reply #11 on: May 19, 2018, 08:11:31 pm »
The polygon part is fine. But the typical cheap PCB manufacturers offer 5/5 or 6/6 mil track/clearance. I typically route everything using 10 mil tracks and spaces when possible. So you will have to rethink your layout.
Alex
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #12 on: May 19, 2018, 08:18:40 pm »
Currently looking like this:





--
Carl
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #13 on: May 19, 2018, 08:26:32 pm »
The polygon part is fine. But the typical cheap PCB manufacturers offer 5/5 or 6/6 mil track/clearance. I typically route everything using 10 mil tracks and spaces when possible. So you will have to rethink your layout.

Alright.. Well, when I read that, I thought, bugger.. nightmare. Re-think. But, now that I know that the polygon pour is smart and will leave clearances around other nets, I think I'm comfortable with adding in vias and signal tracks on the bottom layer, instead of going between pins, and then re-pouring the bottom ground layer.

I'm going to have a go after my tea :)

Thanks!
« Last Edit: May 19, 2018, 08:28:44 pm by carl0s »
--
Carl
 

Offline treez

  • Super Contributor
  • ***
  • Posts: 1079
  • Country: gb
Re: Critique my first PCB
« Reply #14 on: May 19, 2018, 09:32:45 pm »
here is my PCB layotu guide attached.

Also, Dave Jones guide to PCB layout
http://alternatezone.com/electronics/files/PCBDesignTutorialRevA.pdf

Thats Dave Jones who runs this site
 
The following users thanked this post: carl0s, Chris56000

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #15 on: May 19, 2018, 11:18:58 pm »
I was reading Dave's 2004 PDF the other night!! :)

Anyway, here is my latest revision. Better. I made the drill holes 12mil too. They were 10mil before.





--
Carl
 

Offline ANTALIFE

  • Regular Contributor
  • *
  • Posts: 247
  • Country: au
  • ( ͡° ͜ʖ ͡°)
    • Muh Blog
Re: Critique my first PCB
« Reply #16 on: May 20, 2018, 06:03:06 am »
My first though is that it looks like you have a switching DCDC converter, not sure of the current/power requirements but if it was me I would try connect each component that is part of the power path with a thicker track or a plane like this:

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #17 on: May 20, 2018, 09:56:46 am »
My first though is that it looks like you have a switching DCDC converter, not sure of the current/power requirements but if it was me I would try connect each component that is part of the power path with a thicker track or a plane like this:

Yes I thought that might come up. I'm just not quite sure how to do it in Altium other than by literally drawing the polygons, and I can see them ending up rather ugly :-)
I might have a go though.

It's an AP5724 DC to DC converter. http://www.internetsomething.com/lcd/AP5724%20backlight%20driver.pdf

There's 6 LEDs in series, at 20mA, 18v total, so 360mw total. They say the above driver chip is 84% efficient, so expected draw of 430mw. Call it 500mw. I'm not really sure I know enough about this stuff, but I gather it's current that matters. So the 500mw should pull 151mA from the 3.3v supply. I've used 10 mil traces which an online calculator says should be good for 450mA with 1oz copper. The LCD panel itself pulls 15mA. So I'm at about 165mA.

What do you think? I suppose it makes sense for me to learn how to do the job properly though doesn't it..
--
Carl
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #18 on: May 20, 2018, 10:15:54 am »
I've just tidied up some stray ground tracks for now, from before I did the ground fill on the top layer





« Last Edit: May 20, 2018, 10:29:34 am by carl0s »
--
Carl
 

Offline David Chamberlain

  • Regular Contributor
  • *
  • Posts: 238
Re: Critique my first PCB
« Reply #19 on: May 20, 2018, 11:33:29 am »
What happened to the fill on the bottom?
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #20 on: May 20, 2018, 12:14:01 pm »
My first though is that it looks like you have a switching DCDC converter, not sure of the current/power requirements but if it was me I would try connect each component that is part of the power path with a thicker track or a plane like this:

All right, I have had a go! I have beefed up a lot of the tracks as well:

--
Carl
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #21 on: May 20, 2018, 12:14:54 pm »
What happened to the fill on the bottom?

It's still there isn't it? I just didn't have it highlighted it in the image so it was under the soldermask.

« Last Edit: May 20, 2018, 12:17:05 pm by carl0s »
--
Carl
 

Offline carl0s

  • Supporter
  • ****
  • Posts: 218
  • Country: gb
Re: Critique my first PCB
« Reply #22 on: May 20, 2018, 12:58:42 pm »
--
Carl
 

Offline ANTALIFE

  • Regular Contributor
  • *
  • Posts: 247
  • Country: au
  • ( ͡° ͜ʖ ͡°)
    • Muh Blog
Re: Critique my first PCB
« Reply #23 on: May 20, 2018, 02:14:31 pm »
My first though is that it looks like you have a switching DCDC converter, not sure of the current/power requirements but if it was me I would try connect each component that is part of the power path with a thicker track or a plane like this:

Yes I thought that might come up. I'm just not quite sure how to do it in Altium other than by literally drawing the polygons, and I can see them ending up rather ugly :-)
I might have a go though.

It's an AP5724 DC to DC converter. http://www.internetsomething.com/lcd/AP5724%20backlight%20driver.pdf

There's 6 LEDs in series, at 20mA, 18v total, so 360mw total. They say the above driver chip is 84% efficient, so expected draw of 430mw. Call it 500mw. I'm not really sure I know enough about this stuff, but I gather it's current that matters. So the 500mw should pull 151mA from the 3.3v supply. I've used 10 mil traces which an online calculator says should be good for 450mA with 1oz copper. The LCD panel itself pulls 15mA. So I'm at about 165mA.

What do you think? I suppose it makes sense for me to learn how to do the job properly though doesn't it..

The way I see it if the LED's expect to consume 360mW and the converter is 84% efficient then this means 70mW will be dissipated as heat in the SOT23-6 package. Given that θJA is 162°C/W this means that IC will rise by ~11°C above ambient. Not that bad but for the sake of it I would still use a polygon to help dissipate the heat, and give the current a much less resistance pathway (lower ohmic loss, not that it matters that much with your current draw).

As for polygons you can either manually place them down and adjust as you go like:
Or you could use another layer (like MECH 1) to define the shape and then create a polygon on copper layer, like (Create Polygon from Selected Primitives): https://www.altium.com/documentation/15.1/display/ADES/PCB_Cmd-ConvertSelected((ConvertSelected))_AD

Also I think your latest iteration with polygons looks better, but there is still room for improvement. To get an idea of a good layout have a look at the appnote:
https://www.diodes.com/diodes-part-files/AC/AP5724/User%20Guides%20and%20EV%20Boards/AP5724-EVM.pdf
Notice how all components part of the power path (inductor, diode, filter caps, IC...) are all connected via a large polygon

Offline Dave

  • Super Contributor
  • ***
  • Posts: 1200
  • Country: si
  • I like to measure things.
Re: Critique my first PCB
« Reply #24 on: May 20, 2018, 04:42:19 pm »
The current paths in that SMPS look unnecessarily long. You want the high currents to have short, uninterrupted current paths from the input capacitors to the output capacitors.
You could improve this by rotating the inductor by 90° clockwise and move those input capacitors closer to the output caps. Also, fatten the traces up around the diode.
<fellbuendel> it's arduino, you're not supposed to know anything about what you're doing
<fellbuendel> if you knew, you wouldn't be using it
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf