Author Topic: Hey guys, I just finished designing my first board. Could I get a once over?  (Read 5895 times)

0 Members and 1 Guest are viewing this topic.

Offline thomasb9511

  • Contributor
  • Posts: 19
  • Country: us
Don't be too harsh esp. if I broke some design rules.
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4309
  • Country: au
  • Question Everything... Except This Statement
how about post some images, for those of us not using eagle, e.g. top and bottom layer,
 

Offline thomasb9511

  • Contributor
  • Posts: 19
  • Country: us

Top copper layer

Bottom layer

Schematic
 

Offline Skimask

  • Super Contributor
  • ***
  • Posts: 1425
  • Country: us
You could place a few more ground plane stitching vias to extend the ground plane to those blank areas and make more filled ground.
And you've got plenty of room to fatten up every one of those traces rather than using the minimum trace widths.  Same with the clearances.
And better add a few more decoupling caps across Vcc and GND.
« Last Edit: March 12, 2016, 06:28:21 am by Skimask »
I didn't take it apart.
I turned it on.

The only stupid question is, well, most of them...

Save a fuse...Blow an electrician.
 

Offline thomasb9511

  • Contributor
  • Posts: 19
  • Country: us
You could place a few more ground plane stitching vias to extend the ground plane to those blank areas and make more filled ground.
And you've got plenty of room to fatten up every one of those traces rather than using the minimum trace widths.  Same with the clearances.
And better add a few more decoupling caps across Vcc and GND.


So via stitching is what I did and it ok to do?
I'm rerouting with 10-15 mil traces. And widen or lessen the clearance?
And I can't believe I forgot the decoupling caps. 10uf eletro and 10uf ceramic caps be ok?
 

Online daqq

  • Super Contributor
  • ***
  • Posts: 1550
  • Country: sk
    • My site
You are using the minimal widths for traces available on most signals as well as the minimal clearance available in copper pour - while this will work there is no reason not to wider traces - this will remove any risks of using limit values of clearences/widths.

As was advised previously - more local decoupling would be great - both at the input and output of U2 and on the processor.

Also, your SCK trace running under U2 splits two power rail signals - it would be more proper to split the SCK signal and run the two power rails without interruption.
Believe it or not, pointy haired people do exist!
+++Divide By Cucumber Error. Please Reinstall Universe And Reboot +++
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4309
  • Country: au
  • Question Everything... Except This Statement
Signal lines under the crystal,
Decoupling cap is quite far away from the micro power pin,
Crystal layout is sub optimal, could be much tighter,

On your 3 pin regulator, you could move your ground via much closer to the pad,

Moving C3 closer to the regulator pin means you could move your 5V and ground jumper points closer to J5, reducing the length, and a trace running half way across the board,


Moving your ICSP header between the micro and PORTB means you could reduce your connection length,
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4309
  • Country: au
  • Question Everything... Except This Statement
the first 3 i suggested are things that should be fixed to improve the devices immunity to less than desirable conditions,

The rest are just suggestions
 

Offline Skimask

  • Super Contributor
  • ***
  • Posts: 1425
  • Country: us
Quote
So via stitching is what I did and it ok to do?
Decent start, but you can add more to fill in those open spaces on the top layer.  But I'd save that for somewhere around last.  You got other stuff to fix.

Quote
I'm rerouting with 10-15 mil traces. And widen or lessen the clearance?
Fatter traces, fatter clearances.  In the future, when you decide you want to change something, you've got a bit more room to play with.

Quote
And I can't believe I forgot the decoupling caps. 10uf eletro and 10uf ceramic caps be ok?
Watch Dave's last video.
I didn't take it apart.
I turned it on.

The only stupid question is, well, most of them...

Save a fuse...Blow an electrician.
 

Offline thomasb9511

  • Contributor
  • Posts: 19
  • Country: us
Any better guys?

Top copper layer

Bottom layer

Schematic
 Added bypass caps
fatten up traces and clearance
moved everything closer together
 

Offline radar_macgyver

  • Frequent Contributor
  • **
  • Posts: 380
  • Country: us
Looks a lot better. I suggest adding a copper fill (polygon) under the heat sink tab of the 3.3V regulator. This acts as a heatsink. Consider routing the crystal nets around the crystal rather than underneath. You may also want to increase the clearance between the fill poly and the traces. Finally, this may just be a personal preference - I don't like using long diagonal traces, when all the parts on the board are oriented vertically or horizontally (ie, none are rotated 45 degrees). This lets me route using fewer vias.
 

Offline Skimask

  • Super Contributor
  • ***
  • Posts: 1425
  • Country: us
I'd also move the outer dimension (the bounding dimension, the edge of the board) out a bit so the ground plane has a continuous path on both top and bottom around all four sides.

And echo the previous comment about the clearances on the fills and traces (I think it's the 'isolate' parameter).  Tight clearances on the fills make for easy chances to short some oddball trace directly to ground.
I didn't take it apart.
I turned it on.

The only stupid question is, well, most of them...

Save a fuse...Blow an electrician.
 

Offline thomasb9511

  • Contributor
  • Posts: 19
  • Country: us
Increased the polygon isolation
Added a heatsink pour for the regulator
Enlarged the board slightly

Top

Bottom
 

Offline Skimask

  • Super Contributor
  • ***
  • Posts: 1425
  • Country: us
Now you can still add more stitching vias to increase the ground plane area on the bottom layer.

Other than that, looks pretty good to me.
I didn't take it apart.
I turned it on.

The only stupid question is, well, most of them...

Save a fuse...Blow an electrician.
 

Offline thomasb9511

  • Contributor
  • Posts: 19
  • Country: us
Redid the board layout entirely
Larger board size
Added a lot more via stitches

Top

Bottom
 

Offline ptodorov

  • Contributor
  • Posts: 11
  • Country: bg
thomasb9511 Can you please post the final brd file as well? I'm working on a 3D visualization tool for Eagle board files and would like to test with your design :) thanks
 

Offline elgonzo

  • Supporter
  • ****
  • Posts: 690
  • Country: 00
Holy moly... Did a hedgehog sleep on your PCB, or where are all those vias coming from?

Note that specifically with regard to your board, the via stitching has no negative side effect but it also has no purpose either. Your board is neither dealing with (somewhat) higher currents, nor is it dealing with high(er) signal speeds/frequencies. It's just a simple 328P board. So, why the obsession with all those vias?

There are only two things on your board that could possibly (i am stretching the meaning of "possibly" here) benefit from via stitching (if at all).

One would be a seam of vias around your board edges which would counter possible EMI radiated from your board. The other would be the copper pour functioning as a heat sink for your VREG (using vias as "thermal vias" to connect the heat sink copper pour on the top with a copper pour on the bottom, thus increasing the thermal capacity of the heat sink). Side note: I do not expect EMI or the size of the current heat-sink copper pour to be really a problem for your board design...

With regard to when and why via stitching is recommended/necessary, read the following thread: via stitching in PCB's (random pick, there are probably more threads here which say something similar along those lines).

Remember that i said that the via stitching on your board has no negative side effect. So, if you like 'em, keep 'em. Don't worry. Just try to understand what the reasons requiring via stitching are and whether they apply to your board...
« Last Edit: March 20, 2016, 11:08:40 am by elgonzo »
 

Offline TheDirty

  • Frequent Contributor
  • **
  • Posts: 440
  • Country: ca
A little late, but are those slots specified on the USB connector?  If this is a cheap chinese PCB batch vendor, like elecrow, seeed, ... they may not support those slots.  I've had to change some slots to larger holes in order to get these through.
Mark Higgins
 

Offline Karel

  • Super Contributor
  • ***
  • Posts: 1374
  • Country: 00
Redid the board layout entirely
Larger board size
Added a lot more via stitches

Check ratsnest. You forgot at least one connection.
The difference between theory and practice is less in theory than
the difference between theory and practice in practice.
Expensive tools cannot compensate for lack of experience.
 

Online blueskull

  • Supporter
  • ****
  • Posts: 12281
  • Country: cn
  • Power Electronics Guy
Whenever putting an RoHS symbol, you also need to put (if my memory served me correctly) an eX symbol (e0, e3 or e4, which are the most common ones) to indicate which solder alloy or alloys combination you want to use.

http://www.ipc.org/3.0_Industry/3.4_EHS/LeadfreeLabelingStd.ppt
 

Offline AndyC_772

  • Super Contributor
  • ***
  • Posts: 3446
  • Country: gb
  • Professional design engineer
    • Cawte Engineering | Reliable Electronics
Personally I never put an RoHS logo on the board, because the PCB artwork isn't what determines whether or not the finished product is RoHS compliant. You can, for example, assemble a compliant bare board using tin-lead solder, and then the assembly is non-compliant but the logo is still there.

Offline gauravmp

  • Regular Contributor
  • *
  • Posts: 75
  • Country: us
I haven't readrough all the comments and someone might have already pointed this out. I notice that your name is not written in silk screen. It is instead a copper GND surface. Change that in the top/bottom layer setting and you should be  fine. Else, you won't be able to see your name. It'll just appear as a trace.
 

Offline vzoole

  • Regular Contributor
  • *
  • Posts: 122
  • Country: hu
I prefer solid ground as possible like this:
(I used Eurocircuits basic rules so easy to make it)


 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf