Here is my second PCB I've designed, please critique!

Go To Last Post
14 posts / 0 new
Author
Message
#1
  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi Everyone,

Please give me any suggestions to improve it:

http://www.sadevelopment.com/pre...

I've tried to follow all the suggestions I've received in the past, although making all the components face the same direction on the board isn't one of them. I usually rotate a component so that the track route better. I try to if I can keep them going all the same direction however.

I do still need to mask out some ground plane under the LCD, etc...

Thanks,

Alan

[Alan, this really belongs in General Electronics - I'll move it there - Cliff]

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Looks good, except you should run a track through the ground pins, not rely on the polygon pour to connect them. That's particularly in the case of C1, C2, C14, where the connection looks quite unreliable. Also, I don't know what layout package you use, but can it be made to remove dead copper on polygon pours? The little isolated islands on the ground plane are a bit unprofessional.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

As you don't have a VCC plane, route any high current paths directly to the power input. (like your piezo) Do not share this trace with the logic on your board, as this trace could have large switching transients on on.

Writing code is like having sex.... make one little mistake, and you're supporting it for life.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi Guys,

First, thanks for the help!

Peret: I've got to remove the islands manually.. Here is an update with more detail. I think what you mention about C1/C2/C14 just looks that way because of the PDF. Here are both layers:

http://www.sadevelopment.com/pre...
http://www.sadevelopment.com/pre...

Glitch: Should I put in a VCC plane on a 2 layer board? I've thought about doing it - are they any disadvantages other than I would need to make sure it isn't too cut up with all the top layer traces...

Thanks,

Alan

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

You mean Vcc copper pour. A power/ground plane is a whole dedicated power or ground layer in a multi-layer board, although it might have the odd track on it.

Leon Heller G1HSM

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi Leon,

You are correct, I meant Vcc copper pour.

Thanks,

Alan

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

I don't think you need a VCC plane. Both your VCC pins are decoupled at the chip. I take it LCD pin 15 is power for a backlight. If T2 is PWMing that backlight, you might not want to share its VCC line with the one that provides your ADC reference - it would be easy enough to run a separate VCC back to the regulator output capacitor. Which should perhaps be larger, but I'm critiquing the layout, not the circuit design.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi,

T2 is PWMing the backlight. Do you think I should run two traces from R4. One to LCD Backlight + and one to the VRF1/uC/ISP?

I am using a 48uF ceramic cap at C18 for the regulator output cap.

I added some extra pads thermally connected to ground near grounds I thought could use some extra trace width to ground. I connected these added pads with a top trace. You will see them on T1/T2/T3 and other grounds...

Please critique away, I am welcome to all suggestions!

Does anyone have a tip on tacking the cylindrical crystal to the PCB. Should it be to an isolated pcb area or grounded? I have the crystal surrounded by a small ground pour on the top as well.

Updated:

http://www.sadevelopment.com/pre...
http://www.sadevelopment.com/pre...
http://www.sadevelopment.com/pre...

Thanks,

Alan

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Quote:
T2 is PWMing the backlight. Do you think I should run two traces from R4. One to LCD Backlight + and one to the VRF1/uC/ISP?

Yes, but take the backlight track off C18, not R4.
Quote:
Does anyone have a tip on tacking the cylindrical crystal to the PCB.

The crystal doesn't need to be secured unless you think it will fall off or be knocked off. It shouldn't need to be grounded and you shouldn't solder to a cylindrical can anyway. You may want to secure it mechanically with a dab of hot melt or rubber cement.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

alank2,

What type of PCB will you be using for this? (FR4 PTH & Soldermask etc)
How do you plan on assembling the board?
How many do you plan on making?
Is this for a commercial product?

The tracking to the right of the MCU looks tighter than it needs to be - no need to push clearance tolerance on PCB unless you have to.

Pretty decent job if this is only your second pcb :)

oddbudman

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi,

oddbudman wrote:
What type of PCB will you be using for this? (FR4 PTH & Soldermask etc)

Yes. FR4 PTH + Soldermask. My first couple boards will probably be a no soldermask prototype of it from expresspcb.com

oddbudman wrote:
How do you plan on assembling the board?

By hand. This board is better than my first design because it moves buttons, etc., on the PCB so I can assemble quicker.

oddbudman wrote:
How many do you plan on making?Is this for a commercial product?

Not sure yet. I will probably try to sell in small quantities.

oddbudman wrote:
The tracking to the right of the MCU looks tighter than it needs to be - no need to push clearance tolerance on PCB unless you have to.

It exceed 12mils. Should I make it larger simply because there is room? All my small tracks are 12mils as well and my larger power tracks are 40mils.

oddbudman wrote:
Pretty decent job if this is only your second pcb :)

Thank you; I appreciate it! :)

Alan

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

12thou should be pretty comfortable for a commercial pcb house.

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

Hi,

Thanks for the help everyone; it is appreciated!

Alan

  • 1
  • 2
  • 3
  • 4
  • 5
Total votes: 0

- Most of your silk text will be covered by components. I'd move the ones for connectors and buttons so they will remain visible.
- Put a "1" or "*" next to pin 1 on the connectors; the square pad will not be visible once the connector is in place.
- Your resistor networks are butted together. Some need more space between them or they will hit each other.
/mike