Please review my first SMT board/schematic...

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

Hi,

This is more on my first SMT project, a tiny breadboard meter that measures voltage and current that plugs into a breadboard.

Do you guys see any issues - I am planning on soldering by hand...

Everything is on the underside except display (u4), buttons (sw2/sw3), and the two jumpers (j1/j2).

The power switch and DC barrel jack are also on the underside.

Thanks,

Alan

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

Have you run a DRC on the board? TP1 seems to crash with the other 2 components next to it.

Also some components are outside the PCB area, or at least their outline seems to be.

Nothing disastrous but a DRC would bring that out along with anything else that might be wrong.

John Samperi

Ampertronics Pty. Ltd.

https://www.ampertronics.com.au

* Electronic Design * Custom Products * Contract Assembly

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

Hi John,

Yes, I've run the DRC and cleared away all the issues it found. Eagle doesn't seem to care/report about silk extending past the board edge.

TP1 is just a test point for reading voltage, so it is ok if its silk runs into the other headers a bit.

I've got the power switch silk extending past the board edge, and actually have the DC power jack slightly extending so you can see it from the top of the board (it is on the underside).

Thank you for looking at it - do you think I've got the SMD components far enough apart for easy solderability...

Thanks,

Alan

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

Hi Alan,

Cool project.

Two thoughts:

Since nothing I build ever gets mass produced I don't worry about incremental costs from "extra" components.

If you wanted to, you could add a series resistor on the Port C pins going to the PB Switches to ground. The reason to consider doing so is that if your initial code mis-configures a pin, or if the program ever runs amuck, you won't have the pin shorted directly to ground.

You might also consider a power switch mounted on the top, with the slider mounted facing upwards, instead of sideways.

The reason is this: If the switch is top mounted, facing upwards, then the User is pushing downwards, (and sideways). This pushes the PCB down against the prototype board. With a sideways facing switch, at the farthest point from the fulcrum created by the pins which insert into the prototype board, there may be a greater chance the user will flip the power supply board upwards, or even dislodge it completely, especially if they are trying to turn it off in a hurry.

With 6 mounting pins per rail this might not even be an issue, but it is even less likely to be an issue if the User is pressing downwards and sideways, instead of just sideways, and perhaps accidentally upwards and sideways.

It is easier to picture this in my mind than it is to explain it in writting!

JC

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

I find 25mils to be sufficient for things like 0805 components. You seem to have lots of space between chips.

With the DRC I allow the "standard" rules which came with my package (not Eagle) which seems to be OK with the people making my boards.
It did ANNOY me very much when I first got it as I didn't care much spacing for overlays but I ended up succumbing to the higher authority
to stop it from nagging me. I get plenty of that elsewhere. :lol:

John Samperi

Ampertronics Pty. Ltd.

https://www.ampertronics.com.au

* Electronic Design * Custom Products * Contract Assembly

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

Oh man! Time for a poll:

How many protoboard Users put the V+ and Grounds:

1) Both Ground rails towards the center of the board, V+ rails on the outsides of the board?

2) Both V+ rails above both Ground Rails?

I always put the Ground rails on the inside, closest to the center of the protoboard.

I guess it doesn't matter, but either way I'd be sure to put a BIG + and Gnd label overlying the rails.

JC

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

Thanks JC, good ideas!

Here is some more info about this project and a video of the prototype from another thread:

It handles voltage from 0-20V, current from 0-1000mA, relative mode, low/avg/high mode, fast low/avg/high mode, and calibration.

Video showing its features:

http://www.youtube.com/watch?v=0...

Image:

Thanks,

Alan

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

Hi,

js wrote:
I find 25mils to be sufficient for things like 0805 components. You seem to have lots of space between chips.

Excellent; thanks!

DocJC wrote:
Oh man! Time for a poll:
How many protoboard Users put the V+ and Grounds:
1) Both Ground rails towards the center of the board, V+ rails on the outsides of the board?
2) Both V+ rails above both Ground Rails?

Interesting - all my boards are labeled +/- or have a red line on top for +/vcc and a blue line below for -/gnd.

I'm going to label them and move that pesky TP1 and the same time!!

Thanks,

Alan

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

Ah, you have the FANCY boards.

Most of mine are generic white.

JC

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

Hi,

DocJC wrote:
Ah, you have the FANCY boards.
Most of mine are generic white.
JC

Well, I don't know about fancy... My better boards are from Jameco (which are rebranded Wish or Wisher brand).

Thanks,

Alan

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

Hi,

I updated my board with a few changes (images in post #1 are updated).

I made the power switch on with the position upward and off with it downward.

I improved some traces.

I thickened the main power lines.

I labeled the breadboard pins with + and -.

I added a ground test point.

Thanks,

Alan

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

Use a kelvin connection on R1 to R6. At the moment you have current running through your sense point that can give you errors. Move R1 away from the current path and use another track from R6 to R1.

Add a transzorb for overvoltage and reverse polarity protection.

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

Hi Kartman,

I've looked at the Kelvin wiki page and I'm still not following you... Can you post a schematic of the changes? I appreciate it!

Thanks,

Alan

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

Hi,

So use a sense resistor like this?

http://www.ohmite.com/cat/res_lv...

Are the V terminals the same side? Current would flow from one I through to the other I and the V terminals would be for sensing the voltage?

Thanks,

Alan

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

No such luxury on an ipad!

Realise that your pcb tracks are resistors. Depending where you sense the voltage across R6 is critical. Thus, the kelvin connection is where your sense tracks are separate from the current carrying tracks. You did this on the other side of R6. Therefore rather than have R1 connected in the middle of a current carrying conductor, move it and use a small track to connect it to R6.

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

Hi Kartman,

I think I get where you are going with this now. I'll modify the PCB and repost some pictures in a little bit here.

Thanks,

Alan

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

Hi Kartman,

How about it now? I also added the other resistor that the datasheet said would "maximize the dynamic range of the circuit".

Thanks,

Alan

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

Yes, exactly what i was talking about!

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

Thanks Kartman!

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

I think you can optimize the LED segment traces in such way no crossings are necessary, basically one straight lane from the MCU to RN1.

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

Hi,

Good idea jayjay1974, I optimized it for connecting to the display first, but perhaps I should have done it the other way around since there is more room around the display than the uC for track routing...

Thanks,

Alan

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

See also traces from U1 to R1.

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

Hi,

Do you guys think I need to reduce the solder mask exclusion size around these pads? This is the default size that Eagle came up with, but it doesn't create much between pads that has mask. That area lacks copper though so I don't know if this is fine or not.

What do you guys think?

Thanks,

Alan

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

Bump!

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

What is the pad size and spacing?

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

Hi,

ltc6102
msop-8
0.017 x 0.049 pad size
0.65mm

Actually, I don't see a way to edit the stop mask size in Eagle - I thought I could just go to the stop layer and right click it, but this does not work...

Thanks,

Alan