Can you review my PCB design?=)!

[eKoh]

Hello there=)! I am kinda new to the PCB designing and this is my 2nd semi-large pcb design. As I want to improve, I would like to see what my errors are and which things I can improve=)

Bottom Layer:


Top Layer:


And down here I attach the files.

Mediafire - TDS_v3.1.rar

Thank you=)!

[dmills]

I don't think you have ground continuity (The ground by the SDA pin connects to an island on the blue layer with no connectivity to the other ground pins (Also the right hand connector does the same thing on several pins).

Also, why the almost plane on the red layer for 5V when it would be better to use that plane for ground?

Decoupling caps are a good and happymaking thing, especially when one of the supply rails is so indirect.

Why did DRC not catch the disconnected ground islands? I would fix this and then re run the DRC (and clear the resulting errors) before going any further, especially as I think I still see some rat lines on there.

73 Dan.

[MarkS]

You need to rethink your parts placement. Is the board design set in stone? You are using the Arduino R3, which has female headers. I'm assuming you are going to use male headers on the bottom of your board to mount the Arduino? If so, you can place nearly everything else on the top side of your board within the Arduino outline and both reduce your board size and make routing MUCH easier. You should be able to route this as a single layer board + ground plane.

[hammy]

Your mounting holes look like fiducials.
The way you route the traces is wasting space (and is -sorry- strange ).
There are at least two or three islands in your ground pour. Why such a large area without copper in the middle of the board?
Is the DRC ok?

[generic_username]

as hammy said, you should first run an ERC and DRC check ( Board view second last column if memory serves me right)
others have pointed out that your ground is not continous as you can't see any ground vias connecting that island.

As a suggestion for future design, do you home etche your PCB or are you letting it manufacured? if home made I would check the drill size to match with a drill you own and if you have space make the vias bigger - easier to solder and more resistant if you have to solder/ unsolder this pin a lot.

Some parts can be moved much closer together to save PCB space- I guess space is not critical here but would be good practice keep the layout compact.
just my 2 cents

[HSPalm]

The white text, is it on silkscreen layer? I think it may be too small/thin to be visibly screen printed.

[MarkS]

I was bored, so I did this:



I don't recommend that you use this. I do not know your design needs; this is to show how you can stack parts to reduce board size and simplify traces. Also, I'm a hobbyist and this probably has design flaws that would be immediately apparent to a seasoned PCB designer that I undoubtedly missed. I am also not 100% certain that there will not be interference between the I2C pull up jumpers and the Arduino.

As you can see though, all but one of the power traces are on the bottom layer and all but a handful of signal traces are on the top layer - no vias! There are no isolated regions on the ground plane. I swapped the GND and 12v signal on the 3-pin header to allow for easier routing and to ensure that the GND pin had more contact with the ground plane. With the GND pin in the middle, as you had it, it had only a single connection between it and the plane. This may not have been necessary, but seemed cleaner.

Now that I think about it, why do you have two separate I2C buses? The I2C bus is addressable. i.e., multiple parts on a single bus. You should only need one and this would greatly simplify the design.

Your mounting holes look like fiducials.

This is how Eagle draws unplated holes.

[MarkS]

With a single I2C bus:

[Feynman]

Does the XBee module have some kind of embedded antenna? In that case you might be required to remove copper underneath that antenna.

[MarkS]

Does the XBee module have some kind of embedded antenna? In that case you might be required to remove copper underneath that antenna.

The XBee datasheet makes no mention of this, or any PCB layout instructions, other than it is designed to be used with female headers.

[Mattylad]

Its not a good idea to have groundplane under the antenna unless the design docs specify it.

In this case they seem to say not.
read page 27
https://www.digi.com/resources/documentation/digidocs/pdfs/90002002.pdf

Also have a look at:
https://www.sparkfun.com/products/8665

[MarkS]

Its not a good idea to have groundplane under the antenna unless the design docs specify it.


In this case they seem to say not.
read page 27
https://www.digi.com/resources/documentation/digidocs/pdfs/90002002.pdf


Also have a look at:
https://www.sparkfun.com/products/8665

That's good to know. I missed that while looking through the datasheet. Regardless, I'm done with this. This isn't my project and the OP has seemed to have abandoned this thread. My efforts were to direct him towards layouts he may not have considered. I cannot even be sure he has looked at this thread since his last post.

[eKoh]

That's good to know. I missed that while looking through the datasheet. Regardless, I'm done with this. This isn't my project and the OP has seemed to have abandoned this thread. My efforts were to direct him towards layouts he may not have considered. I cannot even be sure he has looked at this thread since his last post.

I am sorry that I haven't relpied. I've read almost all the answers I got, but I am super mega busy with school stuff, my free time is super limited. I'll reply on this sunday (after 2 tests in a row :s)

Nvm, I'll post some stuff quickly.

These are my manufacturer's capability:



And these are the modules I am using:



* Kinetis KL 25z (Its pinout is compatible with arduino)
* MCP2515-CAN (I planned to use Screws with this module, because it is only being hold by their pins, that's why the 2 holes near the 8pins connector)
* DB25
* XBee Pro S2C (I need it to be facing the opposite way that the DB25 does, this is to make it easier to place the shield in the actual prototype)

[westfw]

These are my manufacturer's capability

"mechanical etching" without plated-through holes?   You may need to do something else for the connectors where you are not able to solder on both sides...

I like that you have nice thick traces.  You should think about increasing the clearance and isolation parameters so the gaps are wider too.  (or perhaps not - this will cause additional tool wear and routing time...)

[eKoh]

These are my manufacturer's capability

"mechanical etching" without plated-through holes?   You may need to do something else for the connectors where you are not able to solder on both sides...

Oh I see, the mechanical etching it is how is called.
And for the "vias" I use a small cable welded through both sides. It worked for a pcb I made before, but I dont know if there is a better way to do it.
 
quote author=westfw link=topic=84632.msg1160713#msg1160713 date=1489571550]

I like that you have nice thick traces.  You should think about increasing the clearance and isolation parameters so the gaps are wider too.  (or perhaps not - this will cause additional tool wear and routing time...)

I tried to do that, to make it easier to weld, but the results I got are those "islands" that appear when I increase the isolation for the ground plane. Is there a better way to do that?

[ebastler]

for the "vias" I use a small cable welded through both sides. It worked for a pcb I made before, but I dont know if there is a better way to do it.

That should work nicely for the vias. But how do you handle the connectors (posts and Sub-D connector, or whatever it is) where you need to connect some of the traces on the component side?

[richardlawson1489]

Have you checked file in FREE PCB File Check tool? It will help to correct some Design Issues Automatically.