GNS Breakout - comments before fab?

[gregcope]

Hi All,

I have designed a M0 breakout board for a CAM-8M ublox GNS module.  The idea being that this keeps the battery backup powered all the time, but an LDO with an enable pin powers the main VCC of the module so that it can be powered off most of the time.

https://github.com/gregcope/MoteinoM0CAM-M8

Any feedback before I send it off?  Never made an SMD board before.  Or used an LDO.  Be gentle.

[Felix]

Looks pretty good!
I would add some extra vias under the module in the GND pour.
I would also eliminate the vertical GND pad connections and only keep the horizontal ones.
Does your GNSS module come with an antenna?

[gregcope]

Looks pretty good!

Thanks!  I will take that as high praise considering its attempt one!

I would add some extra vias under the module in the GND pour.

Done

I would also eliminate the vertical GND pad connections and only keep the horizontal ones.

Do you mean on the module?  These are required.  It has outputs/inputs on three sides.

Does your GNSS module come with an antenna?

Yes.  That is what the hatched out restricted area is in the top middle.  The hardware PDF has some recommended requirements around GND plane size to improve performance (e.g. 10mm either side) that I cannot quite meet or understand.  I am hoping the GND plane of the Moteino and other boards will compensate for that.

You can add external, however that needs more parts, that I do no yet understand and the internal one is supposed to be pretty good.

Many thanks Felix.

[Felix]

For the GND pads of the module - I meant you don't need thermals on more than 1 side. You have them connected between themselves in addition to the external GND plane.
That's not a mistake or anything, but it will make it difficult to hand solder the module because those pads will sink a ton of heat.
Also if you ever want to desolder the module with hot air, you will really struggle if the GND pads are connected to the larger GND plane with a LOT of "trace". It increases the thermal mass of the module making it difficult to rework it.
I often limit those thermals to a single or dual thinner trace rather than the fat default traces.

[gregcope]

Ah.

I did notice that eagle is connecting them underneath too.  No idea why... will try deleting them and seeing if it beelts.

[Felix]

To eliminate some of the GND thermal connections in Eagle you will have to draw some small RECTANGLES on the tRestrict layer, where those thermals are, that will break their connection.
To make their width smaller, you have to edit the WIDTH of the GND pour polygon.

[gregcope]

I am planning to hand-solder this board.

Will see what i can do.

[gregcope]

So I ordered this version; https://github.com/gregcope/MoteinoM0CAM-M8

[gregcope]

And yes... noticed the top right ground via is not connected... no real issue for MK1a

[gregcope]

Got a board back from JLCPCBs.  They did not do a great job of the castellated holes, rest looks okay.

Hand soldering 0603 SMD parts is quite tricky.  Need a finer point on my iron.  No idea how I cam going to solder the CAM-M8.

Poor photo from my iphone.

[gregcope]

And an update...

Everything works ~ which I am quite pleased about, as this is my first nontrivial board and a first with SMD parts.

Only issue is ... I cannot seem to pick any satellites;

Code Select Expand

$GNRMC,,V,,,,,,,,,,N*4D
$GNVTG,,,,,,,,,N*2E
$GNGGA,,,,,,0,00,,

I do not quite understand the LNA and ground plane requirements from here;

http://ozzmaker.com/wp-content/uploads/2016/08/CAM-M8-FW3_HardwareIntegrationManual_UBX-15030063.pdf

I think I need a much bigger board (min) 40mmx20mm instead of 20mmx20mm, which without an external antenna it will not work as a MO add-on board.

[Felix]

Even if you go outside?

[gregcope]

Will try it, but i was in the same spot as my other GNS recieves ...

May try today.  Its not raining (yet) today

[Felix]

The reason I asked is because it has a tiny tiny antenna. I don't expect that will work very well inside at all.

[gregcope]

Ah.  It works. Sort of.

Firstly i noticed a mistake in my design is that i forgot to join RF_OUT to RF_IN (ie get the antenna connected)

When i did that it started to get a time signal.  I then moved it to clear sky and it finally got a fix.

Secondly and its my mistake, ignored the comments about minimum ground plane size as I thought it would inherent from elsewhere.  It needs a min of 45x20 mm and suggested is 80 x 40 mm with no traces, just GND pour.

So not sure i can make it work as a breakout board without making it allot larger; which is what i will do for my project.

The rest of my design worked well (ldo/caps/resistors). Which is fab as this is my first SMD/ldo project, so i can reuse the design on a larger board!!!!