RF PCB layout, please critique (be vicious!)

[Alexorcist]

Hi! This is my first post here at the EEVblog, and yes, it's an assignment-type question 

Anyway, I have been learning RF layout through countless PDF guides and Application Notes and am looking to design a FMCW Radar. Attached are front and back renders of the Radar PCB as well as a PDF schematic.

Here are the Specs:

All Minicircuits Parts (I will make some stages discrete if I ever get access to a VNA)
900-1500 MHz Operating Frequency (Attempting to use this as a Ground Penetrating Radar)
Grounded Coplanar Waveguide traces at 50 Ohms Z0
Stackable Design with M2 mounting holes to attach a case for shielding
4-layer board (middle 2 layers are solid ground) because OSHPark uses FR408 with a DK of 3.66 for 4-layer boards

Please comment on any PCB design Faux pas and/or thoughtless errors on my part. (Anything, be picky!)

Thanks, (and hopefully with the forum's help i can conjur some black magic and have this board work on the first try  )
Aleksa

[T3sl4co1l]

No clue what the footprints are (or if they're correct), or why they need so many ground pads... I'll assume you've checked that.

It doesn't look like there's clearance around any pads, or if there's +V or anything going on here.  That might just be the pictures.

I would note this: avoid via-in-pad unless you have a very good reason for it (e.g. because you have no choice as with QFNs, or for heat dissipation).  I guess you just copy/pasted the grid there, so, just shuffle those around a little where they're touching things.

If all you're doing is slapping stuff together over ground, without having to cram it together around everything else, there's not much you can screw up.  It's when you need things tight, and correct, and you're doing impedance elements in the board, that things get really tricky.

Also, if you have nothing on inner layers at all (just ground), you might as well go with a 2 layer build.  50 ohm coplanar waveguide is quite a bit larger at standard board thicknesses, but it doesn't look like you'll run out of space or anything.

Cheers

Tim

[Alexorcist]

Thanks  , i was wondering why kicad let me put the vias on the ground pads and  may have gotten a bit too crazy about the 100 thou grid when via stitching (not to mention that the board will cost half as much on 2-layer)

Aleksa

[Alex Eisenhut]

Ouch, you better put thermal spokes or you'll find you need lava to solder the parts in.

[Alexorcist]

I was going to grab some from Alibaba...

Thermals are a good idea though, just added some now.

Thanks,
Aleksa

[marshallh]

BTW due to an error in oshpark's rendering engine, Soldermask apertures overwhelm the copper layer. So what you see in the picture isn't copper, but the soldermask openings.
VIP for thermals is fine, and unavodable. It would be a good idea to un-tent the vias ont he opposing side so that you won't get gas trappage.

[nctnico]

I'd put the stitches along the RF traces instead of in a grid.

[LukeW]

Adding thermal reliefs to the groundplane is like adding an inductor in series with the ground pin on each chip, and although it's very small, it does negate some of the low-ground-inductance advantage of that groundplane.

Normally I'd be used to something like a QFN chip with a ground pad underneath and I'd be less concerned about the ground path, but a module like the Minicircuits TAMP-272-LN+ (or any others in the same module form factor) doesn't have that. But then again it does have 9 ground pins, so if they are all connected then the ground inductance should be minimal, even if thermal reliefs are used.

Just for interest, I've also attached a pic of a layout I've done recently - for comparison.

There are vias in the exposed ground pad under the RF chip at bottom left, and the ground pad of the MMIC at bottom center (3-terminal Minicircuits amp, DF782 package) and also under the end-launch SMA connector. (This ends up with a very strong mechanical bond as well as good ground.)