PCB design: surface mount layout help (tracks)

[lcipher3]

So I'm doing a surface mount board for the first time. I've done a few dozen though hole projects, etc. It's going to require a different strategy I guess!

In my through hole designs it sure is nice to have the option of FRONT or BACK (2 sided board) due to the nature of "through holes". That pretty much gives you XY access to all parts. I would also usually do a ground plane on the BACK and have a ready available easy ground.

Any surface mount PCB people with some tips? Use a lot of vias? What's your ground strategy? How do I use the "BACK" side effectively?

 

[bowanderror]

Is your board 100% SMD (including IO, power & ground headers)? Usually you'll have some through-hole components and pads for IO & power, so that gives you some built-in connections to the bottom layer. Beyond that, vias are usually required for boards with a high percentage of SMD components. Try to keep them to a minimum, and it's good practice to run ground vias next to power/signal vias if you have any of them. I'd still use a bottom ground layer and top Vcc layer if that's what you're used to.

Sparkfun has a good tutorial on laying out mixed TH/SMD boards.

 

[vigilante398]

I like keeping all the components on one side personally. Yes you have room to do both sides, but all components on one side makes assembly easier, and it makes debugging a lot easier, especially if something needs troubleshooting after it's in the box. So absolutely throw vias everywhere (an exaggeration of course, but don't be afraid to use them where needed), take advantage of space. Sensitive circuits, of which there are few in the effects world, like to have a solid, unbroken ground plane. Realistically most circuits can get by just fine by filling in ground over unused space when you've routed everything else. Having a solid DC reference, be it ground or VCC, is a good idea for reducing noise as well. I personally fill all unused space on both sides of the board with ground, but doing one ground and one VCC has advantages as well.

 

[lcipher3]

Thanks - appreciate the tips. I think I have a strategy - now trying to understand BGA and its requirements, therma vias, etc.

 

[Feral Feline]

@lcipher3, please update as you progress — very interesting thread!

 

[vigilante398]

Thanks - appreciate the tips. I think I have a strategy - now trying to understand BGA and its requirements, therma vias, etc.

What are you doing that needs a BGA? Depending on the package you probably will need more than 2 layers. Most of the BGA designs I've done were FPGAs, and for those it's common practice to put a via for every single pin so you have access to the signal from all the other layers both for easy routing from any layer and access to exposed vias for probing in troubleshooting. The common practice I followed was to break the BGA into a 2x2 grid and each quadrant had the vias offset diagonally, i.e. pads on the top left of the package had vias above them to the left. This is the cleanest way I've found to work with them, and leaves a "+" shaped gap in the center of the package where there are no vias. This is for signal access, not thermal properties, I've only ever needed to worry about thermal issues on a BGA when the BGA was a high-current DC converter.

 

[lcipher3]

Its an LTM8054 for a stepper motor driver (not my selection, not my choice.)

 

[vigilante398]

Its an LTM8054 for a stepper motor driver (not my selection, not my choice.)

You should be fine with a two-layer board then, follow the layout guidelines in the datasheet and use their recommended via placement, and you should be good to go.

 

[lcipher3]

Thanks - am I right in assuming that there are no thermal isolation pads on the top surface (to ground)? that the solder mask is what "borders" the pad for the bga package?

 

[vigilante398]

You should absolutely have solder mask between BGA pads, and I would also recommend putting a solid ground pour on the bottom layer under the LTM8054. Unless you're mounting a heatsink or heat pipe to the IC itself (which I don't usually do for anything less than a massive processor), your ground connection is going to be the main thing that spreads the heat out and gets it away from the IC, so you want the ground pour as big as is reasonably possible. Bonus points if you have a chassis connection connected to ground so heat can be dissipated to the chassis itself. The point of the thermal vias is to share the heat between the top layer ground pour and bottom layer ground pour. I haven't read the LTM8054 datasheet (that's your job) so I don't know how much power you're dumping with it, but a two-layer board with a lot of ground space and a lot of vias in between the two ground pours should do the trick.

 

[jubal81]

@vigilante398 , are you still populating your PCBs yourself or using pick&place service?

 

[vigilante398]

@vigilante398 , are you still populating your PCBs yourself or using pick&place service?

I've switched over to pick-and-place. I do too many builds and populating by hand was taking up too much time. Plus the assembly houses get their parts direct and don't upcharge them, so I'm saving money on components at the same time. It was a win-win switching over.

 

[lcipher3]

You should absolutely have solder mask between BGA pad.

Thanks - I get that. I mean there should be direct connection to the ground pads (circles) with no thermal pad relief like in a normal ground thru hole pad.

 

[vigilante398]

Thanks - I get that. I mean there should be direct connection to the ground pads (circles) with no thermal pad relief like in a normal ground thru hole pad.

View attachment 17494

Ah gotcha, sorry I misunderstood the question. Thermal relief on the BGA pads themselves are probably optional, you won't be hand-soldering it (obviously), it will likely be reflowed in an oven. As for the thermal vias I would leave them as direct connect, no thermal relief. You want those to be able to spread the heat efficiently between the two (top and bottom) planes, so the more conductive material there the better.