Power Board Layout

You are not logged in.

Please Log In for full access to the web site.
Note that this link will take you to an external site (https://shimmer.mit.edu) to authenticate, and then you will be redirected back to this page.

Powerboard Layout

OK last week-ish you did the schematic for your LM3671 buck converter. It was pretty simple...like what...six or seven parts counting the connectors? The schematic of your modern buck converter is pretty simple too. Here's the reference design from the LM3671 datasheet.

The general schematic of our Buck Converter (taken from datasheet)

What about layout? Can you just put things wherever for this board like you did with the sensor board with little fear of electrical issues? Not really...the Buck Converter is a switching supply and one that moves a lot of current and makes a lot of electrical noise as well so we need to be a bit more mindful of how we lay things out. Page 21 of the data sheet has some protips about laying out the board and then Figure 38 (shown below here) is a recommended layout of the board.

TI's recommended example PCB layout (taken from the datasheet).

The list of items they provide is pretty standard and a good number of these you shouldn't even need to worry about for right now. The big takeaway for you is:

  • Big, short traces on any route carrying a lot of current. The inductor and capacitors we have low series resistances, it would be a shame to throw that characteristic away by putting long nasty high-resistance PCB traces in your circuit introducing lots of parasitics.
  • Keep components close by
  • Try to electrically isolate the SW terminal (that's the end of the inductor that is going to be kicking all over the place with weird voltages when getting switched).
  • Keep the feedback path away from the SW terminal if possible (route around it/try not to go under it).

There is another point about making sure the current is always looping about in the same direction on both phases of the switching sequence. I've sketched out what they mean below for reference, but between you and me I think you'd have to try really hard to do what they're saying not to do.

The current loop in both phases of this buck converter's operation shown both in the schematic and on their recommended layout.

One thing that would be nice to experiment here is with non-standard traces. You can see in their recommended layout they're clearly doing some nice pours to make sure all the copper is getting used. While big, thick standard traces are definitely good, you may also want to try to emulate these pours. You've done one pour so far, a ground pour on the back side, but now you can get some practice doing some smaller ones.

After positioning your parts in a way that you think will work well, do a small pour on the front copper. When you click, attach it to the net of interest (for example the SW net that connects the SW pin of the LM3671 to its inductor) and set the pad connection to be "Solid" for this pour rather than "Thermal Reliefs" (doing so will allow the pour to connect all the way to the pad. Actually lay out a nice polygon around where you want to connect.

Do a copper pour on the front and when you click, link it to the appropriate net (here I'm doing the SW net). For this net make sure to specify that pad connections are "Solid" rather than "Thermal Reliefs."

When done, run your pour (the "b" key) and you should have something like this:

With some careful attention to detail I have a nice, short tapered connection from pin 5 of the buck chip to the inductor.

Try your best on this layout. Our buck converter and its needs are not too demanding in my experimentation, but who knows, you students always figure out interesting ways to break things so I'm excited to see how your design turns out.

Submitting your design

Once you are satisfied with your pcb, submit to git. (as a reminder, see the instructions from ex02/sensorboard_schematic for more details about how to set this up)