Is the PCB routing for this LM5143A-Q1-based buck converter right?

Question

Thanks to your advice on StackExchange, I'm in the final stage of developing my first LM5143A-Q1-based (link to datasheet) buck converter! It may be a bit rushed as I need to prepare this for a high school project and I'm still learning, but positive criticism is highly welcomed! The problem now is, routing. I would appreciate it a lot if you could take a look at it and tell me if there are any issues. What could be improved?

EDIT: High Quality (.SVG) images are available to download at this link. I wanted to place them in this post but the website doesn't accept this format.

This is the schematic, all done in Kicad:

This is the layout: Top Layer, all components mounted here

GND Layer

VIN Layer

The Bottom Layer, yes, big trace

There are a couple of quick questions I have about the visuals:

1. Take this via for example. Does the black area between it and the PWR (VIN) plane mean it's isolated from the plane? Else it would be shorted!

2.Take this via for example. If the standard trace goes into the filled zone, does that mean it's making contact and they're connected? Since it should

3. If the via is itself isolated, is there any reason to make another isolation copper island like in the photo below?

4. Is there any reason to use these "thermal reliefs" over standard tracks? (I did it since I heard they're good)

The layout was highly inspired by Brian's 4 layer board. (except from his perfect copper islands) From him and all the resources I searched, I understood a couple of basic design rules:

1. Ground Plane always underneath IC
2. Keep traces as short as possible (well, except for that huge L1-L2 connection on the back... How big of a problem will it be?)
3. Use filled zones instead of traces when possible
4. Keep all high freq parts on the same side

Thank you in advance for any advice! It's the first time I'm doing something like this and I loved learning it!

Answer 1

A couple observations: the DRC will answer a lot of these questions. If you have a trace going to a polygon on the same net but for some reason they're not connected, DRC will tell you. If you have a via or hole touching a trace or poly it's not supposed to, DRC will tell you, assuming you have your rules set up correctly. Your silkscreen is going to pop a lot of errors; it's easier to lay out your components the first time with silkscreen in mind rather than do a major redesign just to make designators visible.

You do not need the extra isolation around the vias. The black ring shows you that nothing will touch it (make sure all your copper layers are visible). A lot of them seem oddly sized, make sure your board fab house can handle them. If you plan on using them as plated through-holes for wires, then make them actual 1x1 PTH instead of giant vias. I can see several that will be unusable once components are populated. If they are supposed to be vias, the usual way is to add several instead of one giant one.

A lot of the polygons are oddly shaped and only half-intersect with the things they're supposed to. Sometimes you can't make everything look pretty but e.g. that poly for Earth on the lower left could use some love.

What is Earth? I don't see it anywhere on your schematic. If you mean GND, then make it one net only.

How are you planning on soldering this? If you are using a hot plate, then thermal reliefs are not necessary, but make rework easier. If you are using an iron and/or hot air then they are. Critically, your high current input/output pads are connected to huge polys and traces with four spindly thermal relief spokes.

Speaking of spindly, the traces on the bottom layer seem narrow. Like unmanufacturable narrow.

I would suggest looking at the datasheet for the chip, specifically the "layout" section. Power switchers are a bit picky about their layout. You're learning, which is great and this isn't a knock on you, but I doubt this board will function as it is currently laid out.

Finally, it doesn't look like you've taken thermal considerations into account. Page 56 of the datasheet describes how to remove heat from the exposed pad on the underside of the package using vias to a ground plane, which is missing from your design. There are other components that would probably benefit from being attached to a plane as well.

Answer 2

First of all, good job!

I'm not an expert in KiCad, but whenever you have such question, you can check the gerbers. They never lie since it's the file your manufacturer will use!

Here are the answer to your questions:

1 Take this via for example. Does the black area between it and the PWR (VIN) plane mean it's isolated from the plane? Else it would be shorted! -> Yes it's isolated from ground.

2.Take this via for example. If the standard trace goes into the filled zone, does that mean it's making contact and they're connected? -> I would say so, but be careful, based on other software (Altium) the behavior when repouring might surround your trace. Here it doesn't seem to be an issue.

1. If the via is itself isolated, is there any reason to make another isolation copper island like in the photo below? -> Not to my knowledge. I'm not working in very high voltage, but I don't see any reason to place that (except plane filling FYI-> when you have 8+ layer, you must ensure all your plane have copper on so the PCB remain flat)

2. Is there any reason to use these "thermal reliefs" over standard tracks? (I did it since I heard they're good) -> Thermal relief are very important whenever a huge part of copper is connected to a pad. Either a plane or a trace. Otherwise, it will be very hard to solder since the pad will remain cold. Not having thermal relief can also make component stand up.

Here are some of my comments on your layout

All the rules you have listed are good in general design. So, why did on the bottom layer didn't you place a plane!? (It's large, yes but it can be larger!)

Having huge vias, in general is not as good as several smaller. The impedance of one large via can't match 20 smaller one.

Your power plane (Vin) is highly degraded near the IC. I don't know your clearance constraint but they seem a bit loose which make the plane weaker.

Usually, you would want your stackup for a four layer to be (top to bottom) Components and most traces, GND, PWR, Rest of traces. The reason why this is the best topology is that the most trace are close to the gnd which give them a better impedance control. Also, it increase the capacitance between the GND and supply (this is the best decoupling capacitance since it has a very low ESR). Finally, it allow a way easier debugging since you can cut trace (I once had to cut a trace on a third layer, you don't want that!).

You have some very narrow trace that are quite long. I'd make them a bit wider so they are less lossy.

You seems to have some very small vias. Even if not a lot of power goes tough them, they are harder to manufacture and will increase to a more expensive board and a higher failure rate.

I haven't review the layout. With a quick check, I think your output capacitors are way to far away from your chip, but I'm unsure.

If I had an advice to give you is to get the best PCB design, spend as much time doing and redoing your component placement. That's what makes the difference! And with practice, it will take you less and less placement to have a good and neat PCB.

The image is too pixelized for more comments, but I'm impressed! I have seen worst from actual PCB designers!