Electronic – Layout advice for LDOs


I'm developing a four layer board which is powered by 3 voltages – 1.8V, 3.3V and 5.0V. The board has the following stackup:

  1. Signals
  2. Ground
  3. 3.3V
  4. Signals

The ground and 3.3V plane are completely unbroken. No signal or power trace travels on them.

I'm using three LP38690DT LDOs to provide power – here's my circuit.

Power Regulators

Click here for larger picture.

My concern is the layout for these devices. The datasheet suggests the following

The best way to do this is to lay out CIN and COUT near the device with short traces to the VIN, VOUT, and ground pins. The regulator ground pin should be connected to the external circuit >ground so that the regulator and its capacitors have a "single point ground".

I was somewhat confused by the term "single point ground" but I tried to follow the advice given in the datasheet to the best of my ability – but I am not sure if I am correct:

enter image description here

Note that the text in red is only there to give clarity to the folks here – I will delete it afterwards. Each regulator is connected directly to the capacitors and the ground pin of the regulator is connected directly to the capacitor's ground pin directly. Is this what the datasheet meant I should do?

The datasheet goes on to say

Since high current flows through the traces going into VIN and coming from VOUT, Kelvin connect the capacitor leads to >these pins so there is no voltage drop in series with the input and output capacitors.

What does it mean by Kelvin connect? I know what a Kelvin Connection is – what I don't understand is what does it mean in context for a LDO.

My third question is regarding all three regulators. As I mentioned, each IC is referencing ground from the same via that connects it's capacitors to the ground plane. However, should I connect all three regulators to the same ground point i.e. should all 3 regulators connect to the "single ground point/via"?

Finally, the input voltage is being fed by a 4-point through hole connector which carries 6V on two conductors and GND on the other two. The GND pins are connected direcly to the ground plane. Is this OK or should I connect the GND pins to the GND pins of the regulators directly via thick traces?

NOTE: the layout picture does not show anything connected to the output of the regulators. This is OK. I still have to connect my ICs to the power. ALSO: the maroon color underneath the regulators is not a net. This is Altium's way to show "Rooms" in PCB layout.


Most of the current is drawn from the 5V supply. The 5V supply connects to a LCD display which will draw a max. of 400mA (when backlight is on) – but normally around 250mA.

The 3.3V supply will draw a max. of 300mA (discontinuous) but normally around 150mA or less.

The 1.8V is the supply for the core of the CPLDs that my board has. I was unable to estimate this but I've measured it. At startup, this was around 30mA but then reduced to 0mA. My meter, it seems, was not sensitive enough to actually measure the current. I reckon 200mA would be a safe bet for this.


enter image description here

I hope this is what folks here meant. I wasn't sure if I should one large copper pour or three separate ones so I went with 3 separate ones.


enter image description here

I've now made made one giant copper pour instead of 3 independent ones. I was't sure how to connect my 3.3V voltage to my power plane using multiple vias so the above is my attempt. I made a small fill and connected it directly to my output capacitor. From there I have 4 vias, each 25 mill in size, connecting directly to my power plane. Is this a better way to do it?

The clearance between the fills and other objects is about 15 mills. Should I increase this?

Best Answer

But overall you are over-thinking the importance of the GND. It's important, don't get me wrong. It's just that there are other things that are as important, and getting the GND correct is relatively easy.

You specified the voltages, you didn't specify the current. Without knowing the current, we don't know the heat generated by the LDO's. And the heat will greatly influence the way the PCB is laid out. I am going to assume that the heat generated is non-trivial.

Here's what I would do...

  1. Rotate the caps 90 degrees (sometimes clockwise, sometimes counter-clockwise). What you are doing is putting the caps GND pins together and shortening the distance between the LDO's GND and the caps.
  2. Make all of your traces wider. At least as wide as the pad it's connecting to. Use multiple VIA's if you can.
  3. Put the +6v traces "somewhere else". Either on the back side of the PCB or on the right of the LDO's. This will make sense shortly.
  4. Put a copper plane on the top layer, under and around the whole thing. Connect this to the GND layer using multiple VIAs. I would use about 10 vias per LDO, mostly around the huge GND pin. The GND pin of both the LDO's and caps should be connected to this plane DIRECTLY, without any "thermal relief". This plane should be reasonably large, although the exact size depends on the space available and how much heat the LDO's will be giving off. 1 or 2 square inches per LDO is a good start.

There are two reasons for the copper plane. 1. It gives the heat from the LDO's someplace to go to be dissipated. 2. It provides a low impedance path between the caps and the LDO.

The reason for all of the vias are: 1. It allows some of the heat to be transferred to the GND layer. 2. It provides a low-impedance path from the LDO to the GND layer.

And the reason for the fatter traces and multiple vias is simply for a lower impedance path.

I will warn you, however: Doing this will make hand-soldering of the LDO's difficult. The copper planes + vias will want to suck the heat away from the soldering iron and the solder won't stay melted for very long (if at all). You can get around this somewhat by using a hotter soldering iron, or better yet pre-heat things by using a heat gun to warm up the entire PCB first. Don't get it hot enough to melt solder (use your normal iron for that). By preheating the whole board the demands placed on your iron will be less. IMHO, this isn't a big deal but it is something to be aware of and plan for.

This method will also give you a nice connection to GND, way better than anything you've told us from the datasheets.

Update, based on new information from the original poster:

Your 5v regulator is dropping 6v to 5v (a 1 volt drop) at 400 mA. This is going to produce 0.4 watts of heat. 6v to 3.3v at 150 mA = 0.4 watts. 6v to 1.8v at 200 mA = 0.84 watts. Total 1.64 watts for all three LDO's. While this isn't crazy, it is a fair amount of heat. Meaning that you must pay attention to how this is going to get cooled otherwise it will overheat. You're well on your way to getting that done properly.

You want a single plane, not three. And the plane should extend out as far as possible, I recommend at least double the area of the LDO's themselves. The larger the plane, the better the cooling effect. If the plane is really large then you'll want to put at least four vias for every square inch. By sharing the plane, the three regulators are sharing the cooling. If you didn't do this then one regulator could get really hot while the other two are just warm.

Another optimization that you can do is with how the +6v comes in to each LDO. At the moment it goes around the cap, to the LDO. Just have it go straight into the cap, without wrapping around. This will allow you to use thicker traces and keep things a little shorter. That small amount of GND plane that wraps around the cap isn't helping much anyway.

You'll want several vias from the output of the LDO to wherever that power is going. Not just the single via that you have now.