Buck converter - any significant EMI difference between LM5010 and LT7101? - Page 1
Forum section: electronics / projects

author: Clear as mud
author_rank: Regular Contributor
timestamp: July 30, 2020, 08:23:03 pm
content: I'm building a buck converter to supply 5 volts at 1 amp. The input voltage can vary between 36 and 59 volts.I'm concerned about EMI performance because this will power an ADC circuit for voltage measurement (and other loads too).LT7101 seems to be a newer chip, and specifically claims to be "low EMI."https://www.analog.com/media/en/technical-documentation/data-sheets/LT7101.pdfLM5010 is I guess the lower-cost choice ($3 instead of $10 in low quantities). Page 20 of the data sheet gives some circuit examples to reduce ripple. In the interest of not getting too complicated, I probably would go with the middle one "reduced ripple."https://www.ti.com/lit/ds/symlink/lm5010.pdfThis is a one-off circuit, so the cost difference is not important if it really does help EMI. Also, I don't know if there would be a real cost difference, considering the external components. It looks like the LT7101 doesn't require much. I don't really have any experience with designing buck converters, so any advice is appreciated. I plan to read the data sheets carefully and follow the recommended layout, but I'm not sure which controller IC to use. If there is some other chip you would recommend, let me know.

author: KT88
author_rank: Frequent Contributor
timestamp: July 30, 2020, 11:18:54 pm
content: The LM5010 is a non synchronous buck while the LT7101 is a synchronous buck. The external diode is always more challenging when it comes to EMI... The larger die area for low side FET adds to the cost. For good EMI it is worth to have look at the LT7101 eval board.LTSpice has built in jigs for easy first tests...I usually choose the higher switching frequencies as they allow for smaller loop areas (it’s a bit counter intuitive but the layout is easier as the inductor can be smaller).The most critical part is the layout...a lot can be screwed up with that....CheersAndreas

author: temperance
author_rank: Super Contributor
timestamp: July 31, 2020, 12:00:24 am
content: How many bits is the ADC? How fast is this converter. What's does the power supply rejection of the ADC look like,...Without those numbers you cannot take meaningful decisions.-The buck regulator you choose doesn't matter that much. Just keep it in continuous conduction mode to reduce switching node ringing and reduce peak currents.-isolate the analog circuit power supply by properly filtering the supply. Low value SMD resistors up to case size 1206 work flawless up to 10 GHz (values <50R). If that's not enough: add a ferrite bead + resistor + low value ceramic capacitor filter. (the resistor dampens the resonance caused by the ferrite bead inductance and the ceramic cap. A few Ohm till 10Ohm will do)-For the digital signals add series resistors in every signal line in order to reduce the peak current caused by stray capacitance of the interface. Those current are flowing trough the GND bond wire of the ADC.-Think about where the return current will flow for the digital interface.-Keep GND planes clean around the analog circuit. (by steering current around the sections which need isolation if required.)-Keep input circuitry symmetric for good EMC performance so the input interface does not turn common mode signals into differential mode signals.-Use shielded inductors with low stray capacitance. Inductors with a high resonant frequency have low stray capacitance (for the same inductance). Otherwise switching noise will pass trough the inductor.-Don't use ceramic caps at the output of the buck reg as bulk capacitance. A 100nF X5R/X7R + a low ESR aluminium cap works much better. Those ultra low ESR ceramic caps can be difficult to tame.

author: Clear as mud
author_rank: Regular Contributor
timestamp: August 01, 2020, 02:54:25 pm
content: Followup questions:1. Upon close inspection of the picture of that demo circuit board for the LT7101, it looks like the smallest capacitor is an 0402 size. The other capacitors look to be 0805 and larger. (The picture can be found on theproduct page.) If I am designing for hand assembly and don't want to use smaller than 0805 components, would it make much difference for EMI? That is the boost capacitor- I would have to extend the end of it further up, and not have the ground plane come in there close to the chip like that. Placing one 0402 capacitor by hand would not be a big problem, if it needs to be that small for the lowest noise. I think the peninsula on the ground plane doesn't really do much, but the boost cap loop area would be larger, with a larger size capacitor, and I think the current there has high-frequency components.2. I am not sure what is meant by this:Quote from: temperance on July 31, 2020, 12:00:24 amDo you mean if the Vin+ has a filter bead, then there should also be one on the ground? So that the 5V circuit ground would be isolated from the input voltage ground? I do not think that I want to do this, because the voltages I am measuring with the ADC actually come from the high-voltage side through a voltage divider. I guess this leads to another question:3. I probably should have asked this first: can I get a good accurate measurement using a 12-bit ADC powered from a 5V switching regulator, when the voltages the ADC is measuring come from the Supply side of the regulator? Like, I know I probably wouldn't get all 12 bits useful, but would it be possible to get 10 useful bits, with the right voltage divider selection? The ADC is part of the main chip on the Teensy 4.1 board: the 5V powers the board, then an on-board LDO takes it down to 3.3V for that microncontroller.

author: KT88
author_rank: Frequent Contributor
timestamp: September 04, 2020, 10:47:48 pm
content: 1. Try the boostrap capacitor in at most 0603 better 0402 - I handsolder them pretty easily - Tweezers with an angled tip, presoldering one pad and 'glueing' the part to it - adjusting it if nescesary -solder the other pad and at last the first pad again with a little bit of fresh solder...Background. The Boostrap cap sees extremely fast transients. The conducted and rradiated emissions of poorly chosen- and placed Boostrp cap can be extremely annoing....The other components that are not involved in the switching don't matter a lot - 0805 is usually fine.2. Doesn't apply here. If the component choice and layout are well designed there is only DC (good enough to achieve 16+Bits system performance - answers 3.)...and no filter bead on GND. Offline supplies and isolated DC/DC are a different topic though....Not asked but matters a lot: No slotted GND plane underneath the Circuit!!!

author: Clear as mud
author_rank: Regular Contributor
timestamp: September 12, 2020, 08:50:55 pm
content: Thank you!I actually didn't notice the reply until just now, over a week later. I have made other posts including the layout, but didn't get a reply. I assume that means it's not terrible. Pictures of the final layout are attached here.When you say no slotted GND plane, you mean GND should be solid underneath the entire buck converter circuit? Should PGND and GND be combined in this region? I kept them as separate nets so that I could more easily lay out zones and not have the PGND zones overlap with GND.The top layer has several zones of Vin, Vout, and PGND. Second layer (just underneath the top) is GND and PGND. This is what I was most unsure of. I considered making it all PGND, and keeping only the two traces as GND. Third layer is Vin and Vout, with the dividing line between them right under the LT7101 chip. Bottom layer is PGND.Power comes in from the lower right. Input capacitance shown is a 10uF electrolytic on the back of the board, and 2.2 uF surface-mount ceramic. The net tie (PGND and GND) is the three holes under the input capacitor, with copper polygons connecting them on top and bottom layers. Boost capacitor is the 0402, switch inductor is 10uH, output capacitors C21 is 10 uF and C20 is 0.1uF.More information and pictures of the entire board are in my otherentirely too detailed post.

author: KT88
author_rank: Frequent Contributor
timestamp: September 12, 2020, 09:18:40 pm
content: Unfortunatly your documentation is pretty hard to digest - it requires almost some reverse engineering...A good way to present it, is to name the images meaningfull, like layer 1 . Top side, Layer2 Gnd etc. that makes it much easier to get an idea of what is going on.I wouldn't split a topic like this into multiple threads - a lot of information goes missing that way...Thes images are a little bit better to read in this post but I'm not sure how the layers are stacked...You usually want to have GND directly below the top layer except you have good reasons to do otherwise.You don't put traces or slots in this layer except for some partitioning to keep noisy and fragile parts of the circuit apart (same GND though).On the top side you use a lot of fill creating loops - they might create single windings with a short...not a good idea. The layout of the eval board is a pretty good template...

author: Clear as mud
author_rank: Regular Contributor
timestamp: September 13, 2020, 01:32:51 am
content: Sorry for making it unclear, but the layers are stacked in the same order as I posted the pictures. Red is the top layer, yellow the second, pink the third, and green is the bottom layer. Did you see the schematic in my other thread? It explains a lot, I'm posting it again here.I get what you're saying about the loops on the top layer - basically, get rid of them because they might act as an antenna for magnetic fields.On the next layer down, the yellow layer, part of it is GND and part is PGND. I think you're saying that the two grounds should be combined as a solid plane underneath the whole regulator circuit. That will be harder to do, but I still can probably do it. I don't know how other software handles net ties, but in KiCad they're a bit of a pain. I will have to combine them to one net and then manually keep the areas separate that I want to stay separate, which means changing a lot of the fill zones.

author: Clear as mud
author_rank: Regular Contributor
timestamp: September 14, 2020, 01:05:35 pm
content: Looking at the schematic I posted last time, are the resistors R28 through R33 too much resistance? They are the ones between the Teensy and the level shifter. Someone recommended them to reduce noise in the circuit.I got the modifications to the 5V regulator layout done. New pictures attached, with more explanatory file names this time. I am seeing a little glitch in the copper pours where two zones on the same net with different priority levels overlap each other. Hopefully that will not appear in the gerbers, but if it does, I'll have to fix it somehow.(I'm still missing a couple of component 3D models, and the 3D model of the filter module is incomplete.)

author: Siwastaja
author_rank: Super Contributor
timestamp: September 14, 2020, 01:15:59 pm
content: You have 4 layers available but still no solid ground plane? This is going to be bad for EMI. Or am I missing something, do you have isolation somewhere?

author: Clear as mud
author_rank: Regular Contributor
timestamp: September 14, 2020, 06:23:54 pm
content: I do intend for it to be isolated areas.The entire top part of the board is for a commercially-available 12V 300W DC-DC converter and its filtering. It is aEBVW025A0B Barracuda Series DC-DC Converter Power Module, made by GE. In the middle of page 12 of the datasheet is a suggested schematic for filtering, using a bunch of capacitors and aFLT007A0 filter module(also made by GE, of course). I followed the suggested circuit, except for two changes: where it shows C4 and C5 as 3x10n each, I instead used a 10n, a 100n, and a 1u capacitor for each; and it shows Vout- grounded to the other grounds in the middle of the diagram, I isolated Vout- instead. On page 5 of the FLT007A0 datasheet is a suggested layout for the filter module and DC-DC converter module. I followed that, also with some changes: I flipped the filter module around so that it's center ground point "chassis ground" faces the other module instead of the input voltage side (to match the schematic on the other data sheet); I extended "chassis ground" to be a ground plane surrounding and going underneath everything on this top section of the board; and I compressed everything together by moving the two big capacitors to the back side of the board so that I could fit it within 100mm. If there is a future revision of the board, I probably will extend it out to 122 to 125mm long so that it all fits in a row on one side of the board.The only things that cross the isolation between that top section of the board and the other areas are:The power and ground supply at the right sideOne 12V trace intended only to measure the presence/absence of 12V power (accuracy not needed). This can be seen on layer 3 in the pictures on my previous post, a trace labeled +12V.The bottom left section of the board (with the Teensy 4.1 board on it) is also isolated, being the only part that uses low-voltage DC power. Vout from the LT7101 comes from its copper zone on layer 3 to the top layer and goes through an LC low-pass filter to become the 5V power net. Ground comes in on layer 2. There are two output signals and two voltage input signals that cross this isolation. The two output signals control the battery-switching MOSFETs, and are shown in the attached image (I just fixed the isolation there, that was messed up when I combined the nets PGND and GND).

author: KT88
author_rank: Frequent Contributor
timestamp: September 14, 2020, 07:18:16 pm
content: So far I have a coarse understanding of what you try to achieve: Two batteries (switched alternatively) which go into an isolated DC/DC converter into a 12V output.Through a diode ORing circuit you have a non-isolated buck for the system. The relay is again isolated - the PWM outputs are not. Is there an isolation for the PWM somewhere?I would suggest to draw a block diagram which clearly shows where you have isolation and which signals (GNDs) belong to each block.If the 12V LED supply is isolated why isn't the PWM?

author: Clear as mud
author_rank: Regular Contributor
timestamp: September 14, 2020, 07:36:51 pm
content: Yes, perhaps the power for the LED strips should be isolated as well, with an extra capacitor on the power rail down there near the LED strip outputs.