Need help with component placement/PCB layout for a buck LED driver (LT3755) - Page 1
Forum section: electronics / projects

author: exscape
author_rank: Contributor
timestamp: March 27, 2018, 09:36:37 pm
content: First off, please excuse the messy layout; this is a draft showing rough placement. Most things are is sloppily placed, especially bottom-half traces and vias which are just there to make basic connections. (I'm fairly happy with the the IC and surrounding caps/resistors, though.)Note: pin 2 of the output capacitor (C9) is not connected in the picture -- oops. I'd connect that with a trace straight upwards to under C12 (input electrolytic).The way these drivers work is that they sense the current through RLED (100 mV full scale) to adjust the output, so the RLED traces ought to be the most sensitive ones. I'm far from happy having them so far from the IC, but if I keep the layout in the center and move the sense resistor up, the LED connector (and perhaps output cap) needs to follow, along with a VIN trace; it gets ugly fast.I'm not sure how important absolute accuracy or noise on RSNS is; the datasheet lists it as "the current sense input for the control loop". I'm not entirely happy with the routing, but the only suggested layout in the official datasheet does the same thing (i.e. routing it under the MOSFET, to a copper area that leads to the shunt resistor), so I figure it's OK.LT3755 datasheetI've tried to find better placements, but this is the best configuration I've found so far.The main issue (as far as my knowledge goes) seems to be the long RLED traces. At low dimming settings, the differential voltage on those traces can go down to about 10 mV; noise on them could presumably cause flicker/oscillation/instability.I'd certainly welcome criticism of everything else as well, but especially help with component placement.

author: KhronX
author_rank: Frequent Contributor
timestamp: March 28, 2018, 02:04:56 pm
content: Just a few ideas, in no particular order:Does the "VIN" trace need to go THAT close to the lower pad of L_W?C12 has the "wrong" orientation of the "foot" - the shape reminds me of SMD electrolytics, and the flattened corners are on the positive side.Any chance of rotating the current-sense shunt in a north-south direction, so you wouldn't need to route the pair of traces "through" the output connector?Looks to me like you'd have plenty of room to move the whole group of chip-plus-passives-around-it more to the left, and thus minimize the trace length going to the MOSFET gate, as well as the "Sense" one.I'd "even" move Rsns_W and C10-12 a bit to the right, and further up. C9 a bit more to the right, and then the inductor would have room to be moved slightly lower too (ie. "southwards").

author: RobK_NL
author_rank: Frequent Contributor
timestamp: March 28, 2018, 02:15:11 pm
content: Quote from: KhronX on March 28, 2018, 02:04:56 pmAnd, if you also rotate that group 90 degrees clockwise, you can gain even more. Plus it gives you the chance to optimize the placement of C8 and C14.

author: exscape
author_rank: Contributor
timestamp: March 28, 2018, 02:23:09 pm
content: Quote from: KhronX on March 28, 2018, 02:04:56 pmWow, thanks! I'm not sure what's going on there -- I enabled pin numbers in the schematic, and it has two pairs -- "1, 2" (positive, negative) close to the plates, and "2, 1" at the end of the pins. I'll delete and re-add them to the schematic and see if that takes care of the pin confusion. Perhaps I should use or create a polarized symbol, too.Quote from: KhronX on March 28, 2018, 02:04:56 pmNo, I only routed it to show the overall layout. Almost everything will be re-routed if I keep this layout.Quote from: KhronX on March 28, 2018, 02:04:56 pmHm, I can't get the traces in the correct order that way; the VIN sense trace needs to come in on top (or to the right, when routing it upwards), but in naturally comes to the left.Quote from: KhronX on March 28, 2018, 02:04:56 pmQuote from: RobK_NL on March 28, 2018, 02:15:11 pmAbsolutely, I'll keep those in mind as well.Thanks!Since you gave plenty of useful minor adjustments, do you think the overall layout is OK (with the suggested tweaks)?I'd prefer to have RLED about a *fifth* of the distance away from the IC pins or so, but perhaps not at the price of making the high-current traces far longer.

author: KhronX
author_rank: Frequent Contributor
timestamp: March 28, 2018, 02:29:56 pm
content: That sort of package for C12 is a polarized one, so yeah, using the right one for whatever component you'll use on the actual board, might be a good ideaThat current shunt CAN be "vertical" in TWO ways, y'knowOne of those two variants is bound to allow the two traces coming off it, to be in the right "order".No real idea what you meant with that last sentence though (nor why exactly you'd want that), or how it fits into... anything, reallyEither way, if you move the Rsns_W, C10-12 group a bit to the right and further up (which would almost "mould" onto the existing copper islands kinda like Africa and South America "fit together"), you could also rotate C9 so its "Vin" pin is "north" and the other one is "south". That might / should enable you to move the output connector a bit further north, and shave a good few mm off the vertical size of the board.

author: exscape
author_rank: Contributor
timestamp: March 28, 2018, 02:39:54 pm
content: Quote from: KhronX on March 28, 2018, 02:29:56 pmEh, how so?The sense traces are high impedence traces, and 1 mV of coupled/induced noise on them would matter (since that would be a noticeable of the sense reading of 8.8 mV at 0.4 A, which is an output current I'd like to work reliably). Surely routing them around half the design is very suboptimal?

author: KhronX
author_rank: Frequent Contributor
timestamp: March 28, 2018, 02:44:23 pm
content: Try that - the two traces can come out towards the right side, between the shunt and the output connectorThat way they won't have to meander "through" the connector (footprint).Once you do that, actually, you could even rotate the connector by 180deg, and get even shorter power traces, i think.PS: "I'd prefer to have RLED about a *fifth* of the distance away from the IC pins or so" - a fifth of the distance... of what?That's what confused me...

author: KhronX
author_rank: Frequent Contributor
timestamp: March 28, 2018, 02:50:40 pm
content: It's a bit of a hack-job, but my Paint skills only go SO far

author: exscape
author_rank: Contributor
timestamp: March 28, 2018, 02:51:53 pm
content: Quote from: KhronX on March 28, 2018, 02:44:23 pmOh! Sorry. I meant a fifth of the distance they are in my original layout.I'll try to implement all the feedback given so far after dinner (which is very soon).

author: KhronX
author_rank: Frequent Contributor
timestamp: March 28, 2018, 02:55:26 pm
content: Well, if you implement the ideas in my second "example photo", i think you'll be shaving off maybe 20% of the current-sense trace lengths.I may well be wrong, but precisely because they're relatively high-impedance inputs, the absolute length of the traces is less important than their equal-ness (kinda like with balanced signaling - as long as the same amount of noise gets into both, it's all good, they end up going into a differential / instrumentation amplifier anyway, so the noise'll get cancelled out). But of course, the shorter, the better

author: exscape
author_rank: Contributor
timestamp: March 28, 2018, 06:42:00 pm
content: Okay, so I moved RSNS (not sure why I didn't place it up there to begin with, but stuff like this is why I asked for help).That meant I could make the copper previously connecting to it smaller, and make space to move the VIN caps upwards by about a 1210 cap's width (so about .1 inch). However, that would move them away from the diode and switch node, and my understanding is that every millimeter matters there. Should I really move them?In the paint-reworked picture (which is great, by the way) the diode is closest to the high-ESL polymer capacitor.

author: RobK_NL
author_rank: Frequent Contributor
timestamp: March 28, 2018, 08:11:37 pm
content: Is there any specific reason why you are using analogue dimming rather than PWM?Based on my experience with the LT3756, the analogue dimming is not particularly linear in the lower regions.

author: KhronX
author_rank: Frequent Contributor
timestamp: March 28, 2018, 08:26:51 pm
content: Aaaaaand you can't swap the locations of the two ceramics with the polymer?Although now that i look at things a bit more carefully... is there any particular reason why the bulk / bypass caps for theinputare in the MIDDLE of the board (as opposed to, say, closer to the DC input jack)?Take the FET and rotate it 90deg counter-clockwise. Keep Rsns next to it, with the vias going to the ground plane.Take C10-11-12 (which will need rotating 180deg) and the diode, and "swap places" between them and the inductor. Or rather, keep the diode somewhere "in the middle", and swap the inductor location with the caps.You were worried about power trace length anyway, so...Quote from: exscape on March 28, 2018, 06:42:00 pm

author: exscape
author_rank: Contributor
timestamp: March 29, 2018, 10:00:04 pm
content: Alright, now we're getting somewhere!I started implementing the latest comments, but ran into a snag that I can't remember now when moving and flipping the capacitors. However, I spotted a different possibility, which ended up working rather nicely.Feedback?Possible (hopefully minor) issues I've spotted:1) VIN comes from below the diode, but the bypass caps are above. Does that matter? I need more both knowledge and intuition when it comes to capacitor placement and parasitic inductances.2) The RLED sense traces cross with a via, which allows for a fairly nice placement of RLED.3) The GATE trace is a bit longer (but still only(?) 11 mm)

author: KhronX
author_rank: Frequent Contributor
timestamp: March 29, 2018, 11:29:57 pm
content: Make a copy / backup of the state you got to this far, and see what my ideas end up looking like."Take the FET and rotate it 90deg counter-clockwise. Keep Rsns next to it, with the vias going to the ground plane.Take C10-11-12 (which will need rotating 180deg) and the diode, and "swap places" between them and the inductor. Or rather, keep the diode somewhere "in the middle", and swap the inductor location with the caps."Or at the very least, see if you can get that bigger Vin filter cap closer to the DC jack, and the inductor pads on the "north-south" axis, so you can then run the Vin trace under the inductor (as opposed to snaking around half the board). That cap would have plenty of space between the DC jack and the LED driver chip, for example. You might have to nudge it and the surrounding parts a couple mm to the right, but that shouldn't be an issue. Otherwise that area's just "wasted" space anyway.PS: Any reason why the source current-sense resistor and the two ceramic caps HAVE to have their ground connections right next to each other? I'd move the Rsense to the other (left) side of the FET, somewhere.PS2: My hunch is that, in the great scheme of things, this is a pretty low-power setup, so the parasitic stuff is nowhere near as big a concern as in something considerably more beefy (i'm thinking of something like a high-power class-D amplifier, with supply voltages >50V and currents in the double digits). So i wouldn't sweat that

author: exscape
author_rank: Contributor
timestamp: March 30, 2018, 09:47:29 am
content: Quote from: KhronX on March 29, 2018, 11:29:57 pmI'll have a go at it.Quote from: KhronX on March 29, 2018, 11:29:57 pmThe datasheet specifies that "the ground point of these two switching current traces should come to a common point then connect to the ground plane under the LT3755" (which I've realized that I'm not quite doing, but that's an easy fix if needed), with the two traces/nodes referred to being:"1) from the switch node through the switch and sense resistor to GND, and2) from the switch node through the Schottky rectifier and filter capacitor to GND"In a closely related datasheet (for the LT3797, which I'm also using -- that layout will probably be tougher since it's 3 channels/RGB, though thankfully far lower power) they also state:"The placement of the sense resistor RSW_SEN should be close to the source of the MOSFET and GND. The SENSEP and SENSEN sense node traces should run parallel to each other to a Kelvin connection on the positive and negative terminals of RSW_SEN."The sense setup there is identical to the LT3755, only that it has a separate pin (vs GND on this one) for the negative sense connector. I figure that the statement of placing the sense resistor close to the source applies here as well.And yeah, compared to the setups you mention, this is "low" power -- output power is about 60 W at most, or ~12-13 V and 4.5 A. Still feels like fairly high power to me.

author: KhronX
author_rank: Frequent Contributor
timestamp: March 30, 2018, 10:33:44 am
content: This is essentially a boost-converter (with a slightly funky arrangement, granted), right? So for a given output power (higher voltage than input, but lower current), your biggest currents (and associated spikes) will be on theinput, won't they?That's just one extra reason to want that Vin trace as short as possible, not wandering around half the board, methinks<edit> Scratch that, i took a look at the datasheet and you're using it in the... buck mode, i guess? Whatisyour intended load, by the way?

author: soubitos
author_rank: Frequent Contributor
timestamp: March 30, 2018, 11:08:46 am
content: I'd move the power input to the right of the IC, keep the sense resistor AS CLOSE AS POSSIBLE to it and use the bottom layer of the pcb... also with similar ICs i like to start laying out the IC from the IC in the center and build around it placing each component where is should be in relation to the IC itself.

author: exscape
author_rank: Contributor
timestamp: March 30, 2018, 12:20:15 pm
content: Quote from: KhronX on March 30, 2018, 10:33:44 amYeah, it's a buck converter (I did put that in the title). The intended load is two Cree XHP70.2 LEDs in series (Vf total 11-13 V depending on the current), powered from a ~17-20 V power supply.Since it's a buck, theinputis indeed discontinuous (the output has the inductor in series), so I suppose having VIN shorter would be preferable.Quote from: soubitos on March 30, 2018, 11:08:46 amThere are other things on the board as well, so I don't think moving the DC jack will be easy (it needs to be on either the left or the right board edge, and I'm not even sure where the right edge will be yet).What would you place on the bottom layer? Almost every guide I've read to prepare suggest that all power components should be on the same side of the board, at least.