Dual dcdc converter layout and grounding - Page 1
Forum section: electronics / projects

author: OwenH
author_rank: Contributor
timestamp: July 30, 2023, 10:53:23 am
content: Hi,I’m designing a compact PCB layout that uses two Vicor PI3740-00 Buck-Boost modules to generate output voltages of 12V and 24V from an input voltage of 10-36V. The 12V output Vicor IC will be synchronized with the 24V output Vicor IC. The PCB will have either a 4-layer or 6-layer stack-up with 2oz copper on all layers.I’ve started laying out the components and currently have the Vicor ICs back-to-back with the power inductors for the 12V and 24V circuits at opposite sides of the board. The SGND area of the ICs is back-to-back in closer proximity with the SGND area between them.The Vicor modules have PGND and SGND internally connected to create a star ground. I’m unsure how to handle grounding when using two of these modules. Currently, I have power traces for the DC-DC switching circuits on the top layer and PGND directly below on the next layer to reduce EMI. SGND is currently in the area between the two ICs and not below the switching area of the two ICs and power inductors.The Vicor ICs have PGND and SGND connected internally to create a star ground. Will this likely be an issue if I’m using two ICs both connecting SGND to PGND internally? At the moment, I also only have SGND in the area between the two ICs but would it be best to extend this out onto an entire internal layer to create a full SGND plane?Lastly, there is going to be a hot swap controller on the input using a current sense shunt and a MOSFET switch. This is because the device will be hot-plugged into battery power, and I need to control the inrush current. Should the hot swap IC be connected to SGND or rather PGND?I appreciate any advice or suggestions you can offer. Thank you!Owen

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 30, 2023, 07:44:50 pm
content: If SGND is connected internally, then don't connect it to anything else externally (except the associated components). You can't have a star ground (implied: single star) with two stars tied! Do the layouts independent, and make considerations only where they have to connect (say, voltage reference, EN, PG, clock, etc.). "Considerations" may include source termination or slew-rate-reducing resistors, local bypass caps, ferrite beads, common mode chokes (to couple the voltage between SGND domains into the signal spanning between them), etc.For EMI purposes, whatever's going on by the modules is made irrelevant if both input and output(s) travel some distance away from the local ground loops, to a common location, where further EMI filtering is placed. With input bypassed to ground at a point, and output bypassed to the same point, ground loop is eliminated (there's no voltage drop across a point). What kind of layout passes for "pointlike" is another matter, depending on frequency, component size and ratings, etc.Also,nearlyirrelevant, as there could still be radiation from the local area. If the filtering point is made at a location common to a shield which surrounds the active area, then radiation is also sealed. Whether that's achievable on-board (without shield cans or an enclosure), or in the available board area, is another matter.Or if you need to get signals out of the SGND domain onto cables or whatever (remote sense, EN, PG, etc.?), you'll have to find some solution to filter those to the same common mode reference.Tim

author: OwenH
author_rank: Contributor
timestamp: July 30, 2023, 08:33:50 pm
content: Thanks for the detailed response Tim!Are you saying that it would be best to use a separate SGND for each dcdc converter? Then each SGND is connected to its connected to PGRN at its respective switching regulator IC? And then the hot swap IC will be grounded to the PGND.Won't separating the SGND be an issue when routing the sync out from one converter to the sync in on the other? I figured I should sync the converters to avoid harmonics but maybe its best not to synchronise the converters at all?Also in regards to EMI I plan to use both sides of the pcb and put the input and output filters on the the bottom side of the board as well as the input and output connectors. Also the device will be inside a machined and sealed aluminium housing which should help block emitted EMI. I'm trying to fit this on a 62mm x 42mm pcb which might be a bit overly optimistic given that it doesn't leave a large amount of clearance between each converter.Owen

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 30, 2023, 08:58:00 pm
content: I'm not familiar with these chips so I don't know what kind of between-SGNDs voltage to expect, or how noise-immune the sync line is. You might arrange to try several options, see if simply connecting it works, or if it behaves better with other mitigation in there.Yes, hot swap referenced to PGND.Filters right by the inner current loop isn't a great idea, as mentioned. You don't get much shielding through 2oz foil layers, plus they're riddled with vias / clearance thereto.Perhaps you have enough height to add a riser or mezzanine board for filtering? Or a panel-mounted connector board, say?Or if you have shielded connectors, and can deal with the ripple/noise elsewhere in the system as long as it's not radiating from the cables?Tim

author: OwenH
author_rank: Contributor
timestamp: July 30, 2023, 09:21:40 pm
content: I will reach out to Vicor and see if they can advise me on the SGND issue with the two converters.The 2nd stage output filter is placed on the bottom of the board but only has about 6-7mm clearance to the current loop. Maybe if I go to a 6layer board and have 2 ground planes separating that would help? I might be able to move the 2nd stage output filters to the connector board but everything needs to be really tight and it may be difficult to fit the inductor in that area. Also Ideally this board would be used in multiple designs and not having the 2nd stage output filter on the main board might make it less convenient.Owen

author: T3sl4co1l
author_rank: Super Contributor
timestamp: July 31, 2023, 01:09:22 am
content: Of the CLC filter, the innermost C is the bypass on/by the device itself. The L can be anywhere, it's a series element. Prefer shielded type inductors so you aren't coupling switching noise directly into the EMI choke by near fields. The outer C can (should, even?) be on the connector board.Probably astupidpreposterous idea, but for sake of representation: the L could even be strung up between boards, as part of the wiring, or instead of (or as part of) the board-to-board connection.Note that the converter board will probably be isolated from chassis GND, to avoid making a GND loop with the connector board, which will be [chassis GNDed] (preferably at multiple points, such as the shell pin(s) from metallic connectors, mounting screws, etc.).Tim