Power supply PCB layout and routing feedback - Page 1
Forum section: electronics / projects

author: Chris.M
author_rank: Contributor
timestamp: June 03, 2013, 01:58:35 pm
content: Hello all,I'm working on a positive and negative output power supply, and was wondering if I could get some feedback.The design is by G. Randy Slone from the book TAB Electronics Guide To Understanding Electricity and Electronics.To start with, I have attached the PCB component layout.The components with reference designators HSx are heatsinks and those with CONx are soldered wire connections (transformer secondaries, POTs, binding posts).Also, the two series pass transistor, Q1 and Q2, will be mounted to an external heatsink, and will be soldered via wires to the PCB.Before I start routing, is there anything that would be a cause for concern that I should change or watch out for?All comments welcome.Cheers,Chris

author: metalphreak
author_rank: Frequent Contributor
timestamp: June 03, 2013, 03:21:40 pm
content: Capacitors C1 and C2 could do with a bit more spacing from the bridge rectifier. You seem to have a bit of room if you shuffle the R1/R2 away a bit. You want to keep any electrolytic components a good margin away from heat sources if you can. It also gives you the option of later using larger diameter caps with the same lead spacing. Otherwise I don't see any other issues. Just double check the dimensions on the PCB layout match the physical parts you are going to use. I've been caught out on this once or twice

author: c4757p
author_rank: Super Contributor
timestamp: June 03, 2013, 03:50:59 pm
content: Yeah, it looks pretty good to me too. One quick point I'd make is to put some sort of pin marker on Q1 and Q2 so they don't get wired wrong. You remember which end is where now, but give it time and you may find yourself squinting at the layout trying to discern the orientation.That's really only if I must force myself to be picky, though. It's fine IMHO.

author: mariush
author_rank: Super Contributor
timestamp: June 03, 2013, 04:06:38 pm
content: C4 polarity is wrong in the schematic but being ceramic capacitors it probably doesn't matterMight wanna replace that flat square bridge rectifier with one that has the leads in one row and is positioned vertically on the board (or at least add the holes for it). Like this one :http://www.digikey.com/product-detail/en/GBU4M-BP/GBU4M-BPMS-ND/1140594You'll have more distance between it and the large input capacitors and will also allow you to heatsink it if needed.

author: MacAttak
author_rank: Unknown
timestamp: June 03, 2013, 05:23:27 pm
content: You misspelled "Positive Rail" on the layout. Could be a make-or-break issue

author: Chris.M
author_rank: Contributor
timestamp: June 04, 2013, 01:26:28 am
content: Quote from: metalphreak on June 03, 2013, 03:21:40 pmHave moved C1 and C2 further away from the rectifier. Thanks for the heads up, will double check them.Quote from: c4757p on June 03, 2013, 03:50:59 pmYes, that could ruin my day. Have annotated the pins as suggested.Quote from: mariush on June 03, 2013, 04:06:38 pmIndeed it does have the wrong polarity. Its actually like that in the books schematic. See:https://www.eevblog.com/forum/beginners/need-some-help-with-randy-slone%27s-power-supply-in-tab-guide-to-understanding/msg105970/#msg105970Have fixed that, although you are right, they are ceramic caps so polarity wasn't going to be troublesome.As for the rectifier, I had one like that originally, but thought the trace clearance would be too small. Turns out that its okay if I neck the traces.What do you think of the space saving? Doesn't look like I gained that much. I don't mind buying another rectifier, but considering I already have the square one, do you think the spacing saving is worth changing it?Quote from: MacAttak on June 03, 2013, 05:23:27 pmFixed.Thanks for all your feedback guys, appreciate it.I was thinking of adding in some bleed resistors and an LED to the bigger caps. Have attached a small schematic.I still need to test this but won't get around to it until tonight. My initial thinking though is that R1 and the LED would be enough, but my second thought is that the cap would discharge to 2.1V and then the LED stops conducting, so the cap won't discharge any further?I therefore decided to add in the 1000ohm in parallel to help discharge the remaining 2.1V and it will speed up the discharge as well.Does that look okay?As for power wastage, I calculate there to be 15mA through the LED and 34mA through R2 so that gives ~50mA total, @ 34V that's 1.7W.Is that too much to be wasting on "always on" bleed resistors?

author: mariush
author_rank: Super Contributor
timestamp: June 04, 2013, 02:07:19 am
content: Yeah, use whatever rectifier you have, it's not a big deal. I personally like the ones thoseThe point of bleeder resistors is simply to discharge them enough to not shock you if you accidentally put the fingers on the solder points. Below a few volts, you won't be bothered even if you short the leads with your hands.I would probably put a bleeder resistor only if the voltage is over about 16-25v and then I'd probably use something like 2200-4700ohm. For less voltage, you can just get a 100-470 ohm 0.5-1w resistor and short the leads for a few seconds to discharge them.

author: Chris.M
author_rank: Contributor
timestamp: June 04, 2013, 11:25:16 am
content: The routing of the board is done.How does it look? Feedback, changes, etc. welcome.There's a few things I wanted to ask.When your routing a branch or a path that branches, does it matter which component becomes the central point?For example, for transistor Q1 (top, slightly left of center), for the Emitter (marked E), would it matter if I connected E to R3 and then from R3 to R6? They are all at the same potential, but I'm wondering if there are circumstances that make a difference.Is it okay to have via's in a high current path?Looking at CON10 (middle, right hand side), this is a main current path, but I had to jump over a trace using a via. I have placed two via's (noticed Dave does it but with more than two). Have I got enough via's? Or should I have done it with the smaller trace going from R6 to transistor Q6?Are the high current traces thick enough?On the positive output, the current is limited to 1.5A using transistor Q6. The traces are 100mil in all places except one,where its 85mil. According to Dave's PCB tutorial, 80mil should handle 4A, but some online calculators are only giving a max current of ~2.3A.

author: c4757p
author_rank: Super Contributor
timestamp: June 04, 2013, 11:40:23 am
content: Quote from: Chris.M on June 04, 2013, 11:25:16 amIf there is current flow, you'll have the trace resistance between them, so just calculate how much voltage will be lost and whether that is acceptable. If it's just a signal trace it shouldn't matter.QuoteCalculate the resistance and temperature rise.You can use multiple vias to increase capacity.QuoteThat's because it depends on temperature rise and how much voltage loss is acceptable to you, just like with the vias. 100mil should be enough, but when in doubt there's no reason not to increase the size if it will fit.Also, do you really need double-layer? See if you can get it onto one layer - you're close!

author: Chris.M
author_rank: Contributor
timestamp: June 04, 2013, 01:12:27 pm
content: Sorry for the long post, but I find this interesting to learn.Quote from: c4757p on June 04, 2013, 11:40:23 amSo to see if I understand, attached is the two different paths I could have taken.The following is assuming 1.5A.Looking at the orange path first for the left side, I measured the length to be ~530mil, the calculator gives a 7.47mV drop.The orange path on the right side, I measured the length to be ~720mil, the calculator gives a 10.1mV drop.The difference between the left and right is 2.63mVThe blue path on the left was ~980mil, which gives a 13.8mV drop.The blue path on the right was ~1100mil (I assume I start from E again), which gives a 15.5mV drop.The difference between the left and right is 1.7mV.So regardless of the route, best case I drop 13.8mV from E and worst case I drop 15.5mV from E.So c4757p, does this mean that if I ignore the 1.7mV difference, the two branches are equivalent? It makes no difference which route I took? Does it matter that the current for R6 had to go through the solder joint of R3 for the left side?Quote from: c4757p on June 04, 2013, 11:40:23 amThe via's have a 100mil outer diameter with 40mil holes.A 40mil hole gives 4.8A, so that would be more than enough.I assume the via length is referring to the board thickness? 1.6mm?Quote from: c4757p on June 04, 2013, 11:40:23 amWhen you said temperature rise, it triggered. The figures Dave has in the tutorial match the trace widths for external layers in air. I was looking at the widths for internal layers. By external layer, does it mean the outer two most layers? Even though they are underneath solder mask? Or is that without the solder mask?Quote from: c4757p on June 04, 2013, 11:40:23 amWell I was planning to get the PCB manufactured, so the 2nd layer was there, I figured I may as well use it and make the routing a little easier.Regardless of this, is there an advantage to having everything on the one layer?I have attached the ground path I would need to route (plus the two traces done with via's). It looks rather difficult now without ripping up all the traces and starting again. Mostly just around the bottom right, that part seems impossible without snaking a trace right around the outer edge of the board.Is there a trick to this?

author: mariush
author_rank: Super Contributor
timestamp: June 04, 2013, 06:38:52 pm
content: You can use 0 ohm resistors (or plain wire) to get across traces and keep the board single layer. I'd do it single layer just for the fun of it, or as a challenge, sounds like something easy to do.Traces on external layers will handle a bit more current, no need to be very concerned about it.

author: Chris.M
author_rank: Contributor
timestamp: June 05, 2013, 12:22:17 am
content: Quote from: mariush on June 04, 2013, 06:38:52 pmYeah, turns out it was. How's it look?I used 50mil traces for GND (blue) instead of 100mil with 1 jumper. Will that be okay?Had to put a jumper on a signal path (orange path). Also okay?Quote from: mariush on June 04, 2013, 06:38:52 pmFair enough.

author: mariush
author_rank: Super Contributor
timestamp: June 05, 2013, 01:44:39 am
content: It looks OK.I personally really don't like that type of bridge rectifier. So much pcb space wasted...Kinda weird layout of that blue trace. Try to place it further away from the AC traces.Otherwise, maybe think about mounting those 4 resistors (R3 to R6) vertically on the board, as if they're capacitors with 2 leads, like in the picture below. Shouldn't make the board too high, you already have those heatsinks... and should get them a bit further from heatsink so less temperature drift (if that matters in your design)

author: Chris.M
author_rank: Contributor
timestamp: June 05, 2013, 12:13:37 pm
content: Attached is a fresh attempt. (Positive output is now on the bottom half of board, negative output is now on top half)Have tried to keep the capacitors and resistors as far away as possible from the heat (rectifier and transistors).This layout looks much cleaner.What do you think?Quote from: mariush on June 05, 2013, 01:44:39 amHehe, I got that feeling you didn't.With the type you suggested, I noticed that Dave comments on components that stick up and are unsupported because they might break off from vibrations if transported often. Ie. no heatsink to bolt too.Have you found this to be a problem? Is this a non problem if the instrument sits on the bench all day?Quote from: mariush on June 05, 2013, 01:44:39 amYeah, I thought so too once I finished. You confirmed my opinion.Hopefully the new layout is better.Quote from: mariush on June 05, 2013, 01:44:39 amThanks for that, this is a possibility.

author: Chris.M
author_rank: Contributor
timestamp: June 06, 2013, 02:16:29 am
content: Any thoughts on the latest board?This is my first PCB so I'm trying to get a feel for what to look out for.

author: David_AVD
author_rank: Super Contributor
timestamp: June 06, 2013, 03:11:09 am
content: Are those traces on the top layer? If so, be careful running them under the sharp edges of the heatsinks (assuming they touch the PCB).

author: Chris.M
author_rank: Contributor
timestamp: June 06, 2013, 03:18:19 am
content: I take it your referring to the 3 little traces and the chunky one under HS1 to HS4?Yes, its a single layer board. Is it possible for the heatsinks to pierce through the solder mask?Should I place all the traces on the bottom layer then, and leave the top blank?

author: David_AVD
author_rank: Super Contributor
timestamp: June 06, 2013, 03:34:04 am
content: In my experience, single layer boards (through hole, not SMD) have the traces on the bottom side.I have seen heatsinks cut (melt? they do get hot remember) through the solder mask.

author: free_electron
author_rank: Super Contributor
timestamp: June 06, 2013, 02:19:43 pm
content: Before we dig in to the pcb layout we first need to take a look at the schematic and figure out what parts we actually need ....Your schematic is lacking part numbers for the transistors. Are you sure all three need a heatsink and are in To220 or to126 case ? I smell something wrong.... Ive never seen a power supply in this topology with all transistors on heatsinks....Second : the resistors. Have you done an analysis of what power these need to be ? Some of your footprints are waay too large, some are small....I cant calculate power because you have not told us what is the maximum voltage you want out of this supply.Assuming it's 20 volts ( so 40 volts total )In the output path the max current is 20volt(470+1000) = 13 milliamp.The 470 ohms then gets a Pdiss of 13mA x 7 volt (470 ohm x 13mA ) or roughly 100mW.The potmeter is 150mW.Good.Now, the resistors like the 2200 ohm for the diode chain. 20 volt 2200 is roughly 10mA ( its a little less but i round toward safe side for easy calculation) 20 volt 10mA is 200mW .. Why do i see a 3 watt honker on the board ?The 1000 ohm resistor gets 1/2 watt ... Why do i see a 3 watt honker ?And so on.This is an oft overlooked step. People grab a schematic and they start doing the board... Without picking the parts suitable for the job ! Power dissipation in parts is never looked at.

author: Chris.M
author_rank: Contributor
timestamp: June 07, 2013, 04:02:08 pm
content: Quote from: free_electron on June 06, 2013, 02:19:43 pmGood idea.Quote from: free_electron on June 06, 2013, 02:19:43 pmI have updated the schematic to include part numbers.Indeed, I think I went overboard with the wattage for all of my components including the unnecessary need of heatsinks.The series pass transistor is an 2SC5200 probably overkill for a PSU? Tcase of 150WThe other two transistors are TIP31C's. Tambient of 2WQuote from: free_electron on June 06, 2013, 02:19:43 pmYes, I have attached two analysis files with working for the positive side. An analysis for the pot wound in the two extreme positions with a load to put it into current limiting (~1.5A).I was not able to work out how much current transistor Q6 takes when its current limiting the output.Any hints??Quote from: free_electron on June 06, 2013, 02:19:43 pmSo the power supply has positive and negative output.~4V - 15V (adjustable)Current limited @ 1.5ADrawing a smaller load, my calculations show that it can get closer to the 30 VCC, so I have used 34V (filtered supply voltage without rectifier drop) in the analysis as the worst case.Quote from: free_electron on June 06, 2013, 02:19:43 pmMy numbers would seem to be in the ball park, they differ because we used different output voltages.Quote from: free_electron on June 06, 2013, 02:19:43 pmYeah, went overboard with 5W resistors (those big wire wound ones with the white ceramic case).Quote from: free_electron on June 06, 2013, 02:19:43 pmYeah, even though I did the calculations, I put in components well above what is needed. This has come back to bite me as they take up more room making a much larger board.So if I were to put together a parts list based on the calculations I have (would you have time to check them over?), does these maximum power dissipation and component selections look okay:R1 = 850mW max (therefore 2W)R3 = 115mW max (therefore 0.25W)R6 = 1100mW max (therefore 2W)R7 = 65mW max (therefore 0.25W)R9 (pot) = 150mW max (therefore 0.25W, I have 3W already)TIP31C = ~35mW (NO Heatsink needed)2SC5200 = 50W when limiting at short circuit (I have a large external heatsink)Bridge Rectifier - 400V, 6A (If heat is not an issue, I can go with the one like what mariush suggestedhttp://www.digikey.com/product-detail/en/GBU4M-BP/GBU4M-BPMS-ND/1140594)

author: Chris.M
author_rank: Contributor
timestamp: June 12, 2013, 11:12:17 am
content: Quote from: free_electron on June 06, 2013, 02:19:43 pmOkay, so I have updated the analysis calculations since my last post as some of the intermediate calculations were off by a little, but it left the end power dissipation calculations the same.I have prototyped the design, and can confirm that the voltages match those in the calculations.There is also no heat coming from the regulating transistor Q3 or the current limiting transistor Q6. Nor is there any heat from the rectifier.I'm happy with the power dissipation figures and we can change the resistors to the smaller wattage ones in my previous post, remove the To220 heatsinks and change the rectifier to a vertical one. This has already saved me 15mm of board space.free_electron, what are your thoughts on the pcb layout?

author: Rerouter
author_rank: Super Contributor
timestamp: June 12, 2013, 11:49:42 am
content: as you have the board space, perhaps shift Q1/Q2 a bit further away from your caps,rotate R1/R2 in parallel with Q1/Q2, this will simplify routing, then have R2/R4 run across the power trace it feeds into the Q3-Q6/Q4-Q5make D5-D7 a mirror of D2-D4,if possible, Q4 and Q5 would be easier to route if turned 180 degrees each, but I'm guessing your using a common heatsink which restricts you from doing that..that's more from a simple to route with stupidly thick traces line of reasoning as opposed to what some of the other guys might chime in with, later,

author: Chris.M
author_rank: Contributor
timestamp: June 13, 2013, 10:22:45 am
content: Thanks for the feedback Rerouter.What you said clicked, so I started again incorporating some of your suggestions and those from earlier feedback and I think I now have a good layout in terms of being clean.Can anyone see any potential issues that my routing may cause? Does it look okay?

author: Rerouter
author_rank: Super Contributor
timestamp: June 13, 2013, 11:06:37 am
content: now i'm left with only 1 more recommendation, and this is more from a lifetime aspect, on your R1/R2 traces beef them up, you can only ever support them in one axis by bending the leads so giving it a big bulk of copper to support it means a much smaller risk of a track lifting than your piddly base traces currently,i see Scania tachometers once a week with the exact same problem...

author: poorchava
author_rank: Super Contributor
timestamp: June 20, 2013, 08:04:39 am
content: Looks pretty good to me. I see that you managed to do it on a single layer. If you want to make the pcb at home I suggest that you make those thin traces a bit thicker. You have enough space for that.

author: Chris.M
author_rank: Contributor
timestamp: June 20, 2013, 01:29:58 pm
content: Quote from: Rerouter on June 13, 2013, 11:06:37 amThanks for the heads up, have beefed up the traces. Also increased the pad sizes.Quote from: poorchava on June 20, 2013, 08:04:39 amThanks poorchava. The smaller traces are now all 50mil, with the higher current ones 120mil.Looks like it's ready if I haven't missed anything.