Group Actions
Engagement
  • Author Author: Andrew J
  • Date Created: Date Created
  • Views 1569 views
  • Likes 8 likes
  • Comments 29 comments
Related
Recommended

YAPS Part Twelve - Design revisited: reworking the layout and PCB

Andrew J

Two things became very clear to me once I got into the detailed testing of the project:

  • I have completely stuffed up the grounding and layout of the components.  In particular the Switching Regulator has a convoluted route back to Vin -ve and the route it does have takes it right under the sensitive components (until I bodged in a couple of wires).  Layout is too far apart for many components, including the bypass and decoupling caps, and non-conducive to managing noise.  There are no test points with the result that I have blown a number of components including 3 ports on the very expensive 4Duino.
  • I really didn’t have enough knowledge about DC-DC Switching Regulators - I sort of hinted at this in my design post - which becomes clear as you read the answers to some of the advice being given.  In some respects that might be a good thing as maybe I wouldn’t have started on this!  However, I apologise to those who have graciously helped out nonetheless and hopefully I've at least made a start in remedying that.

 

On the plus side, testing showed that functionally it works so I can get my 0-15V, 0-3A out.  I set about sorting out my understanding so that I could properly layout the board, but also have a much better understanding of how that part of the circuit is working so I can properly probe and test it.  There is excellent coverage of the subject from Micro-Rohm, starting with Switching Regulator Basics, that covers DC-DC switchers in some detail but at the same time keeps the language easy to follow.  There are also a multitude of papers from TI and Analog and the data sheets for buck converter ICs have been helpful - the LT1624 datasheet is still confusing though.

 

The design is still basically the same, with most changes to the Switching Circuit and Linear Regulator Circuit.

 

Switching Circuit

Essentially the same but with the following changes (annotated in red):

 

image

  1. Test points for the LTC1624 pins and output at the inductor
  2. A placeholder on the gate driver (pin TG) for a small resistor, R2, to adjust the rise time of the MOSFET to help counteract ringing if necessary.
  3. A placeholder for a boost resistor, R3, (pin BOOST) at the switching node to help with ringing there, if necessary.  Possibly a ferrite bead rather than resistor.
  4. A placeholder for a Snubber at the switching node, R5 and C9 ( to help with switching noise if necessary.
  5. A placeholder for a ceramic capacitor on Vout, C15, if I want to experiment with adjustments there.
  6. Upsized the sense resistor to a 1206/500mW part, same 10mOhm resistance.  Takes a bit more area but should be more resilient than the 0805, particularly as I’ve blown it up 3 times!  I’m mostly thinking of ease of replacement.
  7. Upsized the inductor to 50uH: the part I’ve chosen has better specs for resistance, self resonance frequency and saturation current than the original 10uH part (although in fairness, the other part’s specs should have been ok.)  LTSpice simulation shows that ripple on the output - and through the Feedback Circuit - is significantly improved.
  8. The MOSFET is now a SMD component - IRF8721 - with the same (slightly better) specs than the TO220 IRLB8721.

 

The main concern for the MOSFET was a power dissipation characteristic of only 2W.  I did some soak testing for temperature gain of the existing MOSFET and calculated wattage from that - see below.  The TO220 package doesn’t take up a lot more space than the SMD component (considering just the leg soldering area) but it is a lot more awkward to position and route to.  I did vacillate a bit on this as I know the existing part works : I’ve replaced the existing Mosfet 3 times - once when I blew it up, once when I swapped it for a better part, and once when I de-soldered it for testing when I thought I might have damaged it.

 

The resistor placeholders R2 and R3 will be populated with a 0 ohm (<5mOhms) resistors initially; R5 and C? will remain unpopulated.  Depending upon what I see during the testing I can populate one of more of these placeholders with actual resistors/ferrite beads and resistor and capacitor in the case of the Snubber.  My understanding is that care is needed with changing the MOSFET timing (BOOST and Gate resistors) as it will increase the switching losses.

 

MOSFET Temperature Soak Testing

I ran the existing circuit at a range of volts and amps for an hour - 50 mins with the 5Ohm load as I had to leave to do something else and didn’t want to leave it unattended - and captured temperatures at 10 min intervals.  I took the peak temperature for the IRLB8721 MOSFET and using the original Ambient Temperature and the MOSFET’s Tja specification, calculated the power from the temperature rise (temp diff / Tja).  Even in the worst case temperature rise, power dissipation was 0.333mW, well within the replacement's power dissipation rating even after de-rating to 150C.

image

image

image

I’d be very interested to hear feedback on this.  I could switch it back to the TO220 package before I get the board made if I’ve messed up the calculations.

 

Linear Regulator Circuit

Again, essentially the same but with the following changes (annotated in red):

 

image

  1. Test points for the LT3081 pins
  2. Placeholders for addition ceramic capacitors at the input to the regulators, C18 and C19
  3. Placeholders for Ferrite Beads,  R13, R18 and R19, to help with ripple and frequency noise, if necessary.  These will initially be populated with 0Ohm resistors.
  4. Moved the Schottky Diode from the Current Source circuit into the Linear Regulator circuit.

 

The placeholders for Ferrite Beads are interesting because I have to take into account component sizes as well as their placement on the high-current path.  Scanning around on Farnell, CPC, RS, Digikey, getting a correspondence of size between 0Ohm resistors and Ferrite Beads (at this stage I don’t know if I need them nor what specs if I do) is nigh-on impossible.  So I’ve gone with a 2512 (6.4mmmx3.2mm) size resistor and custom-sized the pads so that 1812 ferrite beads can be used - this seemed to give me the best tradeoff in size correlation.

 

PCB

Hopefully the images I've pasted are viewable but I've attached the Gerbers as well.  With the layout needed, I've gone with a 4-layer board to achieve it - it's a bit more expensive but for the sake of £20-ish it feels worth it given the difficulty of trying to do this with 2-layers, at least that's how I perceive it.  It's also resulted in a slightly larger board at 100mm x 95mm (current version is 100mm x 75mm.)

 

Layer Stack

Top: components, high current traces, high current ground traces, signal traces

Layer 2: Shield Ground

Layer 3: Signal Ground

Bottom: Signal traces

 

Test Points

I’ve added in pins for testing of components that have caused me great difficulty in the past:

  • The Switching Regulator pins: I’ve separated out the Switching and Boost pins from the more sensitive pins.
  • The Mosfet gate pin: I will want to be measuring ringing and noise at this point.
  • The Linear Regulators
  • The Current Sense INA260: both Vin and Vout from that chip

I’ve taken the approach of using pins that I can actually either clip a probe to or stick the probe tip into; each has an associated ground pin into which I can insert the short, springy probe ground to avoid have a large ground wire affecting measurements.

 

Ground Plane vs Star Ground

Before I get into the layers in more detail, I want to start off with this as it’s come up a bit in comments.   As I researched this it became clear that TI, Analog, Micro-Rohm and others all recommend ground plane; however I cannot also ignore Gene’s comments and advice, which comes from experience, to avoid these and use Star Ground.  So where does that leave me: I don’t yet have the experience of implementations (of both approaches) to determine which would be best nor can I make multiple boards with different configurations - the costs are just too high.

 

So, I have to make a decision and what I’ve gone with is the advice from TI, Analog, Micro-Rohm:

  • All high current ground traces are on the top layer except for two places where I had to go down to layer 2
  • Layer 2 is a Shield Ground which connects solely by the -Ve PCB terminal for Vin.  There are no other connections to this layer.  However, there are vias and through-holes plus the two high current traces that needed to be routed off the top layer.  There is also a Keep-Out underneath the Inductor (L1).
  • Layer 3 is a Signal Ground layer which connects solely by the -Ve PCB terminal for Vin.  There are no other traces on this layer but there are, obviously, connections for all low-current components.   There are also through-holes and vias and a Keep-Out underneath the Inductor (L1).

How does one avoid creating TH 'slots' (holes in a row) in these layers?  I have no idea.  Quite a few come from the test points I’ve incorporated: even using SMD points would require vias for the ground pins unless I avoided those.

I’ve avoided Thermal Vias as testing to date shows that’s not necessary and it would make more holes through the layers.

 

Check list

Now I have a better understanding of the Switching Regulator, I’ve been able to take a better understanding of layout practices from my reading of data sheet layouts from TI and LT (Analog) as well as the explanation and points presented by Micro-Rohm:

  • Keep the bypass capacitor (Cby1) as close to VDD of the switching regulator as possible.  TICK
  • Keep the loop consisting of Input Cap (Cin1), Sense Resistor (R4), Mosfet (Q1), Schottky Diode (D1) as short as possible.  TICK
  • Keep the loop consisting of Schottky Diode (D1), Inductor (L1) and Output Cap (Cout1) as small as possible.  TICK
  • Traces carrying high currents off the ground plane and away from the sensitive feedback circuit.  TICK
  • Keep the Switching Node - SW pin, D1, L1 and Q1 Source small.  TICK.
  • Use kelvin connections from the feedback circuit connected just after the Output Capacitors.  Vfb should connect directly to the resistors.  TICK
  • Feedback circuit should be connected to the + plate of Output capacitor.  TICK - actually, there are more than one output capacitor and it connects just after the last one as per TI advice.
  • Keep the connections from feedback resistors to the Vfb pin (R6 and R7 - and really also Q2) short and away from the Switching Node.  TICK
  • Gate drive trace should be as close as possible to the Mosfet (Q1) gate.  TICK.  in my opinion - given ‘close’ is relative and I can’t physically get the larger parts any closer!  Part manufacturers don’t help with their pin layout either.
  • Signal and Power Grounds separated.  TICK
  • Does the input capacitor (Cin1) +ve connect to Sense Resistor (R4) as closely as possible. TICK
  • Does Cin1 connect as close as possible to GND pin of Switching Regulator.  TICK - in as much as this makes zero sense as their grounds are meant to be kept seperate!
  • Is ground of Cin1 and Cout1 separated by at least 1-2cm. TICK
  • Is the Inductor (L1) close as possible to the Switching Regulator.  TICK
  • Is the wiring to the Inductor input as small as possible.  Is the wiring distance between the Inductor terminals as great as possible. TICK
  • Are there no ground or signal traces under the Inductor.  Is the Ground Plane kept from underneath the inductor. TICK
  • Are the Inductor and Output Capacitor (Cout1) as close as possible.  TICK
  • Signal and Power Grounds must be kept separate.  TICK
  • Top Layer Power Grounds and Inner Layer Power Grounds must be connected by numerous vias.  TICK (there are only two places where I have routed Power Ground to the inner layer.)
  • Power Ground should be connected to a common ground or signal ground near an Output Capacitor.  NO TICK - grounds and ground planes are connected at one point only near the Power in terminal, based on discussions/advice here.  I believe this point is based on the grounds for the Switching Regulator only, not the 'load circuit' - I have done that with the feedback circuit and IC GND connections.

 

Quite a substantial checklist but I think I’ve hit them all including the last point.  The grounds are tied at the -Ve pin for VIn but in Kicad I can only do this with a Net tie component - it’s not possible to specify a pin or pad as belonging to multiple nets.  You can see the Net tie in the PCB top layer by the -Ve pin of the PCB terminal.  I think this is ok - any noise from power ground that hits the Shield Ground would route out here.

 

Silkscreen and Solder Mask

To make it easier to see some of the following images, here's just the silkscreen and solder mask:

image

 

Top Layer

image

(Green traces are bottom layer traces)

High Current traces, shown with green arrows, route along the right, bottom and right side.  Ground traces, shown with cyan arrows route in a similar manner: where I have ducked down to layer 2, dashed cyan arrows, (the Shield Ground) I have used vias to connect the traces - I've just noticed that the fourth short arrow at U3 should be a dashed one.  These are 0.508mm diameter with 0.254mm drill but would it be worth making them bigger?  The check list calls for “numerous” but could I do with fewer of them to reduce via holes through the layers?

 

Components are placed quite close to each other - much closer than in the last version.  It looks do-able hand-soldering.  In particular, the feedback circuit is well away from the power traces and route through traces to just past the output capacitors.  You can see that I route the GND return under the power ground (on the signal layer) to connect there by the output capacitors as well - it is equally possible to connect at the point it ducks down but I’ve kept the traces together as recommended by the check list.

 

Shield Ground Layer

image

This is intended to keep noise away from the non-power components although I could well have misunderstood the concept.  Nothing directly connects to this layer except the NETTIE so it isn’t directly used by anything as a path to ground.  Should I have limited the area to under the high-current traces only?

 

Signal Ground Layer

image

This is used as a ground plane by the non-power components - i.e. those not directly related to carrying high-current to Vout.  There are multiple connections on this layer but no traces.  All the cheaper manufacturing companies preclude the use of blind or hidden vias so they all route through 4 layers.

 

Bottom Layer

image

This carries signal traces that can’t route on the top layer.  There’s not that many of them really.

 

Summary

I think I’ve made a much better job of laying out and routing the design this time.  The first version was so bad it wasn’t even worth trying to start dealing with the sources of noise but my hope is this will prove capable of proper measurement and action: the placeholders for ferrite beads/capacitors/resistors can at least allow some modifications to be made as a result and the test points will prevent me blowing components up.  I'm more than happy to provide additional information if anyone is interested.

 

A summary of my questions:

  1. Would it be advisable to swap the MOSFET back to the TH version I used before which is more capable of dissipating power?
  2. Is the use of TH pins for the GND connection with my test points - so I can use the short GND wire on my probe - better than removing those holes through the planes?  Alternatives would be to use SMD test points with vias (smaller diameter) or doing away with GND test points and using the longer crocodile clipped GND wire.
  3. Layout guidance uses a lot of relative terms such as ‘close’ and ‘as possible’.  Is the trace from the Switching Regulator (U1) to the gate of the MOSFET (Q1) too long?
  4. The GND connections for the feedback circuit, Switching Regulator and the ITH/Run pins route around to connect to PWRGND just past the Output Capacitors (one piece of advice read.)  Would it be better to route these directly to the +ve and =ve pads of Cout1 - the 100uF output capacitor (another piece of advice read.)
  5. They don’t just connect to PWRGND just past the output capacitors, they also route under PWRGRND to do so: I could avoid doing that and connect at the point the trace jumps down.  Is it better to leave as-is?
  6. The PWRGND traces all route back on the top layer to the -Ve pin on VIN.  Very close to this point is the single connection for Shield Ground and Signal Ground.  Would it be better placing this nettie close to -Ve pin on Cout1?
  7. The Shield Ground is the full size of the board.  Should I just place this under the high-current routes or does it not make any difference?
  8. From experience, does this look hand-solderable if care is taken with the order of placement of components.
  9. I have no copper fills on the front or back layers.  If I added these and tied them to the nearest ground plane the vias would pass through all 4-layers.  Ultimately, I don’t know if it would improve anything so I didn’t bother as more holes in the layers seems ‘a worse thing’ but am I wrong?

 

I’d be very interested in thoughts and observations on my approach so I don’t make the same mistakes as last time.  In particular, given that grounding was a major issue in the current version, what’s your views on how I’ve done this time.

 

Next: Part Twelve Reprise - Design revisited

Back: Part Eleven - Further Testing

Attachments:
YAPSv12Gerbers.zip
Parents

  • A quick update on this.  I received the boards and populated but I don't think I did a great job of soldering - which is a shame as I'd done alright up to now.  Anyway, turning on, I could only get 19V out (rather than the max 15V) and no amount of twiddling with the Voltage/Current Pots did anything; one of the Linear Regulators got to 80C quite quickly whilst the other didn't rise in temperature at all.  Current pot had zero impact; the voltage pot turned output voltage down to 10V when it was fully wound to 0Ohms.  The load switch also dropped the voltage to 10V (which was in line with the 0Ohm Voltage pot) so somewhere along the line something was wrong and slinging out a minimum 10V.  I found a dodgy connection on the output of the second Linear Regulator and also found that the Mosfet was completely open - connectivity between drain and source and gate.

     

    I resoldered the Linear Regulator and that seems ok now - at least, I can see continuity from the output leg and the tab which was erratic before.  I also removed and replaced the Mosfet.  I did check for overshoot on Vin first: set the trigger to 29V on a rising edge and turned on, but there was no triggering. 

     

    At the moment I am getting around 20mV on the Switching Node.  Gate is swinging up to around 5V but the Switching pin seems to be doing nothing.  I suspect that the DC-DC converter has blown: might not be surprising if the Mosfet was open and 26V was flowing through the gate, switch and feedback pins. It could be the Schottky Diode.  Of course, there could now be issues with the Linear Regulators, the Current Source and other components. 

     

    So the upshot is, I'm deciding whether its worth restocking the parts yet again.  Some of these I only seem to be able to source from the US and all told, it would be another £40 or so.  I may be as likely to damage them soldering as not which is a concern (I'm assuming the Mosfet wasn't faulty until I soldered it to the board but I suppose it may have been)  I could assume the parts on the first version board are ok and remove them - I'd need to invest in a hot air rework station for that.  If I could work out what was actually wrong so I had a little more confidence on what to change I'd be happier.

  • in reply to Andrew J

    Hi Andrew,

     

    Sorry, I'm only just getting to this now, and have read through the blog post and comments. You've done a lot of work to the PCB! It sounds like a lot of the earlier issues with the PCB are ironed out now, but the issue seems to be damaged parts, due to loose/unsoldered connections possibly?

    This can happen with hand soldering the really tiny parts, but there are some tricks to reduce the risk a huge amount. After it is soldered, if you have a stiff brush (ideally an antistatic one, but a toothbrush could work perhaps) then some isopropyl alcohol can be put on the board, and scrubbed around each IC, MOSFET, etc. It gets the flux dissolved, so you can wipe it off with (say) paper wipes used for cleaning screens/specs. Then, using the reverse side of a thin blade (e.g. scalpel) you can gently nudge each pin (while looking through a magnifier if needed), to see if it is stuck, and if it moves then it needs re-soldering.

    Also, although a soldering mat etc helps, you can go a long way to eliminating any damage to the components in a prototype, by soldering the ICs and MOSFETs last, and definitely not having any soft loose things like suit, blanket, cushions etc that could rub.

    Do you know how the controller inputs that you mentioned got blown? Was it an accidental connection to the wrong pin? How is it wired to the board (soldered, or jumper pins)? If jumper pins, the risk is reduced by using a full-length socket, instead of single jumper pin sockets, (and the're normally low-cost for the 2.54mm pitch connectors).

    Regarding component cost, the LT stuff is pricey, so if you can get free samples that could help (they will usually send two of each). Similarly On Semi will supply a fair qty of Schottky diodes as samples (although they are cheaper anyway).

    It would definitely be good to use (say) 10 ohm for R2, since it will protect U1 if something happens with Q1, and double-check D2 has both ends soldered, since an open circuit there risks damaging both of the linear regulators. Also, just in case there's any spikes of high voltage on the input (it is possible when switching on/off some supplies) a TVS diode on the supply input could be used (just soldered across the input terminal if you've already got the PCB made up), rated so that it protects beyond the max expected voltage on the input).

    Best of luck with the project, it feels like you're close to ironing out all the issues.

  • in reply to shabaz

    Thanks Shabaz.

     

    I don’t know what might have blown it, my suspicion is I damaged the MOSFET when soldering but I don’t know.  I could tell because I could get continuity across the Gate pin and Vin pin on the DC-DC converter which could only happen if the converter itself was blown or there was continuity from Vin to Drain to Gate to Gate on the converter.  Which was the case.  I have tested for overshoot on startup but that’s not happening but maybe too fast for the scope to pick up??  I assume when you say solder a TVS over the input, you mean between the output of the Power stage (rectification and smoothing) to the control stage.

     

    I’ve changed the MOSFET and no longer have that continuity but I’m getting practically nothing on the Switch node, circa 1v, instead of a square wave from approx -0.3v to 26V.  I am getting a square wave on the Gate pin from circa 0V and 5V (which is expected as it rises to Switch node +5V.)

     

    I suspect that the DC-DC converter is also damaged.  It was a lot harder to solder this board up because, I think, of the two ground planes on layers 2 and 3.  I probably should have used a hotter iron.

     

    I use an ESD mat connected to mains ground with a wrist band connected to the mat.  I also have one of those stiff brushes - one you recommended actually - and use IPA and lint-free paper to clean up after soldering.  I also test each pin I solder for bridging and firm connection.

     

    I made very little change to the circuit: some 0Ohm jumpers which I could swap for ferrite beads if needed; additional capacitance on the input (extra 30uF) based on calculations.  I changed the output capacitance based on calculations but that reduced.  Output capacitance is ‘enough’ when the needed ESR is reached. 

     

    If I could wish for anything it would be the ability to test things in-circuit and to have a PCB surface with some friction image  Living in the real world, what I’ve done now is invested in a hot air rework station.  I still have the V1 board which works functionally so I intend to methodically swap over the chips to see what, if any, are damaged.  Hopefully using hot air will reduce chances of damaging anything further.  I will then take it from there.  I may even switch to another PCB (I had 5 made) in case there is damage or bad manufacturing, on the one I currently have soldered up.  This may take a while as I’m off on holiday for a week but I will report back.

  • in reply to Andrew J

    Hi Andrew,

     

    I find hot air stations hard to use personally, but there's people on youtube that make it look a breeze.

    The MOSFET is a SOIC package and those are best soldered with an iron by holding it in place with tweezers (sometimes I may tape an IC down with Kapton tape or paper tape, but not on a MOSFET, and since it's a SOIC-8, it's easy to hold with tweezers) while soldering down the first pin. There's low-risk of soldering-iron heat damage for those, so it may have failed afterwards (i.e. after power was applied). By the way, in the circuit, there is no gate protection until U1 is soldered, so U1 should be soldered before the MOSFET is soldered, just for a bit extra protection during assembly.

    For removing the MOSFET, the hot air should work for you (I have an under-powered hot air tool so I find that difficult, and lift pins with iron+tweezers one at a time, which is bad for the pads, but I've not needed to do it much, usually I'm removing passives etc : (.

    Regarding the comment about U1 being harder to solder on this PCB, it sounds very likely the iron temperature is the issue, not the PCB. Can I ask what iron you're using (i.e. how many watts, and what tip shape)? The SOIC packages with no thermal pads underneath should be really easy to solder on, but depends on the iron. I'll record a short video of soldering down a SOIC and post a link, if it helps spot any differences in workflow (not saying my workflow is good, just that it seems to work for me sufficiently for prototypes).

    The TVS I was thinking to be across PI and GNDPWR connections, i.e. across J1 on the PCB. What input supply voltage are you using at J1? I can look for a suitable TVS for that.

  • in reply to shabaz

    Remember those SMD practice kits I tried a while back?  Well, they've come in handy for practicing with the hot air station, de-soldering and re-soldering parts.  I've found it not too bad - it's an ATTEN 858D+.  I was going to get a Quick 861DE which seems very popular, but for that price I could get the Atten, a de-soldering gun for TH parts, some solder paste, and still have more than £100 in the bank!  I couldn't really see the need for 1200W or 200L of air for home use.  Both the hot air station and gun seem to work well.

     

    How you describe soldering the SOIC is how I do all the ICs.  I've not had any problems soldering in the past so maybe the part was defective to start with (unlikely) or maybe it blew for some other reason.  I'm presuming that if, on the board, I can see continuity between Drain, Gate and Source, and continuity between U1 Vin and U1 Gate via the MOSFET that the MOSFET it blown.  I have a Hakko FX-888D station and I use either a T-18-D12 tip (for the small parts/pads) or a T-18-C2 for the larger pads/TH parts.  I was using 300C but did up it to 320C - I've had good results with 300C in the past, but that was on 2-layer boards which would have a greater separation between the top and bottom layers.  I think that 350C would be better on the 4-layer.

     

    What I have found this afternoon testing parts, by de-soldering and putting them onto the V1 board one-by-one, is that the DC-DC convertor is ok, the Current Source is ok, one of the Linear Regulators is ok, and one is bad - I'm getting 0V output on the 'good' board with it in place.  So I'm swapping it over with a good one from the V1 board to see if that helps.  I'm now thinking that if it was faulty and causing problems in the output, then given there was no call on the power from the DC-DC convertor it was turning the MOSFET off.  It has a comparator internally that turns the MOSFET off if the transient output  overshoots by >7.5%.  That seems a bit backward on second thoughts actually (plus the gate was driven at 5V), but the output from the Switching Node was 1.8V to the Linear Regulators so an alternative reason may be the feedback voltage is so low that it wasn't operating at a high enough frequency or perhaps ITH/RUN was pulled down.  Unfortunately I've disconnected it now.

     

    Voltage in at J1 is 27V.  I would want to keep it below 28V (in terms of any spike.) 

     

    I am seeking one bit of advice: now that I've found a faulty part, is it worth building the circuit up on a fresh board?  Currently, the DC-DC converters, Current Source, Linear Regulators are off the board.  I would need to de-solder the Schottkys, Inductor and Input/Output Electrolytics but I have a spare MOSFET and plenty of other passives.  I'm thinking that it would give me a chance to get them off and test them before soldering back on again.  If there is another problem with the board, putting these back on the same one may result in something blowing again?  I may be being paranoid of course, hence the request for advice.  What do you (others) think?

Comment
  • in reply to shabaz

    Remember those SMD practice kits I tried a while back?  Well, they've come in handy for practicing with the hot air station, de-soldering and re-soldering parts.  I've found it not too bad - it's an ATTEN 858D+.  I was going to get a Quick 861DE which seems very popular, but for that price I could get the Atten, a de-soldering gun for TH parts, some solder paste, and still have more than £100 in the bank!  I couldn't really see the need for 1200W or 200L of air for home use.  Both the hot air station and gun seem to work well.

     

    How you describe soldering the SOIC is how I do all the ICs.  I've not had any problems soldering in the past so maybe the part was defective to start with (unlikely) or maybe it blew for some other reason.  I'm presuming that if, on the board, I can see continuity between Drain, Gate and Source, and continuity between U1 Vin and U1 Gate via the MOSFET that the MOSFET it blown.  I have a Hakko FX-888D station and I use either a T-18-D12 tip (for the small parts/pads) or a T-18-C2 for the larger pads/TH parts.  I was using 300C but did up it to 320C - I've had good results with 300C in the past, but that was on 2-layer boards which would have a greater separation between the top and bottom layers.  I think that 350C would be better on the 4-layer.

     

    What I have found this afternoon testing parts, by de-soldering and putting them onto the V1 board one-by-one, is that the DC-DC convertor is ok, the Current Source is ok, one of the Linear Regulators is ok, and one is bad - I'm getting 0V output on the 'good' board with it in place.  So I'm swapping it over with a good one from the V1 board to see if that helps.  I'm now thinking that if it was faulty and causing problems in the output, then given there was no call on the power from the DC-DC convertor it was turning the MOSFET off.  It has a comparator internally that turns the MOSFET off if the transient output  overshoots by >7.5%.  That seems a bit backward on second thoughts actually (plus the gate was driven at 5V), but the output from the Switching Node was 1.8V to the Linear Regulators so an alternative reason may be the feedback voltage is so low that it wasn't operating at a high enough frequency or perhaps ITH/RUN was pulled down.  Unfortunately I've disconnected it now.

     

    Voltage in at J1 is 27V.  I would want to keep it below 28V (in terms of any spike.) 

     

    I am seeking one bit of advice: now that I've found a faulty part, is it worth building the circuit up on a fresh board?  Currently, the DC-DC converters, Current Source, Linear Regulators are off the board.  I would need to de-solder the Schottkys, Inductor and Input/Output Electrolytics but I have a spare MOSFET and plenty of other passives.  I'm thinking that it would give me a chance to get them off and test them before soldering back on again.  If there is another problem with the board, putting these back on the same one may result in something blowing again?  I may be being paranoid of course, hence the request for advice.  What do you (others) think?

Children
  • in reply to Andrew J

    Hi Andrew,

     

    Given the tip size and iron rating, your settings are in the right ballpark for SOIC.. maybe the temperature can be raised slightly. I too use a ~1mm tip, and set to 330 degrees C, for 2 or 4 layer. The time taken to do one join is ~2sec, but even if it took 4 sec, it's unlikely to cause damage due to soldering heat. If it's taking longer than a couple of seconds from start to finish for a joint, then the temperature should be raised.

    For the TVS, this would be good to use: VTVS28ASMFVTVS28ASMF

    There's not much headroom (the DC-DC converter has a max rating of 36V) so the TVS is worth including just in case.

    Also, this MOSFET is a drop-in replacement: IRF7469TRPBFIRF7469TRPBF  and has higher VDS, again just in case (because the other one has 30V rating) so is worth considering too.

    As you say, if there's continuity between any of the terminals, then it is faulty.

     

    If there is a follow-on board, a zener across the gate-source of the MOSFET could be an option too: BZX84C12LT1GBZX84C12LT1G (and have the 10 ohm between the gate and U1. It shouldn't be needed though, so not worth creating another PCB just for this.

     

    I did record an example of SOIC soldering on a 4-layer board anyway, this is with 0.38mm solder, about the thickest usable for large surface mount (for TSSOP or smaller, thinner is better):

  • in reply to shabaz

    My technique is pretty much the same: tack one corner, solder down one side then back up the other.  I have   0.274mm solder for the small parts and 0.48mm for larger parts.  I also have 0.6mm lead free which I bought by mistake!

     

    I know I was taking a bit of a chance with the MOSFET I had as there wasn’t a lot of headroom.  On V1 board I was seeing a bit over 26V but didn’t measure any overshoot.  With the MOSFET you suggest there, the input capacitance, CISS at 2000pF, is at the limit of what the data sheet states: the Boost capacitor must be 50X larger than the total MOSFET input capacitance.  With a 0.1uF Boost capacitor (which the data sheet says is adequate in most applications) that puts input capacitance at 2000pF.  I spent quite some time finding a part with a lower CISS, the trade off seemed to be Vds.  There are thousands upon thousands of these things though, as you know, so I didn’t check them all!!  Any thoughts?

     

    I will try a TVS - I can solder it across the PCB terminals on the bottom of the board.

     

    R2 is a 0Ohm placeholder for a resistor (or perhaps ferrite bead) to help control ringing on the gate if necessary so a 10Ohm could go in there.

  • in reply to Andrew J

    Hi Andrew,

     

    A 0.1uF X5R or X7R boost capacitor should hopefully still work, at least, worth a try to use the 40V MOSFET. I'm hoping that plus the gate resistor and the TVS should together provide some resilience, fingers crossed! : ) I think a gate resistor is worth adding by default, even with the 40V MOSFET. The MOSFET could have a tiny heatsink stuck to it if needed.

  • in reply to shabaz

    Thanks - I'll give it some thought along with what I'm going to do.  At the moment, it's not going well enough for those to help image

     

    I have the circuit re-assembled and I can now get 15V /1.5A with the 10Ohm load (actually around 15.5V.)  But:

    • When I first turn on, Vout might be as high as 17V.  I've noticed if I turn the load switch off, or pots down then the switch back on or pots back up it goes to 15V.
    • Feedback voltage is 1.5V rather than 1.19V
    • The Mosfet is rising to 90C or so after a few minutes (I've now put a small heatsink on it so it subsequently got to around 65C)
    • One of the Linear Regulators is running cool - 35C or so - and one had reached over 105C after a few minutes
    • The voltage after the Output Capacitors is around 22V instead of around 17V (it should be approx. 1.7V higher than the output voltage because of the feedback circuit)
    • When I turn the load switch off, or turn the Voltage Pot down to 0Ohms, output should be 0V 0A, but it is 20mV 0A.

     

    None of these were problems in the first version which functionally worked ok - the output was just too noisy.  The circuit is pretty much the same but with some changes:

    • Layout is completely different.  Also, 4 layers instead of 2 with two ground planes on the inner layers. 
    • There are an abundance of test points - through holes for either probes direct or test pins - so that I can measure points of the circuit without interacting with pins directly (and blowing things up which was a too-common occurrence on V1)
    • I put some zero ohm jumpers in a number of places that I could swap out if needed.
      • Between the DC-DC Gate pin and Mosfet Gate
      • Between the Boost Cap and switching node
      • Between the Output Capacitors and the Linear Regulator Vin
      • Between the Linear Regulator output pin and output capacitors
    • Placeholders for a resistor and capacitor for a snubber circuit at the Switch node.  Not populated.
    • Placeholder by each Linear Regulator for a low value capacitor to improve Vin input if needed.  Not populated.
    • Placeholder by the output PCB terminal for a low value capacitor to improve Vout if needed.  Not populated.
    • Changed the Mosfet to a surface mount version of the one I was using.  Minor characteristic changes (all better) except for power dissipation which is significantly less.
    • Changed the Inductor from 10uH to 50uH - based on calculations and improvements observed in the LTSpice simulation
    • Changed the input capacitance from 110uF to 140uF (100 electrolytic, rest ceramic)  From calculations I made - actually, calcs showed 40uF ceramics and 50uF electrolytic but I couldn't find a component with the right ESR at 50uF.
    • Changed the output capacitance from 150uF to 131.11uF (100 electrolytic, rest ceramic).  Meets required ESR plus decade caps for noise.
    • I also added in a 15nF capacitor into the feedback circuit as I bodged this into version 1 and improved output quite a bit (for example, the 15V 3A output with a 5Ohm load was achieved rather than 14V and 2.8A.)

     

    For the brief time I can run it and measure the output, I'm seeing about 2mV pk-pk noise at 15.5V, 1.55A which is pretty good I think, albeit not very definitive testing (x1 probe, AC coupled)

     

    I can't see what in those changes could have made such a dramatic difference, any ideas?  I'll think about it over the next week whilst I'm tramping the North York Moors.  I may be inclined to desolder and build up on a fresh board - I have 5 of the new ones - test components as I go (e.g. passives, diodes, transistors, inductor) and take things back to how they were in V1, or at least as close as I can (e.g. 10uH, 110uF input, 150uF output) as a start point.  It feels though there's something more fundamental wrong with it at the moment but I can't tell what and I don't want to keep throwing more money at it without knowing why.

  • in reply to Andrew J

    Hi Andrew,

     

    I think they could all be related to one issue perhaps, because things like the linear regulators should be behaving identically, since it's the same circuit for each of them, just paralleled. I think there's a chance it is either some glitch or overshoot that's damaging parts (e.g. on the supply input to the board, or the output of the DC-DC converter), because 27V is  close to the limit of the ICs and MOSFET. I don't feel all these issues could be related to the PCB layout, if the paths have been shortened (on the earlier PCB, there was a very long path for the ground to the input capacitors, but now it's short). If it is passing CAD tool error and design rule checks, then the board should be electrically identical to the earlier PCB, but just with a better layout. Things like holes for the test points are not likely to be an issue either. Hard to know what to suggest : ( Anyway I'll think on it more too. I hope you enjoy your hols!!