Hi Guys
I am trying to get a MCP73833 working however it seems to be acting strange. I have two versions wired up identically however the PCB layouts are different. One works fine and the other one making a really high pitched sound and the charge current is not what it should be. See layouts below. The first one works, the second one does not. I have also attached the schematic of the circuit.
Microchip forums are here: https://www.microchip.com/forums...
Analogue & Interface: https://www.microchip.com/forums...
I have measured the input voltage and it is at 4.28V. Looking at the input with the scope on the layout that does not work its looks like the controller is switching. This is what it looks like with a low pass filter on the VIN line (10ohm resistor and a 47uf cap). If I do not add a low pas filter on the VIN line then the charger does not even come on.
I have changed the cap size on the low pass filter from 10uf to 100uf and the problem persists however the switching wave on the VIN line becomes flatter.
10uf Cap on VIN
100uf cap on VIN
Here is a picture of the working layout. Here there is no low pass filter and only a 1uf capacitor
Microchip forums are here: https://www.microchip.com/forums...
Analogue & Interface: https://www.microchip.com/forums...
Oh im sorry if this is the wrong place.
jgmdesign 
Oh im sorry if this is the wrong place.
Not entirely.
I agree with Andy that you would do better in teh microchip forums, but theres nothing wrong with asking here, in this forum as maybe another freak has used the part and can shed some light.
I thought I used that device in a design, but upon further review I see I used the MCP73871-2CC. Not the same at all.
All teh best on your design
JIm
I don't have any experience with this charger chip, but one thing I notice between the two is the length of the traces in the input/output from the i/o connectors, especially in regards to the input trace on the second PDB, that will act as an inductor. You may want to try moving the chip closer to one or the other, or if possible, move both i/o ports closer to the chip, i.e. move the battery connector closer to the USB connector, along with the whole of the circuit.
Jim
I don't have any experience with this charger chip, but one thing I notice between the two is the length of the traces in the input/output from the i/o connectors, especially in regards to the input trace on the second PDB, that will act as an inductor. You may want to try moving the chip closer to one or the other, or if possible, move both i/o ports closer to the chip, i.e. move the battery connector closer to the USB connector, along with the whole of the circuit.
Jim
Thanks Jim. I was thinking the same however then i will need to extend my battery wires as the battery has to be on the opposite side of the PCB as the USB plug. One think I never mentioned is the PCB is 90um thick copper so its really thick. Will this possibly also contribute to this issue? I thought thicker traces and thicker copper = less resistance/impedance = better?
You could have a bad chip.
Thermistors can have a lot of accuracy variation---are you using the exact same one on testing both boards?
Make sure you don't have a polarized cap installed backwards---that could cause serious do-do (like a semi-short).
Is the TVS high enough to where it is not having any effect---it should be idle & non conducting.
Why is pin 7 not hooked up in pcb#2?
PIN7: PG, TE MCP73833: Power Good output, MCP73834: Timer Enable input
make sure you have the correct chip installed!
You could have a bad chip.
Thermistors can have a lot of accuracy variation---are you using the exact same one on testing both boards?
Make sure you don't have a polarized cap installed backwards---that could cause serious do-do (like a semi-short).
Is the TVS high enough to where it is not having any effect---it should be idle & non conducting.
Why is pin 7 not hooked up in pcb#2?
PIN7: PG, TE MCP73833: Power Good output, MCP73834: Timer Enable input
make sure you have the correct chip installed!
Thanks for your reply, I have confirmed that it's not a bad chip by reflowing 3 PCB's with all simular results.
I have made sure all my caps are connected correctly. The 1uf cap on Vin is a tantalum polarized cap and it is installed correctly.
The tvs diode is not conducting at all. I also removed it without any difference.
I did connected PG/TE pin to Vin with a 470 ohm resistor and an LED like the small layout without any difference. I also cut the trace connected to the PG/TE pin on the smaller layout and it continued to work correctly which made me conclude it cannot be the unconnected pin that's causing the problem.
I will make another Pcb with a tight layout for the charge controller. It just sucks because it costs money and time.
Do you think I need to run two ground planes connected at only one point to seperate this circuit to other circuits? I need to include a boost regulator and a LDO regulator on the same board. Can they all share one low impedence ground pour? Or should I seperate them and only connect them at one point?
I thought thicker traces and thicker copper = less resistance/impedance = better?
I would too! Another thing I notice, in the first layout, the input/output caps are placed on the input/output traces, while the second has them on out-board wings of traces.
Move the input/output caps to be on the I/O traces, rather then on rt/ang wings, this also places the gnd side of the caps on the same plane with the gnd pin of the chip, rather then looping around the other traces, and shortens the path. This is similar to the first PCB layout.
It looks like you can try this layout, out by modifying the existing PCB (scrape away the soldermask and move the existing caps ) for testing without having to spin another board.
If all else fails, it might be worth trying to connect some areas of the ground plane that got broken. Scrape some solder mask off and use solder wick or whatever is handy to fix it.
Thanks ki0bk I never even saw I did this. I quickly moved the caps as per your drawing and have the same result no change or improvement. I removed the low pass filter and it still fails to work without it.
Will do thanks for the suggestion. I'm off to bed now will have a crack at it tomorow.
Looks like to me on the second board pin 7 is not connected to anything
Could you be the victim of a crappy connector? not sure what you have, but they don't appear too stout.
Your regulator supply should have at least one high-freq ceramic cap....tantalum is so-so, but offers much better ESR than old-school electrolytics (until tants go kaboom from high inrush).
Note on the output---too low of an esr (like ceramics, tants) can cause regulator's instability, usually mentioned on a datasheet as a warning or selling feature (this wonderful reg works with ceramic)...does this datasheet mention anything?
Could you be the victim of a crappy connector? not sure what you have, but they don't appear too stout.
Your regulator supply should have at least one high-freq ceramic cap....tantalum is so-so, but offers much better ESR than old-school electrolytics (until tants go kaboom from high inrush).
Note on the output---too low of an esr (like ceramics, tants) can cause regulator's instability, usually mentioned on a datasheet as a warning or selling feature (this wonderful reg works with ceramic)...does this datasheet mention anything?
Well I did build 3 PCB's and they all did the same. I built two smaller layout and they both worked which is telling me it must be layout but I just don't get how the layout must be so tight. The data sheet says a ceramic or tantalum can be used on the output. Does not make any mension of input cap type.
Looks like to me on the second board pin 7 is not connected to anything
agree with you. on the second board pin 7 does not seem to be connected to anything.
This is similar to a previous suggestion (#11) with more detail.
Note that you have choked off your capacitor somewhat...even though it is connected to a plane, the plane connects to almost nothing, except through a VERY TINY thin strip (in gray) between the legs of the little chip. Is this strip even 100 mils wide?
Why is the big blue trace going out of its way to ruin your gnd plane???? It's as through you wanted to choke things off!!!
Add a piece of heavy bus jumper wire as shown...did that fix things up. You could try adding a 0.01uF cap to the thermistor pin--in case of noise pickup (though it seem unlikely to be a thermistor issue).
You pcb layout does not look like the example in the datasheet. Your low pass filter with a 10Ohm resistor is not going to help - no wonder it oscillates.
Are you using a QFN package? If so, it is common to have bad solder joints that look ok.
k its looks like the controller is switching
Adding on to #20, is Vin coming from at least a 2 amp USB charger (adapter*)? If not, what happens when it does?
*some screwball decided to call wall power supplies/adapters as "chargers", when they have absolutely no charging circuitry, charging monitoring, charging controls, etc. Now we are truly stuck. I just went through china to select actual chargers & ended up with boxes full of adapters called chargers...finally found a few that were actually chargers.
Adding on to #20, is Vin coming from at least a 2 amp USB charger (adapter*)? If not, what happens when it does?
Add a piece of heavy bus jumper wire as shown...did that fix things up. You could try adding a 0.01uF cap to the thermistor pin--in case of noise pickup (though it seem unlikely to be a thermistor issue).
I tried these with no luck. I think i might have to re-order boards
Are you using a QFN package? If so, it is common to have bad solder joints that look ok.
Yes i am using QFN package and ive soldered 3 boards now with the same result on all 3 so i doubt its a solder joint issue.
Yes its coming from my cellphone fast charger adapter.
What happens when you run it from a real, actual bench supply? Some fast chargers (like my samsung) have smarts in them..so they may be trying to take action (changing modes, turning off, etc) based on the loading dynamics. You want dumb-as-a-rock straight power going into your board...try a supply to see if that makes a difference..
try a supply to see if that makes a difference
I did try this when i saw the voltage on the input was 4.1V (post#3). I used my bench 5V power supply and i got the same results. My bench supply is an LM2596 set at 5V.
Yes i am using QFN package and ive soldered 3 boards now with the same result on all 3 so i doubt its a solder joint issue.
Unless you can prove it, it is certainly possible. I've been caught out by that type of thinking more times than I can count.
Unless you can prove it, it is certainly possible. I've been caught out by that type of thinking more times than I can count.
Fair enough. How can i eliminate this possibility? Reflow for longer and hotter? add more flux? I attached a picture of the joints, look pretty but that does not say much.
I use a multimeter to measure the diode junction on each pin. Might not work for bipolar parts, but works well for cmos part.
Looking again at your schematic; I see stuff like this:
What does that mean ?
It's usual to indicate component reference and value separately ((e.g. R1 15K).
I think I've worked it out. You've fitted a 1.5K resistor in that position.
Wait-a-minute: Looking at that resistor again, it's wrong:That should be a 1K
I think you've Fubar'd your PCB design by moving the component references adjacent to the wrong components. Hence you fitted wrong values to the 2nd iteration.
My bench supply is an LM2596 set at 5V.
Well that's just barely a "bench" supplY. It could be a rather weak supply, depending on the specifics. What size of output capacitors does it have? And what is powering that chip? Could be a 100ma transformer. Can it supply at least double of what you are expecting to use?
Why does it look like lettering is on your component soldering pads? That should be avoided at all cost.
Only the designator should appear on the PCB (R1, R2, R3, C1, C3, IC1, etc)
Looking again at your schematic; I see stuff like this:
What does that mean ?
It's usual to indicate component reference and value separately ((e.g. R1 15K).
I think I've worked it out. You've fitted a 1.5K resistor in that position.
Wait-a-minute: Looking at that resistor again, it's wrong:That should be a 1K
I think you've Fubar'd your PCB design by moving the component references adjacent to the wrong components. Hence you fitted wrong values to the 2nd iteration.
edit. You are right the schematic is wrong it should be 1.5k im charging a 700mAh battery. Don't want to charge it at 1A.
Well that's just barely a "bench" supplY. It could be a rather weak supply, depending on the specifics. What size of output capacitors does it have? And what is powering that chip? Could be a 100ma transformer. Can it supply at least double of what you are expecting to use?
Why does it look like lettering is on your component soldering pads?
Winterbottom was pointing out that if you accidentally move your labels around to the wrong resistor, it could cause mayhem.
Have you verified "R1" & "R2" on your schematic are the correct ones one your board (meaning the labels didn't get swappped).
Also, note you should typically be calling them R1, R2, R3...etc, unless you have something truly better to call one
The value is NOT to be part of the name. Doing so immediately voids the warranty.
Oh ok I get what you mean thanks for that Winterbottom. Will keep that in mind for future designs.
I've always directly put the resisistor value on the silkscreen and the schematics etc. It's just easier looking at the circuit and seeing the actual value instead of a reference to a value. Ive gathered this is not the traditional approach? Why is that?
In terms of manufacturing, you only really need the reference. Unless you need to put the value for a specific reason, it is otherwise just useless information. Going back to the olden days when all the lettering was done manually, it was just more work for little use. Convention is the reference and for polarised components, a means of determining the correct placement - pin 1, cathode etc be it a dot, thick line, arrow etc. For connectors this is especially useful. I also make pin one a square pad rather than a round or rounded pad.
Many modern boards don't have any references or placement information - the machines know what goes where and which way to place them and so does the vision system that checks it. There are considered unserviceable, so references aren't needed for us humans.
So the important information for us hobbyists are:
Component references
Placement hints
Connector pin1
Board number/name/revision/date
Why is that?
Say your board has twenty 333 ohm resistors eight 200K, five 4.7k, ten 49.9k resistors.
Something is wrong with the motor driver & you can maybe diagnose by looking at the voltage where its 200K & 49.9k resistors form a sensing divider. ....pick up your board....which resistors are those? Don't forget to also put the factory upgrade in place -- two 4.7K's are replaced by 7.95 K...which are those? Oh, now the label is misleading too.
I put the value or part making on the assembly drawing, which I look at while doing pick and place. The marking of many SMD parts has little to do with their part numbers, for example, the K38 (an n-ch MOSFET) and DMB (a p-ch MOSFET). I would have to look at the bill of materials (BOM) to find the part numbers.
That is one problem with SMD...the smaller sizes (ex: 0603) may not have any markings at all....so if you oops swap 10k & 100k or 0.0001 uF & 0.0022 uF you will never know (or be able to figure out whaaaaaaat happened). Especially painful if a little cup was filled with the wrong part value. I always use 3-leg diodes so it is impossible to install them backwards---a small victory.
I keep the parts in tape until starting to place, then peel some tape back and expose one or two for the [pick-up-tool]. I cut strips of tape for each board and mark (the paper strips) with the first reference (e.g., R1 is the 1k Ohm strip, R2 is the 10k Ohm strip, and so on). Loose parts go in the trash; I am not tracking that stuff unless it is an expensive IC. I sometimes salvage those and put them in a foil wrap for protection, which also identifies them for prototype use. Everything stays in the bag Digikey/Mouser sent it in. I need to wise up about my two-leg diode selection.
[pick-up-tool]: https://www.beadcorp.com/bepivato.html
Those are all good ideas for making a board, the issue arises when you encounter a board (maybe open something up, or someone gives you a bunch of board & sez ...these don't work.
That can also easily happen if a machine is loaded wrong..egads.
Maybe its time to bring back color codes ...since they can be small dots, they don't have to have much resolution--they can be very thin stripes, even on 0402 parts. charge an extra $2 per reel for marked ones.
I got my new boards today and reflowed one. It is now working. I think it was def a poor layout issue and a poor ground pour layout that was broken in more than one place as you guy had showed me. Thanks so much for all the assistance I really appreciate it. Leason learnt: Always stay as close to the data sheet recommended layout as possible and don't choke off caps. Also the numbering of parts i need to change you guys make good points.
What happened to your lettering? ---it seems extremely small, though it could be the pic. There is plenty of room--use it.
Why do some letters look like they are blurred into other letters? Don't they show up on your screen that way? Make sure all letters are positioned.
Some parts have borders drawn around them, but you placed the letters into the borders---why? Don't you want to be able to read them?
What happened to your lettering?
Ya I set the font to a smaller size, cant remember why. Will fix it before I do a production run thanks for reminding me.
Ya I set the font to a smaller size, cant remember why. Will fix it before I do a production run thanks for reminding me.
Do you look at the layout before you have it made? Not sure why you'd wait til later. Maybe it just looks good zoomed in !! One guy told me he had plenty of trace separation---surprise when the boards arrived!!
What's this DRC thing????
