mosFETs and Transient Voltage Protection (schematic Uploaded)

[eetech00]

When you push the button, it giggles like the Pillsbury Doughboy.

It's a switch system for a hobbyists machine.  3d printer, Laser, Router, etc.

Hi

Didn't mean to upset you...just wondering what its function was...
Sorry..

eT

[Falcon69]

Didn't upset me.

But I did mention it earlier in the thread.

[Falcon69]

so,

I got the boards back and assembled this circuit.  Everything works as intended, except for one thing....

The tactile (momentary) switch I am using.  If I place my finger across the contacts across the back of the pins as I press the tactile switch and release, it works as intended, on/off.  But, I take my finger off, and it is, well, variable.  Sometimes in turns off, sometimes it stays on.  In this particular circuit, the tactile switch turns on ALL the LED's in the circuit, making it easy to check to see if an LED has burned out or not.

As you can see in the circuit I uploaded, I placed a 1k resistor in series with the tactile switch, along with a 0.1uF capacitor to ground. This tactile switch and related components are located on the "front Panel LED Indication' part of the schematic.

How can I fix this problem?  Could it be as simple as changing the value of the capacitor?  If so, what value would be best?  Or should I change the value of the resistor?  Or, Maybe, place a 1M ohm resistor across the leads of the tactile switch?

I have also noticed that when power is first initially turned on, all the LED's flicker on for a fraction of a second. Can that big fixed? Maybe a slow start on without effecting the operation of the circuit?



One other thing, I noticed the voltage regulator gets very hot.  On the circuit board I had made, I only used the recommended footprint pattern for that chip.  I can touch the chip, but only for a few seconds before it starts feeling like it's burning my finger.  Is this normal for these voltage regulators to feel like that?  It's a 3A voltage regulator, with only about 1A flowing through it (what the circuit draws, and max of 2A when the tactile switch is pressed to turn on all LED's).

Thanks in advance for any and all help

Jason

[T3sl4co1l]

Well, a pulldown on the other side of the switch wouldn't hurt...

I didn't look extensively (for aforementioned reasons), but I only saw CMOS logic inputs attached to that net, nothing at all to define the logic level otherwise.

The regulator is... making 5.2V or so, and... it's about the shittiest "low dropout" LDO I've seen... never less than 0.8V drop, any current.  Gee, thanks.  So, you need over 6.5V for operation of this thing.  Plus the bother of two divider resistors.  Why not just a boring old 7805?  They make them in DPAK too.  Then you don't have to worry about pesky capacitor ESR choices either (stability plot says >0.1uF should be < 0.08 ohm ESR... have fun with that).

Anyway, it's rated to 125C, and, I guess, power limited, somehow, but they don't happen to tell us how that is achieved.  Thanks again, ST.

If you literally used only the minimal footprint, with no copper pour, you're asking for problems.  If you have copper pour (about 1 in^2 worth) around the heatsink pad (no thermal reliefs), and/or vias to a bottom side pour, you're okay for about two watts under ambient conditions.  If it's going in a box, have fun with that, too...

Was this thing going to run from a 7.0V regulated source, or something?  1A is an awful lot to expect from a linear regulator with no heatsink, let alone if the supply is the full 24V permissible.

Consumption should vary with number of LEDs lit, but I would expect with, what, 40 LEDs or so at 5mA each, you're not much over 0.2A total.  So... better go find the other thing(s) that's hot...

And if you can, scope every node to see if 1. it's sitting still when it's supposed to be (not bat shit crazy oscillating or something), and 2. make it transition (press the corresponding buttons, whatever) and see if there's bounce or overshoot or whatever.

Tim

[Falcon69]

thanks Tim,

I'm not sure I understand. I thought 7805 regulators only output 5 volts. I want to see about 5.25 volts.  The logic chips accept up to 5.5volts, and I'm trying to compensate for the voltage drop along the length of wire for the switches.

With that ST voltage regulator I am using, I can't connect that big pad to the ground plain, as the big pad is the OUTPUT to the circuit. I could enlarge the pad though, if that helps.  Could you suggest another voltage regulator that works better?

The LED's on the switches (8 of them, with 2 LED's each) put out the full 20mA each, or close to it.  They all go on when the tactile switch is pressed. I am trying to keep those LED's as bright as possible, as they will be placed on machines for visibility.

I found this circuit for the Debounce problem.  I think this should solve it?

[Falcon69]

Well, been trying to figure this out. I understand what you're talking about with the heat dissipation and only 2W with a 1² inch of copper pour.  I can;t get that with the current space I have.

I've seen these on eBay  http://www.ebay.com/itm/5V-USB-DC-7V-24V-to-5V-3A-Step-Down-Buck-KIS3R33S-Module-for-Arduino-LM2596-LU-/271666790063?pt=LH_DefaultDomain_0&hash=item3f409a3eaf

How do they do these? They advertise 7-24v input, 5 volt out at 3A.?

Here's a picture of the current board, and a picture of the newly laid out one underneath for the voltage regulator.  The bottom copper pour is about the same size as well.  With the amount of traces I have, it's just hard to find space without adding more board, which is not something I'm wanting to do.

So, based on what I did with the copper pour, will that work okay?

Oh, and to answer your question from before Tim....the circuit will most likely be powered from a 12 volt wall power supply.  But, I want to give them the option of 9v to 24 volt, as some power supplies for machines these will be used on, output 24 volts.

Also, that schematic I posted for the debounce circuit for the tactile switch, Will that work, at those values?

Tim, you had mentioned a pulldown resistor on the other side of the tactile switch.  Which side we talking about?  The circuit side, or the power side?

Thanks again!

Jason

[DutchGert]

Well, been trying to figure this out. I understand what you're talking about with the heat dissipation and only 2W with a 1² inch of copper pour.  I can;t get that with the current space I have.

I've seen these on eBay  http://www.ebay.com/itm/5V-USB-DC-7V-24V-to-5V-3A-Step-Down-Buck-KIS3R33S-Module-for-Arduino-LM2596-LU-/271666790063?pt=LH_DefaultDomain_0&hash=item3f409a3eaf

How do they do these? They advertise 7-24v input, 5 volt out at 3A.?

Here's a picture of the current board, and a picture of the newly laid out one underneath for the voltage regulator.  The bottom copper pour is about the same size as well.  With the amount of traces I have, it's just hard to find space without adding more board, which is not something I'm wanting to do.

So, based on what I did with the copper pour, will that work okay?

Oh, and to answer your question from before Tim....the circuit will most likely be powered from a 12 volt wall power supply.  But, I want to give them the option of 9v to 24 volt, as some power supplies for machines these will be used on, output 24 volts.

Also, that schematic I posted for the debounce circuit for the tactile switch, Will that work, at those values?

Tim, you had mentioned a pulldown resistor on the other side of the tactile switch.  Which side we talking about?  The circuit side, or the power side?

Thanks again!

Jason

U seem to use a lot of hatched unconnected copper on your board. In general unconnected copper is a bad idea so I would use it as extra ground plane with some via's and make it a solid plane while you are at it

[T3sl4co1l]

Those headers are too close together... good luck assembling them at all if they're just too wide, and so much for retention clips if you put this on a high vibration machine. e.g.
http://www.digikey.com/product-detail/en/3505-8110/3M15483-ND/761036

The screw terminals should be okay though; 5.08mm pitch (and some others) are available in long rows, or as stackable pieces (mind the assembly order for the dovetailed kind).

That debounce circuit is fine, but: remove the diode and drop the capacitor to 0.1uF.  Maybe raise the pullup to 1M as well.  The Schmitt trigger is optional if you're not driving clocked logic (in which case exchange VCC for GND to get the same logic states).

Switching converters with http://www.ti.com/product/LM2596/technicaldocuments or other are a good idea.  The circuit is typical, or you can get a dev kit.

Tim

[Falcon69]

The headers are actually a single one in 2x17 pins. I pull-out 6 of the pins.  I just drew it that way, because I didn't feel like redrawing an IGS file or a new pattern.

So a circuit like this is what you mean for the debounce?


As far as the regulator, I think I'm going to forget it.  Cost too much, and many more components.  I'm going to just supply a 5volt wall plug style power supply with the board.  I just don't have the space to add all those components on this board without making it MUCH larger.

I just looked on ebay, they have lm2596 chips for about 30 cents each.  I'm weary about buying IC's off eBay. If I can get that cost down, and design the boards similarly to the one i posted above, maybe it would work? I would need a footprint size of about 25 x 50cm.  I think I can manage that.  It looks like they use the whole bottom layer as a heatsink. The downside is, they've placed all their vias into the pad.  I'm not sure I could get that reflowed.

http://www.ebay.com/itm/1-DC-DC-Buck-Converter-Step-Down-Module-LM2596-Power-Supply-Output-1-23V-30V-/181409861491?pt=LH_DefaultDomain_2&hash=item2a3cdecf73

[T3sl4co1l]

Yup!

A switching converter takes less space than a linear regulator, at least if you use a high efficiency part in a usefully sized package.

Probably the only reason they offer DPAK-5s and such are because they're the old, low efficiency bipolar designs, for maintaining old designs, and new designs for ham-fisted solderers.. if that's you, sorry.

I've seen converters up to 5A in 'thermally enhanced' packages (SO-8 with pad, DFN/SON, QFN), and with operating frequencies typically around 400kHz, the inductors don't need to be large either (and often can't be, if the controller is peak current mode -- something to keep in mind).

I don't see that voltage is a big deal in this project, even with long cables on the switch thingies.  Find the minimum voltage tolerance on the furthest connection, and evaluate current flow and voltage drops all the way back to the power source (regulator / adapter).

Tim

[Falcon69]

I drew this up after reading the TI data sheet for the LM2596

If I understood it correctly, this should work if I chose to go this route?

This should allow a Delayed Startup which I hope would fix the voltage surge when the power is connected? That of which, made all the LED's blink on for a fraction of a second.

[Seekonk]

I haven't read all these pages, but your feedback should be on the output side of the inductor.  What you have drawn could be very interesting.

[Falcon69]

you are correct, I missed that on the data sheet. Fixing it now, thank you.

[Falcon69]

tim, on the debounce circuit, I was reading that putting the diode in results in the cap recharging faster.  But you had mentioned, since I had no clocked circuit, just cmos logic gates attached to the circuit, the was no reason for the inverter. By that same logic, there's no reason for the cap to recharge faster then, correct?  Just want to make sure I understand.

Also, I was reading somewhere that the switch contacts may fail prematurely if that diode is NOT in place. Can you verify?  I will need to fix that somehow. Although, that switch won't be pressed 24/7, so probably not a big deal.

[T3sl4co1l]

Diodes are for inductive contacts, doesn't matter here.

Maybe debounce doesn't matter, it's a nice-to-have in principle.  The pulldown anyway is most important.

Tim

[Falcon69]

Hey Tim,

I spent about 6 hours today looking at the schematic for problems, etc.

I found quite a number of logic chips that would be 'floating' in most conditions, i.e., switch off, or switch on, etc.

A redid the PCB and placed a 100k resistor on all those to ground.  That should solve the problem.

My question is, with those logic chips confused on what state they were in, cause a large current draw somehow that would be one of the main causes as to why that Voltage Regulator was heating up, other then lack of pcb footprint and heatsink to dissipate the heat?

It would certainly attribute to the tactile switch operating funny, I am guessing as well.

[T3sl4co1l]

Intermittent operation is more important.  It's unlikely but quite possible that current consumption increases with floating inputs, supposedly on the order of a few mA per input.  Whether all at once behave this way, seems unlikely.

Tim

[Falcon69]

Ya, I understand.

It has to be that tactile switch thingy.  I'll print up some new boards with the added fixes, and see if that works.  It should.  Other then the switch problem and the voltage regulator, everything else was working just fine.

[Falcon69]

That voltage schematic up above of the lm2596, anything I should change on the values or size of resistors?

I'm thinking I will switch the voltage regulator I am using for that one.  I don't want to take the chance of botching another circuit board.  But, I want to make sure that schematic up above is going to work.

If someone could help out with this, it would be greatly appreciated.  If Ya every come to Oregon, I owe ya a beer.

Jason

[T3sl4co1l]

Hmm, doesn't seem like anything obviously wrong or that can't be fixed with parts choice later.  The feedback capacitor is kind of odd though, you usually want to keep output ripple away from the feedback pin.  This input is usually part of a differential amplifier, which can get unbalanced by RF and therefore the voltage shifts in a weird way (dependent on supply voltage and load?).

But whatever the case, if you're following the datasheet/appnote suggested circuit and values, it should go fine.

You should learn the art of dead bug construction.  You could get all these parts, construct the circuit, and test it, alone and with your circuit, without having to order PCBs at all...

Tim

[Falcon69]

Okay, thank you Tim

The resistor values are all okay, 1/10 watt?

That 680uF capacitor, it is really large in a 35v.  Can that be reduced?  The max input to the voltage regulator would be 24volt. (probably more like 12volt realistically, but I want the option for 24volt)

[Falcon69]

hmm, I was just looking at the ONSemiconductor datasheet for that LM2596 chip.

They are using a 100uF instead of that 680uF.  That is a much more manageable size.  Can that value be used instead?

[T3sl4co1l]

Yes, but it needs to be rated for the ripple current, which is why they use an excessively large value.

I also see 120uF and 220uF suggested in the TI datasheet.

You could probably plop down 10-47uF 25V in aluminum polymer, if you're feeling fancy.  They are a little more $.

Beware that, because it's a good capacitor, it will tend to resonate with the power line inductance -- which the TVS helps with (clamps peak voltage), but the regulator input itself is negative resistance at low frequencies (current draw goes up as voltage goes down), so you want to avoid that as well.  Typical 6' twisted pair or 'zip cord' style cable is going to be a few microhenry, which would resonate with 47uF at 16kHz, and an impedance of 0.2 ohms.  Might be close enough to the regulation bandwidth to matter.  Nice thing about electrolytics, they come with ESR that dampens (100uF and under 1 ohm ESR would be fine I would think).  So does tantalum, but you don't really want to use that in a power input application (too vulnerable to peak currents, too large a value needed).

But anyway, 220uF 25V isn't big, are you really that pressed on space now?

Same idea goes for the output filter cap, except you probably don't want a low-ESR (polymer or ceramic) part there because the ESR is in the feedback loop (again, check datasheet/appnote).

A subsequent filter probably wouldn't hurt; it doesn't need to be much, maybe 1uH and 1-10uF (ceramic), just to help keep stray RF from the converter away from those long lines you've got.  The bypasses spread around the logic chips will help suppress that, too.

Tim

[Falcon69]

Okay, spent all day on it, think I got it.

Here's the pics for the finished board layout.  I was able to fit all the extra parts for the voltage regulator on there.

Here's the schematic for the voltage regulator part of circuit. 

Does everything look fine now?  I know the components are packed in there pretty tight, is that going to be a problem?

[Falcon69]

oh, wanted to add...

I am going to take off the copper hatched pour for the top side (even though I hate the plain look), but it seems everyone is saying that will hurt the performance of this PCB.  I may just get these in black solder mask in that case.