Will this mosfet circuit work?

[rs20]

Oh!  Can't you just put a TVS diode in there to suck up the transient voltage?  I think TVS diodes reset once the transient is passed and circuit should operate as normal then.

This is also a good suggestion,  although whether it's actually a suitable solution depends on how strong that 60V spike is. If the power supply is happy to provide that 60V at 100A, your TVS is going to have trouble dissipating 4000W, I suggest. I'm not sure how likely this is to be an issue in practice. (Often you use a TVS along with a fuse, so that when that lightning strike hits, the fuse sacrifices itself.)

TVS diodes aren't stateful devices, so you're right that they "reset" once the transient passes. (Pedantic: But I wouldn't use the word "reset", because that implies that the TVS "triggered" or "latched" into a conducting state. They don't, TVS diodes are just fast-reacting (sometimes bi-directional) zener diodes with a particular V/I characteristic.)

[liquibyte]

I think I'm going to ditch the mosfet idea in favor of the real world circuit that redwire built and tested.  I've done a spice sim, and please don't laugh at my ignorance with it because I know almost nothing about LTSpice, and am not even sure I did the thing right.  In the real world circuit that has been built, R1 is 39K, R2 is 4.7K and there's an R3 in between R2 and C1 that's 2.2K, C1 is 47uF, and Q1 is a TIP141.  I'm not even sure that the way I have things would actually work but the real results with the different parts are not too far off from what I have here.

Edit:  forgot the output pic.

[revilo951]

fixed

What simulation program is this!?

[liquibyte]

fixed

What simulation program is this!?

http://www.falstad.com/circuit/

It's actually kind of handy too.

[rs20]

I think I'm going to ditch the mosfet idea in favor of the real world circuit that redwire built and tested.  I've done a spice sim, and please don't laugh at my ignorance with it because I know almost nothing about LTSpice, and am not even sure I did the thing right.  In the real world circuit that has been built, R1 is 39K, R2 is 4.7K and there's an R3 in between R2 and C1 that's 2.2K, C1 is 47uF, and Q1 is a TIP141.  I'm not even sure that the way I have things would actually work but the real results with the different parts are not too far off from what I have here.

Edit:  forgot the output pic.

That circuit will work fine too. The only disadvantage with using a BJT is that it will drop 0.7V (and get quite hot if your circuit consumes several amps). You can't see this in your simulation because your load is a tiny capacitor; put a resistor in there to simulate a real load. The circuit I described here will waste less power in the transistor, and will consume (theoretically) zero quiescent current because the MOSFET doesn't require bias current like the BJT does. I'll edit this post with a sim later.

[liquibyte]

I've been trying all night to get the spice simulation working on the circuit you described and I just can't get it to behave.  I've got the input spiking but no matter what I do, the gate source voltage does too and then so does the output because the mosfet is conducting.

[rs20]

Your pulse source isn't working properly. To be fair, it seems to be a bit of a bug with LTSpice maybe, since you asked for all sources to start at 0V, but your pulse source isn't doing that (EDIT: No, not a bug at all -- the startup option starts DC supplies at zero, it makes no promises about other supplies, like pulse). Hence, the capacitor is pre-charged to 18V, and the switch is on the whole time. ( Reasonably easy to methodically debug, first step was to ask "why is the FET switched on already? Why is Vgs nonzero the whole time? Shouldn't the capacitor start at zero? It's not starting at zero! Shouldn't the supply start at zero? It's not! etc" )

Use .tran 2 startup, I can't wrap my head around this logarithmic time axis thing (the left hand half of the graph is full of the random details of how LTSpice ramps up the voltage sources, it's distracting). But more importantly, change the pulse source to PULSE(0 18.3 0 35m 810m 1m). (Bolded because this is the one take-away sentence that fixes your problem ). Get rid of the top resistor, a FET doesn't require bias current. With these changes, the FET turns on after only 0.4s, since the Vgs threshold is orders of magnitude less than supply, but it's easy to tune that by making the resistor bigger. I've got it working here, but it's 1am here so I can't be bothered with screenshots right now 

[liquibyte]

I have a hard time wrapping my head around spice for some reason.  0 18.3 0 35 810 1 did the trick along with changing R1 to 180K to keep the delay until after the pulse settled.  The gate is still seeing the pulse according the the simulation though, wouldn't that be an issue that would destroy the mosfet in the real world?

[rs20]

The gate is still seeing the pulse according the the simulation though, wouldn't that be an issue that would destroy the mosfet in the real world?

You should be measuring Vgs (Vg - Vs), not Vg. (Google how to measure relative voltages). The gate could be at a million volts with respect to ground, and it would be just fine as long as the source is within 20 volts of a million volts.

[Dave]

You can plot the difference in LTspice by subtracting one function from the other: V(n00_) - V(n00_). You right-click on an existing trace name and edit the function there or hit Ctrl-A in the graph window. You can really do all sorts of weird and wonderful math.

[liquibyte]

The gate is still seeing the pulse according the the simulation though, wouldn't that be an issue that would destroy the mosfet in the real world?

You should be measuring Vgs (Vg - Vs), not Vg. (Google how to measure relative voltages). The gate could be at a million volts with respect to ground, and it would be just fine as long as the source is within 20 volts of a million volts.

I got it, thanks.  You've been really helpful the last couple of days, I appreciate you're patience.

[rs20]

You can plot the difference in LTspice by subtracting one function from the other: V(n00_) - V(n00_). You right-click on an existing trace name and edit the function there or hit Ctrl-A in the graph window. You can really do all sorts of weird and wonderful math.

Or you can just press the mouse down on the gate node of the schematic, and drag over and release on the source node. No need to manually type formulae if you just want a relative voltage.

[liquibyte]

You can plot the difference in LTspice by subtracting one function from the other: V(n00_) - V(n00_). You right-click on an existing trace name and edit the function there or hit Ctrl-A in the graph window. You can really do all sorts of weird and wonderful math.

Or you can just press the mouse down on the gate node of the schematic, and drag over and release on the source node. No need to manually type formulae if you just want a relative voltage.

That's the way I looked it up.  Other than some of the math going way over my head, I've been learning a lot using it.  This is going to be one useful program going forward.

[Dave]

Or you can just press the mouse down on the gate node of the schematic, and drag over and release on the source node. No need to manually type formulae if you just want a relative voltage.

Thanks for the tip, that does save some time.

[liquibyte]

Or you can just press the mouse down on the gate node of the schematic, and drag over and release on the source node. No need to manually type formulae if you just want a relative voltage.

Thanks for the tip, that does save some time.

I found this guide that had a few other useful tips in it along with that one.

[T3sl4co1l]

D1 is backwards relative to M1.

In the MOSFET symbol itself: you see the little triangle 'pointing at' the middle line segment?  That's the contact to the substrate.  The junction dot says it's shorted to the source terminal (part of the channel).  The substrate and channel form a PN junction.  What the triangle / arrow is telling you is, there's a PN junction here, and it conducts (conventional / hole current flow) in this direction.  In other words, the intrinsic body diode.

Every Single Symbol that shows an 'antiparallel diode' around the MOS structure is redundant: that diode is already there, people just willfully ignore it.

So please don't make the same mistake: there is never any reason to put an independent diode across a MOSFET in a simulation.  It's already present and accounted for.  Definitely don't fool yourself by accidentally putting one in backwards and hoping in vain that, by putting that diode there, you can somehow tell the circuit which way you intend current to flow!

Tim

[liquibyte]

D1 is backwards relative to M1.

In the MOSFET symbol itself: you see the little triangle 'pointing at' the middle line segment?  That's the contact to the substrate.  The junction dot says it's shorted to the source terminal (part of the channel).  The substrate and channel form a PN junction.  What the triangle / arrow is telling you is, there's a PN junction here, and it conducts (conventional / hole current flow) in this direction.  In other words, the intrinsic body diode.

Every Single Symbol that shows an 'antiparallel diode' around the MOS structure is redundant: that diode is already there, people just willfully ignore it.

So please don't make the same mistake: there is never any reason to put an independent diode across a MOSFET in a simulation.  It's already present and accounted for.  Definitely don't fool yourself by accidentally putting one in backwards and hoping in vain that, by putting that diode there, you can somehow tell the circuit which way you intend current to flow!

Tim

Thanks for the advice.  I will definitely remove it from everything I'm working with.  I think that was explicitly mentioned earlier in the thread too.  Can you tell me if I'm doing the current part of this simulation correctly?  I'm not sure how this works but the plot looks right when I do it like the following.

[T3sl4co1l]

Is V2 the PULSE and I1 a true ideal DC current source?

You don't need to put DC voltage in series with a PULSE, though you can and it doesn't hurt anything.  You can set the ON and OFF voltages to arbitrary levels, including a DC bias, so it's redundant.

What hurts is, the voltage sources DO NOT MATTER, because when SPICE says "constant current", it means constant.  You can put the ass end of the current source to any other node connected by voltage sources, and it makes no difference.  Doesn't matter if the voltage across the current source is positive or negative, large or small, current is current.

So, all that you're seeing is a capacitor charging, into a diode-strapped MOSFET (not really, but sort of), into a load resistor, basically.  It's not at all representative of a real circuit, and isn't showing you what you want it to.

Remember, SPICE doesn't know what your intent is.  (Silly and obvious, but also easily forgotten!)  It's just ideal models slapped together.  It's entirely your responsibility to make a model that's realistic.  Usually, you should be experienced enough to already know what's going to happen before you even hit 'simulate', which makes it somewhat redundant, but this should give you some perspective: unless you're doing something really "out there", you never use SPICE to determine functional performance ("does it do what I think it should", let alone "I don't know what to think"!), only to tweak the parameters and optimize the circuit to what you need.

Which... doesn't help you any, I know, because that's like saying "you're dumb, give up and read a book", and you're just trying to figure things out.  Just be very weary that, if you're trying to learn based on what SPICE gives you... it's only as good as what you're putting into it.  Nothing written in SPICE is absolute, definitely not if you're unsure about your model.

(Also... Comic Sans?  Reeeeally?... )

Philosophy aside, I think what you wanted to be going for is, a voltage source (PULSE alone, or PULSE plus DC -- or whatever, any voltage source combination is valid) with a series resistor, corresponding to either the short circuit capacity of the power source you're looking to model, or to the rated current at some voltage drop.  Two examples: a 50V 2A (nominal) supply might drop to 45V at full load, in other words, a (50 - 45) = 5V drop, which looks like 5V/2A = 2.5 ohms.  (Evidently, the short circuit current would be 50V / 2.5 ohm = 20A.)  Another example, maybe you know your supply's short circuit current is 50A, in which case 50V/50A = 1 ohm.  This is a Thevenin voltage source.

You can also do it by using a current source (PULSE, DC or whatever, any combination in parallel) in parallel with the same resistor.  This is a Norton current source.  The two are related by having the same resistor (one series, the other parallel), and I = V/R relating the two sources.  Don't mind that the current source appears to be delivering short-circuit power into its resistor: that's virtual watts, you're just using that for its behavior at the terminals.

Tim

[liquibyte]

I'm going to do more studying and come back to this as it relates to what I'm trying to accomplish.  I've read about trying to model real world results and how much of a pain it is to do in spice and ultimately futile to boot but I think it is helping me understand a few things regardless.  I'll try my best to figure out how to set things up with as accurate a model as can be done just for the practice I suppose.  Either way, I do appreciate the help.  I like to read your posts even if I don't always understand everything in them because, no matter what, I always come away with something new learned and that's always a good thing.

As for the font, it was set at Arial but I'm running this through wine so I guess I don't have my fonts set up right there.  I tried changing it to Courier, Times, and Verdana but it stayed the same regardless.  Finally I tried Tahoma and that I guess I have set up right, so from now on I promise not to post crappy fonts if I can help it. To be honest, I don't think I have Comic Sans installed so I have no idea how it was rendering that way.

[T3sl4co1l]

Thanks

Weird... actually on closer inspection, it looks like the graph is labeled with something normal like MS Sans, and the .TRAN label is some normal, kinda tilted sans, I don't remember which.  But the schematic labels are all kinds of goofy, not Comic come to think of it, but something just as random.  Go figure!

Tim

[liquibyte]

Thanks

Weird... actually on closer inspection, it looks like the graph is labeled with something normal like MS Sans, and the .TRAN label is some normal, kinda tilted sans, I don't remember which.  But the schematic labels are all kinds of goofy, not Comic come to think of it, but something just as random.  Go figure!

Tim

I have no idea why it's so wonky but at least one of the options worked right.  I could swear I had MS fonts installed but it turns out I didn't.  I do now so that's not going to happen again.  I should see if I can move my DejaVu fonts over and have them picked up by the program because I like the way they look.

I started reading and then found things like this that is probably going to make my head hurt.  I don't want to turn into a voltnut, or spicenut if you will, but my OCD is liable to take over at some point and I'm going to have to model a mosfet or an op amp for the fun of it.  At this point I'm just glad I got the theoretical working.  I'll have to see if I can find a PFET to try the circuit out and if it works I'll be one happy camper.  The problems I've had with this power supply would probably have made most people quit or at least move on to something else but it's helping my learning experience so I'd say it can't be all bad.  I'm determined to fix it or, if it can't be, at least learn enough as to why and then just design something new.

[rs20]

D1 is backwards relative to M1.

No it's not, it's a PFET and in a PFET the diode arrow points towards the Source. (Assuming you're talking about the diagram in #30? Or did someone go back and retroactively change a diagram?). I agree that the diode need not be explicitly added to the diagram though, of course. I believe the original circuit in #30, without the current source added, is a reasonable model (modulo the unnecessary but harmless body diode)?

You don't need to put DC voltage in series with a PULSE, though you can and it doesn't hurt anything.  You can set the ON and OFF voltages to arbitrary levels, including a DC bias, so it's redundant.

In this case, he wants the voltage to start at 0 (which, AFAICT, is not enforced by using ".tran xxx startup"), then rise to a high value, then fall to a stable nominal voltage. Since the pulse settings only have 2 voltage values available, it can't be done with a single pulse source. His solution, a pulse atop a DC source (that respects startup) is a bit hacky, but its as good as any other method I can think of.

[liquibyte]

D1 is backwards relative to M1.

No it's not, it's a PFET and in a PFET the diode arrow points towards the Source. (Assuming you're talking about the diagram in #30? Or did someone go back and retroactively change a diagram?). I agree that the diode need not be explicitly added to the diagram though, of course. I believe the original circuit in #30, without the current source added, is a reasonable model (modulo the unnecessary but harmless body diode)?

I haven't gone back and changed any of them, I promise.

You don't need to put DC voltage in series with a PULSE, though you can and it doesn't hurt anything.  You can set the ON and OFF voltages to arbitrary levels, including a DC bias, so it's redundant.

In this case, he wants the voltage to start at 0 (which, AFAICT, is not enforced by using ".tran xxx startup"), then rise to a high value, then fall to a stable nominal voltage. Since the pulse settings only have 2 voltage values available, it can't be done with a single pulse source. His solution, a pulse atop a DC source (that respects startup) is a bit hacky, but its as good as any other method I can think of.

That's exactly what I was after.  I wanted a spike that lasted for ~300ms or so and then went away allowing a final steady voltage of 43.7V which is what I measure after rectification and filtering.  I needed to be able to tune the resistor and cap value based on where that pulse ended.  I'm still not done simulating because I want to, as Tim said, get the models as accurate as possible as a learning exercise.  Is there a better way to simulate a transient surge that I may not be aware of?  Leaving the accuracy of the part models aside, I need to be able to simulate to 30V @ 3A with a startup transient of around 64V.  I haven't measured the effect on the current but, to be honest, I don't think I have the right equipment for that.  I only own one multimeter and it's not all that great but seems accurate enough as kind of verified by my latest acquisition of a 465B.  The bad part about all this is that I can't really see the transient with the scope with any accuracy because it's happening to fast and I can't store it.

One thing I've noticed is that after I added the current with a better load to the simulation, the spike doesn't behave as it did before.  I still get a spike but it's not rising up to the 64V I wanted, it's only topping out at 44V.  I think it may be because the load I have on it is R=limit(10,V(n002)**2/90,10).  I'm still new to this so I'm absolutely sure I'm doing it wrong.

Quick edit:  I've also tried R=limit(14.56667,V(n001)**2/131.1,14.56667) which seems to give better results as far as stability goes but adding the 18V on top of 43.7V isn't doing what I would expect.  I have to explicitly state 64V in V2 now.

[T3sl4co1l]

D1 is backwards relative to M1.

No it's not, it's a PFET and in a PFET the diode arrow points towards the Source. (Assuming you're talking about the diagram in #30? Or did someone go back and retroactively change a diagram?).

Hmm, thought I was looking at #30.  Perhaps I was a bit hasty, it does look the right way around!

I agree that the diode need not be explicitly added to the diagram though, of course. I believe the original circuit in #30, without the current source added, is a reasonable model (modulo the unnecessary but harmless body diode)?

I'd say, with the current source replaced with a suitably chosen resistor.  That'll be more representative of a typical power source.

In this case, he wants the voltage to start at 0 (which, AFAICT, is not enforced by using ".tran xxx startup"), then rise to a high value, then fall to a stable nominal voltage. Since the pulse settings only have 2 voltage values available, it can't be done with a single pulse source. His solution, a pulse atop a DC source (that respects startup) is a bit hacky, but its as good as any other method I can think of.

Yeah, PULSE has four states in order: initial, slope, final, slope, <repeats>.  You need more than one source if you need more than two static states, and an overshoot pulse requires three.  You could also do a PWL source (a table of points and times describes the voltage), or build one yourself out of discretes (which has the advantage of potentially being representative of what's actually making the pulse in the first place, and the disadvantage of being hard / tricky / tedious to design and calculate the parameters of).

Tim

[T3sl4co1l]

That's exactly what I was after.  I wanted a spike that lasted for ~300ms or so and then went away allowing a final steady voltage of 43.7V which is what I measure after rectification and filtering.  I needed to be able to tune the resistor and cap value based on where that pulse ended.  I'm still not done simulating because I want to, as Tim said, get the models as accurate as possible as a learning exercise.  Is there a better way to simulate a transient surge that I may not be aware of?

What is this, actually?  A load dump or something..??

What are the characteristics of this pulse?

One thing I've noticed is that after I added the current with a better load to the simulation, the spike doesn't behave as it did before.  I still get a spike but it's not rising up to the 64V I wanted, it's only topping out at 44V.  I think it may be because the load I have on it is R=limit(10,V(n002)**2/90,10).  I'm still new to this so I'm absolutely sure I'm doing it wrong.

Quick edit:  I've also tried R=limit(14.56667,V(n001)**2/131.1,14.56667) which seems to give better results as far as stability goes but adding the 18V on top of 43.7V isn't doing what I would expect.  I have to explicitly state 64V in V2 now.

Like I said, because your source is entirely constant current, the response is dominated by the bulk capacitors and load resistor, and the VPULSE does nothing at all.

Tim