jagdisk,?(Oops!) jagdish,

OK, you might have connected the pins correctly.? I am accustomed to seeing schematics drawn where the signal flow is from left-to-right, but I think you drew it somewhat the other way -- or maybe sideways.? I guess you're switching the AC power source V1 to load resistor R1, and switching it on the high side.? And I guess you do not yet have a controlling input signal, just the "200E" resistor R2 connected to its gate.

So ignore that part of my comments.

Andy

jagdish,

I did not actually look at your schematic until now.

Apparently the ACST device is some sort of passive thyristor device, right?

(If so, consider using LTspice's built-in TRIAC symbol instead of an auto-generated one.)

Where is the power source?? Normally I expect that a triac (or a triac-like device) switches a circuit that has some sort of power source and a load.? It looks like you forgot to add the power source!

Are you sure you have the pins connected correctly?? Normally a Triac's control input is the "G" pin, and the circuit being switched is connected to the A (Anode) and K (cathode) pins.? But that is not how you connected it.? I'm guessing that you have it wrong.

These two 'mistakes' could be causing your simulation problems.

I do not recommend using "E" as the units letter after the resistor values.? Usually "E" is used for scientific notation, such as "200E-3" or "200E6".? I'm guessing you wanted it to be "200E0"?? I strongly recommend removing the "E".

Andy

jagdish uploaded "ACST_Files.zip".

There are a number of problems here.

First of all, please DO NOT upload any of the .RAW or .LOG or .NET (LTspice output) files.? They are not needed.? If we have your complete schematic and models, then we can press the "Run" button ourselves, and we can see the result ourselves.? In the future, do not include those files.

Second, this is yet another model with "Questionable curly braces", followed by "Unrecognized parameter" errors.? Those errors happen because whoever made your model used the {curly braces} too liberally, unnecessarily adding them where they are not needed, and apparently confusing LTspice.? I guess this is a problem that LTspice has with its strict interpretation of the curly braces operator, which PSpice might not have.? In any event, some people who make SPICE models seem to do that, to add them unnecessarily.? It's a simple but tedious matter of editing their model to fix the unnecessary double {{curly braces}}.

The third problem is the "Time step too small" error.? Those "time step too small" errors have plagued SPICE users for half a century.? They generally happen when there is something strongly nonlinear and/or deficient inside one of the models.? Many SPICE models are badly made.? Aside from fixing the actual models (which can be much harder than it sounds), there are things you can do to alleviate and maybe eliminate that error from your simulation.? Many of them are listed in LTspice's "FAQ" file, which is here:

Files > z_yahoo > FAQ > faq_17-2.txt
/g/LTspice/files/z_yahoo/FAQ/faq_17-2.txt

Download that file, open it in a program other than Notebad, and read it.? Find the section about "time step too small errors" and start reading.? It lists several things to try.? No one solution always works, which is why there are so many.

FYI, I tried adding ".options cshunt=1e-15".? It did not work, but it lets the simulation run longer before having that error.? So it's only a start.? Read and follow the "FAQ".? With luck, you can fix this error yourself.

And FYI, those {curly brace} errors in point #2, might not actually cause anything wrong to happen.? I have fixed that problem many times, but never saw that it caused a significant difference in the waveforms.? So those warnings and "errors" might be false.? In any event, they are almost surely unrelated to the "time step too small" error.

Andy

It is possible (but maybe unlikely) that 'mliccione89' does not need this TIA to be linear.? Maybe all she/he wants to do, is to detect and observe pulses, in which case it might be OK that it is nonlinear.? If so,?then maybe it is OK to use the power supply voltages and the closed-loop gain that were used in the original schematic, where the amp is driven into saturation, and where the fact that it would oscillate doesn't matter when it's in saturation.? But if that were the case, I also want to suggest that the simulation might not be as accurate as you desire.? And maybe it's a waste of a good op-amp that is not being used as an op-amp.

Andy

On Fri, Jul 14, 2023 at 09:34 AM, eewiz wrote:

All due to the failure of one little air blaster.

Great story :)??
Arcs don't need 138kV btw - I had an automotive 6-layer PCB with just 12V (at about 1000A, car battery) that got wet, formed a cathodic short (took 6 hours), then struck an arc.? The arc then whizzed all round the board like a Pacman tornado - greatly helped by the power planes, until everything caught fire and a million pound prototype car was destroyed.?

Why only the ONE little air blaster?? ?I know it's easy to be wise after the event, but an FMEA should have picked-up the catastrophic consequences.?
It's relevant to LTSpice in that simulation is a tool of "best practise" - where good design process can eliminate future disasters, and FMEA is a similar thing.? ?

开云体育

On 14/07/2023 12:17, Tony Casey wrote:

changing the feedback resistor to 5p6 seemed to be about the optimum

...changing the feedback *capacitor* to 5p6 seemed to be about the optimum

开云体育

On 14/07/2023 12:17, Tony Casey wrote:

Next, you have defined a -2.5V supply (Vn), but used it.

Next, you have defined a -2.5V supply (Vn), but *not* used it.

This schematic does not run, as uploaded. Andy explained why (.options lines split up). The "+" character at the start of a line, tells LTspice to append this line to the previous one. When these are not within the same directive block, they will be not be associated with the intended line, and be appended to some other line that they are not supposed to be associated with.

The .options... were put in the the original fixed schematic because of issues with the opamp model used in that schematic. They should not be used as a default in others, where it isn't necessary.

You also used the "startup" option in the .TRAN directive, but there seems to be no reason why it would be needed. Only use these things where necessary and for good reason. Here, there isn't one.

Next, you have defined a -2.5V supply (Vn), but used not it. Is it, by any chance, intended to be the opamp's negative supply? If so, you can't use +5V for the positive supply, because the datasheet says in the absolute maximum ratings section:

Supply Voltage V+ to V– ...........................................5.5V

With the opamp's V- supply pin grounded, the pulsed source the input voltage falls below the inverting input's minimum level and the ESD protection diodes are forced into conduction.

I reconfigured the circuit to use ±2.5V supplies, including biassing the photodetector from -2.5V.

The photodetector model is producing 5mA pulses. You feedback resistor is 1k, so potentially the output should reach 5V, which is, of course, is beyond the supply rail. Therefore, it can't. So, assuming you need the output voltage to be a linear function of the input current, we need to reduce the feedback resistor, so the opamp isn't clipping - I reduced it to 390 for a little margin. But...

The LTC6268-10 opamp is only stable for closed loop gains in excess of 10x. That's what the "-10" suffix means. I would refer you to page 13 of the datasheet for some stability considerations. In summary, at high frequencies, the feedback gain is approximately Cin/Cfb. Your photodetector seems to have a junction capacitance of 2p, requiring a feedback capacitor of <200f. This is probably lower than the internal capacitance of the opamp. I don't know which PD you have in mind. I checked out some very high speed InGaAs PDs (infra-red for LIDAR etc) from Marktech of the sort of speed (2Gbps) you seem to be looking for. They seem to have a higher junction capacitance than 2p - more like 12p...

Anyway, without treatment this TIA oscillates. It will take a quite a bit of tweaking to make it properly stable. With your original arrangement, it appears not to oscillate, but that is misleading because most of the time it is saturated on the rails.

What exactly is your requirement? Just picking the fastest opamp you can find isn't necessarily the right approach. FYI, substituting an LTC6268 (unity gain stable version) made the TIA stable without further tweaking, but it still had some ringing - changing the feedback capacitor to 5p6 seemed to be about the optimum, but on a real circuit that might not quite be so. It isn't, of course, as fast.

开云体育

The spark plug in a spark-ignition engine has a gap of about
0.020 inches, and the voltage required to initiate a spark across this gap is
about 20,000 volts.

Hello,

I am trying to make overvoltage switch using ACST from STmicroelectronics but seems can't simulate its spice model. Any help will be appreciated. Please find all the files over here,

/g/LTspice/files/Temp/ACST_Files.zip

Regards,
jagdish

FYI -

The LTC6268-10's input voltage range just reaches the V- supply pin but does not go below it even a little.? So it's taking a risk, having the negative supply pin grounded, with the +IN pin also grounded.? In fact the voltage on the -IN pin reaches -0.66 V in the simulation, which is below the allowed input voltage range.

Andy

When you have a command such as this on a schematic:

? ??.options cshunt=1e-14
? ? + noopiter
it is essential to have all three lines in the same SPICE Directive.? But in the schematic you uploaded, the second and third lines and the first line are in separate SPICE Directives.? You can't control how the lines are ordered in the SPICE Netlist (well, actually you can, but it is not how you'd expect, it depends on the order they were added to the schematic).? As a result, the "+ noopiter" and "+ gminsteps=0" come after and add to your ".tran" line, and that doesn't work.

That causes an error, and your simulation can't be run.

Remedy: put the "+ noopiter" and "+ gminsteps=0" lines in the ".options" line's SPICE Directive.

Andy

Tom wrote, "One should never use a gas tube protector across an AC or DC line. Once they fire they will not shut off unless the voltage/current drop below the sustaining level. "

But with AC, doesn't that happen twice every cycle?? Or does the discharge tube take a few seconds to recover?

Andy

They are basically the same principle except the neon gas both lowers the trigger voltage and makes it predictable. Neon bulbs must operate within power limits while spark gap power is only limited by physical size and material.

Spark gaps are etched into PCBs all the time to provide some protection from surges. Unfortunately PCB and air spark gaps exhibit widely varying breakover voltage dependent on gap, temperature, humidity, contamination and altitude.?Spark gaps should never be placed across an AC or DC line. If the line voltage is high enough, they effectively become a short once triggered.

Spark gaps are widely used for protection. The most common is the ceramic gas tube protectors for Telecom. They come in 2 and 3 lead versions. 3 lead used for balanced lines.

In the old days, the gas could have radioactive isotope added but that is very rare today except for certain military and industrial applications. Waveguide Radar receive protectors back in the day were filled with a radioactive isotope gas and a HV priming voltage.

One should never use a gas tube protector across an AC or DC line. Once they fire they will not shut off unless the voltage/current drop below the sustaining level.?

Thanks so much for the detailed explanation!

I actually ended up switching to the LTC6268-10 and found that I'm able to actually get some semblance of a response from that opamp at my smallest pulse width. I am not trying to exactly duplicate the pulse; I am trying to detect that there is a pulse at all so I am thinking (hoping) that this is a sufficient response.

Here's the circuit?if you are interested in continuing to follow this saga. There shouldn't be any other files required except for the LTSpice circuit itself.

开云体育

The difference is gas pressure. Obviously, the spark gap has atmospheric pressure, about 100 000 Pa, but the pressure in a neon lamp is much lower: 100 Pa to 3000 Pa.

One thing I was never clear on, is the difference between a spark gaps and neon discharge lamps.? Are they the same principle?? They seem so widely different.? Spark gap discharge is very hot, leading to eventual destruction of the spark's electrodes.? Neon lamps are "cold" discharge.? Are they the same principle, just orders of magnitude apart?? Or different like night and day, which coincidentally end up with similar electrical properties?

The physics aside, it might end up making a difference for electrical modeling.? Or then again, maybe not.

Andy