Many of the "Neon" bulbs you could buy in the old days aren't readily available anymore. You could buy blue, red, yellow, orange..etc. They are filled with different gas mixtures other than
Neon and some have a radioactive isotope added to lower the ionization voltage. One could buy bulbs screened for voltage/current ranges for use in protection and regulator circuits.
Neon bulbs are still used in AC power strips and as cheap surge protectors for signal and RF lines.?
|
The gas tubes respond in several microseconds. For AC line voltages, they will effectively be a short during each half cycle. If one doesn't have an inline fuse, both wiring and spark gap could suffer damage.
Varistors are the preferred device for use across AC lines but they have their own issues. If the surge event causes catastrophic failure of the varistor, it can catch fire and damage equipment. Varistors should have a thermal fuse in-line to avoid possible fire hazard. Three lead varistors have a built in thermal fuse.?
|
Re: .FERRET directive does not work.
I've never used ferret before, but I thought I'd try it.
My observation is the same as yours: it works in LTspiceIV and
LTspiceXVII 17.0.36, but not in 17.1.9.
This is new bug. It should be reported.
--
Regards,
Tony
On 16/07/2023 00:57, skyraider2 via
groups.io wrote:
toggle quoted message
Show quoted text
I have tried to
use the ".FERRET" directive in LTspice XVII version (X64): 17.1.9
and I get an error message saying trouble downloading file.
It works in LTspice IV.
Am I missing something or is this a bug?
* 02_sample-tran-ferret.asc
V1 Vout 0 1
.tran 10m
.ferret
.backanno
.end
For reference see
|
Re: .FERRET directive does not work.
Did you try to download more
than once? Any download may fail for no apparent reason. If
the problem persists, please report it to ADI at the email
address in the Help.
======================================================================================
Best wishes
John Woodgate OOO-Own Opinions Only
Rayleigh, Essex UK
I hear, and I forget.
I see, and I remember.
I do, and I understand.
Xunzi (340 - 245 BC)
On 2023-07-15 23:57, skyraider2 via
groups.io wrote:
toggle quoted message
Show quoted text
I have tried to use the ".FERRET" directive in LTspice XVII
version (X64): 17.1.9 and I get an error message saying trouble
downloading file.
It works in LTspice IV.
Am I missing something or is this a bug?
* 02_sample-tran-ferret.asc
V1 Vout 0 1
.tran 10m
.ferret
.backanno
.end
For reference see
|
Re: Regarding basic simulation of ACST
jagdish, I narrowed it down to these two main problems, and a possible third one: (1)? The model file st_ACST.lib that you uploaded has a few internal models that are defined in the wrong place, outside of the subcircuit that they should have been part of.? As Tony found, they used parameters that were undefined outside of the subcircuit, and that caused errors. I moved the ".ENDS" line down several lines to include the model definitions, and that fixes that problem. (2)? You made a mistake when you auto-generated your symbol.? Don't use that symbol anymore.??The library file contains several subcircuits, and the one you should have used was this one: ? ? .subckt ACST310-8FP A K G
NOT this one, which you used:
? ??.SUBCKT ACST A G K PARAMS:
That one was for an internal subcircuit.? Consequently, your symbol had the pins in the wrong order (but more on that below), and it had the wrong name, and it had a whole string of parameter definitions which should not be there at all.
But you did not need to auto-generate your symbol.? LTspice has a normal TRIAC symbol already.
However, if you use LTspice's TRIAC symbol, there is one more problem.? The symbol expects the pins to be in this order: A-G-K.? But the model for your ACST310-8FP were in this order: A-K-G.? So I edited your .lib file to change that pin order.? (For some strange reason, half of the models in the file used the A-K-G order, and others used the A-G-K order.? I fixed them all.)
I uploaded my corrected version as ACST310-8FP_AI.zip.? Use the modified .lib file.
Andy
|
.FERRET directive does not work.
I have tried to use the ".FERRET" directive in LTspice XVII version (X64): 17.1.9 and I get an error message saying trouble downloading file. It works in LTspice IV. Am I missing something or is this a bug? * 02_sample-tran-ferret.asc
V1 Vout 0 1
.tran 10m
.ferret www.analog.com/media/jp/technical-documentation/data-sheets/j1028fc.pdf
.backanno
.end
For reference see
|
Don't have time for words, but all very good things to consider.?
|
The discharge concept becomes simpler if instead of thinking about the electric field between the electrodes which is the driver for the discharge process. Of course the shape and distance between electrodes determine the electric field, but the the electrons are only driven by the electric field. Putting in the geometry at this point only confuses the issues.
Consider this, a free electron will travel along the electric field from the negative electrode to the positive electrode and gather energy in the process.
If there is neutral gas along the path, the electron can bounce off of a gas molecule while transferring some of its energy to the molecule. If the electron has an energy less than the ionization energy of the gas molecule, that is all that happens (e + i --> e+ i). If the electron has more than the ionization energy of the gas molecule, then the electron will give up some of its energy to the molecule causing an electron from the molecule to be ejected. The result of this is? e + i --> 2e + i. We then have can have an avalanche process producing huge number of electrons which will result in a high current between the electrodes.
What determines the probability of an electron colliding with a neutral molecule and ionizing it?? 1) the electron has to have energy greater than the ionization potential of the particular type of gas molecule? 2) The probability of a electron-molecule collision. This probability is very roughly the area of the molecule (cross-section) and the number density of the molecule in the gas times the path length between the electrodes. Pc ~ A x Nd x L. More commonly this is expressed as a distance = mean free path (MFP) for the electron molecule problem.? If the MFP is shorter than the distance between electrode there should be a ionizing collision. If the MFP is much smaller than the inter-electrode spacing there will be many collisions.
Now, if the energy acquired while traveling one MFP is greater than the ionization potential of the gas, then the electrons ejected from the ionized gas can, themselves can gain enough energy to ionized even more gas molecules. Anotherwords, we have self-sustaining discharge highly dependent on the inter-electrode voltage, the gas pressure and the gas type.
How do we get the first electron that we need to trigger the discharge?? It can come from a cosmic ray, a radioactive element in the chamber, a UV light source. Also, a high enough voltage across the electrodes (producing a high electric field) can cause: 1) electrons to be torn directly from the molecules or electrons can be torn away from the metal electrodes (field emission).??
This is the qualitative basics. Real world is a bit more complicated, but these concepts might give you a qualitative understanding of the principles involved. Certainly, look at the Paschens Law information.
BTW? If an electrode has a sharp point, like a needle, that geometry results if a high electric field near the point. That's how field emission electron sources are made.? If you heat the electrode hot enough, the electrons in the metal can get hot enough to be ejected from the metal; i.e., thermionic electron sources.
--
jlballe
|
Re: NTE618 varactor spice model please
|
Re: NTE618 varactor spice model please
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
Tony wrote:
.. the measured duty cycle (at the 50% points) is a non-linear function or Ton/Per, being 0.55 at Ton/Per=0.5.
This is the reason why to set a 50% actual duty cycle:
Ton = (Per - Trise - Tfall)/2
Well, not really, this is not the reason why.? You should always use Ton = (Per - Trise - Tfall)/2 if you want a 50% duty cycle, no matter whether you use your own (non-zero) rise and fall times, or if you let LTspice choose its own defaults.? As long as the actual Trise and Tfall are not zero -- which by definition they must be -- then you must account for them when choosing Ton to get any desired duty cycle. The mistake people make is thinking that "Ton" means the time that the signal is above the mid voltage.? It is not.? Ton is the time that the signal is fully at 100%, at Von.? The pulsewidth is always greater than that, because of Trise/2 and Tfall/2.? Everyone forgets that. Andy
|
NTE618 varactor spice model please
Hi,
Does anyone have a spice model for the NTE618 varactor please??
Failing that, any other high-capacitance varactor such as the MVAM108 family?
Thanks,
Chris.
|
Re: 74HCT165 Can't resolve .param vcc1=vcc
Hari K,
The Description for the file you uploaded also asks this question, "How can I add the parameters like VCC, Speed, tripdt1 in the simulation file I have added it in the symbol itself(as seen in the schematic)."
You don't need to add parameters VCC and Speed because they were already present on the symbol, until you changed them.? (By changing them you effectively removed them.)
But the parameter "tripdt1" --? Why would you want to add that parameter?? There was a parameter "tripdt" already defined.? It is there, because the model file 74HCT.lib uses that parameter.? Why would you create a new parameter, named "tripdt1", and what would you use it for?? The model (library) file wants to see a parameter named "tripdt".
If you simply place the 74HCT165 symbol on your schematic, don't change it, and add the node "VCC", and add the ".lib" command, it should just work.
Andy
|
Re: 74HCT165 Can't resolve .param vcc1=vcc
Hari K's file "wakeup.asc" is about this:
I have trying to simulate the parallel in serial out shift register 74HCT165 with the library downloaded from this group (74HCT.lib) but I can't complete the simulation as there is a warning message of " can't resolve .param vcc1=vcc is popping up while running the simulation. How can I add the parameters like VCC, Speed, tripdt1 in the simulation file I have added it in the symbol itself(as seen in the schematic). Please suggest a solution for this issue,
There are problems I see here. You forgot to include the symbol for the 74HCT165.? I found one in? 74HCT.zip, but I don't know if that is the one you used.? ALWAYS include all symbols that didn't come with LTspice.? That symbol didn't come with LTspice.? There is a chance that this wasn't the symbol you used, which is why it is essential to upload the one you used. You forgot to include the library (model) file.? I found one at? 74HCT.lib, but I don't know if that is the one you used.? ALWAYS include all models that didn't come with LTspice.? That model file didn't come with LTspice.? There is a chance that this wasn't the library file you used, which is why it is essential to upload the one you used. Your schematic is a severe "eye test".? It is very difficult to read.? Everything is so small, so far apart, with so much space between everything (which is what makes everything look so small).? Did you create this schematic yourself?? Or did you download or copy it from someone else?? It makes a difference, because you might have copied a schematic that worked when used with different symbols and models, but doesn't work with the ones I tried. The ".lib" command you used to load 74HCT.lib needs to be fixed, of course, because probably nobody else in the world has the directory "D:\Ltspice simulation\Mysimulations".? I recommend not using a fixed location (full file spec) such as that.? Instead, leave 74HCT.lib in the same directory with your schematic, then use ".lib 74HCT.lib" and it would work on anyone else's computer too. But I digress. You forgot to add a node named "VCC".? All of these 74xxxx.lib library files that Helmut Sennewald created depend on a node named "VCC" which should have the supply voltage on it.? I see that your schematic has a +5V voltage source in the lower left corner, but it's driving a node named "+5V", and there is nothing driving a node named "VCC".? I couldn't see anything else connected to the "+5V" node, so I renamed it to "VCC".? That's one problem fixed, which you would have run into eventually. Now, let's turn to the real problem. The 74HCT165.asy symbol (from the symbol file that I downloaded) has this on its SpiceLine attribute: ? ??VCC=5? SPEED=1.0? TRIPDT=1e-9 But in the symbol that is on your schematic, the SpiceLine attribute was changed to this: ? ??vcc1=5 speed1=1.0 tripdt1=1e-9 That is the problem that caused the error message you saw.? Someone (you?) has edited that attribute, on the symbol in the schematic itself, changing VCC to vcc1, and SPEED to speed1, and TRIPDT to tripdt1.? That doesn't work.? Everything is case-insensitive, so the lower-case letters don't matter; but the "1" that's been added to the end of every parameter name makes it not work. Right-click on your 74HCT165 symbol on the schematic.? Edit the SpiceLine attribute.? Remove the "1" from each of the three parameter names.? Click OK. That fixes that problem. I found other problems too. Andy
|
|
|
74HCT165 Can't resolve .param vcc1=vcc
|
74HCT165 Can't resolve .param vcc1=vcc
harikrishnan.k uploaded a file "wakeup.asc" to the Temp folder, but forgot to include the models, forgot to include the symbol, and forgot to send a message. harikrishnan.k, please go back and READ the group's main? webpage?again.? This is very important, and there is no excuse for not reading it and not following what it says.? The files you upload should be complete including ALL symbols and ALL models that did not come with LTspice.? You forgot to do that.? Also, don't just upload a file and expect anyone to help you.? When uploading a file always write a new message.? Tell us what file you uploaded, and what the question is about. Andy
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
Thanks, Tony.? Per-Ton =
Toff+Trise+Tfall.
======================================================================================
Best wishes
John Woodgate OOO-Own Opinions Only
Rayleigh, Essex UK
I hear, and I forget.
I see, and I remember.
I do, and I understand.
Xunzi (340 - 245 BC)
On 2023-07-15 14:04, Tony Casey wrote:
toggle quoted message
Show quoted text
Trise = Tfall = min(Ton/10, (Per-Ton)/10)
.. would be a more succinct way to express it. Thanks for dragging
it out of me. ?
--
Regards,
Tony
On 15/07/2023 14:57, John Woodgate
wrote:
Good, but what does 'the law is
mirrored' mean?
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
Trise = Tfall = min(Ton/10, (Per-Ton)/10)
.. would be a more succinct way to express it. Thanks for dragging
it out of me. ?
--
Regards,
Tony
On 15/07/2023 14:57, John Woodgate
wrote:
toggle quoted message
Show quoted text
Good, but what does 'the law is
mirrored' mean?
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
Good, but what does 'the law is
mirrored' mean?
======================================================================================
Best wishes
John Woodgate OOO-Own Opinions Only
Rayleigh, Essex UK
I hear, and I forget.
I see, and I remember.
I do, and I understand.
Xunzi (340 - 245 BC)
On 2023-07-15 13:52, Tony Casey wrote:
toggle quoted message
Show quoted text
I have uploaded a test
schematic that measures the actual rise and fall times of a
pulse source with default rise and fall times, i.e. both set to
zero.
The measurements show that the algorithm is:
For Ton ≤ Per/2: Trise = Tfall = Ton/10
For Ton > Per/2: the law is mirrored
I have verified this for Ton = Per/1000 to 999*Per/1000.
As a consequence of:
Toff = Per - Ton - Trise - Tfall
.. the measured duty cycle (at the 50% points) is a non-linear
function or Ton/Per, being 0.55 at Ton/Per=0.5.
This is the reason why to set a 50% actual duty cycle:
Ton = (Per - Trise - Tfall)/2
--
Regards,
Tony
On 14/07/2023 23:32, Bell, Dave
wrote:
I dug out the test case, and tried down
into femtoseconds.
Best I could get was 100fs for a setting of
100fs
?
Dave
?
?
Andy wrote:
“Remember to never set Trise or Tfall to
0.? That signals SPICE (and LTspice) to substitute non-zero
default values, and they won't be anywhere near 0.? It's a
SPICE thing.”
?
Indeed! I tried this a while back.
1ns yielded 1ns Tr and Tf
0 yielded 100us Tr and Tf
1p was too fast to zoom into, but jumping
to marked data points, I got … 1ps
?
?
Dave
|
Tony Casey
John Woodgate