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
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
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:
toggle quoted message
Show quoted text
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
|
Hello All
Bonkers wrote:
Why only the ONE little air blaster?
Forgive me, I took a bit of dramatic license. That plant was completed in 1954 and I would assume that there were FMEA analyses performed on commercial switch gear of that era. I agree that it probably was (should have been) a redundant air blast system.
But wow, what a spectacular failure.
All for now
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
Dave,
If you're talking about risetime, it can be quite a lot smaller than 100 fs.? I would say arbitrarily small, but eventually you reach the limits of double precision math.? Remember not to let LTspice's waveform compression get in the way.? And there are limits of how far you can zoom in, but even that can be overcome if you know how.? And if you don't, there's waveform cursors.
Andy
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
I dug out the test case, and tried down into femtoseconds.
Best I could get was 100fs for a setting of 100fs
?
Dave
?
toggle quoted message
Show quoted text
From: [email protected] < [email protected]> On Behalf Of
Bell, Dave (US)
Sent: Friday, July 14, 2023 1:06 PM
To: [email protected]
Subject: EXTERNAL: Re: [LTspice] ISL70444SEH declaration issue?
?
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
?
|
Re: PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
SPICE used "0" to tell it to apply a default value.? It is most apparent with Trise and Tfall, but it works in a number of other places too.? Typing 0 can even mean "infinity" in a couple of places, where that is the default.
If you use 0 for Trise or Tfall, SPICE calculates default rise and fall times as a function of other things, including the Stop Time of the simulation.? The default rise or fall time usually looks "small enough" when looking at the entire waveform, but not when you zoom in.
Andy
|
PULSE default rise and fall times (Trise=0 Tfall=0) (was: ISL70444SEH declaration issue?)
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
?
|
Re: ISL70444SEH declaration issue?
Handling a pulse that is only 0.7 ns wide is certainly a challenge.? For SPICE simulations, if you were to use 1 ns rise and fall times, and if you say that the desired pulsewidth is 0.7 ns at the pulse's 50% point (which is likely how it is specified), then you need to subtract 1 ns from the intended pulsewidth, to come up with the "on" time ("Ton") of your SPICE current pulse source.? Obviously that doesn't work for a 0.7 ns pulsewidth!? So you must decrease the Trise and Tfall times of your PULSE source in SPICE.? For example:
I1 N001 N002 PULSE(0 5mA 1us .0.5n .0.5n 0.2n 15u 20)
would give you 20 pulses that are 0.7 ns wide at 50% = 2.5 mA.
Just be aware that Ton is the time AT 100% of the pulse amplitude, so mentally add half the rise and fall times to get the effective pulsewidth at 50%.? Conversely, subtract half of (Trise+Tfall) from the desired pulsewidth, to get Ton for SPICE.
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.
Andy
|
Re: ISL70444SEH declaration issue?
Hi guys- Thanks a ton for your continued support. Tony posed the question about what my requirements really are. Here are the most relevant:
- Overall, my goal is to have enough of a response so that I can detect when a pulse is missing, potentially by way of a comparator down the line. The pulse widths can range between 0.7ns wide and ~4ns wide and occur about every 15us.
- In my system I will have access to +/-5V supplies. I'm going to go back to looking for an op amp that can utilize these supplies.
- The photodetector will be biased at -5V to minimize junction capacitance.
A quick note, I do have a real photodetector identified with the properties I've entered into the simulation. You are correct to assume that it's an InGaAs detector. As far as your comment about picking the fastest opamp and hoping for the best, I guess I am having a hard time grasping what the right approach is to selecting an opamp for this case. I hope the above helps.
|
Re: LTC1922/LTC3722 model and simulation
For some reason, the examples\jigs folder has been redesignated as
examples\Applications in LTspice 17.1.x.
On 14/07/2023 17:02, Udo
Huhn-Rohrbacher via groups.io wrote:
LTspice offers
example circuits under > examples \jigs\1922-1 ,as well as for
the 3722-1.
--
Regards,
Tony
|
Re: LTC1922/LTC3722 model and simulation
Thanks, Udo?
I have found the example , look to work OK ,?
|
Re: LTC1922/LTC3722 model and simulation
R Clark,
As Udo wrote, LTspice has examples in .ASC for those parts, and for almost every part made by Linear Technology and Analog Devices.? You already have those example schematics on your computer's drive.? An easy way to find those example circuits is this:? Starting with your schematic that has one of those parts, right-click on the LTC1922-1 or LTC3722 symbol that is on your schematic, and choose "Open this macromodel's test fixture."? Now you have that example schematic open in LTspice, and you can run it and plot the results.?
When you wrote, "Phase shift is not working? / I must miss something,"? what was the phase shift?? If something is not working in your simulation, please consider uploading YOUR schematic to the group's "Temp" folder, as John recommends.? It should be the actual schematic .ASC file (NOT a picture of it), and it should include all symbols (.ASY files) and their models for anything that did not come with LTspice, but nothing else.
Andy
|
Tony Casey
John Woodgate
eewiz
Bell, Dave