Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 11:34 AM, John Woodgate wrote:
I understand, but LTspice Help doesn't even mention the possibility of a print step parameter.
It does, but it is easily missed:
Syntax:?.TRAN <Tstep> <Tstop> [Tstart [dTmax]] [modifiers]
????????.TRAN <Tstop> [modifiers]
The first form is the traditional .tran SPICE command. Tstep is the plotting increment for the waveforms but is also used as an initial step-size guess. LTspice uses waveform compression, so this parameter is of little value and can be omitted or set to zero.
?
In the Simulation Command editor, it labels it "Tprint" rather than "Tstep".? It is the same thing.
?
I had forgotten that LTspice can use that parameter as a first-guess for the internal Timestep.
?
IMO, it is not because of waveform compression that LTspice otherwise does not use Tprint or Tstep.? It's because that parameter was the step size for the line-printer output, which LTspice does not do.
?
Andy
?
|
Re: Simulation runs very slowly: test.asc
it's mostly the Ti?s LDO causing spurious fuzz at startup and later attempting to hang the spice engine . . .
?
? ideal shared/common/not-uncoupled supply
?
ADi?s Op Amp looks mostly ok
?
? what is that you attempt to adjust with Op Amp ?
|
Re: 20nm PTM file not working in LTspice
I notice that the 20 nm model file specifies:
+lmin ? ?= 1e-008 ? ? ? ? ?lmax ? ?= 2.4e-008 ? ? ?
?
This tells me that the model does use MKS dimensions, and your MOSFET sizes must be specified in units of meters, not microns.? To make that work, you would need to edit every MOSFET symbol on the schematic and change the L and W and PD and PS values from microns to meters.
L=0.18 --> WRONG
L=0.18u --> OK
?
You would need to do that in any simulator.
?
The same is most likely true of the 180 nm models too.? Although it does not have LMIN and LMAX parameters, the default dimensions are most likely Meters, not Microns, because SPICE's standard is Meters.? If you simulated it with values like 0.18, it would have simulated incorrectly.
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 11:25 AM, Say Die. wrote:
I just gave you the basic idea so you can find it easily. ?
"Basic idea" is not enough.? If you did that with LTspice, it would give you an error.? Filenames have extensions, and the extension must be included.
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
Say Die,
?
Your 180 nm model file, "180nm_whole.model", can be used in LTspice, because it uses LEVEL=49 models.? The names of the MOSFETs on your schematic must be "CMOSN" and "CMOSP".
?
However, the 20 nm model file "20nmFinFET.model" is NOT OK because that one is HSPICE-only.? Do not try using it in LTspice.? Do not seek a way to convert them from LEVEL=72 to something else.? There is not a way to do that.
?
If you used that model, please note these two things:
- The names of the MOSFETs on your schematic must be "NFET" and "PFET".
- It says it is designed for a nominal VDD = 0.9 V, not 1.8 V.
?
If your schematic has MOSFET names of "NMOS" and "PMOS", you get the early-1970s models which were designed for MOSFETs that had not reached even the 1 micron size.? Definitely not for 20 nm.? More like 20 um = 20000 nm.
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
We like everything to be precise. That
prevents mistakes, as far as possible.
On 2025-04-04 16:24, Say Die. via
groups.io wrote:
I just gave you the basic idea so you can find it
easily. ?
On Fri, Apr 4, 2025 at 11:05 AM, Say Die. wrote:
Uploaded in temp the name would be - 180nm_whole and
20nmFinFET
Actually, no, that is not their filenames.
?
The actual filenames are "20nmFinFET.model" and
"180nm_whole.model".
?
Andy
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
Re: 20nm PTM file not working in LTspice
I understand, but LTspice Help doesn't even
mention the possibility of a print step parameter. No matter,
there are much bigger issues to settle.
On 2025-04-04 16:18, Andy I via
groups.io wrote:
On Fri, Apr 4, 2025 at 11:02 AM, John Woodgate wrote:
Andy, the .TRAN statement
is .TRAN 1ns 120ns. Probably meant to be .TRAN 120ns 1ns,
where the 'superfluous 's'? is indeed accepted.
No, ".TRAN 1ns 120ns" is correct too.
?
When there is more than one parameter, the first parameter is
the print step size.? LTspice ignores it when it is there,
because LTspice never prints character-based "waveforms" to its
output file.? That is old-school SPICE, printing crude waveforms
in the output file.
?
When there is more than one parameter (and only then), the
second parameter is the Stop Time.? ".TRAN 1ns 120ns" is
identical to ".TRAN 0 120n".? Either one is correct.
?
Andy
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
Re: 20nm PTM file not working in LTspice
I just gave you the basic idea so you can find it easily. ?
On Fri, Apr 4, 2025 at 11:05 AM, Say Die. wrote:
Uploaded in temp the name would be - 180nm_whole and 20nmFinFET
Actually, no, that is not their filenames.
?
The actual filenames are "20nmFinFET.model" and "180nm_whole.model".
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 11:05 AM, Say Die. wrote:
Uploaded in temp the name would be - 180nm_whole and 20nmFinFET
Actually, no, that is not their filenames.
?
The actual filenames are "20nmFinFET.model" and "180nm_whole.model".
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 11:02 AM, John Woodgate wrote:
Andy, the .TRAN statement is .TRAN 1ns 120ns. Probably meant to be .TRAN 120ns 1ns, where the 'superfluous 's'? is indeed accepted.
No, ".TRAN 1ns 120ns" is correct too.
?
When there is more than one parameter, the first parameter is the print step size.? LTspice ignores it when it is there, because LTspice never prints character-based "waveforms" to its output file.? That is old-school SPICE, printing crude waveforms in the output file.
?
When there is more than one parameter (and only then), the second parameter is the Stop Time.? ".TRAN 1ns 120ns" is identical to ".TRAN 0 120n" and to ".TRAN 120n".? Either one is correct.
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 10:57 AM, Say Die. wrote:
Absolutely. i am uploading it in temp
Make sure to let us know when you have done that, and tell us the name of the file.
?
Here is more advice about your schematics:
?
(1)? Nodes (nets) can have only one nodename.? In LTspice, a "Label" is a nodename.? Your schematic mistakenly gives several nodenames (Labels) to the same nets.
?
Net "Q" is also labeled "a" and "y2".? Net "Qbar" is also labeled "y" and "b".? That is unwise, and may lead to problems.
?
Fortunately, LTspice can USUALLY figure it out and make the adjustments for that.? But not always.? You should never do that if you can help it.
?
If you want to add schematic identifiers on the schematic, do that using Comments ("Text"), not Labels.? Every net should have no more than one nodename attached to it.
?
(2)? "PULSE(0 1.2V 0 1n 1n 10n 20n)" is not a symmetrical square wave.? This mistake happens with most new users.? If you wanted that waveform to be a symmetrical 50/50 signal (50% high, 50% low), you need to account for the rise and fall times.? "Ton" is the time that the waveform is at 100%, not the time that it is >50%.? Your waveform is "high" (>50%) for 11 ns and "low" (<50%) for 9 ns.? To make it symmetrical, you need to adjust the "Ton" parameter by subtracting (Trise+Tfall)/2.
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
Uploaded in temp the name would be - 180nm_whole and 20nmFinFET
|
Re: 20nm PTM file not working in LTspice
Andy, the .TRAN statement is .TRAN 1ns 120ns.
Probably meant to be .TRAN 120ns 1ns, where the 'superfluous
's'? is indeed accepted.
On 2025-04-04 15:51, Andy I via
groups.io wrote:
On Fri, Apr 4, 2025 at 10:37 AM, John Woodgate wrote:
.... But your.TRAN
directive is wrong, ...
It is actually OK.? Nothing wrong with writing "120ns".
?
Some would prefer to omit any letter after the first one.?
But SPICE was created in such a way that you can write "nV" or
"nanovolts" or "nanoseconds" or whatever.? It was designed to
ignore all characters after the first letter (except for "MEG"
and "MIL").? Purists like to tell you not to do that, but there
is nothing wrong with it.? It is indeed "safer" to use only one
letter but not necessary as long as you avoid accidentally
writing "MEG" and "MIL" when they are not what you meant.
?
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
Re: 20nm PTM file not working in LTspice
Absolutely. i am uploading it in temp
?
|
Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 10:33 AM, Say Die. wrote:
... About My Project I am not really familiar with HSPICE and the model file is designed for that APP.
Open the HSPICE manuals and read.? It's several hundred pages.
And I also don't know how to change the level that suits LTspice.
You can't.? You should not try.? There is no established way to get from one level to another level.
?
You need to start with the correctly written models, not "fudge" them by arbitrarily changing numbers.
?
Well, OK, you could just change the LEVEL number, but that would be VERY UNWISE.? Please do not do that.? If i were your employer, I would give you the boot if you did that.
?
What I am telling you is that you should not use LTspice with these LEVEL=72 models.? Don't even try.? I thought I made that clear already, but here it is again:? Don't use LTspice with LEVEL=72 models.? If those are the only model files you have, then don't use them with LTspice.
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 10:45 AM, Say Die. wrote:
?should I Upload Model files??
Well, that depends on you.? Do you want actual answers to your questions?
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
Not now, since Andy has said that they won't
work in LTspice. Instead, first try to find 120nm models that
will work in LTspice. Then, if your 120nm circuit works, try to
find 20nm models that work in LTspice. That is the best route to
success.
On 2025-04-04 15:45, Say Die. via
groups.io wrote:
?should I Upload Model files??
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 10:37 AM, John Woodgate wrote:
.... But your.TRAN directive is wrong, ...
It is actually OK.? Nothing wrong with writing "120ns".
?
Some would prefer to omit any letter after the first one.? But SPICE was created in such a way that you can write "nV" or "nanovolts" or "nanoseconds" or whatever.? It was designed to ignore all characters after the first letter (except for "MEG" and "MIL").? Purists like to tell you not to do that, but there is nothing wrong with it.? It is indeed "safer" to use only one letter but not necessary as long as you avoid accidentally writing "MEG" and "MIL" when they are not what you meant.
?
?
|
Re: 20nm PTM file not working in LTspice
?should I Upload Model files??
?
|
Re: 20nm PTM file not working in LTspice
I've explained what I suggest you do. Do you
actually have access to Hspice? If not, forget it and try to use
LTspice, unless you can't find 120nm and 20nm models by any
means.
On 2025-04-04 15:33, Say Die. via
groups.io wrote:
Apologies. It's a bad habit of mine not read instructions
before acting. What should I do now? About My Project I am not
really familiar with HSPICE and the model file is designed for
that APP. And I also don't know how to change the level that
suits LTspice.
?
--
OOO - Own Opinions only
If something is true:
* as far as we know - it's science
*for certain - it's mathematics
*unquestionably - it's religion
|
Rene
John Woodgate