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
|
Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 10:12 AM, Say Die. wrote:
I have uploaded the file also i have notified you guys.
I will fill in the information you forgot to say.
?
The files you uploaded are "FinFETbasedSRAM - 20nm.asc" and "FinFETbasedSRAM.asc".? They are now in the "Temp" folder.? You forgot to put them there, so I fixed that for you.
?
But it is not complete!? You forgot to upload the PTM (model) files.? Without those, your simulations would be useless.? One of your schematics uses early 1970 MOSFETs, which surely are wrong for 20 nm devices.? You gave them ginormous dimensions of 0.18 meters (180000000 nm) by 0.32 meters (120000000 nm), which will be extraordinarily difficult to manufacture.
?
The schematics attempt to load a model file named "180nm_whole.model" but you neglected to upload that, so we can't see where the problem is with your models.? Wasn't that the whole point of this question?
?
I also want to note that you drew your PMOS transistors upside-down.? The Source pin is the one next to the pin for the Gate, and that should be UP (towards the more positive voltage) for your PMOS transistors, not down like you drew them.? You should rotate those symbols twice to get them oriented correctly with Source UP and Drain DOWN.? It might not make a difference (since many MOSFETs are symmetrical), but don't count on it.
?
One of your schematics has a capacitor value of "1micro".? That will give you a 1000 uF capacitance value, because "micro" begins with "m" which is the SPICE multiplier for "milli".
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
Yes, but you uploaded two files instead of a
.ZIP, and didn't upload the model files in it. I looked at your
120nm .ASC. I'm not an expert in IC design, but it looks as
though it might work. But your.TRAN directive is wrong, although
LTspice interprets it sensibly. It should just be .TRAN 120n,
unless you also wanted to set a 1ns maximum time-step, in which
case it should be .TRAN 120n 1n.
On 2025-04-04 15:12, Say Die. via
groups.io wrote:
I have uploaded the file also i have notified you guys.
?
--
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
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.
?
|
Re: 20nm PTM file not working in LTspice
On Fri, Apr 4, 2025 at 10:12 AM, Say Die. wrote:
I have uploaded the file also i have notified you guys.
But you did not read and follow what John Woodgate wrote!? Neither did you follow the instructions on the group's main webpage!
?
Shame on you for not even trying.
?
Andy
?
|
Re: 20nm PTM file not working in LTspice
There is a special very hot place reserved for
supervisors who set students problems that the supervisor
doesn't know how to solve.?
You might do better to use LTspice, but work
only with the .ASC and models you can find in the group's
archives (the folders with names beginning with 'z...' on the
Files page), together with advice from Andy and others. Or, if
you know, or you supervisor will tell you, which foundry would
make the device you design, you can ask the foundry for 20nm
models.
We can't help with Hspice or any other version
of SPICE.
On 2025-04-04 15:03, Say Die. via
groups.io wrote:
I am just a student and half of the things you said went
bouncer T-T. My HoD told me to make this project because i
attended Semi-conductor training program in SVNIT SURAT. Even he
don't know how to build this circuit and he want me to build and
i am ready ofc, because i love vlsi and designing, but if i know
nothing about it how should i do that. not giving excuses tbh. i
def want to learn that's why i came here. i'll try to send the
file?
?
--
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 10:03 AM, Say Die. wrote:
I am just a student and half of the things you said went bouncer T-T. My HoD told me to make this project because i attended Semi-conductor training program in SVNIT SURAT. Even he don't know how to build this circuit and he want me to build and i am ready ofc, because i love vlsi and designing, but if i know nothing about it how should i do that. not giving excuses tbh. i def want to learn that's why i came here. i'll try to send the file?
OK, here is the dumbed-down version of what I wrote:
?
Your model files ("PTM" files) will not work in LTspice.
?
Don't try.? Get the right model files for 20 nm and for the SPICE simulator you intend to use.? If they are LEVEL=72 models, LTspice is not an appropriate simulator because LTspice does not accept LEVEL=72 models.
?
I understand you might be a newbie who is trying to design and simulate circuits about which you know almost nothing.? So I advise you to learn everything you can about MOS circuit design, process scaling, and circuit simulation.? ?There is much that you need to learn.? Anyone can tell you to "go for it", but that might be bad advice especially if both he and you don't know what you are doing, and could get you into a boatload of trouble.
?
If the only models you have are LEVEL=72 models, use the right program with them (HSPICE) and don't try using LTspice with those models.
?
If the only models you have were made for the older 180 nm process, I urge using EXTREME CAUTION with them in an attempt to represent the 20 nm process.? That is not how CMOS scaling works!? There will be different process (PTM) models for each step along the way from 180 nm down to 20 nm, and the 180 nm process files would be wrong for simulating anything designed and built for 20 nm devices.? Anyone who builds those parts (what we call the "FAB") can get you the right model files for the 20 nm process.? Now maybe that is what they did already.? ?Scaling down from 180 nm to 20 nm requires both changing the sizes of the transistors (which is usually specified on the schematics), and changing the SPICE model files; both steps need to be done.? I want to make sure you understand that.
?
By the way, please go easy on the abbreviations.? Not everyone understands all the acronyms you used.
?
Andy
?
?
|
Re: 20nm PTM file not working in LTspice
I have uploaded the file also i have notified you guys.
?
|
John Woodgate