LTspice for IC vs other software, TSMC180nm process pramaters

Hi all,
I am simulating a switched-capacitor circuit on LTspice. My ultimate goal is to layout and fabricate the circuit. what is your recommendation regarding the software? I got lots of advice some they recommend LTspice for any level of circuit simulation and some they said maybe only good for power supply stuff. I am seeking your input in this regards?

second, I am also using TSMC180nm prcoess in the simulation, file attached. I want to calculate the body effect through the fermi potential and Lambda but it is present in the txt file I have, I found in the literature they assume FermiPotential (PHI) =0.35 (i.e 2*PHI=0.7)

LTSpice is pretty good free alternative for simulations, but it doesn't have tools that would make your life easier like a library manager. Also it doesn't scale as well as spectre, meaning large simulations may take longer. It's good for pretty much anything and is pretty accurate. You can follow this document (which is written by LT so it's a bit one sided but still explains a few mechanics of the simulator) http://cds.linear.com/docs/en/lt-journal/LTJournal-V24N4-01-df-SPICEDifferentiation-MikeEngelhardt.pdf

But if your ultimate goal is fabrication then you'd need a good layout editor, but good ones are not available for free. And more importantly layout will be given to the fab, so it also depends on the requirements of the fab. For example some fabs may provide you with everything for calibre but not anything else (good fabs usually provide everything, but especially if you're getting this service through a third party [multi project wafer companies] they may not provide all the rulesets for all the tools). So you may not be able to choose which tools you're going to use.

In short, LTSpice is awesome for simulation, but there's a lot more to consider if you want to fabricate. And to be honest if you're in a university just ask around if you have access to Cadence tools. It's a complete suite so it'd cover everything you need, and Cadence distributes its software liberally to universities.

bio_man said:

Hi all,
I am simulating a switched-capacitor circuit on LTspice. My ultimate goal is to layout and fabricate the circuit. what is your recommendation regarding the software? I got lots of advice some they recommend LTspice for any level of circuit simulation and some they said maybe only good for power supply stuff. I am seeking your input in this regards?

second, I am also using TSMC180nm prcoess in the simulation, file attached. I want to calculate the body effect through the fermi potential and Lambda but it is present in the txt file I have, I found in the literature they assume FermiPotential (PHI) =0.35 (i.e 2*PHI=0.7)

Click to expand...

This looks like a TSMC proprietary file, no? You should not disclose it.

ThisIsNotSam said:

This looks like a TSMC proprietary file, no? You should not disclose it.

Click to expand...

I found it using google, anyways I tried to modify my post and delete the file but couldn't, can you help?

- - - Updated - - -

kemiyun said:

LTSpice is pretty good free alternative for simulations, but it doesn't have tools that would make your life easier like a library manager. Also it doesn't scale as well as spectre, meaning large simulations may take longer. It's good for pretty much anything and is pretty accurate. You can follow this document (which is written by LT so it's a bit one sided but still explains a few mechanics of the simulator) http://cds.linear.com/docs/en/lt-journal/LTJournal-V24N4-01-df-SPICEDifferentiation-MikeEngelhardt.pdf

But if your ultimate goal is fabrication then you'd need a good layout editor, but good ones are not available for free. And more importantly layout will be given to the fab, so it also depends on the requirements of the fab. For example some fabs may provide you with everything for calibre but not anything else (good fabs usually provide everything, but especially if you're getting this service through a third party [multi project wafer companies] they may not provide all the rulesets for all the tools). So you may not be able to choose which tools you're going to use.

In short, LTSpice is awesome for simulation, but there's a lot more to consider if you want to fabricate. And to be honest if you're in a university just ask around if you have access to Cadence tools. It's a complete suite so it'd cover everything you need, and Cadence distributes its software liberally to universities.

Click to expand...

Thanks alot Kemiyun. I want to use LTspice because it is much user friendly and also I have it in my Laptop. if I have everything verified in simulation I will use Layout tool in Cadence, Yes it is provided by the university but I need to work from specific labs which is not convenient for me.

bio_man said:

Thanks alot Kemiyun. I want to use LTspice because it is much user friendly and also I have it in my Laptop. if I have everything verified in simulation I will use Layout tool in Cadence, Yes it is provided by the university but I need to work from specific labs which is not convenient for me.

Click to expand...

Don't do it. You're trying to avoid the unavoidable. Bear with the inconvenience and use Cadence. I'm pretty sure that the lab would provide a remote desktop access or a VPN for you to check out licenses so that you can work on your computer or at home. I'm saying this because you're going to have to migrate everything to cadence environment again for layout and you're going to have to verify them again. If you really want to go through the whole process two times, then do it, but I'd advise otherwise. Also if you get used to it Cadence tools are not that bad. Sure GUI can use an improvement, and some stuff look complicated at first but it's okay once you get used to it.

I don't want to promote their tools even though I like them I think competition is always better, but LTSpice is not the competitor of virtuoso suite, it's competitor of spectre. It can only do so much and you'll eventually need layout editor, DRC, LVS tools. Just because lab is inconvenient is not enough reason, and I'm not sure if you're aware how much time is actually spent verifying things, like simulating the parasitic extracted versions, fixing things, doing it again. These are going to be super painful in the future, and these will require you to migrate everything to cadence environment anyway.

I also want to develop my own IC flow made out of free (and preferably open source) software one day but it's just not today

I agree with kemiyun that there are ways to do an integrated circuit design with a lot less hassle than using LTSpice.

Whether you can do your simulations using LTSpice depends on whether you have a TSMC design kit for LTSpice. If you do, you can use LTSpice. If you don't you may get some unpredictable results, even if your model library says models are suited for Berkeley Spice version 3. You could check with the people who are responsible for the simulation environment at you university.

Each simulation tools interprets some model parameters in its own way. Often a parameter will go by different names in different simulators or you will have to set a different model level. Sometimes model equations are different. Sometimes a parameter is just missing in one simulator.

You could go through the trouble of translating a model made for one simulator to use it with another simulator. We did that with a BiCMOS model library some years ago after we bought a Spectre licence. At room temperature, simulation results were pretty much the same with both simulators but our circuits behaved differently in simulation at low or high temperatures depending on which simulator we were using.

If you use a simulator with a model made for another simulator your circuit may behave differently from your simulation results after it has been fabricated. You could do your first simulations in LTSpice and double-check your results using whatever simulator your models are made for.

Best wishes
Axel

Circuit design is much more than schematic capture and simulation.
LTSpice will not be much help in layout verification, post-routing
simulation or any of the stuff that you need when it "gets real".
For many device models in LTSpice the primitives lack some of the
geometry fields you would want to see in IC design where this is
a (perhaps, the) critical "knob".

I use it for weirdball stuff sometimes where I have only primitive
models (not a foundry PDK) but there are better ways to go for
real IC design.

If converting models from a pirated PDK you need to beware the
dialect, units, syntax differences along with how some of the
device models treat parameters (e.g. cgdo may be per-W in
IC CAD systems' simulators, but a fixed value in ones that deal
in discretes primarily, like ones that attend PCB tools).

There are numerous free simulators, some with clean-ish paths
from (also free) schematic capture tools.

ThisIsNotSam said:

This looks like a TSMC proprietary file, no? You should not disclose it.

Click to expand...

bio_man said:

I found it using google, anyways I tried to modify my post and delete the file but couldn't, can you help?

Click to expand...

In view of the fact that parameters of the 180nm process have had wide distribution in the years it has been in use, there does not seem to be an objection from forum moderators. Nevertheless copyright may still apply to newer processes, or proprietary processes.