On Sat, Apr 12, 2025 at 09:53 AM, john23 wrote:
Hello,I have created a circuit shown below in ltspice using tsmc 180nm mosfets.
First, you have made some mistakes, which you should fix before progressing further.
?
The P-channel MOSFETs are correctly named so that they use your CMOSP (BSIM3) model.? However, all of your N-channel MOSFETs are still named "NMOS", so all of them are LEVEL=1 MOSFETs using 1975 technology, and are certainly incorrect for 180nm MOSFETs.? You can not expect that simulation to have meaningful results.? They do not use the P-channel .MODEL on your schematic because the model names are incorrect.
?
In order to use the T588F SPICE BSIM models, you need to name your MOSFETs to agree with the .MODELs.
?
It is unlikely (but not impossible) that both N-channel and P-channel MOSFETs would ave the same dimensions.? Often the P-channel MOSFETs need to be wider, in part because of the differences between N and P materials.
?
It is possible (uncertain) that you have the wrong LEVEL number in these two .MODEL statements.? At the top, it states, that the LEVEL should be 8 for SPICE 3F5, and 49 for HSPICE.? LTspice has capability of both LEVEL=8 and LEVEL=49, and it is unclear which one you should use.? LEVEL=8 is described in the Help as:
BSIM3v3.3.0 from University of California, Berkeley as of July 29, 2005
SPICE 3F5 is from U-Cal Berkeley.? LEVEL=49 is not described in the Help, but it does work in LTspice (probably added for compatibility with HSPICE's LEVEL=49 models).? I am not sure but I think HSPICE chose to make their LEVEL=8 differ from the "standard" (Berkeley) LEVEL=8 model, and so they had to fix that problem by making a brand new LEVEL=49.? There is the possibility that LEVEL=8 and LEVEL=49 are either the same or so close (in LTspice) to be indistinguishable from one another, but that is only an uneducated guess.? HSPICE describes their LEVEL=8 as "advanced LEVEL 2", and LTspice clearly states that it is BSIM3, which is what these models are.? (Unfortunately, there is no central clearinghouse for SPICE MOSFET LEVEL numbers.? That creates problems, like this one, where it is unclear which model should be used.)
If you wanted to change the LEVEL number, do it by editing both .MODEL statements on your schematic and change "LEVEL ? = 49" to "LEVEL ? = 8".? Do it in both .MODELs.
unlike the standart way where we bias the mosfets using the large signal furmulas ,I would like to bias the M3,5,1,2 into saturation while M4,6 needs to be linear using charactersitics plots .
What are M3,5,1,2 and M4,6?? I cannot find them on your schematic.
?
Are you trying to adjust the dimensions of the MOSFETs?? Or adjust the voltage sources?? Or adjust the resistance value of R1?? Or all three?
?
Can you pull out individual MOSFETs from the circuit, and sweep them (.DC sweeps) to see their characteristics, then use that information to set up your circuit's biasing the way you want it to be?
?
Andy
?
