TSMC 180nm definitions

Thread Starter

mos_6502

Joined Dec 11, 2017
66
Hi,
where I find or download the complete definitions for TSMC 180nm?

I found something on the net, but I know that there are definitions for at least 4 types of mosfet, and I would be interested in the one with high VTh.
But where can it be downloaded or found? Is it possible to do this from the TSMC website?
 

sjsdorsay

Joined Dec 13, 2015
11
Hi mos,

When I was working on the SiGe 130 nm BiCMOS process from global foundries we had to pay for their model definitions for our particular design and simulation environments; at the time we were using ADS and Virtuoso.

From my experience, the libraries are quite expensive and are typically only available to universities and large companies. Sorry, I don't know much more, it's been a few years since I was working on an IC.

Cheers!
Stephen
 

Papabravo

Joined Feb 24, 2006
21,159
Hello Papabravo,what about the model shown below.
how it compared to the real deal?
Thanks.

https://sanjayvidhyadharan.in/Downloads/tsmc_180_nm/tsmc018.lib
I don't know since I have no basis for comparison. The model I posted came from an e-book as I mentioned. Unless they have all of the parameters in the same location in the text file it would be hard to do a quick comparison. I suppose you could read both files in and output them in a standard format to enable a quick side by side comparison.
 

yef smith

Joined Aug 2, 2020
717
Hello PapaBravo, i have opened the symbol in LTPSICE and i see where is the Source pin as shown bellow.
both our netlists the netlist is not specifiend the g s d b pins in it.
how LTspice know how connect my netlist to the pins of the symbol?
how can i update my netlist to specify him the pins so i will see exactly the ltspice connection to the netlist is a perfect fit?
Thanks.
1679779818657.png
 

WBahn

Joined Mar 31, 2012
29,978
Hi,
where I find or download the complete definitions for TSMC 180nm?

I found something on the net, but I know that there are definitions for at least 4 types of mosfet, and I would be interested in the one with high VTh.
But where can it be downloaded or found? Is it possible to do this from the TSMC website?
Normally you have to sign a nondisclosure agreement and often have to pay a fee to get a fab's models. Plus, there are several different lines that would fall under a generic heading of 180 nm. Are you looking for digital or analog or imager? High voltage? Low power? Epitaxial or non-epitaxial? High voltage transistors? Intrinsic transistors?

Depending on the variant, there are several sets of models available. Room temp, high-temp, low-temp, cryogenic. Then there's the speed models -- fast, typical, and slow -- to allow you to do corner simulations.

These models are often subcircuits because the available transistor model doesn't have enough degrees of freedom to model the actual behavior. When I looked inside the IBM 130 nm models, each transistor was implemented as a subcircuit with over 300 components in it.

The results are generally VERY good simulation results that match actual performance quite closely. The downside is that they tend to be really slow when doing simulations that involve more than a few dozen transistors, though there are often ways to manage that.
 

WBahn

Joined Mar 31, 2012
29,978
Hello PapaBravo, i have opened the symbol in LTPSICE and i see where is the Source pin as shown bellow.
both our netlists the netlist is not specifiend the g s d b pins in it.
how LTspice know how connect my netlist to the pins of the symbol?
how can i update my netlist to specify him the pins so i will see exactly the ltspice connection to the netlist is a perfect fit?
Thanks.
View attachment 290713
The connects are made according to pin order. So you need to look at the device model that is going to be invoked and determine what order the various connections need to be made in, and then you need to set up the symbol to export the call of the model with the pins in that order. In your diagram the pin labeled 'S' will appear as the third signal in the netlist.

Taking the time to get the symbol correct is absolutely critical, because the simulator neither knows nor cares whether your netlist matches your schematic. Fortunately, you should only have to do this once for every symbol in your symbol library and every device model in your subcircuit library.
 

Papabravo

Joined Feb 24, 2006
21,159
The symbols NMOS4 and PMOS4 that come with LTspice, netlist as follows:

NodeSymbolNetlist Order
DrainD1
GateG2
SourceS3
BulkB4
Anything you do that can use a .model card can use the standard symbol(s). As has been suggested, if you want to use subcircuit models you need to verify the correct spice netlist ordering between the symbol and the sub-circuit definition. This is explicitly documented in the LTspice Help which I have copied and highlighted.
M. MOSFET
Monolithic MOSFET:
Syntax: Mxxx Nd Ng Ns Nb <model> [m=<value>] [L=<len>]
+ [W=<width>] [AD=<area>] [AS=<area>]
+ [PD=<perim>] [PS=<perim>] [NRD=<value>].
+ [NRS=<value>] [off] [IC=<Vds, Vgs, Vbs>]
+ [temp=<T>]
 
Last edited:

yef smith

Joined Aug 2, 2020
717
Hello Papabravo,I have this model shown bellow.
Its not a subcircuit.so how LTSPICE know how to use properly the model?
This model could be configured for one type of pin connection?
we dont have this line in my spice model.
Syntax: Mxxx Nd Ng Ns Nb <model> [m=<value>] [L=<len>]

https://sanjayvidhyadharan.in/Downloads/tsmc_180_nm/tsmc018.lib

Code:
.MODEL CMOSP PMOS (                                LEVEL   = 49
+VERSION = 3.1            TNOM    = 27             TOX     = 4.1E-9
+XJ      = 1E-7           NCH     = 4.1589E17      VTH0    = -0.3906012
+K1      = 0.5341312      K2      = 0.0395326      K3      = 0
+K3B     = 7.4916211      W0      = 1E-6           NLX     = 1.194072E-7
+DVT0W   = 0              DVT1W   = 0              DVT2W   = 0
+DVT0    = 0.5060555      DVT1    = 0.2423835      DVT2    = 0.1
+U0      = 115.6894042    UA      = 1.573746E-9    UB      = 1.874308E-21
+UC      = -1E-10         VSAT    = 1.130982E5     A0      = 1.9976555
+AGS     = 0.4186945      B0      = 1.949178E-7    B1      = 6.422908E-7
+KETA    = 0.0166345      A1      = 0.4749146      A2      = 0.300003
+RDSW    = 198.321294     PRWG    = 0.5            PRWB    = -0.4986647
+WR      = 1              WINT    = 0              LINT    = 2.94454E-8
+XL      = 0              XW      = -1E-8          DWG     = -2.798724E-8
+DWB     = -4.83797E-10   VOFF    = -0.095236      NFACTOR = 2
+CIT     = 0              CDSC    = 2.4E-4         CDSCD   = 0
+CDSCB   = 0              ETA0    = 1.035504E-3    ETAB    = -4.358398E-4
+DSUB    = 1.816555E-3    PCLM    = 1.3299898      PDIBLC1 = 1.766563E-3
+PDIBLC2 = 7.728395E-7    PDIBLCB = -1E-3          DROUT   = 1.011891E-3
+PSCBE1  = 4.872184E10    PSCBE2  = 5E-10          PVAG    = 0.0209921
+DELTA   = 0.01           RSH     = 7.7            MOBMOD  = 1
+PRT     = 0              UTE     = -1.5           KT1     = -0.11
+KT1L    = 0              KT2     = 0.022          UA1     = 4.31E-9
+UB1     = -7.61E-18      UC1     = -5.6E-11       AT      = 3.3E4
+WL      = 0              WLN     = 1              WW      = 0
+WWN     = 1              WWL     = 0              LL      = 0
+LLN     = 1              LW      = 0              LWN     = 1
+LWL     = 0              CAPMOD  = 2              XPART   = 0.5
+CGDO    = 6.35E-10       CGSO    = 6.35E-10       CGBO    = 1E-12
+CJ      = 1.144521E-3    PB      = 0.8468686      MJ      = 0.4099522
+CJSW    = 2.490749E-10   PBSW    = 0.8769118      MJSW    = 0.3478565
+CJSWG   = 4.22E-10       PBSWG   = 0.8769118      MJSWG   = 0.3478565
+CF      = 0              PVTH0   = 2.302018E-3    PRDSW   = 9.0575312
+PK2     = 1.821914E-3    WKETA   = 0.0222457      LKETA   = -1.495872E-3
+PU0     = -1.5580645     PUA     = -6.36889E-11   PUB     = 1E-21
+PVSAT   = 49.8420442     PETA0   = 2.827793E-5    PKETA   = -2.536564E-3
+ NOIMOD=2.0E+00        NOIA=3.57456993317604E+18        NOIB=2500
+ NOIC=2.61260020285845E-11    EF=1.1388                EM=41000000 )
 

Papabravo

Joined Feb 24, 2006
21,159
Hello Papabravo,I have this model shown bellow.
Its not a subcircuit.so how LTSPICE know how to use properly the model?
This model could be configured for one type of pin connection?
we dont have this line in my spice model.
Syntax: Mxxx Nd Ng Ns Nb <model> [m=<value>] [L=<len>]

https://sanjayvidhyadharan.in/Downloads/tsmc_180_nm/tsmc018.lib

Code:
.MODEL CMOSP PMOS (                                LEVEL   = 49
+VERSION = 3.1            TNOM    = 27             TOX     = 4.1E-9
+XJ      = 1E-7           NCH     = 4.1589E17      VTH0    = -0.3906012
+K1      = 0.5341312      K2      = 0.0395326      K3      = 0
+K3B     = 7.4916211      W0      = 1E-6           NLX     = 1.194072E-7
+DVT0W   = 0              DVT1W   = 0              DVT2W   = 0
+DVT0    = 0.5060555      DVT1    = 0.2423835      DVT2    = 0.1
+U0      = 115.6894042    UA      = 1.573746E-9    UB      = 1.874308E-21
+UC      = -1E-10         VSAT    = 1.130982E5     A0      = 1.9976555
+AGS     = 0.4186945      B0      = 1.949178E-7    B1      = 6.422908E-7
+KETA    = 0.0166345      A1      = 0.4749146      A2      = 0.300003
+RDSW    = 198.321294     PRWG    = 0.5            PRWB    = -0.4986647
+WR      = 1              WINT    = 0              LINT    = 2.94454E-8
+XL      = 0              XW      = -1E-8          DWG     = -2.798724E-8
+DWB     = -4.83797E-10   VOFF    = -0.095236      NFACTOR = 2
+CIT     = 0              CDSC    = 2.4E-4         CDSCD   = 0
+CDSCB   = 0              ETA0    = 1.035504E-3    ETAB    = -4.358398E-4
+DSUB    = 1.816555E-3    PCLM    = 1.3299898      PDIBLC1 = 1.766563E-3
+PDIBLC2 = 7.728395E-7    PDIBLCB = -1E-3          DROUT   = 1.011891E-3
+PSCBE1  = 4.872184E10    PSCBE2  = 5E-10          PVAG    = 0.0209921
+DELTA   = 0.01           RSH     = 7.7            MOBMOD  = 1
+PRT     = 0              UTE     = -1.5           KT1     = -0.11
+KT1L    = 0              KT2     = 0.022          UA1     = 4.31E-9
+UB1     = -7.61E-18      UC1     = -5.6E-11       AT      = 3.3E4
+WL      = 0              WLN     = 1              WW      = 0
+WWN     = 1              WWL     = 0              LL      = 0
+LLN     = 1              LW      = 0              LWN     = 1
+LWL     = 0              CAPMOD  = 2              XPART   = 0.5
+CGDO    = 6.35E-10       CGSO    = 6.35E-10       CGBO    = 1E-12
+CJ      = 1.144521E-3    PB      = 0.8468686      MJ      = 0.4099522
+CJSW    = 2.490749E-10   PBSW    = 0.8769118      MJSW    = 0.3478565
+CJSWG   = 4.22E-10       PBSWG   = 0.8769118      MJSWG   = 0.3478565
+CF      = 0              PVTH0   = 2.302018E-3    PRDSW   = 9.0575312
+PK2     = 1.821914E-3    WKETA   = 0.0222457      LKETA   = -1.495872E-3
+PU0     = -1.5580645     PUA     = -6.36889E-11   PUB     = 1E-21
+PVSAT   = 49.8420442     PETA0   = 2.827793E-5    PKETA   = -2.536564E-3
+ NOIMOD=2.0E+00        NOIA=3.57456993317604E+18        NOIB=2500
+ NOIC=2.61260020285845E-11    EF=1.1388                EM=41000000 )
You are conflating two different things.

Mxxx Nd Ng Ns Nb <model> [m=<value>] [L=<len>] ; this line is in the spice netlist and it creates an instance of the .model. This is like a function call.

.MODEL CMOSP PMOS ( LEVEL = 49 ; this line is the model definition

Subcircuits and models are similar but there are some differences.
 
Top