transconductance parameter (Kn,Kp) of TSMC 0.18µ

[fasto2008]

transconductance parameter

Hello everyone

I need transconductance parameter Kn of the NMOS and Kp of the PMOS .
from website MOSIS, i download spice model parameter TSMC 0.18µ ,CR018 (CM018) (mixed-mode).
*****************************Spice Model*****************************
.MODEL NMOS NMOS ( LEVEL = 49

+VERSION = 3.1 TNOM = 27 TOX = 4.1E-9
+XJ = 1E-7 NCH = 2.3549E17 VTH0 = 0.3631313
+K1 = 0.5920712 K2 = 3.261973E-3 K3 = 1E-3
+K3B = 2.9061018 W0 = 1E-7 NLX = 1.840449E-7
+DVT0W = 0 DVT1W = 0 DVT2W = 0
+DVT0 = 1.4767146 DVT1 = 0.4177419 DVT2 = 8.829889E-3
+U0 = 255.1380803 UA = -1.597788E-9 UB = 2.53505E-18
+UC = 4.766568E-11 VSAT = 1.010331E5 A0 = 1.80776
+AGS = 0.3951935 B0 = 2.536033E-7 B1 = 5E-6
+KETA = -5.061981E-3 A1 = 5.396345E-4 A2 = 0.8936768
+RDSW = 111.58989 PRWG = 0.5 PRWB = -0.2
+WR = 1 WINT = 0 LINT = 1.840173E-8
+XL = 0 XW = -1E-8 DWG = -5.605289E-9
+DWB = 1.137609E-8 VOFF = -0.0871468 NFACTOR = 2.3018187
+CIT = 0 CDSC = 2.4E-4 CDSCD = 0
+CDSCB = 0 ETA0 = 3.127659E-3 ETAB = 9.485027E-6
+DSUB = 0.018202 PCLM = 0.7464953 PDIBLC1 = 0.2263045
+PDIBLC2 = 2.358517E-3 PDIBLCB = -0.1 DROUT = 0.8266278
+PSCBE1 = 4.915846E10 PSCBE2 = 2.831646E-9 PVAG = 0.010936
+DELTA = 0.01 RSH = 6.6 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 = 8.4E-10 CGSO = 8.4E-10 CGBO = 1E-12
+CJ = 9.619152E-4 PB = 0.8 MJ = 0.3787773
+CJSW = 2.61908E-10 PBSW = 0.8 MJSW = 0.157929
+CJSWG = 3.3E-10 PBSWG = 0.8 MJSWG = 0.157929
+CF = 0 PVTH0 = -6.300783E-5 PRDSW = -2.1729835
+PK2 = 9.978988E-4 WKETA = 8.888859E-5 LKETA = -6.31897E-3
+PU0 = 4.3665601 PUA = 9.428511E-14 PUB = 0
+PVSAT = 1.356405E3 PETA0 = 1.003159E-4 PKETA = -1.583628E-3 )
*
.MODEL PMOS PMOS ( LEVEL = 49

+VERSION = 3.1 TNOM = 27 TOX = 4.1E-9
+XJ = 1E-7 NCH = 4.1589E17 VTH0 = -0.3706453
+K1 = 0.5740728 K2 = 0.0277093 K3 = 0
+K3B = 7.9502396 W0 = 1E-6 NLX = 1.195464E-7
+DVT0W = 0 DVT1W = 0 DVT2W = 0
+DVT0 = 0.6525814 DVT1 = 0.2558611 DVT2 = 0.1
+U0 = 103.6542095 UA = 1.044279E-9 UB = 1E-21
+UC = -1E-10 VSAT = 1.528072E5 A0 = 1.6482476
*******************************************************************
Kn =µ0 * Cox
we haven't the value of Cox

Thank you in advance for your help
Fasto

 

[erikl]

kn kp

Kn =µ0 * Cox
we haven't the value of Cox

Thank you in advance for your help
Fasto

You have TOX
Cox = Epsilon(SiO2) / TOX
Epsilon(SiO2) = Epsilon(0) * Epsilon(SiO2,rel) = 8.854e-12 F/m * 3.9
--> Cox = 8.422e-3 As/Vmjavascript:emoticon('%C2%B2') javascript:emoticon('%E2%89%88') 8.4 fF/(µm)javascript:emoticon('%C2%B2')

HTH, erikl

 

[kishore2k4]

process transconductance parameter

Check this site for detailed explaination of the BSIM3 model. Whenever you start with a new process its a good idea to do characterisation of the the MOSFETs in simulation.

The parameter values you see in the model are not always the actual stuff. They are curve fitting parameters that were extracted from silicon characterisation when the process is first done.

 

[pbs681]

transconductance parameters

Check this site for detailed explaination of the BSIM3 model. Whenever you start with a new process its a good idea to do characterisation of the the MOSFETs in simulation.

The parameter values you see in the model are not always the actual stuff. They are curve fitting parameters that were extracted from silicon characterisation when the process is first done.

normally tox parametr is extracted based on actual measurement.... so, the value from model is quite reliable..... alternatively, you can check this value from foundry document....

as for u0, it is normally curve fitting parameter..... for hand calculation u can use default value from BSIM3 document......

for characterisation, it is good to use large W and large L, ie 10/10um as it has very small effect on the small length and narrow width effect

 

[neter]

process transconductance

Is a Epsilon(SiO2) constant in common use of any porcess (TSMC and UMC) ?

 

[fasto2008]

tsmc 0.18 model parameter

Hello everyone

Realy with your help
Thank you very much,i found Kn an Kp in Spice Model
******************Model***********************

MOSIS PARAMETRIC TEST RESULTS

RUN: T49P (MM_NON-EPI) VENDOR: TSMC
TECHNOLOGY: SCN018 FEATURE SIZE: 0.18 microns


INTRODUCTION: This report contains the lot average results obtained by MOSIS
from measurements of MOSIS test structures on each wafer of
this fabrication lot. SPICE parameters obtained from similar
measurements on a selected wafer are also attached.

COMMENTS: DSCN6M018_TSMC


TRANSISTOR PARAMETERS W/L N-CHANNEL P-CHANNEL UNITS

MINIMUM 0.27/0.18
Vth 0.50 -0.51 volts

SHORT 20.0/0.18
Idss 591 -293 uA/um
Vth 0.52 -0.51 volts
Vpt 4.6 -5.4 volts

WIDE 20.0/0.18
Ids0 22.8 -20.3 pA/um

LARGE 50/50
Vth 0.43 -0.41 volts
Vjbkd 3.1 -4.1 volts
Ijlk <50.0 <50.0 pA

K' (Uo*Cox/2) 170.7 -36.1 uA/V^2
Low-field Mobility 405.36 85.73 cm^2/V*s
************************************************************
Thank you for everyone

FASTO

 

[erikl]

kn nmos

Is Epsilon(SiO2) constant in common use of any process (TSMC and UMC) ?

Yes, it's one of the most stable properties in any silicon semicondutor process. At least you can trust the first 2 figure values of epsilon(SiO2,rel)=3.9 .

Added after 41 minutes:

K' (Uo*Cox/2) 170.7 -36.1 uA/V^2
Low-field Mobility 405.36 85.73 cm^2/V*s
************************************************************
Thank you for everyone FASTO

Very good! And with my calculated values given above
Cox = 8.422e-3 F/m^2 = 0.8422 µAs/V(cm)^2
Cox/2 = 0.4211 µAs/V(cm)^2

... you get exactly these values ;-)
Kn = 405.36 cm^2/Vs * 0.4211 µAs/V(cm)^2 = 170.7 uA/V^2
Kp = 85.73 cm^2/Vs * 0.4211 µAs/V(cm)^2 = 36.1 uA/V^2

Cheers, erikl

 

[abdj_project]

Re: transconductance parameter

Hi,

Can you share the whole library model for nmos and pmos specified below. We see that NMOS is full, but pmos is not described fully here. Could you please share it for us to do some experiments and also the Kp and Kn values you have computed for this library.

Thanks a lot.

Regards,
abdj

Hello everyone

I need transconductance parameter Kn of the NMOS and Kp of the PMOS .
from website MOSIS, i download spice model parameter TSMC 0.18µ ,CR018 (CM018) (mixed-mode).
*****************************Spice Model*****************************
.MODEL NMOS NMOS ( LEVEL = 49

+VERSION = 3.1 TNOM = 27 TOX = 4.1E-9
+XJ = 1E-7 NCH = 2.3549E17 VTH0 = 0.3631313
+K1 = 0.5920712 K2 = 3.261973E-3 K3 = 1E-3
+K3B = 2.9061018 W0 = 1E-7 NLX = 1.840449E-7
+DVT0W = 0 DVT1W = 0 DVT2W = 0
+DVT0 = 1.4767146 DVT1 = 0.4177419 DVT2 = 8.829889E-3
+U0 = 255.1380803 UA = -1.597788E-9 UB = 2.53505E-18
+UC = 4.766568E-11 VSAT = 1.010331E5 A0 = 1.80776
+AGS = 0.3951935 B0 = 2.536033E-7 B1 = 5E-6
+KETA = -5.061981E-3 A1 = 5.396345E-4 A2 = 0.8936768
+RDSW = 111.58989 PRWG = 0.5 PRWB = -0.2
+WR = 1 WINT = 0 LINT = 1.840173E-8
+XL = 0 XW = -1E-8 DWG = -5.605289E-9
+DWB = 1.137609E-8 VOFF = -0.0871468 NFACTOR = 2.3018187
+CIT = 0 CDSC = 2.4E-4 CDSCD = 0
+CDSCB = 0 ETA0 = 3.127659E-3 ETAB = 9.485027E-6
+DSUB = 0.018202 PCLM = 0.7464953 PDIBLC1 = 0.2263045
+PDIBLC2 = 2.358517E-3 PDIBLCB = -0.1 DROUT = 0.8266278
+PSCBE1 = 4.915846E10 PSCBE2 = 2.831646E-9 PVAG = 0.010936
+DELTA = 0.01 RSH = 6.6 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 = 8.4E-10 CGSO = 8.4E-10 CGBO = 1E-12
+CJ = 9.619152E-4 PB = 0.8 MJ = 0.3787773
+CJSW = 2.61908E-10 PBSW = 0.8 MJSW = 0.157929
+CJSWG = 3.3E-10 PBSWG = 0.8 MJSWG = 0.157929
+CF = 0 PVTH0 = -6.300783E-5 PRDSW = -2.1729835
+PK2 = 9.978988E-4 WKETA = 8.888859E-5 LKETA = -6.31897E-3
+PU0 = 4.3665601 PUA = 9.428511E-14 PUB = 0
+PVSAT = 1.356405E3 PETA0 = 1.003159E-4 PKETA = -1.583628E-3 )
*
.MODEL PMOS PMOS ( LEVEL = 49

+VERSION = 3.1 TNOM = 27 TOX = 4.1E-9
+XJ = 1E-7 NCH = 4.1589E17 VTH0 = -0.3706453
+K1 = 0.5740728 K2 = 0.0277093 K3 = 0
+K3B = 7.9502396 W0 = 1E-6 NLX = 1.195464E-7
+DVT0W = 0 DVT1W = 0 DVT2W = 0
+DVT0 = 0.6525814 DVT1 = 0.2558611 DVT2 = 0.1
+U0 = 103.6542095 UA = 1.044279E-9 UB = 1E-21
+UC = -1E-10 VSAT = 1.528072E5 A0 = 1.6482476
*******************************************************************
Kn =µ0 * Cox
we haven't the value of Cox

Thank you in advance for your help
Fasto

 

[erikl]

Re: transconductance parameter

Can you share the whole library model for nmos and pmos specified below.

It's published and available ...

from website MOSIS, i download spice model parameter TSMC 0.18µ ,CR018 (CM018) (mixed-mode).
*****************************Spice Model*****************************
.MODEL NMOS NMOS ( LEVEL = 49

See here.

******************Model***********************

MOSIS PARAMETRIC TEST RESULTS

RUN: T49P (MM_NON-EPI) VENDOR: TSMC
TECHNOLOGY: SCN018 FEATURE SIZE: 0.18 microns

 

[abdj_project]

Re: transconductance parameter

Hi,

Thanks a lot.

So for this model, we should take Kn = 171.2u and Kp = 36.1u right?

Actually Kn = µnCox, where Cox we can calculate as εsi/Tox. Tox is available in the library. But how can we take the µn value. There is a U0 value in the library. Is this what we have to take for calculation? But U0=270.9714861 for NMOS and U0=103.9954725 for PMOS. With this we need to calculate?

When ever you have used this library, have you designed circuits with Kn = 171.2u and Kp = 36.1u ? Because for design Kn and Kp values are very important rt.

Also here K' is specified in library as µnCOx/2. Actually when we design, we use Kn as µnCox only. So do we need to multiply the given values Kn = 171.2u and Kp = 36.1u by 2?

Thanks,
abdj

 

[erikl]

Re: transconductance parameter

So for this model, we should take Kn = 171.2u and Kp = 36.1u right?

Depends on the run lot. For the ...

RUN: T49P (MM_NON-EPI)                            VENDOR: TSMC
   TECHNOLOGY: SCN018                                FEATURE SIZE: 0.18 microns

... I find ...

 K' (Uo*Cox/2)                         170.7     -36.1   uA/V^2

... which is K'=K/2

Actually Kn = µnCox, where Cox we can calculate as εsi/Tox. Tox is available in the library. But how can we take the µn value. There is a U0 value in the library. Is this what we have to take for calculation? But U0=270.9714861 for NMOS and U0=103.9954725 for PMOS. With this we need to calculate?

No. With the extracted U0 values from SPICE you get Kn=228 µA/V² resp. Kp=87.6 µA/V².

When ever you have used this library, have you designed circuits with Kn = 171.2u and Kp = 36.1u ? Because for design Kn and Kp values are very important rt.

I never used this lib, sorry. But if you got these values from a lib (or from TSMC lot run test results), you better use these values; they already represent the K'=K/2 values for your calculations.

Also here K' is specified in library as µnCOx/2. Actually when we design, we use Kn as µnCox only. So do we need to multiply the given values Kn = 171.2u and Kp = 36.1u by 2?

Depends. As mentioned above, these K' values are correct for your calculations (those which need K'=µ*Cox/2).
For those calculations which need K=µ*Cox you have to multiply by 2 of course.

 

[abdj_project]

Re: transconductance parameter

Thanks erikl,

We have few more doubts. We are not at all familiar with mos libraries and hence facing a lot of trouble in simulating circuits. Circuit details given below. Could you please share a mos hspice model library you are using which is working correctly for us to try some circuits. We would like to have level49 library for which we know accurate Kn, Kp, Vth, ΔVth values. Please help as we are finding it very very very difficult to solve issues as we don't understand library values well. Sorry for trouble. Circuit details given below

Actually we were trying to design a simple 2-stage opamp as shown in figure below.


The library we are using is :

-----------------------------------------------------------------------------------------------------------------
MOSIS PARAMETRIC TEST RESULTS
RUN: T49P (MM_NON-EPI_THK-MTL) VENDOR: TSMC
TECHNOLOGY: SCN018 FEATURE SIZE: 0.18 microns
INTRODUCTION: This report contains the lot average results obtained by MOSIS
from measurements of MOSIS test structures on each wafer of
this fabrication lot. SPICE parameters obtained from similar
measurements on a selected wafer are also attached.
COMMENTS: DSCN6M018_TSMC

TRANSISTOR PARAMETERS W/L N-CHANNEL P-CHANNEL UNITS
MINIMUM 0.27/0.18
Vth 0.50 -0.50 volts
SHORT 20.0/0.18
Idss 602 -306 uA/um
Vth 0.51 -0.50 volts
Vpt 4.7 -5.4 volts
WIDE 20.0/0.18
Ids0 32.5 -29.6 pA/um
LARGE 50/50
Vth 0.42 -0.41 volts
Vjbkd 3.2 -4.1 volts
Ijlk <50.0 <50.0 pA
K' (Uo*Cox/2) 171.2 -36.1 uA/V^2
Low-field Mobility 396.63 83.64 cm^2/V*s
COMMENTS: Poly bias varies with design technology. To account for mask
bias use the appropriate value for the parameters XL and XW
in your SPICE model card.
Design Technology XL (um) XW (um)
----------------- ------- ------
SCN6M_DEEP (lambda=0.09) 0.00 -0.01
thick oxide 0.00 -0.01
SCN6M_SUBM (lambda=0.10) -0.02 0.00
thick oxide -0.02 0.00
FOX TRANSISTORS GATE N+ACTIVE P+ACTIVE UNITS
Vth Poly >6.6 <-6.6 volts
PROCESS PARAMETERS N+ P+ POLY N+BLK PLY+BLK M1 M2 UNITS
Sheet Resistance 6.6 7.5 7.7 60.0 316.1 0.08 0.08 ohms/sq
Contact Resistance 10.7 11.3 10.0 4.63 ohms
Gate Oxide Thickness 40 angstrom
PROCESS PARAMETERS M3 POLY_HRI M4 M5 M6 N_W UNITS
Sheet Resistance 0.08 1003.5 0.07 0.07 0.01 929 ohms/sq
Contact Resistance 9.09 13.82 18.56 21.33 ohs
COMMENTS: BLK is silicide block.
CAPACITANCE PARAMETERS N+ P+ POLY M1 M2 M3 M4 M5 M6 R_W D_N_W M5P N_W UNITS
Area (substrate) 954 1168 104 38 19 13 8 8 3 132 132 aF/um^2
Area (N+active) 8533 54 20 14 11 9 8 aF/um^2
Area (P+active) 8271 aF/um^2
Area (poly) 63 17 10 7 5 4 aF/um^2
Area (metal1) 38 14 9 6 5 aF/um^2
Area (metal2) 38 14 9 6 aF/um^2
Area (metal3) 40 15 9 aF/um^2
Area (metal4) 37 14 aF/um^2
Area (metal5) 37 1025 aF/um^2
Area (r well) 937 aF/um^2
Area (d well) 582 aF/um^2
Area (no well) 144 aF/um^2
Fringe (substrate) 267 228 60 55 41 25 aF/um
Fringe (poly) 57 39 29 23 20 19 aF/um
Fringe (metal1) 56 35 23 20 aF/um
Fringe (metal2) 49 35 27 24 aF/um
Fringe (metal3) 53 36 31 aF/um
Fringe (metal4) 60 42 aF/um
Fringe (metal5) 72 aF/um
Overlap (N+active) 806 aF/um
Overlap (P+active) 650 aF/um

CIRCUIT PARAMETERS UNITS
Inverters K
Vinv 1.0 0.75 volts
Vinv 1.5 0.80 volts
Vol (100 uA) 2.0 0.07 volts
Voh (100 uA) 2.0 1.65 volts
Vinv 2.0 0.84 volts
Gain 2.0 -20.24
Ring Oscillator Freq.
D1024_THK (31-stg,3.3V) 341.78 MHz
DIV1024 (31-stg,1.8V) 437.60 MHz
Ring Oscillator Power
D1024_THK (31-stg,3.3V) 0.07 uW/MHz/gate
DIV1024 (31-stg,1.8V) 0.02 uW/MHz/gate
COMMENTS: DEEP_SUBMICRON
T49P SPICE BSIM3 VERSION 3.1 PARAMETERS
SPICE 3f5 Level 8, Star-HSPICE Level 49, UTMOST Level 8
* DATE: Dec 6/04
* LOT: T49P WAF: 4002
* Temperature_parameters=Default
.MODEL CMOSN NMOS ( LEVEL = 49
+VERSION = 3.1 TNOM = 27 TOX = 4E-9
+XJ = 1E-7 NCH = 2.3549E17 VTH0 = 0.363908
+K1 = 0.5802969 K2 = 3.304956E-3 K3 = 1E-3
+K3B = 2.396754 W0 = 1E-7 NLX = 1.77724E-7
+DVT0W = 0 DVT1W = 0 DVT2W = 0
+DVT0 = 1.3696919 DVT1 = 0.3863182 DVT2 = 0.0111435
+U0 = 270.9714861 UA = -1.376705E-9 UB = 2.283988E-18
+UC = 4.585445E-11 VSAT = 1.233076E5 A0 = 1.9044296
+AGS = 0.4187403 B0 = 3.768681E-7 B1 = 5E-6
+KETA = -7.542091E-3 A1 = 0 A2 = 0.6017329
+RDSW = 105 PRWG = 0.5 PRWB = -0.2
+WR = 1 WINT = 0 LINT = 2.02308E-8
+XL = 0 XW = -1E-8 DWG = -3.807594E-9
+DWB = 1.068482E-8 VOFF = -0.0948017 NFACTOR = 2.1860065
+CIT = 0 CDSC = 2.4E-4 CDSCD = 0
+CDSCB = 0 ETA0 = 2.722866E-3 ETAB = 6.028975E-5
+DSUB = 0.0169785 PCLM = 0.9517499 PDIBLC1 = 0.2819015
+PDIBLC2 = 1.777888E-3 PDIBLCB = -0.1 DROUT = 0.8756738
+PSCBE1 = 1.693724E9 PSCBE2 = 1.087562E-9 PVAG = 0
+DELTA = 0.01 RSH = 6.6 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 = 8.06E-10 CGSO = 8.06E-10 CGBO = 1E-12
+CJ = 9.49893E-4 PB = 0.8 MJ = 0.3794582
+CJSW = 2.73954E-10 PBSW = 0.8 MJSW = 0.1405486
+CJSWG = 3.3E-10 PBSWG = 0.8 MJSWG = 0.1405486
+CF = 0 PVTH0 = -3.287967E-4 PRDSW = -0.7911922
+PK2 = 1.224586E-3 WKETA = 1.156014E-3 LKETA = -8.317948E-4
+PU0 = 5.4645434 PUA = -3.6636E-12 PUB = 0
+PVSAT = 1.281655E3 PETA0 = 5.04222E-5 PKETA = -2.434571E-3 )
*
.MODEL CMOSP PMOS ( LEVEL = 49
+VERSION = 3.1 TNOM = 27 TOX = 4E-9
+XJ = 1E-7 NCH = 4.1589E17 VTH0 = -0.3723517
+K1 = 0.582664 K2 = 0.025102 K3 = 0
+K3B = 7.8640626 W0 = 1E-6 NLX = 1.119035E-7
+DVT0W = 0 DVT1W = 0 DVT2W = 0
+DVT0 = 0.7283176 DVT1 = 0.2728546 DVT2 = 0.1
+U0 = 103.9954725 UA = 1.104002E-9 UB = 1.966409E-21
+UC = -1E-10 VSAT = 1.627261E5 A0 = 1.8594332
+AGS = 0.4028628 B0 = 3.925957E-7 B1 = 7.24909E-7
+KETA = 0.0255352 A1 = 0.3805726 A2 = 0.3
+RDSW = 314.5914718 PRWG = 0.5 PRWB = 0.0474718
+WR = 1 WINT = 0 LINT = 3.454427E-8
+XL = 0 XW = -1E-8 DWG = -2.154664E-8
+DWB = 7.096045E-9 VOFF = -0.086282 NFACTOR = 1.9157973
+CIT = 0 CDSC = 2.4E-4 CDSCD = 0
+CDSCB = 0 ETA0 = 5.405243E-4 ETAB = -4.331663E-5
+DSUB = 0 PCLM = 1.1570147 PDIBLC1 = 3.444441E-3
+PDIBLC2 = -1E-5 PDIBLCB = -1E-3 DROUT = 0
+PSCBE1 = 9.035097E9 PSCBE2 = 3.439858E-9 PVAG = 0
+DELTA = 0.01 RSH = 7.5 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 = 6.5E-10 CGSO = 6.5E-10 CGBO = 1E-12
+CJ = 1.156831E-3 PB = 0.8394653 MJ = 0.4087666
+CJSW = 2.186128E-10 PBSW = 0.8 MJSW = 0.3058017
+CJSWG = 4.22E-10 PBSWG = 0.8 MJSWG = 0.3058017
+CF = 0 PVTH0 = 2.442628E-3 PRDSW = 7.6708227
+PK2 = 2.159356E-3 WKETA = 0.0248885 LKETA = -4.739423E-3
+PU0 = -1.5943037 PUA = -6.13575E-11 PUB = 1E-21
+PVSAT = -50 PETA0 = 8.732925E-5 PKETA = 3.424629E-3 )
*
-----------------------------------------------------------------------------------------------------------------------------

We have tried to design with Kn=342.4µA/V2 and Kp=72.2µA/V2 w.ref to value given in library (K' (Uo*Cox/2) 171.2 -36.1uA/V^2) and threshold voltage Vt also we selected from library as Vth=0.5V and ΔVth=0.08 as we saw in some modes, Vth=0.42V as given below :
------------------------------------------------------------------------------------------------
TRANSISTOR PARAMETERS W/L N-CHANNEL P-CHANNEL UNITS
MINIMUM 0.27/0.18
Vth 0.50 -0.50 volts
SHORT 20.0/0.18
Idss 602 -306 uA/um
Vth 0.51 -0.50 volts
Vpt 4.7 -5.4 volts
WIDE 20.0/0.18
Ids0 32.5 -29.6 pA/um
LARGE 50/50
Vth 0.42 -0.41 volts
Vjbkd 3.2 -4.1 volts
Ijlk <50.0 <50.0 pA
-----------------------------------------------------------------------------------------------------------------------
We donot know why, after designing, opamp is not working correctly. We designed for UGB = 150 MHz and SR=30V/us for a supply of 0-5V. With this we get only 33Mhz UGB and open loop gain is also only 77dB. Why could this be happening? What change should we make in our design to correct it.

Sizes of transistor we obtained are :
S1=S2=462
S3=S4=11
S5=S8=2
S6=1553
S7=141
Cc = 3pF, Cl=10pF and Ibias=90µA
Where S=W/L. Should we keep L=0.18u or can we keep it as 1u? Also is there a max limit on the width and length of transistors of the library.

Thanks in advance.

Regards,
abdj

 

[erikl]

Re: transconductance parameter

Could you please share a mos hspice model library you are using which is working correctly for us to try some circuits. We would like to have level49 library for which we know accurate Kn, Kp, Vth, ΔVth values.

It depends on what you intend: If you want to get a chip fabricated, it's a MUST to get the libraries (actually the full PDK) from that fab/foundry. If you just want to "play around" until you get a working circuit - for educational purpose, or just because of interest in analog design - you could use any (h)spice model library which is publicly available, e.g. from .

We do not know why, after designing, opamp is not working correctly. We designed for UGB = 150 MHz and SR=30V/us for a supply of 0-5V. With this we get only 33Mhz UGB and open loop gain is also only 77dB. Why could this be happening? What change should we make in our design to correct it.

Manual calculations provide only a rough approximation to the reality. Simulations take into account many more effects (if the models used provide the respective parameters) and so are indispensable to achieve a working circuit.

Should we keep L=0.18u or can we keep it as 1u?

For high accuracy analog design -- where good matching is necessary -- always L > Lmin is used (by a factor 3..5), this however trades accuracy for speed: if high UGB is your priority, stay close to Lmin. There are so many dependencies between various circuit specifications; all this analog design stuff is taught in universities and by textbooks, you have to study it.

Also is there a max limit on the width and length of transistors of the library.

This is quite usual, as it limits the validity of the models for a certain accuracy. Sometimes several different models are used for various W & L ranges.

 

[abdj_project]

Re: transconductance parameter

Hi Erikl,
Thanks a lot for the info. We were able to design the circuits using the 180 nm library Level 49 ( where Kp= 72.2 µA/V2 , Kn= 342.4µA/V2)

We have another query regarding the noise analysis . Can you please guide us on the steps we should follow to perform noise analysis in Hspice . What all parameters need to be taken in to account( like Af, kf, tnoimod , fnoimod, NLEV, GDSNOI for Level1 ) for the flicker and thermal noise analysis in Level 49 ?

Thanks in advance
Regards,
abdj