OPA191IDR orcad spice model

Sunil,

Orcad Spice model is SPICE compatible model thus it's the same as Tina-TI Spice model available on our website - see below.

Just in case, I have attached it in this post.

OPA191.CIR

I have checked with Tina-TI spice model and with the OPA191.cir just attached in post.
Steps followed in according to sloa070.pdf.
In my circuit I am using LMP2021 and OPA191. I could model LMP2021 and simulate successfully.
where as when I am working with OPA191 following are the errors which I have encountered.

ERROR(ORPSIM-15108): Subcircuit VCVS_LIMIT_0 used by X_U1.XU17 is undefined

ERROR(ORPSIM-15108): Subcircuit VNSE_0 used by X_U1.XVn11 is undefined

ERROR(ORPSIM-15108): Subcircuit FEMT_0 used by X_U1.XIn11 is undefined

ERROR(ORPSIM-15108): Subcircuit D_D_0 used by X_U1.XD1 is undefined

ERROR(ORPSIM-15108): Subcircuit D_D_0 used by X_U1.XD2 is undefined

ERROR(ORPSIM-15108): Subcircuit JFET_TG_0 used by X_U1.XT1 is undefined

ERROR(ORPSIM-15108): Subcircuit JFET_TG_0 used by X_U1.XT2 is undefined

ERROR(ORPSIM-15108): Subcircuit JFET_TG_0 used by X_U1.XT3 is undefined

ERROR(ORPSIM-15108): Subcircuit JFET_TG_0 used by X_U1.XT4 is undefined

ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_0 used by X_U1.XR109 is undefined

ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_0 used by X_U1.XR109_2 is undefined

ERROR(ORPSIM-15108): Subcircuit OVLD_THRES_0 used by X_U1.XU7 is undefined

ERROR(ORPSIM-15108): Subcircuit OVLD_THRES_0 used by X_U1.XU2 is undefined

ERROR(ORPSIM-15108): Subcircuit OL_CNTL_0 used by X_U1.XU16 is undefined

ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_0 used by X_U1.XU15 is undefined

ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_1 used by X_U1.XU14 is undefined

ERROR(ORPSIM-15108): Subcircuit CLMP_AMP_0 used by X_U1.XU3 is undefined

ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_2 used by X_U1.XU1 is undefined

ERROR(ORPSIM-15108): Subcircuit CLMP_AMP_0 used by X_U1.XU13 is undefined

ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_2 used by X_U1.XU12 is undefined

ERROR(ORPSIM-15108): Subcircuit CLMP_AMP_0 used by X_U1.XU11 is undefined

ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_3 used by X_U1.XU10 is undefined

ERROR(ORPSIM-15108): Subcircuit CLMP_AMP_0 used by X_U1.XU9 is undefined

ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_3 used by X_U1.XU8 is undefined

ERROR(ORPSIM-15108): Subcircuit VCVS_EXT_LIMIT_0 used by X_U1.XVcm is undefined

ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_0 used by X_U1.XR109_3 is undefined

ERROR(ORPSIM-15108): Subcircuit VCVS_LIMIT_1 used by X_U1.XU5 is undefined

ERROR(ORPSIM-15108): Subcircuit VCVS_LIMIT_2 used by X_U1.XU6 is undefined

ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_4 used by X_U1.XU26 is undefined

ERROR(ORPSIM-15108): Subcircuit VCCS_LIMIT_5 used by X_U1.XU4 is undefined

ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_0 used by X_U1.XR109_4 is undefined

ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_1 used by X_U1.XR104 is undefined

ERROR(ORPSIM-15108): Subcircuit RNOISE_FREE_1 used by X_U1.XR103 is undefined

Pls help

Sunil,

I'm not an expert on Orcad simulator but contrary to your error messages all of the subcircuits are defined - see below:

ERROR(ORPSIM-15108): Subcircuit VCVS_LIMIT_0 used by X_U1.XU17 is undefined

*VOLTAGE CONTROLLED SOURCE WITH LIMITS
.SUBCKT VCVS_LIMIT_0 VC+ VC- VOUT+ VOUT-
*
.PARAM GAIN = 88
.PARAM VPOS = 21.8K
.PARAM VNEG = -21.8K
E1 VOUT+ VOUT- VALUE={LIMIT(GAIN*V(VC+,VC-),VNEG,VPOS)}
.ENDS VCVS_LIMIT_0

ERROR(ORPSIM-15108): Subcircuit VNSE_0 used by X_U1.XVn11 is undefined

* BEGIN PROG NSE NANO VOLT/RT-HZ
.SUBCKT VNSE_0 1 2
* BEGIN SETUP OF NOISE GEN - NANOVOLT/RT-HZ
* INPUT THREE VARIABLES
* SET UP VNSE 1/F
* NV/RHZ AT 1/F FREQ
.PARAM NLF=48
* FREQ FOR 1/F VAL
.PARAM FLW=100
* SET UP VNSE FB
* NV/RHZ FLATBAND
.PARAM NVR=19
* END USER INPUT
* START CALC VALS
.PARAM GLF={PWR(FLW,0.25)*NLF/1164}
.PARAM RNV={1.184*PWR(NVR,2)}
.MODEL DVN D KF={PWR(FLW,0.5)/1E11} IS=1.0E-16
* END CALC VALS
I1 0 7 10E-3
I2 0 8 10E-3
D1 7 0 DVN
D2 8 0 DVN
E1 3 6 7 8 {GLF}
R1 3 0 1E9
R2 3 0 1E9
R3 3 6 1E9
E2 6 4 5 0 10
R4 5 0 {RNV}
R5 5 0 {RNV}
R6 3 4 1E9
R7 4 0 1E9
E3 1 2 3 4 1
.ENDS
* END PROG NSE NANOV/RT-HZ

ERROR(ORPSIM-15108): Subcircuit FEMT_0 used by X_U1.XIn11 is undefined

* BEGIN PROG NSE FEMTO AMP/RT-HZ
.SUBCKT FEMT_0 1 2
* BEGIN SETUP OF NOISE GEN - FEMPTOAMPS/RT-HZ
* INPUT THREE VARIABLES
* SET UP INSE 1/F
* FA/RHZ AT 1/F FREQ
.PARAM NLFF=1.5
* FREQ FOR 1/F VAL
.PARAM FLWF=1E-3
* SET UP INSE FB
* FA/RHZ FLATBAND
.PARAM NVRF=1.5
* END USER INPUT
* START CALC VALS
.PARAM GLFF={PWR(FLWF,0.25)*NLFF/1164}
.PARAM RNVF={1.184*PWR(NVRF,2)}
.MODEL DVNF D KF={PWR(FLWF,0.5)/1E11} IS=1.0E-16
* END CALC VALS
I1 0 7 10E-3
I2 0 8 10E-3
D1 7 0 DVNF
D2 8 0 DVNF
E1 3 6 7 8 {GLFF}
R1 3 0 1E9
R2 3 0 1E9
R3 3 6 1E9
E2 6 4 5 0 10
R4 5 0 {RNVF}
R5 5 0 {RNVF}
R6 3 4 1E9
R7 4 0 1E9
G1 1 2 3 4 1E-6
.ENDS
* END PROG NSE FEMTO AMP/RT-HZ

etc.

Thus the problem must be related to the way you import the OPA191 nelist into Orcad or the way you assign the pin names - they must match the following:  

.SUBCKT OPA191 +IN -IN V+ V- Vout

Hello Ian Williams and Marek Lis.

Followed as per the shared ppt. I have not changed any of the pin no.s or any other parameters.

Still I have following errors

.LIB "C:\Program Files (x86)\Tina Industrial 9.3\SPICELIB\ICDEVS.LIB"
*
* CONNECTIONS: A
* | C
* | |

ERROR(ORPSIM-15116): Unable to find library file "C:\Program Files (x86)\Tina Industrial 9.3\SPICELIB\ICDEVS.LIB".

Index has 4 entries from 1 file(s).

ERROR(ORPSIM-15107): Unable to make index for library file C:\Cadence\SPB_16.5\tools\capture\library\OPA191.lib.

ERROR(ORPSIM-15460): Subcircuit OPA191 is undefined

Pls suggest. 

Thanks Ian Williams. Finally I could simulate.

Project file you shared I couldn't simulate but from that folder I took the model with which my simulation was successful.

If possible can you say why this might had happen?

Hello Sunil,

I'm glad you were able to get the simulation running. I have only started using Cadence recently, but my best guess for why you weren't able to run my project directly is because the required libraries were referenced to locations on my computer. When running from your machine, the references needed to get updated to locations on your local machine.

Best regards,

Ian Williams