Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Pspice InAmp AD620 model not working

Status
Not open for further replies.

middlehein

Newbie level 5
Joined
Aug 5, 2012
Messages
10
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,398
So I am trying to model a AD620 inamp from anolog devices and have their Lib with the AD620 in it and am trying to use that with a basic circuit. I am new to Capture CIS pspice and cannot seem to get the circuit to work without the convergence failing. I thought it might be a floating ref point, but everything is grounded so I am not sure where I am going wrong here. Below is the output and a picture of the circuit.

InAmpmodel not working.png

** Creating circuit file "sweep.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:
* Profile Libraries :
* Local Libraries :
* From [PSPICE NETLIST] section of C:\Cadence\SPB_16.3\tools\PSpice\PSpice.ini file:
.lib "nom.lib"

*Analysis directives:
.TRAN 0 100ms 0
.OPTIONS STEPGMIN
.PROBE N([N00559])
.PROBE N([N00480])
.PROBE N([N00493])
.INC "..\SCHEMATIC1.net"



**** INCLUDING SCHEMATIC1.net ****
* source SCIM IN-AMP TEST
X_U1 N00493 N00489 N00572 N00965 N00559 0 N00180 N00187 AD620/AD
C_C1 N00480 N00493 .1u TC=0
C_C2 N02797 N00489 .1u TC=0
R_R1 N00187 N00180 10meg TC=0,0
C_C3 N00572 0 .33u TC=0
C_C4 N00572 0 .01u TC=0
C_C5 N00965 0 .33u TC=0
C_C6 N00965 0 .01u TC=0
R_R2 N00493 0 1meg TC=0,0
R_R3 0 N00559 1k TC=0,0
V_V1 N00480 0
+SIN 0 1 1000 0 0 0
V_V2 N00572 0 15Vdc
V_V3 0 N00965 -15Vdc
V_V4 N02797 0
+SIN 0 1 500 0 0 0
R_R4 N00489 0 1meg TC=0,0

**** RESUMING sweep.cir ****
.END

**** 08/04/12 20:22:37 ******* PSpice 16.3.0 (June 2009) ****** ID# 0 ********

** Profile: "SCHEMATIC1-sweep" [ C:\Users\heinx055\Desktop\Circuit anaylsis\scim in-amp test-pspicefiles\schematic1\sweep.sim ]


**** Diode MODEL PARAMETERS


******************************************************************************




X_U1.DX X_U1.DY
IS 1.000000E-12 1.000000E-12
BV 50


**** 08/04/12 20:22:37 ******* PSpice 16.3.0 (June 2009) ****** ID# 0 ********

** Profile: "SCHEMATIC1-sweep" [ C:\Users\heinx055\Desktop\Circuit anaylsis\scim in-amp test-pspicefiles\schematic1\sweep.sim ]


**** BJT MODEL PARAMETERS


******************************************************************************




X_U1.QN1 X_U1.QN2
NPN NPN
LEVEL 1 1
IS 100.000000E-18 100.000000E-18
BF 10.000000E+03 250
NF 1 1
BR 1 1
NR 1 1
ISS 0 0
RE 0 0
RC 0 0
CJE 0 0
VJE .75 .75
CJC 0 0
VJC .75 .75
MJC .33 .33
XCJC 1 1
CJS 0 0
VJS .75 .75
KF 700.000000E-18 5.000000E-15
AF 1 1
CN 2.42 2.42
D .87 .87


ERROR -- Convergence problem in transient bias point calculation


Last node voltages tried were:

NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE


(N00180) -.6352 (N00187) -.6355 (N00480) 0.0000 (N00489)-309.0E-06

(N00493)-583.9E-06 (N00559) 12.4040 (N00572) 13.7430 (N00965) 13.7430

(N02797) 0.0000 (X_U1.3)-584.1E-06 (X_U1.4)-309.1E-06 (X_U1.5) 13.2850

(X_U1.6) 13.2850 (X_U1.9) -.6352 (X_U1.10) -.6355

(X_U1.11) 13.2850 (X_U1.12) 13.7000

(X_U1.13) 13.7430 (X_U1.14) 13.1260

(X_U1.15) 13.7000 (X_U1.16) 13.7430

(X_U1.17) 13.1260 (X_U1.18) 13.1060

(X_U1.19) -.6356 (X_U1.21)-570.4E-06

(X_U1.25) 13.6520 (X_U1.26) 12.3420

(X_U1.27) 14.9620 (X_U1.36) 1.0545

(X_U1.38) 12.5920 (X_U1.40) 13.5630

(X_U1.41) 13.9160 (X_U1.42) 10.8920

(X_U1.43) 13.1880 (X_U1.44) 64.1980

(X_U1.45) 12.4040 (X_U1.51) 13.1020

(X_U1.52) 13.1020 (X_U1.53) 14.3850

(X_U1.54) 14.3850 (X_U1.98) 12.5920


These voltages failed to converge:

V(N00559) = 12.48V \ 12.40V
V(X_U1.38) = 13.74V \ 12.59V
V(X_U1.98) = 13.74V \ 12.59V
V(X_U1.40) = 13.66V \ 13.56V
V(X_U1.36) = -446.46uV \ 1.055V
V(X_U1.45) = 12.48V \ 12.40V
V(X_U1.41) = 13.99V \ 13.92V
V(X_U1.42) = 10.97V \ 10.89V

These supply currents failed to converge:

I(X_U1.EREF) = 12.50nA \ 12.44nA
I(X_U1.E3) = 13.74uA \ 11.54uA
I(X_U1.L1) = 9.480mA \ 9.394mA
I(V_V2) = 10.00GA \ 10.00GA
I(V_V3) = 10.00GA \ 10.00GA
I(X_U1.V6) = -10.00GA \ -10.00GA
I(X_U1.V7) = -10.00GA \ -10.00GA

ERROR -- Discontinuing simulation due to convergence problem
**** Interrupt ****
 

Try using solver 0 instead of 1 (1 is the default). You can change it in simulation settings -> options -> advanced.
 

just tried solver 0, and it again failed. One thing I notice is that it says the device X_U1.D14 failed to converge which seems to always be the problem. Is there maybe something wrong with the AD620 model?? I cant figure this out.
 

You want V3 to be +15 instead of -15. Change it and see if that helps.

- - - Updated - - -

I just tried your circuit and it converged fine with solver 0 and correct V3 -- in all other cases it failed to converge.

 
Last edited:

You want V3 to be +15 instead of -15. Change it and see if that helps.

Yes, a typical error. Allocating a negative value to a negative voltage source will result in a positive value.
 

You want V3 to be +15 instead of -15. Change it and see if that helps.

Major thanks to you, that seems to have solve the problem and made me realize what a idiot I am. I had looked at that though it appeared the power source was right because I had - to - and + to +, I completely overlooked that double negative.
 

Major thanks to you, that seems to have solve the problem and made me realize what a idiot I am. I had looked at that though it appeared the power source was right because I had - to - and + to +, I completely overlooked that double negative.

No worries and that is a really common mistake. Save the self-abuse for when you make a stupid mistake that actually deserves it. :lol:

Glad you got it working. Convergence problems are generally a pain - not really the thing you want to be spending design time on.
 

sorry one quick question, I am wandering what are the different solvers.
 

I am not too familiar with the technical details of the solvers, so I can't give you a detailed answer. Solver 0 is the original PSpice algorithm, Solver 1 (the default) was introduced in a later version with a claimed performance increase.

From the PSpice manual back from ver 10.2:

(Solver = 0 selects the original solution algorithm;
Solver = 1 selects the advanced solution algorithm)
Default: 0 (In PSpice A/D Basics), 1 (In all other PSpice products)

Later it goes on to say:

PSpice now contains two solution algorithms for simulation. Solver 1 increases simulation speed over Solver 0, particularly for larger circuits with substantial runtimes. Solver 1 has slightly better convergence characteristics than Solver 0. Having both algorithms available improves convergence, since there are two different algorithms that can perform the simulation.

However, I generally experience more convergence problems, especially with simpler circuits, using algorithm 1.

From ftp://ftp.ehu.es/cidira/dptos/depjt/sistemas de potencia/transparencias/guia sobre convergencia.pdf:

Solver 1 and Solver 0 are two matrix solving algorithms used by PSpice. By default, Solver 1 that has better convergence property, is used. But at times, for a circuit with convergence problems changing the simulation algorithm to Solver 0 helps.

A general rule of thumb seems to be: Try it with solver 1, and if it fails and you've checked your circuit for obvious errors, try it with solver 0.
 

That's not true. Solver 1 is faster and would have superior convergence for most of circuits. PSpice 16.3 also has AUTOCONVERGANCE feature. Which would work for majority of circuits.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top