Simulation Error

Anonymous · ‎10-22-2020

When simulating my instrumentation amplifier, I am getting this error message

PPerror: syntax error

Note: No ".plot", ".print", or ".fourier" lines; no simulations run

This is my system Netlist:

* SpiceNetList

*

* Exported from Instrumentation.sch at 10/22/2020 12:51 PM

*

.TEMP=25.0

* --------- .OPTIONS ---------

.OPTIONS ABSTOL=1e-12 GMIN=1e-12 PIVREL=1e-3 ITL1=100 ITL2=50 PIVTOL=1e-13 RELTOL=1e-3 VNTOL=1e-6 CHGTOL=1e-15 ITL4=10 METHOD=TRAP SRCSTEPS=0 TRTOL=7 NODE

* --------- .PARAMS ---------

* --------- devices ---------

V_V2 VCC 0 SIN(0 5 10)

R_R35 N_40 N_42 240

X_U4 VCC1 N_40 N_42 VCC -VS 0 MEASURE +VS ad8226

V_V4 VCC1 0 SIN(0 7 10)

V_V1 +VS 0 9V

V_V3 -VS 0 -9V

* --------- models ---------

* model file: C:/Users/Suzanna/Documents/EAGLE/spice/ad8226.mdl

* AD8226 SPICE Macro-model

* Description: Amplifier

* Generic Desc: 36V Bipolar InAmp Low Cost&Power G1-1000

* Developed by: PRB IAP ADI

* Revision History: 08/10/2012 - Updated to new header style

* 3.0 (09/2009)

*

* Refer to http://www.analog.com/Analog_Root/static/techSupport/designTools/spiceModels/license/spice_general.h... for License Statement. Use of this model

* indicates your acceptance with the terms and provisions in the License Statement.

*

* BEGIN Notes:

*

* Not Modeled:

*

* Parameters modeled include:

*

* END Notes

*

* Node assignments

* inverting input

* | RG

* | | RG

* | | | non_inverting input

* | | | | negative supply

* | | | | | ref

* | | | | | | output

* | | | | | | | positive supply

* | | | | | | | |

.SUBCKT AD8226 IN- RG- RG+ IN+ -Vs REF VOUT +Vs

** INPUT STAGE

R1 N009 N008 50E3

R2 N008 Inverting_Out 50E3

R3 N013 noninverting_out 50000

R4 REF N013 50k

R5 RG- N003 24700

R6 RG+ N012 24724

D3 N003 P001 D

D4 P002 N003 D

V3 P002 VNEGx 0.84

V4 VPOSx P001 .61

D5 N012 P003 D

D6 P004 N012 D

V5 P004 VNEGx 0.84

V6 VPOSx P003 .61

D7 N005 P005 D

D8 P006 N005 D

V7 P006 VNEGx 0

V8 VPOSx P005 0

D9 N019 P007 D

D10 P008 N019 D

V9 P008 VNEGx 0

V10 VPOSx P007 0

D11 N009 P009 D

D12 P010 N009 D

V11 P010 N016 0.750

V12 N010 P009 0.83

D13 REF P011 D

D14 P012 REF D

V13 P012 VNEGx .3

V14 VPOSx P011 .3

D15 N013 P013 D

D16 P014 N013 D

V15 P014 VNEGx 0.6

V16 VPOSx P013 0.6

E4 Inverting_Out 0 N003 0 1

E5 noninverting_out 0 N012 0 1

Q1 Inv_Fdbk N002 RG- 0 PNP

Q2 Pos_Fdbk N015 RG+ 0 PNP

V1 VBIAS -Vs -10

I1 Pos_Fdbk VBIAS 2E-6

I2 Inv_Fdbk VBIAS 2E-6

C1 N003 Inv_Fdbk 4.035e-12

C2 N012 Pos_Fdbk 4.0e-12

E8 N002 0 N005 0 1

E9 N015 0 N019 0 1

VOSI_Neg N004 IN- 25E-6

VOSI_Pos IN+ N017 24E-6

VOSO VOUT N011 300E-6

C3 RG- 0 .242e-12

C4 RG+ 0 .1635e-12

I23 IN- 0 -22.3E-9

I24 IN+ 0 -22E-9

G1 0 IN+ N020 N021 .7e-9

R13 IN+ N020 10e9

R14 N020 IN- 10e9

R15 +Vs N021 10e9

R16 N021 -Vs 10e9

G2 0 IN- N020 N021 .7e-9

E10 VPOSx 0 +Vs 0 1

I3 +Vs -Vs 300E-6

E11 VNEGx 0 -Vs 0 1

R17 VBIAS Inv_Fdbk 10e9

R18 Pos_Fdbk VBIAS 10e9

H3 N006 N004 V24 14

V24 N001 0 0

R19 N001 0 .0166

H4 N011 N009 V25 100

V25 N007 0 0

R20 N007 0 .0166

H5 N018 N017 V26 14

V26 N014 0 0

R21 N014 0 .0166

G4 0 N005 N006 N005 1E-3

G5 0 N019 N018 N019 1E-3

G6 0 N003 VBIAS Inv_Fdbk 1

G7 0 N012 VBIAS Pos_Fdbk 1

G8 0 N009 N013 N008 1

R10 N005 0 10e9

R7 N003 0 10E9

R11 N019 0 10E9

R8 N012 0 10E9

R9 N009 0 10E9

H1 VPOSx N010 POLY(1) VOSO 0 0 8000

H2 N016 VNEGx POLY(1) VOSO 0 0 8000

* MODELS USED

*

.model D D

.model PNP PNP (BF=10E5 VAF=20000)

.ENDS AD8226

* --------- simulation ---------

.control

set filetype=ascii

DC V_V2 10 100 0.18

write Instrumentation.sch.sim V(+VS) V(MEASURE) I(V_V3) I(V_V1) I(V_V4) I(V_V2)

.endc

.END

Can u help me find a way out. Thanks.

holger.vogt · ‎10-28-2020

I only recently have discovered this blog, and my answer of course will be too late to serve any immediate needs, but still there is an answer.

You are using node names like +VS and -VS in your netlist. ngspice-26 cannot cope with these node names (which include math characters). So the remedy simply might be to use VSP and VSN or so.

ngspice-33 will do the simulation, but still fail when executing the 'write' command. This is happening because the 'write' command will allow using equations of vectors (thas is node values) to be written, not only plain vectors. The function parser cannot distinguish between + - / being part of a node name or being part of an equation and therefore bails out.

I am preparing a new ngspice version which allows to set a switch, to do writing without equations, just saving plain vectors (node values). Then many additional characters are allowed for node names, not just alphanumerical characters.

ngspice-33 already has better error messaging, for example this error message would have shown the offensive line and column.

Anonymous · ‎10-28-2020

Thank you so much holger.vogt. This helps. I am able to simulate the circuit

Community

Simulation Error

Simulation Error

Simulation Error