I dont know what this error means LTSpice - Page 1
Forum section: electronics / general

author: alexdecaran
author_rank: Newbie
timestamp: July 11, 2021, 09:41:14 am
content: Hi, this is my first post on the forum, although Ive been reading it for quite some time now. The thong is that I dont know how to solve this error in LTSPICE. I am trying to measure a 3 phase line to line voltage and then transform it from diferential to single ended (This part is not finished yet).Can any more experienced user take a look?

author: Ian.M
author_rank: Super Contributor
timestamp: July 11, 2021, 11:02:25 am
content: You've included "AMC3330.lib" twice, once as a library from the ModelFile attribute of the symbol and the other explicitly on your schematic as.inc AMC3330.lib- remove one and that error goes away.However once that's fixed it throws (in the SPICE Error Log):Fatal Error: Undefined subcircuit: stdopampwhich is because there is no model for stdopamp in AMC3330.lib, which is written for T.I's TinaTI simulator.The only useful reference I could find googlingTina-TI stdopampwas on Stackexchange, and from it I dug out this model:Code:* STANDARD OPERATIONAL AMPLIFIER MACROMODEL SUBCIRCUIT* CREATED USING 08/05/06* (REV 1.53 03/05/16, simplified 1.5, VDROPOL referenced to VP ).SUBCKT STDOPAMP INP INM VP VM OUT+ PARAMS: GAIN=200K RIN=2MEG RINC=1E9 CIN=1p CINC=1p ROUT=75 SLEWRATE=500K FPOLE1=5+ VDROPOH=1.9 VDROPOL=1.9*FPOLE2=1MEG*.PARAM PI = 3.141592.PARAM IS = 1.0E-12.PARAM VT = 0.02585.PARAM IMAX = 100.0E-2.PARAM C1 = {IMAX/SLEWRATE}.PARAM R1 = {1/(2*PI*C1*FPOLE1)}.PARAM GM1 = {GAIN/R1}*.PARAM R2 = 100*.PARAM G2 = {1/R2}.PARAM GOUT = {1/ROUT}*.PARAM C2 = {1/(2*PI*R2*FPOLE2)}.PARAM VDF = {VT*LOG(1 + IMAX/IS)}*RINM1 INM VP {2*RINC}RINM2 INM VM {2*RINC}RINP1 INP VP {2*RINC}RINP2 INP VM {2*RINC}RIN INM INP {RIN}CINM1 INM VM {CINC}CINP1 INP VM {CINC}CIN INM INP {CIN}*EVP VPI 0 VALUE = { V(VP)-(VDROPOH + VDF) }EVM VMI 0 VALUE = { Limit(V(VP)-(VDROPOL - VDF), V(VM) + VDF, V(VP) + VDF) }EVP VPI 0 VALUE = { Limit(V(VP)-(VDROPOH + VDF), V(VM) + VDF, V(VP)) }GIQ VP VM VALUE = {5M*ABS(V(P1,OUT))}GMO2 VM OUT P1 VM {0.5*GOUT}RO2 OUT VM {2*ROUT}GMO1 OUT VP VP P1 {0.5*GOUT}RO1 VP OUT {2*ROUT}*C2 P2 GND {C2}*R2 P2 GND {R2}*GM2 GND P2 P1 GND {G2}EGND GND 0 POLY(2) (VP,0) (VM,0) 0 .5 .5D3 VMI P1 D_1D2 P1 VPI D_1C1 P1 GND {C1}R1 P1 GND {R1}*GM1 GND P1 VALUE = { LIMIT( GM1*V(INP,INM), -IMAX, IMAX) }GM1 GND P1 VALUE = { IF (TIME < 1e-30, GM1*V(INP,INM), LIMIT( GM1*V(INP,INM), -IMAX, IMAX)) }*GM1 GND P1 VALUE = { Limit( V(VP,VM)/(Abs(-VDROPOH + VDROPOL)+1m), 0, 1 )*IF (TIME < 1e-30, GM1*V(INP,INM), LIMIT( GM1*V(INP,INM), -IMAX, IMAX)) }.MODEL D_1 D( IS={IS} XTI=0 EG=0.8).ENDSAdding that model gets us a step further but it still isn't fixed. I then get:u1:amp:input:c3: both pins shorted together -- ignoring.Fatal Error: Voltage source E:U1:HLDO:U1:GND is shorted making an over-definedcircuit matrix...You will need to correct the circuit or add some series resistance.which I believe *may* be due to the topology of your circuit round the AMC3330. As I hate reverse engineering large models in netlist format to readable schematics, I am disinclined to investigate further.Maybe use the Tina-TI simulator the model was designed for?

author: alexdecaran
author_rank: Newbie
timestamp: July 11, 2021, 11:05:46 am
content: Thank you so much!!! You've been super helpful, Ill try to use TINA.