Author Topic: I dont know what this error means LTSpice  (Read 1395 times)

0 Members and 1 Guest are viewing this topic.

Offline alexdecaranTopic starter

  • Newbie
  • Posts: 2
  • Country: es
I dont know what this error means LTSpice
« on: July 11, 2021, 09:41:14 am »
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?

 

Offline Ian.M

  • Super Contributor
  • ***
  • Posts: 13216
Re: I dont know what this error means LTSpice
« Reply #1 on: July 11, 2021, 11:02:25 am »
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: stdopamp

which 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 googling Tina-TI stdopamp
was on Stackexchange, and from it I dug out this model:
Code: [Select]
* 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 .5

D3         VMI P1  D_1
D2          P1 VPI  D_1
C1          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)
.ENDS

Adding 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-defined
  circuit 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?





 

Offline alexdecaranTopic starter

  • Newbie
  • Posts: 2
  • Country: es
Re: I dont know what this error means LTSpice
« Reply #2 on: July 11, 2021, 11:05:46 am »
Thank you so much!!! You've been super helpful, Ill try to use TINA.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf