[SOLVED] Convergence problem in transient bias point calculation

[Iulian Cepoiu]

hi
I am new here and was wondering if you can help me with this error (PSPICE)

**** INCLUDING pac-SCHEMATIC1.net ****
* source PAC
C_C1         GND N00143  1u  
R_R1         N00246 N00290  10k  
X_10k    N00290 GND N00143 SCHEMATIC1_10k 
X_U1         N00143 N00246 +15 -15 N00290 uA741

.subckt SCHEMATIC1_10k 1 2 t  
RT_10k         1 t {(1K*(1-0.5))+.001}
RB_10k         t 2 {(1K*0.5)+.001}
.ends SCHEMATIC1_10k

**** RESUMING pac-SCHEMATIC1-pac.sim.cir ****
.END

**** 10/26/14 16:55:42 ************** PSpice Lite (Mar 2000) *****************

 ** Profile: "SCHEMATIC1-pac"  [ C:\pac-SCHEMATIC1-pac.sim ] 


 ****     Diode MODEL PARAMETERS


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




               X_U1.dx         
          IS  800.000000E-18 
          RS    1            


**** 10/26/14 16:55:42 ************** PSpice Lite (Mar 2000) *****************

 ** Profile: "SCHEMATIC1-pac"  [ C:\pac-SCHEMATIC1-pac.sim ] 


 ****     BJT MODEL PARAMETERS


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




               X_U1.qx         
               NPN             
          IS  800.000000E-18 
          BF   93.75         
          NF    1            
          BR    1            
          NR    1            
          CN    2.42         
           D     .87

ERROR -- Convergence problem in transient bias point calculation


Last node voltages tried were:

NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE


( +15) 3.210E+06 ( -15) 3.210E+06 ( GND) 3.210E+06 (N00143) 3.210E+06

(N00246) 3.210E+06 (N00290) 3.210E+06 (X_U1.6) -.0124 (X_U1.7) 3.210E+06

(X_U1.8) 3.210E+06 (X_U1.9) 0.0000 (X_U1.10) 3.210E+06

(X_U1.11) 3.210E+06 (X_U1.12) 3.210E+06

(X_U1.13) 3.210E+06 (X_U1.14) 3.210E+06

(X_U1.53) 3.210E+06 (X_U1.54) 3.210E+06

(X_U1.90) 290.0E-06 (X_U1.91) 40.0000

(X_U1.92) -40.0000 (X_U1.99) 3.210E+06


These voltages failed to converge:

V(GND) = 10.00GV \ 3.210MV
V(N00143) = 10.00GV \ 3.210MV
V(N00246) = 10.00GV \ 3.210MV
V(N00290) = 10.00GV \ 3.210MV
V(X_U1.11) = 10.00GV \ 3.210MV
V(X_U1.12) = 10.00GV \ 3.210MV
V(X_U1.6) = 14.89KV \ -12.35mV
V(X_U1.7) = 10.00GV \ 3.210MV
V(X_U1.53) = 10.00GV \ 3.210MV
V(X_U1.54) = 10.00GV \ 3.210MV
V(X_U1.90) = 2.363KV \ 290.03uV
V(-15) = 10.00GV \ 3.210MV
V(+15) = 10.00GV \ 3.210MV
V(X_U1.99) = 10.00GV \ 3.210MV
V(X_U1.10) = 10.00GV \ 3.210MV
V(X_U1.13) = 10.00GV \ 3.210MV
V(X_U1.14) = 10.00GV \ 3.210MV
V(X_U1.8) = 10.00GV \ 3.210MV

These supply currents failed to converge:

I(X_U1.egnd) = -3.070mA \ -643.99pA
I(X_U1.vb) = -2.232A \ -123.50nA
I(X_U1.vc) = -2.277A \ -54.37uA
I(X_U1.ve) = 60.22mA \ -54.24uA
I(X_U1.vlim) = 2.363A \ 290.03nA
I(X_U1.vlp) = 2.323nA \ -40.00pA
I(X_U1.vln) = -2.403nA \ -40.00pA
I(X_U1.hlim) = -4.726nA \ -580.16e-18A

These devices failed to converge:
X_U1.dc X_U1.de X_U1.dlp X_U1.fb X_U1.q1 X_U1.q2

ERROR -- Discontinuing simulation due to convergence problem

 

[FvM]

It's a trivial problem caused by a typical PSpice beginners problem.

You'll notice that the initial transient solution shows, among other a node voltage ( GND) 3.210E+06.

"GND" isn't the PSpice reference potential. It's a node name associated with the ground symbol used in your simulation circuit. Instead you'll use the "analog ground" symbol which is connected to node "0", the actual PSpice ground node.

 

[BigBoss]

PSPICE like simulation programs don't like "floating points" and they frequenctly stop due to this error.There is a floating point in your circuit ( V_ of the OPAMP because of very high impedance ) and you'd better to connect a 1G Ohm or 100M Ohm ( for instance ) from this node to GND.
You circuit might be unstable too, check the stability by AC simulation creating Bode Gain and Phase response.

 

[Iulian Cepoiu]

Thank you! the GND were the problem.