hi everyone

I have finished my design in OrCad capture v9.1.I have used the libaries from pspice and the circuit as shown in the image does not have any results.I have biult the circiut on a braedboard an it worked just fine.What i need from the simulation results is the signal plots.

Here is what i get from pspice

--------------- Simulation Profile: SCHEMATIC1-trial ---------------
Simulation running...
** circuit file for profile: trial
Reading and checking circuit
Circuit read in and checked, no errors
Calculating bias point for Transient Analysis
Starting power supply stepping
Convergence problem in transient bias point calculation
These voltages failed to converge:
V(N00268) = -15783.9 / -15746.1
V(N00318) = -15755.4 / -15718.1
V(N00305) = -15755.4 / -15718.1
V(N00265) = -15812.4 / -15774.1
V(N00292) = -15753.8 / -15716.5
5 of 32 errors shown. See Additional Info for complete list...
These supply currents failed to converge:
I(X_U3.egnd) = -0.0145334 / -0.0143071
I(X_U1.egnd) = 0.0145334 / 0.0143071
I(X_U3.vb) = -4.03935e-006 / -3.76304e-006
I(X_U3.vc) = -0.0103194 / -0.0101437
I(X_U3.ve) = 4.23898e-010 / 4.21974e-010
5 of 9 errors shown. See Additional Info for complete list...
These devices failed to converge:
X_U1.fb
Unable to calculate bias point
See output file for details
Simulation complete



Thnx

Ps the request for this project where to use capture and pspice only.

Attached Images

trial_3.jpg (46.0 KB, 591 views)

 

here is the netlist

* source NEW
X_U3 N00268 GND +15V -15V N00292 LM318
X_U1 GND N00305 +15V -15V N00265 LF411
R_R5 N00268 N00318 10k
C_C1 N00305 N00265 1n
R_R1 N00318 N00305 {100k*0.5+.001}
R_R3 N00292 N00318 560
R_R4 N00265 N00268 10k
D_D1 N00456 N00318 D1N4001
D_D2 N00318 N00462 D1N4001
D_D3 N00456 GND D1N4001
D_D4 GND N00462 D1N4001

 

My approach would be to break the circuit so that you are only simulating the first amp, then add the second, and finally the third. I usually just attach a dummy load to the amp. This will narrow where the possible problem is in your simulation. I am not familiar with that version of spice, but the -15000 when it is trying to linearize the circuit about the bias point looks suspicious.

 

There are no voltage sources in your netlist. Simply naming a node "+15V" does not apply a voltage to it. You need to add batteries.

Something is wrong with your diode clamp circuit. I suspect D3 and D4 are backwards. As an aside, I think 1N4148s would work somewhat better than 1N4001s.

 

Thnx but the the damm circuit still will not work on pspice...I put in some dc power supplies fot the +/-15 v needed fot the op-amps but still i get a ton of errors

new netlist source NEW
X_U2 N01668 GND_POWER N01551 N01554 N01678 LM318
X_U3 GND_POWER N01823 N01560 N01557 N01665 LF411
V_V1 N01560 GND_POWER 15Vdc
V_V2 GND_POWER N01557 -15Vdc
V_V3 GND_POWER N01554 -15Vdc
V_V4 N01551 GND_POWER 15Vdc
C_C1 N01823 N01665 1n
R_R4 N01681 N01823 {1k*0.5+.001}
R_R1 N01665 N01668 10k
R_R2 N01678 N01681 560
R_R3 N01668 N01681 10k

the pspice error

--------------- Simulation Profile: SCHEMATIC1-again1 ---------------
Simulation running...
** circuit file for profile: again1
Reading and checking circuit
Circuit read in and checked, no errors
Calculating bias point for Transient Analysis
Starting power supply stepping
Convergence problem in transient bias point calculation
These voltages failed to converge:
V(N01560) = -1.8516e+008 / -2.09455e+008
V(GND_POWER) = -1.8516e+008 / -2.09455e+008
V(N01557) = -1.8516e+008 / -2.09455e+008
V(N01554) = -1.8516e+008 / -2.09455e+008
V(N01551) = -1.8516e+008 / -2.09455e+008
5 of 32 errors shown. See Additional Info for complete list...
These supply currents failed to converge:
I(X_U2.egnd) = 0.0765222 / 0.0069206
I(X_U3.egnd) = 0.0551153 / 0.0326354
I(X_U2.vb) = -3.18479e-005 / -2.39829e-005
I(X_U2.vlim) = 0.0230456 / 0.0225084
I(X_U2.vlp) = 5.98241e-006 / -2.19366e-007
5 of 11 errors shown. See Additional Info for complete list...
These devices failed to converge:
X_U2.dlp
X_U3.dln
X_U2.fb
X_U3.fb
X_U3.j1
5 of 7 errors shown. See Additional Info for complete list...
Discontinuing simulation due to convergence problem
Unable to calculate bias point
See output file for details
Simulation complete



As there are no errors what can be wrong?

Attached Images

skata.jpg (34.3 KB, 561 views)

 

Your -15v supplies are double negated. You need to either reverse those two batteries, or change them to +15v. Also, I think you need to leave the diodes in the circuit, but reverse the polarities of D3 and D4. I don't know if it will converge after this change. If it doesn't, try putting initial conditions (.IC) on the input and output pins of the LF411. Set the input IC to zero volts and the output IC to 5 volts.

Also, the ground doesn't look right. How did you get GND_POWER? Did you change symbols? The previous netlist had GND. Here's the clue: "V(GND_POWER) = -1.8516e+008 / -2.09455e+008". I don't think ground should show up with a convergence error. Ground is the reference for all voltages in the circuit.

 

@Ron Finally finally the circuit works

Muchos muchos gracias

I changed the power supply as described and i also changed the ground in the circuit using the 0/source capysm and it finally works...I can finally relax now :wink:

@ everyone Have a merry christmas and i hope u all spend some quality time with youre loved ones...

thnx again