Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

How to generate impulse response in pspice

Status
Not open for further replies.

analogpr

Newbie level 4
Joined
Jan 13, 2014
Messages
7
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
66
Hi! I am using vpulse source in order to extract the impulse response of a circuit. I use
V1=0
V2=1Meg
TR=1n
TF=1n
PW=1u
However, the simulation pauses and the following window appears. What should i do?
PspiceSetting.jpg
 

analogpr

Newbie level 4
Joined
Jan 13, 2014
Messages
7
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
66
The same window appears again
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
49,419
Helped
14,441
Reputation
29,146
Reaction score
13,239
Trophy points
1,393
Location
Bochum, Germany
Activity points
284,388
You didn't report the error message that appears before the runtimes settings dialog...
 

analogpr

Newbie level 4
Joined
Jan 13, 2014
Messages
7
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
66
I am sorry, you are right FvM. I get these messages:
ERROR(ORPSIM-15138): Convergence problem in transient analysis at Time = 1.001E-06.
These supply currents failed to converge:
I(E_READOUT_E1) = -6.022mA \ -6.015mA
ERROR(ORPSIM-15660): These devices failed to converge
X_READOUT_U1.Q_Q5
X_READOUT_U1.Q_Q9
X_READOUT_U1.Q_Q14
X_READOUT_U1.Q_Q12
X_READOUT_U1.Q_Q11
ERROR(ORPSIM-15661): 5 of 5 errors shown. See output file for complete list
INFO(ORPROBE-3185): Simulation paused

Can i ask you something else? Can i use these values
V1=0
V2=1Meg
TR=1n
TF=1n
PW=1u
with a pulse source in the input of OPA 657(commercial opamp, pspice model) with a negative feedback of course?
Thanks in advance
 

crutschow

Advanced Member level 5
Joined
Feb 22, 2012
Messages
3,983
Helped
940
Reputation
1,878
Reaction score
945
Trophy points
1,393
Location
Colorado USA Zulu -7
Activity points
22,535
Your problem is with convergence. Go to the Spice Analysis (Edit Simulation Command) and try selecting the "Skip Initial Operating Point" and/or the "Start External DC Supply Voltage at 0V" to see if that helps. If not try reducing the accuracy of the parameters in the "Spice" panel of the Tools\Control Panel window by a factor of ten.

A V2 value 1 million volts should not be needed for an adequate impulse response signal. Try a value of perhaps 10V to start. You can vary the value to see if affects the output response. When you find little change in the response then you know going to a higher voltage will have no significant effect on the result.
 

LvW

Advanced Member level 5
Joined
May 7, 2008
Messages
5,858
Helped
1,746
Reputation
3,496
Reaction score
1,346
Trophy points
1,393
Location
Germany
Activity points
39,555
analogpr, which max. time step did you select (if any?) for the TRAN simulation?
 

FvM

Super Moderator
Staff member
Joined
Jan 22, 2008
Messages
49,419
Helped
14,441
Reputation
29,146
Reaction score
13,239
Trophy points
1,393
Location
Bochum, Germany
Activity points
284,388
If your circuit doesn't attenuate 1Meg volts to a level within the OP ratings, no meaningful simulation results can be expected. What are you trying to achieve?
 

analogpr

Newbie level 4
Joined
Jan 13, 2014
Messages
7
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
66
max step size= 0.1u

- - - Updated - - -

I just want to compare the impulse response of an ideal filter with the impulse response of a filter realized by real opamp
 

LvW

Advanced Member level 5
Joined
May 7, 2008
Messages
5,858
Helped
1,746
Reputation
3,496
Reaction score
1,346
Trophy points
1,393
Location
Germany
Activity points
39,555
I just want to compare the impulse response of an ideal filter with the impulse response of a filter realized by real opamp

And what do you expect to get at the opamp output (real model with supply limits) with such a huge input signal ? Impulse response?
 

dick_freebird

Advanced Member level 5
Joined
Mar 4, 2008
Messages
7,570
Helped
2,186
Reputation
4,378
Reaction score
2,080
Trophy points
1,393
Location
USA
Activity points
60,487
You cannot get an impulse (zero width, zero risetime). It
is an idealization.

You could make your source properties "good enough" but
this can challenge the simulator's ability to keep up, as
you see.

Setting minimum timestep lower than risetime would help
solving, but make runtimes unacceptable perhaps. You
may instead perfer to:

- tighten transient voltage and current tolerances
- increase iteration limits for transient by the same
factor that you tightened tolerances (rough guess)
- select a numerical method that converges better
than the default one (Euler, TrapGear2)

Now what "good enough" is, wants some thought as
well. You probably don't need to challenge a 1MHz
op amp with sub-nS risetimes and pulse widths, and
you don't need to feed a 5V op amp a 1kV input
amplitude either. What you want is enough harmonic
content that you can see what you need to see,
within constraints of linear input amplitude range
and so on - ideal filter response being a relevant
point of comparison, only if what you're comparing
is operating linear (or maybe you want to know that
it indeed is - but that still needs you to make it so,
or try).
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top