Sir/mam
i have written a .CIR file containg only capacitor and inductor,
Capacitor initially charged to 60V and initial condition of inductor is zero
there is only two elements in the circuit (Capacitor is directly connected to inductor)
and done transient analysis for current across inductor
there is no resistor in my circuit
so the expected output should a sine wave with no attenuation
but .PROBE is showing attenuation of current value through Inductor with time
i am confused how this is possible as there is no resistor in my circuit
so,please help me to overcome my confusion
i have also copied and pasted my .CIR file fo your convenience:
Example 10
C1 1 0 2.55u ic=60V
L1 1 0 200M ic=0
.tran 0.01 0.5 uic
.probe I(L1)
.end
Copyright © 2020 Cadence Design Systems, Inc. All rights reserved.
I think the resistance of the coil, parasitic capacitances and the losses in the core are considered in the model. Probably that's the reason for the attenuation in current.
Hi Tejas,
Is there any way i can remove it in Pspice?
Hello Sourav,
The current response in LC tank depends on model that you have used for each component in PSpice simulator.
I have inserted the LTSpice result below.
Thanks,
Janayya
Thanks Janayya for your kind information,
can i plot the same in Pspice?
Hi Sourav,
You will get the same result in PSpice, Just specify a "Max step Size" say 100ns. Given below is cir file text
************************************************************************
.lib "nom.lib"
.TRAN 0 400m 0 100n
.PROBE64 I(L_L1)
C_C1 1 0 2.55u IC=60
L_L1 1 0 200m IC=0
************************************************************************
Regards,
Nitin
Thanks a lot nitint sir,thank you so much
Hello,
You would also have to select as method for the simulation "trapezoidal". It is right, that it works with 100n, but it does not make any sense that for a particular max step size it seems to have a resistance and for another value of max step size it seems to work properly. The only cause of this is the simulation method that is being used. For this case, just select trapezoidal.
Regards
Hi RobertoGb
how can we select Trapezoidal Simulation??
Hi,
In simulation settings, in the tab Options select in the left pan the option Transient inside of Analog Advanced. There you will find the Property Name "METHOD". Just click on it and select Trapezoidal.
Regards
Hi RobertoGb,
i am not able to find Simulation Settings in Psipce A/D,
please guide me where is it?
i have also uploaded a snapshot of the same for your convenience
click in this link for the snapshot
https://ibb.co/mKCz8k
with thanks
Hello,
I just forgot that you are working with .cir. Just include this command:
.OPTIONS METHOD= Gear
And select Gear or Trapezoidal
Regards
Hi RobertoGb,
but Trapezoidal Settings aren't giving exact data values!!
for example in the above problem mentioned by me:
I(C1) should be -1.689E-01 at t=4.000E-01
but using Trapezoidal settings it is giving I(C1) = -3.313E-02 at t= 4.000E-01
Hi,
If you use a 100ns for the Max Step Size, it does not mather if you use Trapezoial or Gear method, both results are the same one. However, if you use for example Max Step Size = 1ms, the results with the trapezoidal is correct and with the gear one not.
PSpice default method is a mix of GEAR and TRAPEZOIDAL, with Gear being used at times to prevent numerical ringing. Gear is a more stable integration method, while Trapezoidal is faster and more accurate. PSpice sometimes prefers Gear for numerical stability when it detects oscillations in data. However, this can be less accurate, especially for oscillatory circuits, like the one you proposed.
Regards
thanks a lot
Hi Everyone,
Can anyone tell me what is the default "Max Step Size" in Pspice A/D ?
and how it is different from "print step value"?
for eg.:
.tran 0.01 0.5 0 100ns
here, "print step value" = 0.01 sec ,
"Max step size" = 100ns
Hi Sourav,
Max Step Size:
Spice simulators have dynamic time step control algorithm, which forces simulator to take small steps in case voltages/currents are changing rapidly. On the other hand if nothing much is happening dynamically in a circuit, it increases the time step to improve simulation performance. So by using max step size you schedule parameter changes according to the value entered in
Maximum Step Size text box in the Simulation Profile.
print step value:
Print Step controls how often optional text format data is written to the simulation output file (*.OUT). Unlike max step size it is not linked to the solver algorithms.
Hope this helps!
Thanks
Thank you dshikhar
it solved my queries