15 posts / 0 new
Last post
#1 Aug 10, 2017
sourav
Offline
Last seen: 4 days 17 hours ago
Joined: 2017-07-29 06:48

Getting unknown resistance

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

 

 

Fri, 2017-08-25 12:34
Tejas Pangal
Offline
Last seen: 1 month 3 weeks ago
Joined: 2017-08-24 00:43

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. 

Sun, 2017-08-27 04:50 (Reply to #2)
sourav
Offline
Last seen: 4 days 17 hours ago
Joined: 2017-07-29 06:48

Hi Tejas,

Is there any way i can remove it in Pspice?

Sat, 2017-08-26 02:10
janayya
Offline
Last seen: 3 weeks 13 hours ago
Joined: 2017-07-26 03:05

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

Sun, 2017-08-27 04:54 (Reply to #4)
sourav
Offline
Last seen: 4 days 17 hours ago
Joined: 2017-07-29 06:48

Thanks Janayya for your kind information,

can i plot the same in Pspice?

Sun, 2017-08-27 10:52
nitint
Offline
Last seen: 1 month 2 weeks ago
Joined: 2017-08-27 09:47

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

 

Mon, 2017-08-28 12:47 (Reply to #6)
sourav
Offline
Last seen: 4 days 17 hours ago
Joined: 2017-07-29 06:48

Thanks a lot nitint sir,thank you so much

Wed, 2017-09-13 04:36
RobertoGb
RobertoGb's picture
Offline
Last seen: 11 hours 39 min ago
Joined: 2016-05-24 03:10

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

Sat, 2017-09-16 06:13 (Reply to #8)
sourav
Offline
Last seen: 4 days 17 hours ago
Joined: 2017-07-29 06:48

Hi RobertoGb

how can we select Trapezoidal Simulation??

Mon, 2017-09-18 03:15 (Reply to #9)
RobertoGb
RobertoGb's picture
Offline
Last seen: 11 hours 39 min ago
Joined: 2016-05-24 03:10

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

Mon, 2017-09-18 07:45 (Reply to #10)
sourav
Offline
Last seen: 4 days 17 hours ago
Joined: 2017-07-29 06:48

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

Mon, 2017-09-18 07:54
RobertoGb
RobertoGb's picture
Offline
Last seen: 11 hours 39 min ago
Joined: 2016-05-24 03:10

Hello,

I just forgot that you are working with .cir. Just include this command:

.OPTIONS METHOD= Gear

And select Gear or Trapezoidal

Regards

Mon, 2017-09-18 08:33 (Reply to #12)
sourav
Offline
Last seen: 4 days 17 hours ago
Joined: 2017-07-29 06:48

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

Tue, 2017-09-19 08:02 (Reply to #13)
RobertoGb
RobertoGb's picture
Offline
Last seen: 11 hours 39 min ago
Joined: 2016-05-24 03:10

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 

Tue, 2017-09-19 10:41 (Reply to #14)
sourav
Offline
Last seen: 4 days 17 hours ago
Joined: 2017-07-29 06:48

thanks a lot

Download PSpice Lite and try it for free! Get PSpice Lite
Cadence