Continue to Site

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.

Current in series resonant circuit

Status
Not open for further replies.

SvendD

Banned
Joined
Jun 4, 2018
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1
Activity points
0
Hi

I have series resonant circuit made in LTspice. And was wondering why I do not get the "correct" current. I have attached the circuit and the result.
Unavngivet.png

The circuit have a resonant at approximately 44 Hz. I use a 50 Hz tone with an amplitude of 100V. I then calculate the current and get 790mA. But the simulation give me a peak of 737mA.

My question is why? A LTspice setup issue?

Kind regards
 

Hi,

You ask ask why your calculation is not correct. But you don't show how you calculated it.

Klaus

Added:
I just recognized that you think LTspice is wrong.
But I still think it's a good idea to review your own maths.
 

I'm not going to dive into the math but I'll suggest you run an AC simulation. Then you'll have a chart of current vs frequency and can easily check your calculations at more points, verify the resonant frequency etc. Perhaps create a spreadsheet with your calculations and graph your own curve.

Then you'll have more information in a nice visual form to figure out where the discrepancy might be.
 

I then calculate the current and get 790mA.
Your calculation for idealized devices is correct, but if you want a more realistic result you should consider that LTspice models take into account parasitic elements which are present in actual devices, as for example, the highest inductor, the highest series resistance, which means that for an inductor of about 1H, its series resistance would lie in the same range of the above active load (R1), that is, close to a hundred ohms. In short, for "real-world" devices, the current would be likely much smaller than what was calculated.
 

Thank you for the answers.
I understand, I just thought that LTspice used ideal components? I can see that an inductor has several parameters but all of these are not entered. An inductor has per default 1mohm series resistance, which I sat to zero.
 

Your calculation for idealized devices is correct, but if you want a more realistic result you should consider that LTspice models take into account parasitic elements which are present in actual devices, as for example, the highest inductor, the highest series resistance, which means that for an inductor of about 1H, its series resistance would lie in the same range of the above active load (R1), that is, close to a hundred ohms. In short, for "real-world" devices, the current would be likely much smaller than what was calculated.

LTSpice basic R/L/C models don't generally include parasitics. An exception is the L model which, as noted when you open up its properties dialog defaults to 1mOhm.

C's and R's have no parasitics in my understanding.
 

LTSpice basic R/L/C models don't generally include parasitics. An exception is the L model which, as noted when you open up its properties dialog defaults to 1mOhm.

C's and R's have no parasitics in my understanding.

Perhaps the V1 voltage source could have an inner serial output resistance?
Indded, according to calculations the current should lie in the range of 790mA.
 

I encountered this sort of puzzle. As we know there are the standard formulae for inductive & capacitive reactance:

XL= 2 Pi f L

XC= 1 / (2 Pi f C)

My calculated result did not match the simulator current (even though it was close).

An article reminded me about the further refinement we are supposed to make to our initial calculation (if we want accuracy). Namely to draw those inconvenient parallelogram angles, taking into account the phase change.

Fortunately a simulator makes it easier for us to compare scenarios. Example, AC current through a series RL, compared to AC current through a resistor whose value we adjust until it passes the identical amount of current. Then calculate the impedance contributed by the inductor.
 

Running an AC sim with start and stop frequencies the same causes LTSpice to produce a text report rather than a graph.

The result for this circuit is: 0.785246

Running transient sim with an extra small time step to ensure good resolution gives: 785.21886mA

Pretty close, don't know what to say about the remaining discrepancy.
 

Decrease Transient Simulation Step.
The simulator gives a rough value..

Or

The component models are out of accuracy. ( for instance 1.3 H , it's huge )
Be aware that every element in any simulator is in fact a mathematical model, not a real component.
 
Last edited:
Hi,

The result for this circuit is: 0.785246
This is what my hand math gives.

I still wonder about the OP's calculation.

Klaus
 

I think the reson is that you used a time step too large. Try with something like 1us
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top