0
\$\begingroup\$

I would like to model a low pass filter in LTSpice, but my frequency response looks like a bandpass, similar to an RLC filter.

enter image description here

Is LTSpice incapable of simulating LC filters with an RC one?

\$\endgroup\$
3
  • 1
    \$\begingroup\$ Try changing the bottom end of the X axis to 10 kHz and the top to 100 MHz. It may look more like you expect. \$\endgroup\$
    – vofa
    Feb 7 at 17:43
  • \$\begingroup\$ Nope that is not the problem, this would just shift the peak I expect something similar to this google.com/… \$\endgroup\$
    – Phönix 64
    Feb 7 at 17:45
  • 2
    \$\begingroup\$ Changing the sweep range can not change the circuit's behavior or shift its resonant frequency. You are zoomed in on the resonance, which is there because you have no damping in your circuit. Zoom out. \$\endgroup\$
    – vofa
    Feb 7 at 17:50

4 Answers 4

4
\$\begingroup\$

It looks like a low pass filter to me but with very high Q. That isn't a surprise because you have not restricted the Q of the circuit with either a load resistor or series resistor. The effect of high Q is that you get a massive resonant peak in the mid range that is fogging your eyes from seeing the truth. Look more closely and add some resistance.

Here's what your spectrum looks like on my reasonably-adequate-but-not-crazy-in-yer-face-sparkly website low-pass filter calculator with 0.1 Ω series resistance: -

enter image description here

As you can see, the peak goes off the scale (feature alert) but, if we lowered the Q by increasing the resistance to something like 100 Ω it looks a little more reasonable: -

enter image description here

\$\endgroup\$
0
6
\$\begingroup\$

To expand on the other two answers, here is what you are plotting:

Your plot 5MHz - 10MHz linear sweep. The height of the peak depends on the simulation resolution.

If you change to a 10kHz-100MHz decade sweep, you get this: Decade sweep You can still see the large resonance, and the overall low pass characteristic.

\$\endgroup\$
2
\$\begingroup\$

As others have pointed out, your circuit is high-Q which will exhibit peaking. The Q is limited by LTspice's default series resistance of 1 mohm for the inductor.

The following example shows what happens when you use different resistor values (1k, 2k, 4k, 100k) to change the Q of the circuit using LTspice's .step function. The green trace is when R1 = 1k, the cyan trace is when R1 = 100k. Using a resistor in series with the inductor, instead of a resistor in parallel with the capacitor, will also work.

LPF simulation

In the future, you should refer to a guide on designing RLC filters. There are many books on the subject and also some good online calculators.
Online filter calculator

My favorite book: "Simplified Modern Filter Design", by Philip Geffe, is an old book (1963) with intuitive explanations that most filter books leave out. You may be able to find this in a university library.

\$\endgroup\$
1
  • \$\begingroup\$ Thanks for sharing the book I will look into it \$\endgroup\$
    – Phönix 64
    Feb 7 at 20:43
1
\$\begingroup\$

to complement Andy aka's answer (it's correct):

LTSpice Plot

Circuit

Inductor Setting

Capacitor Setting

\$\endgroup\$
3
  • \$\begingroup\$ 1 megohm is an exceptionally high ESR for a capacitor. Did you mean to put that value in the equivalent parallel resistance box instead? \$\endgroup\$
    – The Photon
    Feb 7 at 18:09
  • \$\begingroup\$ simulates just fine with lower values too \$\endgroup\$
    – schnedan
    Feb 7 at 18:13
  • \$\begingroup\$ I think you meant pF instead of pC for the capacitance value. pC is picocoulombs. Fortunately, SPICE traditionally considers on the first character of the unit. \$\endgroup\$ Feb 7 at 18:41

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.