Hi so I below is a tuned RF amp for 7.2 Mhz. I have one LC circuit coupled to another LC circuit, both are set to be at a center frequency of 7.2 Mhz but when I simulate my circuit to an AC analysis it shows that my center frequency is around 5.2 MHz. Am I doing somethinf wrong?

Thanks

 

When you inductively couple an inductor as in a transformer, the overall inductance seen on the primary changes... this may be what you are experiencing....

 

When one stage "loads" another stage it changes both of them. Have you done a complex conjugate match?

http://www.electronics-tutorials.com/basics/q.htm
http://en.wikipedia.org/wiki/Impedance_matching
http://www.fourier-series.com/rf-concepts/smithchart.html

 

Certainly,there is some effect on the primary inductance,but not enough to change the resonant frequency by nearly 30%.

Consider the retro-type instrument beloved by Hams,--the Grid Dip Oscillator (GDO).

This consists of a tube oscillator,with the inductor of its resonant circuit mounted on the front of the instrument.

In use,this coil is brought in the proximity of a resonant circuit,& the GDO oscillator is tuned through its range.

At the resonant frequency of the circuit being tested,the GDO's grid current drops (dips) ,due to the other circuit "stealing" some energy from the GDO tuned circuit

The GDO dip is broader when it is closely coupled,& narrows as coupling is reduced,but the centre frequency remains the same.

Coupling mainly affects the "Q" of the tuned circuit,not its resonant frequency.
Either you are doing something wrong,or there is a "bug" in LTSpice.

PS:It might be wise to put some decoupling on the V2 line & try again.

 

I don't know how to calculate the equivalent inductance, but if you simulate those unity-coupled resonators, the resonant frequency is equal to what you would get with a single inductor of the same value, and the two capacitors in parallel with it. See attachment. If you assume the capacitance is 270pF, the inductance calculates to be 3.84uH.

EDIT: LTspice does not make errors on simple passive circuits like this.

 

In my comments re the GDO above,I did not take into account the classic case of "overcoupling",as in the GDO case,& many others,this level of coupling is seldom reached.

As coupling is increased beyond "critical coupling",the response begins to take on a "double-humped" shape,with resonant peaks above & below the "centre frequency".

The centre frequency is at,or very close to, the resonant frequency of each circuit considered separately.

These links cover this subject:

http://www.ee.bgu.ac.il/~intrlab/lab_number_7/Two inductively coupled RLC circuits.pdf

http://frank.yueksel.org/other/RCA/Radiotron_Designers-Handbook_Fourth-Edition/09-Tuned-Circuits.pdf

Perhaps LTSpice was not set to sweep higher in frequency & did not see the higher frequency peak.

 

These links cover this subject:

http://www.ee.bgu.ac.il/~intrlab/lab_number_7/Two inductively coupled RLC circuits.pdf

Perhaps LTSpice was not set to sweep higher in frequency & did not see the higher frequency peak.

You would have to sweep a long way as for k=1 the lower peak is at Fo/√2 (as observed) and the upper one at infinity.

 

You would have to sweep a long way as for k=1 the lower peak is at Fo/√2 (as observed) and the upper one at infinity.

That's what I think too. Can you explain the theory?
I ran another simulation, with the two tanks rsonating separately at 9.9MHz and 10.1MHz. With k=1, LTspice put one peak at Fr=1/(2*pi*√(L*(C1+C2)), where L=1uH, C1=258.4pF, and C2=248.3pF.
There was actually another peak at 315GHz, but I suspect it was an artifact of the limits of mathematical precision.

 

You would have to sweep a long way as for k=1 the lower peak is at Fo/√2 (as observed) and the upper one at infinity.

I apologise for not picking up on this,but I guess,as a Tech,I'm not used to working with the impossible!

My version of LTSpice is not functional,(not sure why,& haven't yet tried to fix it) so I couldn't download the OP's simulation.
Does it use k=1 for its default, or did he make a mistake?

 

I apologise for not picking up on this,but I guess,as a Tech,I'm not used to working with the impossible!

My version of LTSpice is not functional,(not sure why,& haven't yet tried to fix it) so I couldn't download the OP's simulation.
Does it use k=1 for its default, or did he make a mistake?

He has K1 set to 1 on his schematic (K1 L1 L3 1).

 

Yep,Ron,I see it now!

I guess I don't speak LTSpice!

The OP is a beginner with RF,so it was probably just an oversight on his part.
A "K" of around 0.2 might have been more appropriate.

 

Yep,Ron,I see it now!

I guess I don't speak LTSpice!

The OP is a beginner with RF,so it was probably just an oversight on his part.
A "K" of around 0.2 might have been more appropriate.

You're probably right. And, as you know better than I do, the response is highly dependent on the value of "K". As you pointed out, a grid (or gate) dip oscillator can be used to tune the circuit, including the coupling.
Or, if you happen to have a spectrum analyzer lying around...

 

That's what I think too. Can you explain the theory?
I ran another simulation, with the two tanks rsonating separately at 9.9MHz and 10.1MHz. With k=1, LTspice put one peak at Fr=1/(2*pi*√(L*(C1+C2)), where L=1uH, C1=258.4pF, and C2=248.3pF.
There was actually another peak at 315GHz, but I suspect it was an artifact of the limits of mathematical precision.

The paper in the link shows the analysis. For a symmetric circuit like this, odd and even mode analysis shows it quite clearly. Even simpler, when k=1, for equal coils, you can simply move the load on the secondary to the primary (as long as it was floating), so it is equivalent to a resonator with the same L and with 2C, hence frequency reduced by 1/√2.