I want to measure a 32.768 kHz crystal resonator (not oscillator) in the frequency and the time domain using a ZURICH HF2LI instrument, which is a network analyzer and oscilloscope in one unit.

The measurement set up is shown below:

enter image description here

For the frequency response:

The "Signal Output 1" is set to have a voltage of 20 [mV] and the "Signal Input 1" is set to have an input impedance of 50 ohm. The instrument has the ability to switch input impedance between 50/1Meg ohm.

The result of the frequency response is shown below:

frequency response

For the magnitude plot (upper trace) of the frequency response, it shows that there is a resonance peak at about 32.7673 kHz which is close to the specification of the 32.768 kHz resonator. It also shows that with 20 mV voltage input, it will output a -100.3 dBV RMS voltage at the 50 ohm input impedance of the instrument, which after my calculation is about 9.66 uV RMS voltage.

Based on this calculation, I would guess that when I use an Oscilloscope function (time response) and give the crystal resonator 20 mV input voltage at 32.7673 kHz it would have a sinusoidal waveform with a voltage peak of 13.66 mV, but the result isn't as expected.

Time response using the oscillscope:

time response

The "Signal Output 1" is set to have a voltage of 20 mV and the "Signal Input 1" is set to have a imput impedance of 1Meg ohm instead told. The instrument has the ability to switch imput impedance between 50/1Meg ohm.

As the result shows, the output voltage is strongly distorted, can't even cleary see a sine wave.

From above discription, I reorganized my questions below

  1. For frequency response and time response measurement, why shuold I change the input impedance from 50 ohm to 1Meg ohm? Could be any relation to calculate? For example, I measured the frequency response both at 50 and 1Meg ohm input impedance. Is there a relation between these two measurement results?
  2. Why can't I match the measurement result between frequency and time response as descibed above?

Have I misunderstood something?

Update:2023/02/23 Sorry for the late reply! The reason why my Rm value is so high is that i'm using another type of resonator in my measurement so the Rm result is not normal compare to the crystal one.

During these days, I have been thinking why for both two different input impedance, the calculated Rm couldn't match even when i swept for a finner range at reasonce with more step.

By my guess, would it caused by the transmission line? So I've done some simulation using transmission line model to verify my assumption and let's start again from the beginning.

Question: Why i couldnt match the calculated result between diffiernt input impedance in a same device?

My assumption: First let's take a look at the measurement result. measurement result fig1. Measurement results at different HF2LI input impedance

And from the measurement result, we could extract the equivalent circuit's element value, I used the 50 [ohm] one in this case. enter image description here fig2. Simulation model at different load (left) and extracted parameter value (righ) base on 50 [ohm] measurement result.

After having the parameter, I used the model (without transmission line effect) in fig2. in LTspice and the results are shown below. enter image description here fig3. Comparison between measurement and simulate results (without transmission line effect)

We could notice that there is a about 7 [dB] difference between measurement and simulate at 1_meg [ohm] || 20 [pF] input impedance, which means that the measurement result of the signal is "lower" than the simulation.

In my understanding (Or maybe i'm wromg), when the impedance is not matching, some of the signal power will loss during transmission.

In this case, the SMA cable has characteristic impedance of 50 [ohm] but for the instrument it has 50 [ohm] and 1_meg [ohm] || 20 [pF] input impedance. Which in real case, I used the SMA cable and connected to the 1_meg [ohm] || 20 [pF] input impedance and resulted in impedance unmatching that will cause the signal "attenuated".

So to verified my assumption, I added a "tranmission line" model in the simulation: enter image description here fig.4 Simulation model with transmission line effect

The characteristic impedance of the cable can calculate using the parameter in fig4. with equation Z0=sqrt(L/C) and L=9 [nH], C=3.59 [pF] here.

The simulate result is shown: enter image description here fig5. Comparison between measurement and simulate results (with transmission line effect)

The result seems perfectly matched but I have some questions remained. How to choose "R" and "len" using LTRA in LTspice? I couldnt find any corresponding in formation. The value i used in this case is referring to another post below LTspice, how to model a TLine

All above is my assumption and I'm not sure whether I'm in a right direction ,any advice will be very helpful to me.


  • 1
    \$\begingroup\$ If this instrument's detector is actually calibrated in units of dBV, then the graph's peak at -100 dBV is about 10 uV, not 13.66 mV \$\endgroup\$
    – glen_geek
    Commented Feb 17, 2023 at 14:48
  • \$\begingroup\$ The non-symmetric frequency response of the upper plot suggests that sweep speed may be too-fast. Can you slow this acquisition? or sweep through the peak with smaller step size? \$\endgroup\$
    – glen_geek
    Commented Feb 17, 2023 at 14:56
  • \$\begingroup\$ @glen_geek , thanks for your remind, I have corrected the wrong value. About the sweep speed and step size concern, I'll do it a liittle bit later! \$\endgroup\$
    – Jack Huang
    Commented Feb 18, 2023 at 1:08
  • \$\begingroup\$ @glen_geek, I have cahnge both sweep speed and step size in a finner way, the response at reasonace change to -90.55 [dBV] (increase about 10 [dBV]), but still can't see a sin waveform from the oscillscope. Will the reason that it could caused by the noise interference? \$\endgroup\$
    – Jack Huang
    Commented Feb 18, 2023 at 8:40
  • \$\begingroup\$ @JackHuang - Hi, You wrote an "answer" but it wasn't the answer to your original question. It was additional info, so it has been added to your question as an edit (i.e. an update) instead. || Since you asked the question, unless you are writing the full & final answer to your own question (i.e. unless you have solved the problem yourself & don't need further help) please don't use the box labeled "Your Answer" below. Instead, to add more information / clarification, please edit the question. Or comment to respond to a minor point. || Please see the tour & help center for more rules. Thanks. \$\endgroup\$
    – SamGibson
    Commented Feb 19, 2023 at 14:06

1 Answer 1


A simulation base on an ABRACON AB26T crystal.
Two different loads are simulated (1 Megohm to the left, 50 ohm to the right), using the same crystal model. Both are excited from V1 with a 0.02 VRMS sine wave source. The 1MEG load resistor has added to it the 12.5 picofarad capacitance suggested by the data sheet...which causes a resonant peak very close to 32768 Hz.

In the OP's setup, cable capacitance, along with instrument input capacitance may differ from 12.5 pf. (This capacitance is only relevant for the high-impedance 1M load resistance):
schematic crystal excitation with 1MEG, 50 ohm loads

A sweep showing magnitude (solid line) and phase (dashed line) for both 1M and 50 ohm loads is shown below. Amplitude across the 50 ohm load resistor peaks at -94 dBV (20 microvolts).
When loaded with 1MEG, 12.5pF, amplitude peaks much higher at -30.6 dBV (29.5 millivolts) at a frequency very close to 32768 Hz:magnitude, phase plot

For transient response, V1 excites with similar 20mV source at 32768 Hz, for 10,000 cycles...at the 0.305 second point, excitation drops to zero, and the crystal "rings" on its own until the simulation ends after one second.
Voltage across the 1MEG resistor is shown, along with crystal current (purple).
Notice that even after being excited for 0.3 seconds, crystal amplitude is still rising and has not yet reached a steady-state condition. From the magnitude plot above, amplitude would have exponentially risen to 29.5mV had excitation been extended awhile longer. Even after one second, the crystal is still ringing-down: transient response with 1MEG load

1.For frequency response and time response measurement, why shuold I change the input impedance from 50 ohm to 1Meg ohm? Could be any relation to calculate? For example, I measured the frequency response both at 50 and 1Meg ohm input impedance. Is there a relation between these two measurement results?

You should be able to see a frequency response similar to the top plot. Note that this must be done quite slowly, giving time between each measurement for the crystal to adapt its current and voltage to each new frequency.
Note that amplitude across the 50 ohm load is quite small. The anti-resonance point near 32788 Hz is likely buried in noise, at least for the 50-ohm load.
One might ask how much amplitude this tiny crystal can accept. The ABRACON spec suggests that maximum power seen by the crystal should be less than one microwatt. If internal resistance is 35k ohm, then one microwatt would corresponds to a driving amplitude of 0.17V RMS, nearly ten-times higher than OP's driving amplitude of 0.02V RMS.

  1. Why can't I match the measurement result between frequency and time response as descibed above?

It is unclear how OP excites the crystal for a transient plot. One way applies a delta function, perhaps by a single sharp edge. This will cause a transient "ringing" of the crystal, but of a very low amplitude.
As the transient plot above suggests, about half-second of excitation is applied before the crystal "rings-up" to full amplitude. A shorter excitation period is unable to ring-up the crystal very much, so its transient response is quite small.
Also, the crystal requires an excitation frequency very close to resonance so that you can see it ring-up or ring-down. For the 1 MEGohm load, with parallel 12.5pf capacitor, resonance occurs quite close to 32768 Hz. for this example.

However, when loaded with 50 ohms, resonance occurs at 32766 Hz (for this example crystal model), and requires more than one second to reach full amplitude. Full amplitude is quite small here, because the 35k resistor that models the crystal losses combines with the 50-ohm load to form a 57 dB attenuator.

  • \$\begingroup\$ Thanks for your answer and opinion! For question 2, I think there's a noise exit that will add to the resonance signal observed from the oscilloscope. I'll try whether could apply a delta function to it. For question 1, I measured the crystal for both two input impedance, but for 1_meg [ohm], the peak at resonance peak is much smaller, about -80 [dB] (50 [dB] difference). Could there be any reason why caused this? \$\endgroup\$
    – Jack Huang
    Commented Feb 19, 2023 at 5:06
  • \$\begingroup\$ The 50ohm load test circuit is the correct one. The reason why 1Mohm load gives you a different result is caused by an impedance transformation, where the crystal's equivalent inductance combines with its internal capacitance, along with capacitance associated with coax, input capacitance of the lock-in. Notice that resonant frequency with 50-ohm load is lower than resonant frequency with 1Mohm load. The 50-ohm load's resonant frequency is very close to crystal's series resonance (which is lower than design freq of 32768 Hz.). \$\endgroup\$
    – glen_geek
    Commented Feb 19, 2023 at 19:44
  • \$\begingroup\$ You meant that for the 50 [ohm] input impedance, the signal from resonator flow through a 50-ohm coaxial cable then into the 50 [ohm] input impedance of instrument only happen reflection once(between resonator and coaxial cable) and for 1_meg [ohm] input impedance it will happen twice(one between resonator and coaxial cable and another one between coaxial cable and 1_meg [ohm] input impedance) so we would chose the measurement result from 50 [ohm] as the correct one because it has smaller loss than 1_meg [ohm] which is more prone to the inital ouput signal from resonator, is that correct? \$\endgroup\$
    – Jack Huang
    Commented Feb 20, 2023 at 2:04
  • \$\begingroup\$ Jack, the resonator itself transforms impedances so that simple analysis at resonance is complex. A 50 ohm internal resistance at lock-in input allows simple analysis for these 32kHz crystals at series resonant freq...it is basically a simple voltage divider between two resistors (crystal's Rm, 50ohms). Your recent value of 107k value for Rm seems somewhat high for this class of crystal, but I might be wrong. Try finding exact series-resonant frequency and do a static measurement there. That's a nice lock-in. \$\endgroup\$
    – glen_geek
    Commented Feb 20, 2023 at 4:18
  • \$\begingroup\$ @glen_gleek, the reason why RM is so high is that im using different type of resonator so it could be abnormal to the one of crystal resonator. \$\endgroup\$
    – Jack Huang
    Commented Feb 23, 2023 at 6:49

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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