Making a Pierce Oscillator

Dear Ashish,

Ashish Papreja said:

So was trying to see that behavior for my Design . I have chosen a crystal oscillator at around 80MHz with Motional Parameters as Rm=86.47 Lm=27.87mH Cm=142aF Co=3.5pF Q=162k.

So I have also Plotted the complex Plane Impedance using MATLAB for different values of C1 and C2.

Like here if C1 and C2 =1pf No matter whatever the gm you may take no oscillations would occur.

...

Ashish Papreja said:

Can you guys help me with what am I doing wrong here?

A few of comments if I may...

1. In my opinion, the paper by Vittoz does provides neither an intuitive nor a "design centric" analysis methodology in my opinion. I do note you tried a different approach (negative resistance based analysis) which is far more "design centric" that I will comment on later.

2. I believe the terminology you intend for the quartz resonator is a "quartz resonator" and not a "crystal oscillator". It may be my 10-20+ years of design quartz resonator based oscillators coming to bite me and annoy you, but the proper terminology for the Butterworth model is a quartz resonator. It mates with your "sustaining amplifier" to provide potential oscillations. The design methodology I use, and have taught numerous other oscillator designers, is basically a negative resistance analysis approach. Not only do I find this approach far more intuitive (in my opinion) than a state space approach, but I have derived the negative resistance expression in terms of basic device transistor parameters which allows me an easy way to tailor a design for a specific quartz resonator.

3. In the analysis you performed to estimate the sustaining amplifier's negative resistance, I am not clear if your analysis included C0 (3.5 pf) as part of the sustaining amplifier's capacitive load C3. If it does not, then as shown in Figure 1 where I plot your quartz resonator's real and imaginary impedances, you will note that the real impedance varies significantly over frequency. I have highlighted the series resonance point. It is very rare for an oscillator to run at exactly series resonance and more typical that it run between series and parallel resonance frequencies as the imaginary impedance of the sustaining amplifier is very rarely exactly 0 ohms (which defines the series resonance). Hence, in your sustaining amplifier negative resistance simulation, make sure you include the C0 as part of the C3 in your schematic and only then might you expect to see oscillations of the magnitude of the sustaining amplifier's negative resistance exceeds your value of Rm = 86.47 ohms.

4. Finally, the accuracy settings and simulation time of your transient simulation play a critical role in observing any potential oscillations. A quartz resonator based oscillator will take typically milliseconds to establish its steady-state oscillation and the timestep of your simulator MUST be chosen to be small per waveform pariod (Tperiod/100 or less). This is not necessarily guaranteed by default simulator accuracy settings. Since you did not indicate which spectre simulator you are using, nor its version, nor any simulator accuracy settings and end time for your transient simulation, I can't comment any further on your settings and the likelihood they are sufficient to both start and observe potential oscillations. Perhaps if you consider the comments I made with respect to the settings you may observe oscillations if the negative resistance of the sustaining amplifier exceeds the required value. Otherwise, might you possibly include the missing information in order that I might comment on each Ashish?

I hope this is somewhat useful..albeit only a brief overview of the issues I observed from your post.

Shawn

Figure 1

Dear Ashish,

Ashish Papreja said:

So was trying to see that behavior for my Design . I have chosen a crystal oscillator at around 80MHz with Motional Parameters as Rm=86.47 Lm=27.87mH Cm=142aF Co=3.5pF Q=162k.

So I have also Plotted the complex Plane Impedance using MATLAB for different values of C1 and C2.

Like here if C1 and C2 =1pf No matter whatever the gm you may take no oscillations would occur.

...

Ashish Papreja said:

Can you guys help me with what am I doing wrong here?

A few of comments if I may...

1. In my opinion, the paper by Vittoz does provides neither an intuitive nor a "design centric" analysis methodology in my opinion. I do note you tried a different approach (negative resistance based analysis) which is far more "design centric" that I will comment on later.

2. I believe the terminology you intend for the quartz resonator is a "quartz resonator" and not a "crystal oscillator". It may be my 10-20+ years of design quartz resonator based oscillators coming to bite me and annoy you, but the proper terminology for the Butterworth model is a quartz resonator. It mates with your "sustaining amplifier" to provide potential oscillations. The design methodology I use, and have taught numerous other oscillator designers, is basically a negative resistance analysis approach. Not only do I find this approach far more intuitive (in my opinion) than a state space approach, but I have derived the negative resistance expression in terms of basic device transistor parameters which allows me an easy way to tailor a design for a specific quartz resonator.

3. In the analysis you performed to estimate the sustaining amplifier's negative resistance, I am not clear if your analysis included C0 (3.5 pf) as part of the sustaining amplifier's capacitive load C3. If it does not, then as shown in Figure 1 where I plot your quartz resonator's real and imaginary impedances, you will note that the real impedance varies significantly over frequency. I have highlighted the series resonance point. It is very rare for an oscillator to run at exactly series resonance and more typical that it run between series and parallel resonance frequencies as the imaginary impedance of the sustaining amplifier is very rarely exactly 0 ohms (which defines the series resonance). Hence, in your sustaining amplifier negative resistance simulation, make sure you include the C0 as part of the C3 in your schematic and only then might you expect to see oscillations of the magnitude of the sustaining amplifier's negative resistance exceeds your value of Rm = 86.47 ohms.

4. Finally, the accuracy settings and simulation time of your transient simulation play a critical role in observing any potential oscillations. A quartz resonator based oscillator will take typically milliseconds to establish its steady-state oscillation and the timestep of your simulator MUST be chosen to be small per waveform pariod (Tperiod/100 or less). This is not necessarily guaranteed by default simulator accuracy settings. Since you did not indicate which spectre simulator you are using, nor its version, nor any simulator accuracy settings and end time for your transient simulation, I can't comment any further on your settings and the likelihood they are sufficient to both start and observe potential oscillations. Perhaps if you consider the comments I made with respect to the settings you may observe oscillations if the negative resistance of the sustaining amplifier exceeds the required value. Otherwise, might you possibly include the missing information in order that I might comment on each Ashish?

I hope this is somewhat useful..albeit only a brief overview of the issues I observed from your post.

Shawn

Figure 1

Dear Shawn,

I am using spectre -W( subversion 15.0.1.257) virtuoso -W(subversion IC6.1.7-64b.500.10).

So, as you mentioned I am using Co of quartz resonator which was 3.5pF as a part of my sustaining Amplifier(here C3) and was trying to Plot the negative real part . 

Unknown said:

I have derived the negative resistance expression in terms of basic device transistor parameters which allows me an easy way to tailor a design for a specific quartz resonator

So I also did the small signal Analysis to obtain the real and imaginary part of Zc which I will get  and plotted the values using MATLAB for different values of gm(This is theoretical). Theoritical analysis shows that my Resistance should be a negative value whereas when I am making the testbench in Cadence for seeing the values I am seeing positive values for the resistance. 

I am not sure whether something is wrong in my biasing(DC op point point shows that both are in region2)  or am I plotting it incorrectly . So , I will show testbench for the same:

TestBench for Plotting Real and Imaginary part of Zc:

So I have removed the Zm(motional branch ) and Placed an isin AC magnitude 1A , then I am plotting real part of differential voltage since I=1A thus Zc= V so for plotting real part I am using this:

real((vfreq('ac "/net1") - vfreq('ac "/out")))

Fig-1

Here as shown in fig-2 it is showing positive real part.

Fig-2

Fig-3 Below shows a basic pierce Oscillator which I am trying to implement with CMOS invertor as a linear amplifier with Rf (feedback resistor)

I guess something is wrong as I am not getting negative resistance that is why my design is not oscillating . Could you please have a look what could be I doing wrong here.

Thanks in Advance

Dear Ashish,

Thank yout for your added information! It is quite useful to me at least!

Ashish Papreja said:

So, as you mentioned I am using Co of quartz resonator which was 3.5pF as a part of my sustaining Amplifier(here C3)

Perfect. This is, from my perspective, the most intuitive means to study the input impedance of your sustaining amplifier.

Ashish Papreja said:

I guess something is wrong as I am not getting negative resistance that is why my design is not oscillating . Could you please have a look what could be I doing wrong here.

Yes - but easily corrected. In Figure 1, I indicate how you have defined the input voltage and input current from which you are trying to compute the real impedance. Note that you have defined the input current as a negative value (i.e, 180 degrees out of phase from the desire phase of 0 degrees). Hence, the sign of your computed real impedance is incorrect. You could also tell by realizing the imaginary part of the sustaining amplifier input impedance just beyond your quartz resonator's series resonant frequency must be capacitive (i.e. negative). I think if you inspect the imaginary part of the sustaining amplifier over that frequency range it will appear inductive - which it clearly cannot be.

Hence, change the polarity of your input AC current source in the circuit, re-simulate, and your existing expression should provide a negative sustaining amplifier real impedance just after 80+ MHz.

I hope this is helpful!

Shawn

Figure 1

Dear Shawn,

Unknown said:

Hence, change the polarity of your input AC current source in the circuit, re-simulate, and your existing expression should provide a negative sustaining amplifier real impedance just after 80+ MHz

Oh, I realized what was the issue.  Thanks for the guidance.

So I was tweaking some values and now I get a negative Resistance of around -114 ohms which is more than my Rm which is 86.47ohms, so I was expecting oscillations in my tran analysis.

So as you mentioned above I am using max steps I am choosing 80MHz corresponds to 12.5ns so 12.5ns/100.

Integration method as tranpoly and errpreset as conservative and end time as 1ms.

But Still, I am not seeing any oscillations. 

Netlist Attached:

https://iiitaphyd-my.sharepoint.com/:t:/g/personal/ashish_papreja_research_iiit_ac_in/EfB78r2z6dFJgYJMLoUvGXgBmLL2va8L6vSVZdll_h25vw?e=IT1WKZ

Do you see anything wrong in my setup when I am doing transient analysis?

Thanks 

Dear Ashish,

Thank you for filling us in with your updated small-signal impedance results and your netlist! I m happy to read your negative resistance analysis is now working as you expect too!

Ashish Papreja said:

Do you see anything wrong in my setup when I am doing transient analysis?

I examined your netlist and it appears to be a netlist for a DC simulation and not a transient analysis. Did you intend to publish the transient analysis input.scs file? As a side note, I do prefer the use of the gear2only integration algorithm in lieu of the trap algorithm. I realize some experts who monitor this forum do no, but in my experience with precision oscillator simulations, it has been more successful.

In any case, I did notice one item that may be responsible for your lack of oscillation. You have the following in your input.scs file:

L0 (net1 net015) inductor l=lm
C1 (net1 0) capacitor c=C1
C2 (vout 0) capacitor c=C2

C3 (net015 net014) capacitor c=cm
C0 (net1 vout) capacitor c=C3
R1 (net1 vout) resistor r=rbias
R0 (net014 vout) resistor r=rm
M1 (vout net1 net8 net8) pmos_rf lr=60n wr=hh nr=1 sigma=1 m=x \
        mismatchflag=0
V0 (net8 0) vsource dc=1.2 type=dc
ic net014=0V net015=0.6

If I trace your nodes correctly, it appears C0 is connected between the gates and drains of your nmos and pmos devices (i.e. net1 is the same node as the two input gates and out is the drains of the two devices) with a bias resistor of 1 megohms between the drains and gates. With your .ic values for net014 at 0 V and net015, and realizing that your DC operating point will short inductors and open capacitors, your two gates are connected to the voltage of node net015 and are set to 0.60V, while your two drains are connected to 0 V. Hence, your sustaining amplifier is not biased to provide high gain and will not have the negative resistance you simulated in your AC analysis. Hence, there is nothing to build-up oscillations until the voltages at the gates and drains of your active devices are near equal. Their ability to change voltage is limited by the current through the devices and will be quite small. It may take a LONG time for the small bias current to change the voltages across capacitors C1 and C2.

in looking at your plot, it appears the output voltage of your inverter is set to the initial value of the gate or  exactly 600 mV - the initial condition of your gates. Did you verify that the DC operating point at 1 ms is the same as that in your small-signal AC negative resistance DC operating point? I am thinking your resulting transient operating point up to 1 ms may not be the high gain state for your inverter and hence does not have the negative resistance you are expecting (and therefore the build up of oscillations are not evident). Did you try eliminating the  initial conditions from your transient analysis?

Shawn

Dear Shawn,

Unknown said:

Did you verify that the DC operating point at 1 ms is the same as that in your small-signal AC negative resistance DC operating point?

Yes Shawn , when I run the ac analysis for my testbench I checked the dc operating point there. and when I am doing tran analysis I see that in options I have selected the save Final Op point and then when I was checking the Transient Operating Point at 1ms they were same .

DC operating Point from Small signal AC negative Resistance Model:-

Transient Operating Point at 1ms:-

Although I find one link which also shows how to simulate the Crystal Oscillator:

https://community.cadence.com/cadence_blogs_8/b/rf/posts/new-mmsim-12-1-harmonic-balance-features-auto-tstab-and-auto-harmonics

When I using the same method I am able to see Oscillations for my circuit.

Althogh from tran analysis it seems that Oscillations didn't start building till 1ms.

Do I have to run for too much longer in tran analysis in order to see oscillations building up . I run once till 20ms to check the Oscillations were still not building.

Link for Updated Netlist:

https://iiitaphyd-my.sharepoint.com/:t:/g/personal/ashish_papreja_research_iiit_ac_in/Ec3IrI9fcnRHoJXD2UsHKgQBNwHfVLbWeBbz4H-LUkm3bg?e=DmPTlP

Thanks in Advance.

Dear Ashish,

I have not forgotten your question! I am trying to juggle my responses with work, so please excuse my tardy response to your last reply.

Ashish Papreja said:

Do I have to run for too much longer in tran analysis in order to see oscillations building up . I run once till 20ms to check the Oscillations were still not building.

I decided to run an analogous set of simulations to try to help out a bit. The test bench with the inverter based sustaining amplifier is provided in Figure 1. I also ran a set of large signal impedance simulations of the sustaining amplifier at 80 MHz with input currents between 0.10 mA and 10.0 mA. The real impedance the sustaining amplifier resonator terminals (including the 3.5 pF C0 of the quartz resonator) of these simulations are shown in Figure 2. What this indicates (and your technology and inverter sizes are different and unknown to me), is that with an +83 ohms quartz resonator arm, the current to the sustaining amplifier will be limited to the current that produces a -83 ohm real impedance - or in this case 1.26 mA. Under this condition, it is important that a 1.26 mA current is sufficient to provide near CMOS levels at the self-biased inverter output. If this is not, although the conditions for oscillation appear to exist, the large signal result may not provide CMOS compliant output waveforms. For example, if you included a follow-on CMOS buffer, there may be not be an output from this buffer if your sustaining amplifier does not produce CMOS levels due to insufficient current.

This curve also shows the impact of using a quartz resonator of lower real impedance than 83 ohms on the resonant current. A lower resistance will result in a greater magnitude of resonant current.

As an example, I am running two 15 ms spectre simulations (I use spectre X 20.1.ISR19, preset ="cx", with a strobe point constraint of 1024 points per 80 MHz period). The transient command is:

tran tran stop=tstop write="spectre.ic" writefinal="spectre.fc" \
saveperiod=1e-03 savefile="checkpoint_1ms" annotate=status \
save=selected strobeperiod=_EXPR_4 strobeoutput=strobeonly

with a run line of:

spectre  input.scs  +escchars +log ../psf/spectre.out  -format psfxl -raw ../psf   +preset=cx +mt=lsf +lqtimeout 0 -maxw 5 -maxn 5 -env ade +dcopt +disk_check=100e9 -ahdllibdir /scratch/noclean/dcd_serdes/sml/simulation/sdd5e_TB/test_inv_bias_decay/maestro/results/maestro/Interactive.10/sharedData/CDS/ahdl/input.ahdlSimDB +logstatus

I have set one to use a resonator with an 83 ohm real impedance and the second to use a resonator with a 4 ohm real impedance and can already see the difference between their quasi-exponential envelopes of oscillation build-ups. I will publish the plots when the simulations complete. 

With respect to your question about expediting the transient simulation to minimize simulation time, I believe this is possible and will provide some guidance in my follow-on post.

Shawn

Figure 1

Figure 2

Dear Shawn,

I am confused with few things above:

Unknown said:

I also ran a set of large signal impedance simulations of the sustaining amplifier at 80 MHz with input currents between 0.10 mA and 10.0 mA.

When I am placing a isin and trying to plot the real part of Z by including the Co what I am seeing is almost same value of Rneg . I guess what I am doing is small signal impedance measurement and what you are saying is large signal impedance , well I am not aware how you are plotting this large signal impedance.

This is how I was plotting the small-signal impedance by sweeping isin values from 0.1m to 1m.

As expected the Real part was same. So lets say here I am getting around -78 ohms here and now if Rm is lets say less than this value 60 ohms just for example you are saying that it still might not oscillate.

Now if I look at figure 2 (from above post) so you are saying that if we want -83 ohms the current in the sustaining amplifier will be limited to 1.26mA and this 1.26mA should be enough that if I again do a small signal impedance check at Iref=1.26mA I should be getting more than Rm value here 83 ohms. then only it will work is that the case?

Just to make things more clear lets say I have a current of Iref of 2mA which is mirrored into my CMOS inverter branch. Now if I check the small signal impedance at this bias current I get -90 ohm whereas lets say Rm was +83 ohm . I am thinking I might get oscillations but bcoz the current would be limited to 1.26mA only so now if I check small signal impedance at 1.26mA it's magnitude should be greater than Rm then only I can expect oscillations. 

Sorry if I might have understood wrongly.  

Dear Ashsih

Ashish Papreja said:

Now if I look at figure 2 (from above post) so you are saying that if we want -83 ohms the current in the sustaining amplifier will be limited to 1.26mA and this 1.26mA should be enough that if I again do a small signal impedance check at Iref=1.26mA I should be getting more than Rm value here 83 ohms. then only it will work is that the case?

I think you need to review exactly what a small-signal AC simulation is providing.

It performs a DC operating point analysis and then creates a small-signal model for the circuit under test and simulates its small-signal transfer function. As a result, the model will NOT change as you vary the value of your AC input current. Hence, if the actual circuit under test shows ANY non-linearity in its transfer function with input current amplitude, this will NOT be modeled properly if you simply change the amplitude of your AC current. In your case, an oscillator with very few exceptions, the circuit transfer function is quite non-linear with input current and you cannot rely on simply changing the input current amplitude in a small-signal simulation to provide an accurate estimate of the resulting circuit response to the current amplitude (in your case the impedance characteristic is the transfer function of interest).

This is why I performed the set of large signal transient analyses where I varied the amplitude of the current to show you the variation in the real impedance value as the input current varies.

Ashish Papreja said:

Now if I look at figure 2 (from above post) so you are saying that if we want -83 ohms the current in the sustaining amplifier will be limited to 1.26mA

Figure 2 indicates that a current of about 1.26 mA provides a sustaining amplifier real part that is exactly equal and opposite to your quartz resonator real impedance. If the 1.26 mA amplitude is NOT sufficient to result in significant enough voltage swing to produce close to a full CMOS rail-to-rail signal as input to your output CMOS buffer, then you may not observe a proper CMOS output signal. A lower quartz resonator impedance than 83 ohms will produce a higher amplitude voltage in your sustaining amplifier and both reduce start-up time. For example, I did re-simulate a version of your self-biased inverter based oscillator using your resonator model using an 83 ohm and 4 ohm resonator. Figures 3 and 4 show the start-up performance for as long as the simulation went before it crashed due to an unrelated effect. The difference in start-up times and amplitudes of the sustaining amplifier differential internal node "vnegr" are both significant. Note that with an 83 ohm resonator real impedance, the output node has not yet reached a full-scale CMOS waveform for the 720 mV supply voltage I am using.

Ashish Papreja said:

I guess what I am doing is small signal impedance measurement and what you are saying is large signal impedance , well I am not aware how you are plotting this large signal impedance.

As mentioned, I am running a series of large-signal transient analyses and determining the sustaining amplifier's large-signal real impedance at the frequency of the applied sinusoid of 80 MHz. I have provided information on this type of analysis for oscillators in many prior forum posts if you are interested.

Shawn

Figure 3

Figure 4