Pierce Oscillator, Oscillations are going down. Cadence software.

Hello,
I'm designing a crystal oscillator using the pierce model. I don't know how to validate my circuit.
So far I managed to measure the gain open loop (which is more than one at the wanted frequency, so oscillations should occur).

Then, when I want to close the loop and visualize oscillations it doesn't start at all.
I read on the internet that I had to set an initial condition on a capacitor to start the oscillations (I set 0V). It did start, but my oscillations are not maintained they are going lower and lower. This is the first problem.

The second one is : That my oscillations are not building up, they start at a huge amplitude immediately then go down.

I don't know what I did wrong. Theory says that I must have an inverter amplifier, I used a Common Source amplifier which amplifies and phase shift the signal so it should amplify the oscillations but it doesn't.

Do you have any clue about what is the problem?

Thank you.

Very simple: The simulator is the problem :lol: For high Q factors, it will not work properly with the standard integration method due to numerical problems.

Use the integration method traponly, and it should work.

Please note that then some of the curves you will see may look like a zig-zag pattern in the rhythm of the simulation time step, physically absurd. You will have to live with these artefacts and trust the trapezoid integration method: it is doing the right thing in the average.

I speak from recent experience: Right now I have an IC going into production, with a low-power pierce crystal oscillator I designed. The only three cases where it maintains oscillation is (1) in my theoretical calculations, (2) with method=traponly, and (3) on silicon

Slainte!
H

Hello, thank you for your help.
By traponly method, you mean using the traponly option in the accuracy tab in the options of the PSS simulation?

--------------------------------------------------

As you built one yourself, may I ask some questions? you are free not to answer the questions as it's not really design.
As nothing is working I'm questionning my theory, or at least the steps I made to get to the quartz model I'm using.

To make my crystal model, I checked some crystals from manufacturers and took some caracteristics like :
Equivalent Serie Resistance = 60 ohm
Cshunt = 3pf (manufacturer saying that 7pF is max, should I take a lower value or the max value? for a worst case scenario)
Cload=10pF

With this I did some math to estimate L1 and C1 as no manufacturer are willing to give me their models.
I took a quality factor Q=10^5. From this I found L1 = 23mH and C1=0.663fF.

Does this way of creating a model good to you?

----------------------------------------------------------

Other question, I'm supposed to oscillate at 40MHz, what should the AC analysis of the open loop gain look like?
Should I have a sharp spike at 40MHz with some gain? (at least more than 1), because right now I have a slow curve, instead of a sharp spike and I'm wondering why, my Q factor is high shouldn't it be a spike?

-----------------------------------------------------------

Did you manage to make your circuit oscillate using the load capacitor in theory? Because my load capacitance should be 10pF, and I only oscillate at the right frequency with something like 0.9pF. I'm running out of ideas...

-----------------------------------------------------------
I have so many questions...

Thank you for your time,

Despite of possible numerical problems, the circuit would at least simulate correctly in AC analysis. So if you don't see a reasonable loop gain, there's something wrong with your simulation circuit, crystal model or amplifier bias point.

The description in the initial post isn't clear in one point. Do you actually see a fading oscillation or just an aperiodical transient?

Transient analysis of crystal oscillators is tricky in so far, that the large Q involves thousands of oscillation cycles to move energy between the crystal and the rest of the circuit. To achieve steady state in finite time, you'll usually want to "deposit" energy in the crystal by defining well considered initial conditions. Regarding mentioned numerical problems, I can just say that I got meaningful crystal oscillator simulations with other SPICE simulators, e.g. Pspice and LTSpice without adjusting transient analysis parameters.

Hello, thank you for your help.
By traponly method, you mean using the traponly option in the accuracy tab in the options of the PSS simulation?

--------------------------------------------------

As you built one yourself, may I ask some questions? you are free not to answer the questions as it's not really design.
As nothing is working I'm questionning my theory, or at least the steps I made to get to the quartz model I'm using.

To make my crystal model, I checked some crystals from manufacturers and took some caracteristics like :
Equivalent Serie Resistance = 60 ohm
Cshunt = 3pf (manufacturer saying that 7pF is max, should I take a lower value or the max value? for a worst case scenario)
Cload=10pF

With this I did some math to estimate L1 and C1 as no manufacturer are willing to give me their models.
I took a quality factor Q=10^5. From this I found L1 = 23mH and C1=0.663fF.

Does this way of creating a model good to you?

----------------------------------------------------------

Other question, I'm supposed to oscillate at 40MHz, what should the AC analysis of the open loop gain look like?
Should I have a sharp spike at 40MHz with some gain? (at least more than 1), because right now I have a slow curve, instead of a sharp spike and I'm wondering why, my Q factor is high shouldn't it be a spike?

-----------------------------------------------------------

Did you manage to make your circuit oscillate using the load capacitor in theory? Because my load capacitance should be 10pF, and I only oscillate at the right frequency with something like 0.9pF. I'm running out of ideas...

-----------------------------------------------------------
I have so many questions...

Thank you for your time,

The order of magnitude sounds reasonable.
I see a typical parameter set for a 50 MHz 3. overtone cystal in the Crystal Cookbook https://www.axtal.com/info/buch.html, it says

Q = 100e3, C1 = 2 ff, C0 = 4.3 pF

So apparently, the impedance would be a bit lower than you assumed. But unless you are referring a specific crystal type (case size etc.) the differences shouldn't matter too much.

And yes, there will be a sharp peak in the loop gain curve.

@FvM
Hello, I'm sorry about my explanations, I don't even know how to describe what I have, here is a screenshot of my tran analysis :
**broken link removed**
The oscillation are at 40MHz but they die rapidly.

And this is the open loop gain in green and in red the gain of the amplifier (common source transistor).
**broken link removed**
Gain at 40 MHz is higher than 1 (around 4), the amplifier i'm using has a 180° shift, so I should oscillate, but I'm not....

I'm stuck, I don't know how to solve my problems, if you need more information I will give them.
Thank you for your time.

The transient response clearly shows a circuit that doesn't fulfill the oscillation condition.

Where do you see gain of 4 in the plot? I would prefer a bode plot with db magnitude scale.

Oscillation condition (complex loop gain = unitity) must be fulfilled. Usually small signal gain at phase 0 is above 1, decreasing to unity by nonlinear amplifier action.

The gain curve looks strange, the frequency step seems too large.

But it's not very fruitful to guess about an unknown circuit,

I know that the transient doesn't look good, but I have the gain, either my phase shift is wrong or my AC analysis is wrong.

Here is the AC analysis of the open loop gain in green with a marker at 40 MHz, the gain is in fact of 5.
**broken link removed**

And Here is the bode plot of the open loop gain with a marker at 40MHz
**broken link removed**

Frequency step has been lowered.

About the oscillation conditions, my gain is higher than 1 to start the oscillations, then the system should "stabilize" itself as the amplifier is not linear and the gain should be equal to 1 at some point, that's what I read on the internet, but I can be wrong.

Do you need the schematic as well? it might take some time to make it presentable, I'm working on it now.
Thank you.

At first sight, the crystal resonance seems to be located at 4 MHz rather than 40 Mhz. For loop gain analysis, the phase must be known.

The phase is actually at -180° at 10MHz instead of 40MHz.
**broken link removed**

And the max gain is at 9.6 MHz.
**broken link removed**

So the problem is the phase? as I'm beyond -180° and not on 180°?

Why did you say that the crystal resonance was at 4MHz?

- - - Updated - - -

Okay, one of my colleague told me to launch a HB simulation instead of a tran, and now I'm oscillating... at 4MHz like you said, but why 4MHz? I don't get it...

Thank you.

- - - Updated - - -

The Crystal cookbook looks quite detailed, is there any English version I can buy?

- - - Updated - - -

Okay, I have been modifying so many parameters at the same time that I set my oscillator to oscillate at 4MHz instead of 40MHz, I don't know how did you notice that on a bode and a phase diagram but it allowed me to check the crystal model.

But how did you see that on the bode anyway?

Thank you both for your help!

- - - Updated - - -

Okay, I have been modifying so many parameters at the same time that I set my oscillator to oscillate at 4MHz instead of 40MHz, I don't know how did you notice that on a bode and a phase diagram but it allowed me to check the crystal model.

But how did you see that on the bode anyway?

Thank you both for your help!

- You need to make sure that you provide sufficient negative resistance. In my opinion if the oscillation starts and then goes down, you need to increase gm (by increasing the current or increasing W/L)
For instance if you use lower R, you will propably see the oscillation building up.
- Besides the traponly method, it is necessary to increase the simulator accuracy (See the Cadence manual on simulating Hard Circuits)
- Also, the step in the transient should be extemely small because of the high Q. If you use an automatic step, this is not sufficient. You should use a step of ~ Period/100

Hope it helps

Combining phase and magnitude plot, it looks like the circuit never reaches the oscillation condition. So apart from the question where we see the crystal resonance in the loop gain, the oscillator is apparently wrongly designed.

The simulation was actually badly configured. I used a harmonic balance and I could see the oscillations.

Why is the phase and magnitude wrong? am I not supposed to have a phase of -180° at least? I'm a little beyond that.
About the gain, am I not supposed to have a gain superior than 1 to start the oscillations? (I have 4-5)

It's still not clear to me how you calculate phase in your simulation. As previously stated, the oscillation condition involves a loop phase of 0 (respectively N*360) degree.

Regarding excess gain, an oscillator will work with factor 4 or 5 gain margin, but ususally expose less frequency stability, more harmonics and phase noise due to the strong clipping required to reduce the steady state gain to unity. This might be still suffcient for a standard quality crystal oscillator.

I'm still investigating, as even if my circuit "works" (still unsure if I can say that it works), I'm not following theory results at all....