Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

[help] on-chip crystal oscillator design

Status
Not open for further replies.
check these IEEE conference paper it might of some help to you..
 

France said:
Could you teaches me how to do crystal OSC tran analysis.

Hi ysz
Your circuit, is right?

thx.
Click to expand...
yes, you could send your nellist to me, I'll help you.
 

I have just joined this forum and this caught my attention. i work on crystal oscillator designs for a living(I work for a crystal company) and i may be of some help here. first off, spice based simulation is not the prefered simulation tool, in the industry harmonic balance is the prefered tool. if you must use spice than it is a good idea to initialise the charge storage elements to speed things up. If you want to look at the FFT be sure to disable the adaptive time stepping algorythm in the options. at 48MHz the crystal may be either a fundamental or third overtone. a good crystal model will have the fundamental, third and fifth elements included. if the device is a third overtone than you will need to add an inductor to keep it from running on the fundamental. here is the measured values for a 48MHz fundamental device: R1=6.8ohms, C1=15.351fF, L1=.71672mH. Be advised that the negative resistance(excess gain) presented by the inverter should be AT LEAST 5 and preferably 10 times the load resonance resistance of the crystal to be production ready with acceptable reliability. hope this helps
jim
 
Crystal guy - you are right. Spice simulation of the crystal oscillator is alway shooting in the dark. There is no way one could simulate exactly how it will perform but it is the same with any spice simulation. General rule as far as I know is that above 30MHz the osc will run in overtone.
I am sure that the circuit (clasical Pierce osc.) will work but first I would recommend to improve the crystal model by adding 2nd and 3rd harmonics. That is hard since crystal maker are not very helpful with spice models or with measured values. CRYSTALGUY - can You help???
I know dozens of people who would love to have "Real" crystal models.
Next I would let simulation run for about 100ms and saved as little as possible. The lock up time could be long. I believe overnight sim should make it.
But also - I suppose that the oscillator is supposed to be parallel mode (based on circuit used) - or is it going to be in serial one? Is it suppose to wirk just with 48MHz xtal or with wider range of freqs? etc
 

the circuit is indeed a Pierce oscillator. these oscillators form the basis of 90% of the IC type oscillators currently used. In this case the crystal is very lightly loaded (4pF from the phase shift caps and, normally, you will have somewhere around 2 to 4pF from the phase delay in the inverter). so the total load is something like 6pF. This is less than most manufaturers will want to make since the load fixture for final frequency adjustment is difficult to do. models for crystals are very dependent on the package. small surface mount devices have a lower frequency limit of around 13 to 17MHz and an upper limit for fundamental operation of around 60MHz. It is not uncommon for people to make mistakes here. 48MHz is a very common frequency these days as i get two or three designs in the lab for these a week for evaluation, Most of these are fundamental crystals. WIth a 6pF load this oscillator will be suseptable to load pulling on the order of 80ppm/pF and the phase noise/jitter will be not so good. for these small surface mount parts the overtones(notice not harmonics they are not exact multiples) are not very active so you can get away with just the fundamental and third overtone branches in the model.
 

Crystalguy - can you direct me to library of xtal models? I have some but with 1st harmonic only.
 

Teddy,
i am afriad there is no library out there that i know of. it is a tedious task generating the models and (as i said) the device models are highly dependant on the manufacturer and the the package. one of the reasons manufacturers are hesitant to provide models is because of the way crystal are spec'd. an example would be that the model may show the R1 value to be around 7 or 9 ohms and this would well represent this value AT 100uW that is spec'd. the maunfacturer spec sheet, however, will say something like "90ohms max". Part of the problem is the fact that these models are really a comforting fiction (albiet, a useful one) that overlooks the rather non-linear behavior of these devices. The unfortunate reality is that at very low current (like the moment of startup) the R1 value may be many times higher dropping down rapidly as the current increases, than going back up as the part is overdriven. Visualize a broad U shaped curve ploting Y=R1, X=crystal power.
 

Do you have a good article about a "one pin crystal oscillator" ?
Can it reach same performances as pierce osc. ?
 

I was simulating the circuit posted by ysz. It does oscillate with the desired freq, however the amplitude is quite small, i.e., a few uV. Is this correct?
 

The important thing is the gain of the inverter should be concern, otherwise the driving abiility of the inverter is important.
And you shoud get right model of crystal like R.L.C value.
 

crystalguy said:
Teddy,
i am afriad there is no library out there that i know of. it is a tedious task generating the models and (as i said) the device models are highly dependant on the manufacturer and the the package. one of the reasons manufacturers are hesitant to provide models is because of the way crystal are spec'd. an example would be that the model may show the R1 value to be around 7 or 9 ohms and this would well represent this value AT 100uW that is spec'd. the maunfacturer spec sheet, however, will say something like "90ohms max". Part of the problem is the fact that these models are really a comforting fiction (albiet, a useful one) that overlooks the rather non-linear behavior of these devices. The unfortunate reality is that at very low current (like the moment of startup) the R1 value may be many times higher dropping down rapidly as the current increases, than going back up as the part is overdriven. Visualize a broad U shaped curve ploting Y=R1, X=crystal power.
Click to expand...
Tahnks for you explanation. I'm a new guy in crystal oscillator design and i'm quite interest in crystal models generation. How can i generate crystal models? Test there Z-f curves and using software to generate RLC models?
 

Then how can I simulate the loop gain and phase margin of the crystal oscillator?
I have designed in this way: simulate the network except the crystal while the parallel capacitor is added to the network, and the real part of the impedance will go negative when frequency is going high, and this negative impedance will compensate the resistance in the series part of the crystal and this will in turn result to oscillating,

my simulation shows that the impedance of the network between extal and xtal goes negative when frequency goes higher ,however, the transient simulation shows that the oscillation voltage swing decreases with time going on, then is this due to the low loop gain?

3x a lot
 

What do you mean by inverter gain? How to fix its minimum? Any maximum?
CrystalGuy, what do you mean by "the negative resistance(excess gain) presented by the inverter should be AT LEAST 5 " ?
.
 

In crystal design, except start problem, the frequency phase noise is also concerned. Anyone can analyze this problem.
the second problem, in many design there all use the two loading capacitor to modify the frequency, but the modified frequency range is very low (it is on about
C0/(Cp+ Cl1*Cl2/(Cl1+Cl2))**1/2) it maybe only several ppm, i want to know what function is this trimming, which is only for getting this few ppm of frequency.
 

tlihu said:
I was simulating the circuit posted by ysz. It does oscillate with the desired freq, however the amplitude is quite small, i.e., a few uV. Is this correct?
Click to expand...

same question, and anyone can say sth. Thanks.
 

andy2000a said:
1. use need 48M Xtal spice R-L-C model ..
2. use AC sim check invert + Xtal have 180 degree phase shift
and frequency = Xtal freq
3. check invert gain
4. close loop use .tran and you must be use hspice .option
method=gear or trap ..
5. assign a initial voltage let spice sim speed up
6. make sure Xtal can really osc

ps. sometime hspice sim Xtal is work but real ASIC is not ..
you should becareful use .option parameter
Click to expand...
I am puzzled on the oscillator design
I konw you are rigth that I get my osc circuit oscillate when invert + Xtal have 180 degree phase shift
But I always think that the invert +Xtal degree phase shift 360 and the gain >1 will make the circuit oscillate,where am I wrong?Thanks
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top