Welcome to our site! EDAboard.com is an international Electronic 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.
You can find a 32.768kHz crystal oscillator with CMOS inverters at http://www.ee.washington.edu/circuit_archive/circuits/F_ASCII_Schem.html .
Regarding the electrical equivalent model of 32.768kHz crystal, there is info in an old MOTOROLA McMOS Data Book as follows: series resistance, Rs=25kohm; Q=50000 (typical); series motional capacitance,C1=0.0039pF; series motional inductance, L1=6000Henry (!); parallel capacitance, Co=3.9pF (these data are for Motorola MTQ 32 type crystal (NT-cut) but obviously many other 32kHz crystals have nearly the same equivalent motional L1 and C1, depending on their cut of course).
In the circuit on the above web site the 15Megohm resistor is important, because it adjusts the inverter into the linear part of the DC characteristic to get high gain, hence oscillation, do not use less then 10Mohm there! Also, it is very difficult to force a 32kHz crystal into oscillation with the usual circuits (Clapp, Colpitts etc) with bipolar transistor, so the easiest is to use the old CMOS (not TTL!) inverters. HCMOS/HCTMOS may be also good but I did not try them, only CMOS.
There is a paper on SPICE crystal oscillator simulation at http://www.corningfrequency.com/catalog/papers/ane_005.pdf but it deals with a 12MHz oscillator.
See also the paper on crystal CMOS oscillators at http://www.eetasia.com/ARTICLES/2001APR/2001APR23_AMD_AN1.PDF where there is series resistance in the feedback path with the given value --it may help oscillation.
I did not do crystal oscillator simulation in SPICE, only in Serenade with bipolar transistor and for a few MHz and higher frequencies.
I built a very low power one (< 5uA) several years ago and it is difficult to get such low power and maintain stability over -40 to 85 temp range.
I used the single pack CMOS and HCMOS while I was building prototypes. I found that the 4069 (I think that was the CMOS invertor I used) was the best of the bunch. Is really does matter on the crystal that you use, so read the application notes and do the sim. Especially if it is a production unit. If is just for fun and you don't want to do the work, I have recently seen 32KHz oscillators. I remember looking for them in the past and did not have much luck.
Anyway, If you still need a good circuit, let me know and I will try to dig it back up.
Reduce the Q of the subcircuit representing the crystal to 100-1k by increasing the series cap and decreasing the series inductance. The reduction should not be too low if your active circuit uses amplitude regulation. The settling time scales with the Q so you can calculate the time. Startup of your simulation, not your oscillator should be by an inititial condition of the series cap in the crystal model. At high Q some volts are needed. Time step maximum set to period/50. The lowest power is a single transistor bipolar pierce. With regulation you do not need margin for tolerances and Q spread.
I am designing a 32KHZ crystal Osc. Rfb is 15mhom, series resistance is 200kohm.-ve resistance is around 2.7times ESR of crystal. It is a pierce CMOS oscillator. In open loop analysis , gain is more than unity at resosnant freq and phase drops below zero at that freq.
But I am not getting startup in closed loop transient analysis.
Decreasing the Q is not a solution as we are increasing motional cap by 50 times which is not possible in real world.
Say crystal motional capacitance for AT cut 32KHZ is around 0.0035pf. If I increase that by 50times, then it is oscillates. Startup time is around
say 100us. Then with real Q, it should oscillate by 100us * 50 =5ms. But nothing is happenning evenif I simulate for 100ms.
(a)So what kind of noise we should introduce to start a closed loop simulation(which is similar to real world) ?
Now I am ramping up power supply in 10ns.
(b)If I increase the motional cap by 50times(Q increased), then it oscillates. I did ac analysis for that crystal model which showed in consistent gain of around 5-6db around that freq range. So if more gain is the requirement, that also I have tried.
I increased the inverter strength so much that always gain is around 4-5db even before the resonance freq, still nothing is happenning with actual Q.
If the Q is too high the simulator static and dynamic accuracy settings simple damp any oscillation built up. The following settings should be used:
1. Force the trapezoid integration method. In this case the mapping from continous poles to discrete time poles is exact at the stability border.
2. Set maximum time step to < 1/100 of the expected oscillation period. Other wise the stepsize choosen by the simulator ignore simple the initial startup.
3. Set the accuracy between 10e-4 and 10e-6. The stepsize also depend on the static accuracy setting.
The startup current source should be in the best case a random number with gaussian distribution and an variance equal to the integrated current noise spectral density over the hole frequency. The problem with realistic single pulse startup is that it inject into the tank less energy because only the very narrow frequency range with the tank Q receive startup energy. I have seen startup with noise source but not with single startup pulse for the same freqency spectrum and noise energy. I did not dive deeper there and it is more than a decade ago.
This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
By continuing to use this site, you are consenting to our use of cookies.