problem of xtal 32768hz spice simulation

Status
Not open for further replies.
J

jordanzl

Newbie level 3
Joined
May 11, 2005
Messages
4
Helped
0
Reputation
0
Reaction score
0
Trophy points
1,281
Activity points
1,335
pspice xtal

I want to simulate the 32768 ossilator and use the classical circuit.
but the simulation result show the frequent is ok but the amplitude is too small,only about 10 mv.
who can tell me where the key problem in it?
the parameter of the invertor?the value of the resisters? the value of the capacitor?

if someone once met the amplitude problem ,thanks to tell me the solution.

thanks
 

xtal pspice

post the netlist you are simlating, including the description of the crystal as well as all initial conditions you use.
 

spice xtal

.tran 0.1us 5ms

VDD VDD 0 PWL (0 0 10n 5 20n 0 30n 5 40n 0 50n 5 60n 0 70n 5)

.SUBCKT XT32768K 1 2
CP 1 2 1.5000P
RS 1 3 30.000K
L 3 4 10.200K
C 4 2 2.3129F
.ENDS

*source OCSILLATE
X_cry Xin Xout XT32768K
R_Rf xin net3 100meg
R_Rd net3 xout 100k
C_Cd XOUT 0 8pF
C_Cg xin 0 8pF
C_Co XOUT 0 4pF
C_Ci xin 0 4pF

M_M170 NET3 xin VDD VDD PMOS W=18.6U L=2.4U
M_M174 NET3 xin 0 0 NMOS W=6.4U L=2.1U
.end

this is the netlist.
 

xtal spice model

First, why you use so strange VDD source?
Second, quartz oscillator start up very slowly. Is your oscillation amlitude still increasing or not? If it is increasing you should increase your simulation time.
 

xtal pspice simulation

the amplitude can increase with the time ,but it is still very small.
i tried to simulate till the 1 second and the amplitude is only about 12mv.the frequncy is correct but the amplitude is so small. so i dont know what the key factor about it.
can you give me some advice,thanks!
 

Plz refer to this post first,

hxxp://
 

enlarge your inverter size
 

what do you mean about "enlarge the inverter size?" increase the W/L ratio?
 

You may try to decrease the transient analysis timestep.
 

jordanzl said:
what do you mean about "enlarge the inverter size?" increase the W/L ratio?
Click to expand...

I'm not sure whether the driven current is small or not, so try to increase the W/L ratio to get more driven current, then observe your output swing

Added after 28 minutes:

for your information
 

to jordanzl :
i also have the same problem, and my amplitude is round mV. i haven't solved it.
 

no guy knows?
 

once i met the same problem. i think that means the xstal didn't star up. you may try to give xstal a initial current, use .ic.
increase your simulation time, and do it again.
 

Now i'm confused that when i used a small timestep then the output would have a large amp.i just don't know why. who can tell me?thanks.
 

Which simulator do you use to simulate? I wonder if you tried other xtal with different frequency,e.g 10Meg Hertz. Did you get the same results?

I just try to do the same thing using orcad/pspice but it didn't work at all even I used a gain block(can drive unlimited current) followed by the inverter.
 

The root cause is the huge inductance in the xtal modle. This can cause very very slow procedure when power on. You can use the .IC command to set the initial current for the inductor, thus you can get the normal amplitude.
 

it is very hard to simulate the transient of 32.768khz . you can using AC simulation do that .
but you must care select the feedback resistor for low frequency crystal
 

What is the typical value of the feedback resistor (Rf) for 32.768K oscillator?
1M ohm, 10M ohm or larger?

Thanks!!!
 

Dear All :

The 32.768K is real time clock BAse , in my experience , YOu just simulate the AC simulation , Check the frquency and Gain vary , It is ok , ANd then check the DC current (gain) , in the DC state , It is hard to check the 32.768K in transient .


Another Issue , In the second amplifier, DOn't using Invertor base amplifier , Using schmit trigger . Becasue power noise will couple in the crystal circuit , Becasue 32.768K is low frequency, The transient is low ,
 

Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…