# how to simulate the input refered noise of an integrator in cadence/spectre

1. ## how to simulate the input refered noise of an integrator in cadence/spectre

As the figure shows, do the noise simulation, but the output and negative input node of the amplifier is not "directly" biased, how to get the input referred noise data from simulation?
Thanks

•

2. ## Re: how to simulate the input refered noise of an integrator in cadence/spectre

Simply specify Iin as iprobe in noise analysis statement.

1 members found this post helpful.

3. ## Re: how to simulate the input refered noise of an integrator in cadence/spectre

Thanks. One issue is that the output of the integrator is vdd or 0, since there is no dc feedback to control it, which gives a wrong simulation data.

•

4. ## Re: how to simulate the input refered noise of an integrator in cadence/spectre

Originally Posted by shanmei
One issue is that the output of the integrator is vdd or 0,
since there is no dc feedback to control it,
which gives a wrong simulation data.
I can not understand what you want to mean at all.

"noise analysis" is same as "ac analysis".
So there is no problem even if there is no dc feedback to control output.

1 members found this post helpful.

5. ## Re: how to simulate the input refered noise of an integrator in cadence/spectre

Depending on the amplifier parameters, you can either achieve useful bias by setting an initial condition for the initial transient solution, or add a very high feedback resistor during simulation.

1 members found this post helpful.

6. ## Re: how to simulate the input refered noise of an integrator in cadence/spectre

Thanks, Pancho_hideboo.

For the dc analysis, it is not stable, the opamp behaves like a comparator.

The integrator only works at the trans-simulation, the input current source keeps absorbing current from the feedback capacitor, and the opamp will keep the voltage of the inverse node of the opamp to be equal to Vref, the output node of opamp voltage is Vout=Iin.*t/C.

For noise simulation, the negative loop seems not start to work, so the output voltage of the opamp is either vdd or 0. Then the simulation result is not right.

- - - Updated - - -

Thanks, FvM.

It is a good idea for setting the initial condition.

For adding a large resistor feedback, it might lead to output to be vdd or 0. Iin*Rf will form a voltage drop delta_V,
then the output voltage of opamp is Vref+delta_V or Vref-delta_V, which might be Vdd or 0 separately.

7. ## Re: how to simulate the input refered noise of an integrator in cadence/spectre

Use analysis dependent switch such as "analogLib/sp1tswitch".

If your circuit is truely unstable in DC, connect very large resistor parallel to capacitor. Here you should set inoisy=no in resistor.
Or use "analogLib/dcfeed".

1 members found this post helpful.

•

8. ## Re: how to simulate the input refered noise of an integrator in cadence/spectre

Originally Posted by pancho_hideboo
I can not understand what you want to mean at all.

"noise analysis" is same as "ac analysis".
So there is no problem even if there is no dc feedback to control output.
You are right. Thanks.

--[[ ]]--