How to measure input referred noise in HSPICE/Cadence?

.noise hspice

I designed a Transimpedance Amplifier (TIA) using 0.18um

Now I face problem in trying to measure input-referred noise of the system.

Can anyone teach me how to do this using HSPICE or Cadence?

hspice measure noise integrate

When you do an AC simulation hspice computes the input and output refered noise. It puts the integrated noise in the output *.lis file.

bastos

input referred noise in cadence

do you mind give me an example netlist on how to do this? do i need to use .noise ?

hspice noise

Here is an example:

.Title RC noise
R1 IN OUT 1K
C1 OUT 0 10p
V1 IN 0 1.0 AC 1.0 0
.AC DEC 10 1 100MEG $ AC analysis is required for noise analysis
.NOISE V(OUT) VIN 10
.PRINT INOISE ONOISE
.OPTION POST
.END

Save the above lines in file 'rcnoise.sp', and run
hspice -i rcnoise -o rcnoise

Then, have a though view for the file rcnoise.lis. You will find input and output noise in that file.

hspice .noise

is it right?
i can not run it correctly with Hspice
it says
**error**: element 0:vin has been
referenced but not defined id= 9

***** job aborted

measure input voltage noise

If you can use cadence why not use cadence directly. Under your analysis select noise. Change everything into voltage. If you wan to measure input referred noise voltage. To measure current you would need a port connected to it.
First of under noise analysis. Select the range of frequencies you wan. Select the output node by clicking select go to your schematic and select the node. It would be automatically updated. The second node select it to point to ground which is /gnd! in cadence analog design environment.
For the input source change it to voltage. A warning will be given cos the Noise figure is calculated based on current. Don't worry about that.
Remember the input source is to inform the simulator where is the input so that it can calculate the input referred noise.
Run your simulation. Nothing came out. Hehe go to result direct plot, You can see equivalent input/output voltage or squared input/output voltage.

This is basically not enough. Pin point the noisy components. Go to result print Noise summary. Select the type of output either in terms of V squared or sqrt at the right up upper side of the form. Select integrated noise meaning the noise at certain frequency. Under filter select the devices you wish to see. Under truncate and sort select by number then choose to top 30 to allow you to see the top 30 contributor of noise. Select apply and wait a while. The printout will have all the information, how much each component contributes and the total output / input referred noise is available.

One more thing. If your device model is BSIM3v3 please take note that the gate resistance thermal noise is not modelled. Trust only 50% of the result.

hspice　noise

xusoso said:

is it right?
i can not run it correctly with Hspice
it says
**error**: element 0:vin has been
referenced but not defined id= 9

***** job aborted

Click to expand...

Sorry. VIN should be V1.

Bro, then what about Mentor Graphic ?

I using Ac analysis to simulate out Input noise and output noise, but how i simulate input referred noise ?

Hughes,

A very comprehensive expln. of Noise summary. Thanks a lot. I was able to get the noise summary.
I now need to calculate the SNR of my DAC output.
How do I go about it. Please help.

Thanks and regards,
Guru

Re: hspice noise

:shock:
HI I have achieved the waveform of input noise and output noise, however i think there is something wrong about the noise value. should output noise equal to input noise times gain? Thanks!

---------- Post added at 08:30 ---------- Previous post was at 08:29 ----------

HI I have achieved the waveform of input noise and output noise, however i think there is something wrong about the noise value. should output noise equal to input noise times gain? Thanks!