AC analysis in cadence

[urian]

Hi,there
I am designing a simple 2 stage opamp,and the vdd is 1.5v and vcm is 0.7v.
I use two vdc instances for the vin+ and vin-,and set AC magnitude to ±500mv and ±1mv for the two vdc.When I run ac analysis and see the gain&phase,I found the result is different.I wonder whether the magnitude of the AC magnitude property of the vdc will influence the simulation.I think the magnitude can be set free before,am I wrong?

Thanks in advance.

 

[jgk2004]

Set your AC to 1, This will normalize your AC response to 1 which will show you what you want. Also if this is single ended you only put the AC response on one input. so Vcm on one and Vcm +AC=1 on the other. Also just to note you need a DC feedback to make sure your amplifier has the correct .Op point to start your AC response.

Jgk

 

[dick_freebird]

I prefer to have "VCC" and "VEE" (your + and -) both returned
to a node on top of a "VCM" source, which has "ACM" AC
amplitude and forces the two rails in unison (also useful for
DC common-mode sweeps).

Cadence has the "iprobe" widget that makes loop analyses
much easier to set up and pull results without so much
calculator expression fiddling.

 

[urian]

Thanks!
Yes,my opamp is diff. input and single output.I test the gain&phase without any feedback configuration,said,in open-loop,and this opamp is used for voltage-follower.As jgk2004 said,I only have to set AC magnitude in one of input instances?Must I need a feedback configuration in the inital design?
And I dont understand the Vcm usage as you say..

 

[jgk2004]

You need to ensure that your transistors are operating in saturation which means your dc operation point is correct. To ensure this, you need to have a DC feedback loop for your initial condition then you break the loop for your AC response. The very easy way of doing this is connecting your amplifier with a low pass filter in the feedback. So make a 1Farad!! cap to ground on your Vinm input then a 100Meg ohm resistor connecting your Vinm to your output. Then your input AC signal on Vinp. This is ok for low frequency amplifier design say below 100MHz GBW. But if your making fast stuff, you will need to use the STB analysis that Freebird is talking about. Connect your amplifier as the voltage follower (your DC feedback), with proper loading, then use the "iprobe" widget in the feedback path (it will "break the loop for you for AC", it is more complicated then this but if you want more info look up middlebrook, tian method). In the STB analysis, just select that "iprobe" unit and simulate. It will then say the DC gain and PM margins in your popup window. If you want to see the gain and phase plots go to your results brower and look it up!

Jgk

 

[urian]

Thank you ,jgk
But if there is no input,how can I ensure the DC operation point is correct? Because this opamp is used for resistor ladder buffer,which means that the input is just dc voltage,and I think it will influence the DC op..Then I have to configure the feedback loop first?
The method you provide is very useful for stb!

 

[jgk2004]

Just connect your input to your DC level! If its a resistor buffer connect it to the resistor buffer and add an AC source in there or a voltage source with the value of the resistor divider and AC=1. Then just simulate!

Jgk

 

[urian]

hi,Jgk
The Vcm of my opamp is 0.7v,with vdd=1.5v.And the input of two opamps laid top and down of the resistor ladder is 0.4v and 1v dc voltage.
Then should I make sure the ICMR of my opamps include 0.4v to 1.0v? Or just around 0.7v?

 

[jgk2004]

If your amplifier is a voltage follower, and your supply is 1.5V, and you will have two amplifiers one at 0.4V and one at 1V on your resistor ladder, then your amplifiers will need to be rail to rail inputs to work correctly. If they are not then you will need to design two different amplifiers, for the 0.4V you will need PMos inputs, for the 1V you will need Nmos inputs!!! Have you taken this into consideration? Also like I said do your AC response with the inputs you are using the amplifiers at! so 0.4V and 1V,
Jgk

 

[urian]

Hi,Jgk
You said my amplifier will need to be rail to rail,does it mean that the ICMR of my amplifier must be 0-1.5v for a single amplifier to operate at 0.4v and 1v input voltage,or 0.4v-1v?
I have simulated a single amplifier,and found that the pmos input diff. pair type can not see the 1v input voltage.And now I am designing another amplifier which is Nmos input diff. pair for the 1v input voltage.Should I do this?

 

[jgk2004]

If you have to have one amplifier do the same job, buffer 0.4 and 1V then yes you need a rail to rail amplifier. If you don't care then yes you need to make another amplifier with Nmos inputs for your 1V buffer. The buffer with pmos inputs will not do it!
Jgk

 

[urian]

thanks,Jgk,I will make two amplifiers to meet the job.I think having only one amplifier do the same job will make the amplifier very difficult to design.