VCO frequency vs tuning voltage - how to display simulation

Hello,

I'm currently working on a vco design. I would like to plot the vco
oscillation frequency vs varactor's tuning voltage. In Hspice I could
create the following test bench:
..tran 10p 10n sweet Vtune 0 1 0.1
which basically creates the output file with waveforms for Vtune from
0.1V to 1V with 0.1V step.
I think I can achieve the same result with spectre test bench commands:
sweepVtune sweep dev=Vtune par=dc start=0 stop=1 step=0.1 {
tran00 tran ....
}

Now, under Hspice's graphical tool for displaying the data, I can plot
all 11 curves vs time. Then change the plot to their frequencies vs
time, then change the x-axis to Vtune and get frequencies vs Vtune
voltage. How can I achieve this in Spectre tool? I've tried using awd
and wavescan but without success. Is there any other tool which can
easily achieve this or I miss some trick under awd/wavescan?
I don't use and don't intend to use Analog Environment. I have created
the test bench manually and would like to plot the necessary data under
some stand-alone tool. I use IC5141 software.

Thank you for your feedback.
Robert

 

[Thomas Ussmueller]

You can either enter a formula similar to the one above in the outputs
section of the ADE (you have to replace /net3 with your net for the
tuning voltage)

harmonic(xval(getData("/net3" ?result "pss_fd")) '1)

or the other, and in my opinion easier, possibility is to use the direct
plot form. In ADE locate the menu Results->Direct Plot->Main Form...
Choose analysis pss and set Function to Harmonic Frequency. At the
bottom you can choose the harmonic you want to display.

You could try and search the internet for a Cadence application note
that describes VCO design with spectreRF. It is very helpful.


Best regards
Thomas


tempora@gazeta.pl wrote:

Hello,

I'm currently working on a vco design. I would like to plot the vco
oscillation frequency vs varactor's tuning voltage. In Hspice I could
create the following test bench:
.tran 10p 10n sweet Vtune 0 1 0.1
which basically creates the output file with waveforms for Vtune from
0.1V to 1V with 0.1V step.
I think I can achieve the same result with spectre test bench commands:
sweepVtune sweep dev=Vtune par=dc start=0 stop=1 step=0.1 {
tran00 tran ....
}

Now, under Hspice's graphical tool for displaying the data, I can plot
all 11 curves vs time. Then change the plot to their frequencies vs
time, then change the x-axis to Vtune and get frequencies vs Vtune
voltage. How can I achieve this in Spectre tool? I've tried using awd
and wavescan but without success. Is there any other tool which can
easily achieve this or I miss some trick under awd/wavescan?
I don't use and don't intend to use Analog Environment. I have created
the test bench manually and would like to plot the necessary data under
some stand-alone tool. I use IC5141 software.

Thank you for your feedback.
Robert

 

Thank you for your remarks. I have modified your expression to get the
plot under awd. FYI, its syntax is:
plot(harmonic(xval(getData("/net3" ?result "pss_fd" ?resultsDir
"/path/to/sim_dir")) '1))

But I must admit that I was a bit lucky here to get the above formula
correct. My last question is where I can get more information on
creating this and similar kind of expressions to plot different things
directly from awd?

I must admit I hoped there was an easier way to plotting such things in
awd or wavescan. But maybe there is a "clicking" way to doing it which
I don't know of.

Anyhow, thank you for your help.

Robert

 

[Thomas Ussmueller]

I haven't written the formula myself. The direct plot form did that for
me. This form form has a "add to outputs" button with that you can copy
the expression created to your outputs field in your analog environment.

The command reference for the functions for evaluating your simulation
data can be found in the ocean command reference (have a look at cdsdoc).

beest regards
Thomas

tempora@gazeta.pl wrote:

Thank you for your remarks. I have modified your expression to get the
plot under awd. FYI, its syntax is:
plot(harmonic(xval(getData("/net3" ?result "pss_fd" ?resultsDir
"/path/to/sim_dir")) '1))

But I must admit that I was a bit lucky here to get the above formula
correct. My last question is where I can get more information on
creating this and similar kind of expressions to plot different things
directly from awd?

I must admit I hoped there was an easier way to plotting such things in
awd or wavescan. But maybe there is a "clicking" way to doing it which
I don't know of.

Anyhow, thank you for your help.

Robert