How to use ParamSweep to Sweep Two Parameters in ADS?

Hello!
Does somebody know how to sweep two parameters in ADS at the same time?
For example, I would like to obtain a result of simultaneously capacitive and inductive tuning in RLC tank.
I've found an example on Agilent web seit, but they use DC sweep along with Parameter Sweep. So it didn't help me.

Thank you in advance!

Nested parameter sweeps are easy to set up.



The outer Parameter Sweep, for L in this case, (Sweep2) refers to the inner Parameter Sweep, for C in this case, (Sweep1) and that in turn refers to the simulation controller SP1 (or HB1 etc.). Each sweep is then configured with the appropriate parameter range or frequency range.

Thank you for the answer RealAEL!
It works, but I've faced with a next problem. This way of sweeping provides a results for each pair of C and L. Actually I don't need all of the values. I've made a two sweep plans, which consist of three different values for C (like 1, 2 ,3) and three values for L (4, 5, 6). So I need the curves only for such pairs C=1 and L=4, C=2 and L=5, C=3 and L=6. Is it possible to do this?

The easiest method to see simulation results for individual pairs of parameter values is not to use parameter sweeps at all. You can do this simply by running the simulation in tune mode.

To do this set the required L and C parameter value to enable Tuning and set the require mix/max/step values for each. Then launch the simulator and in the Tune Parameters UI use the up/down arrows to set the required parameter value pairs. ADS will simulate the circuit at this setting automatically and display the results in the Data Display for that pair of values only.



The alternative approach is to simulate at all values using the parameter sweep and then display only the results for the required pair of parameter values. In my example I have 5 possible values for C at 1pf through 9pf in 2 pF steps (indexes 0 through 4) and 5 possible values for L 1nH through 9nH in 2nH steps (indexes 0 through 4).

To see the simulation results for C=7pF (index=3) and L=5nH (index=2) change the measurement display to index the required data. So for example instead os displaying dB(S(2,1)) which displays all simulation data use dB(S2,1)[2,3,::]). The "::" represents all values in the frequency sweep used for the s-parameter simulation.

A further alternative is instead of specifically entering the exact indexes of the required measurement would be to add two sliders to the Data Display each linked to one of the parameter value L or C. You can then simply move the slider to the required value and the display will show the equivalent simulation data.

I was using Tuning before. It's not proper way for me, since there is no option to save the stored results and it will be lost after closing the Tuning window. (or maybe it's possible?)
The third method also not suitable, because I need to see all of the curves for each interesting pairs. But I didn't know this slider method before. Maybe it will be usefull in future. Thank you!
The second solution is perfect! Thank you, RealAEL, for such detailed explanation. It really helped.

mr_evo said:

So I need the curves only for such pairs C=1 and L=4, C=2 and L=5, C=3 and L=6. Is it possible to do this?

Click to expand...

If you want to do this, the data access component is your friend. You can create an MDF file with the combinations that you want, and then simulate these (and only these) combinations. Very easy and convenient. I have attached a screenshot where I used this for component model fitting. My variables where values and also S2P filenames. It your case, it would be simpler because you only need the values.

volker@muehlhaus, I've tryied this method, but an error occurs. Whats wrong with my simulation settings?

iVal1 in your DAC should be dataindex-1, not INDEX-1

Many many thanks volker@muehlhaus . Now it works.