VCCAP Usage and Documentation

This is implemented with spectre's "vccs" component, so you can find out more by typing "spectre -h vccs" in a terminal window.

As a simple example, if you have the controlling pairs set to 2, and controlling volt 1 as 0, and controlling volt 2 as 1, with Corresp Element 1 as 1p, and Corresp Element 2 as 5p - then the controlling voltage inputs will effectively switch between a 1p capacitor and a 5p capacitor depending on whether the input is 0V or 1V. How smooth the transition is between cap values is dependent upon Delta (which can be between 0 and 0.5). You can also scale the capacitor value using the Scale factor parameter. You can have more controlling pairs to model a different transfer function between the controlling voltage and chosen capacitor value.

I did notice that it doesn't do a fantastic job of timestep control so use with caution.

Regards,

Andrew

Hi Andrew,

Nice to meet you again! Thank you for your help, but I am still confused about the detailed operation. 

Shall I use the vccs and change its type as vccap or shall I just directly use vccap? It looks like the document in terminal is all about vccs and it indeed can be treated as vccap. But then what is the function of the vccap? It does not have any parameters. Is vccap just a symbol and the substantial part is vccs?

Thanks!

Mingqiang

In addition,

I am not sure whether my configuration below is correct. As you can see I used two voltages to control this vcaap, the first voltage is set at 0 and transits to 1.8V after 100ns and the second voltage source is simply set to 0 as always. Then I use transient simulation but gets linear increment voltage at the capacitor's output which is also strange. I doubt my configuration is wrong. If I want to have a capacitor whose values vary between 1pF and 5pF with 0.5pF step, do you think I shall change the driving voltage or I shall change the vccap? Thanks!

It doesn't matter whether you use vccap from analogLib, or vccs with the type set to vccap - they end up being netlisted as the same in the spectre netlist.

I tried these and they are equivalent:

In my case that means that the cap changes from 1p (at 0V across the differential input) to 5p (when 1V is across the controlling input).

You can also use "Linear" mode of the vccs like this:

Yes, the name "Transconductance" and units (Mhos) is a bit odd for a capacitor - this is the C/V of the vccap (so that means 2pF/V). This will be 0F for 0V, and 2pF for 1V.

Andrew.

Thank you very much Sir! I have successfully used the VCCAP by changing the voltage inputs. May I ask an additional question here: how can we observe the capacitor size directly and plot a graph of another variable against it?

I am doing the transient simulation of the capacitor with a hysteresis opamp. I want to plot the the period of oscillation against the capacitor size. The period can be obtained using the function delay() in the calculator and the capacitor size can be calculated using control-voltage*transconductance. However, this means I have to plot the graph manually by retrieving each data from the delay() function and and the capacitor inputs by calculation.

I don't know whether Cadence can convert all these calculations automatically and plot them just like we plot the cgg of mosfet vs input voltage by inputting "save mos:oppoint".

If Cadence cannot automatically do these, I will do them manually.

Thank you again!

Best Wishes,

Mingqiang

Hi Mingqiang,

Yes, you can plot :lx0 for the vccs/vccap (see "spectre -h vccs" again). If you use Outputs->To Be Saved->Select OP Parameters in ADE you can do this directly through the UI - click on the component in the schematic, and then type in lx0 in the Operating Parameters box (the "..." allows you to get the available parameters from a simulation too)..

Andrew

Hi Mr. Andrew,

Sorry to disturb you again! But I have a question about the period plot against varying capacitor.

In the calculator function, we can plot frequency against time. I have obtained a graph as shown below:

However, the frequency is not linearly related to the capacitor value. Hence we want to check whether the period can be plotted against the capacitor's value, rather than against the time period to prove the linearity.

May I kindly ask if you know anyways of doing this. 

Thank you very much!

Mingqiang

Hi there, a quick update. I have found 1/frequency can help me get the period. Now the question becomes how to plot the period against the capacitance. Thank you!!

Dear EEE student,

I believe you need to include an impedance analysis in your transient simulation and, using the current measured through your vcvap, determine its capacitance. The resulting capacitance value can then be plotted against any other waveform using the calculator function. 

As a student, you are hopefully familiar with the relationship between impedance and capacitance. As such, you must consider the phase of the measured current relative to the nodal voltages  across your instance of vccap.

I hope this provides the guidance you were hoping for.

Shawn

Hi Shawn,

Thank you for your reply! However, I don't quite get your point of impedance analysis. Probably I should add the whole picture here.

This is a voltage controlled capacitor and its capacitance is determined myself. This capacitor is used in a Hysteresis opamp and once it becomes larger, the hysteresis opamp outputs square wave has larger period. 

Theoretically, the period of the output waveform should have relationship ln(k)*RC, where k is theoretically determined by the threshold of the v+ and v-. 

However, practical situation is more complex and hence we want to know exact relationship between the period and this C and hence a graph plotting is needed.

Unfortunately, 1/freq in the calculator only plots the output period against time, rather than against the capacitance.

If you know how to plot it against the capacitance, I will appreciate!

Thank you!

Mingqiang