cadence virtuoso available utilities

Dear auto dipper,

 > i have drawn the schematic of a majority circuit in cadence virtuoso IC610 version and have

> done transient analysis over it. want to check the net capacitance of each node.

I am afraid I am little confused about what exactly you are trying to display. If the netlist is based  on your schematic only, then the nodal capacitances are zero as the MOS capacitances are all contained in each device model. The actual "effective" capacitance on each node will depend on the number of devices connected to the node of interest and the specific manner in which they are connected. For example, if a device has its gate attached to the node, not only will the MOS Cgs and Cds contribute to the nodal capacitance, but its Miller capacitance will also contribute to the nodal capacitance. Therefore, to ascertain the capacitance at a specific node requires a series of small-signal analyses where the impedance of each node is determined over the voltage range of the node. For each small-signal analysis, one computes the effective capacitance at a specific frequency from the imaginary part of the impedance seen at that node. The small signal analyses can be done using the Spectre actran analysis feature at the time points in the transient analysis you specify. 

I hope you understand what I am trying to explain. The computation of nodal capacitance from a pure schematic based netlist is not an "automated" process nor is it a trivial computation from a transient analysis.

If your netlist is created from an extracted view of a layout, there is a parasitic tool that can be accessed from the Virtuoso Launch->Parasitics menu item. The specific extracted view to use and the signal grounds are selected in the new Parasitic menu that will then appear under Parasitics->Setup... The resulting nodal capacitances due to the layout parasitic capacitances can be either sent to a file or displayed on the schematic.

I may not have understood your specific request - and apologize if I did not!

Shawn

hi 

just like we include model files from ADE. for example tsmc etc.. so how can one include a file in which i have entered some options like

dcOp dc write="spectre.dc" maxiters=150 maxsteps=10000 annotate=status \
infoname=capinfo2
capinfo2 info what=captab where=file  file="capnodesdc"
dcOpInfo info what=oppoint where=rawfile

Dear auto dipper,

The captab feature is on the Options tab of the transient analysis  GUI of the ADE. However, it will not always produce the proper node capacitance. For example, please read Solution 11177864. This is why I was not sure what you were specifically trying to determine. If you rely on captab, your result may not be consistent with whatt you were hoping to compute.

Shawn

Sorry about all the emails advising new posts - I was trying to clean up the mess caused by the fact that this had been appended to a completely unrelated post (which the forum guidelines explicitly ask you to avoid, as it means readers of the posts who are searching for things in future get horribly confused).

There's no need to modify the run the netlist. It's in the UI in ADE from either the dc analysis or the tran analysis. You get to it via the Options button on the bottom of either form. For transient it's on the misc tab, on DC it's on the main options form. There's a checkbox for captab, and when you enable it, you get options to control the analysis statement directly and choose whether you get node, nodetonode, or nodetoground.

The solution is slightly incorrect - actually nodetonode also gives you the total node capacitance as well as the individual pairs of nodes. nodetoground only tells you the capacitance to ground. The solution doesn't tell you not to use it - and I don't think Shawn did either. You just have to know how to interpret the results.

Also, if you really didn't want to use the UI, there's no need to actually modify the netlist - put the captab info statement in an include file and reference it via a model file. Just create a file like you mentioned earlier, call it (say) "myanalyses.scs" and then use Setup->Model Libraries and then reference the file. But since you can do this from the UI easily enough, it doesn't seem worth it to me...

Regards,

Andrew.

 Hi Andrew,

Thank you for providing the detailed instructions! Your summary of my thoughts isexactly correct. I am not sure what specifically auto dipper is trying to determine and hence wanted to make sure he or she understood how to interpret the results of captab. I was not recommending auto dipper not perform a captab analysis.

Thank you!

 Shawn