Designer’s Guide Community

wangxy829

New Member

Offline

Posts: 2

about "annotate" function in spectre
Apr 04^th, 2005, 7:37pm

dear all:
could you clarify a question for me?
when I am using virtuoso schematic editing, if choose instances like pmos4 or nmos4 from
the standard library "analogLib", then do the simulation in affirma anlaog circuit design environment, we can annotate "dc node voltages" and "dc operating points" in schematic.
but if I choose instances like pfet or nfet from satndart library "Sample", we still can do the simulation, but the annotate function doesn't work, can't annotate the dc pionts anymore
did you encounter this before and how to solve this?

i think the properties of the two libraries are different,
for analogLib , the properties of pmos4 or nmos4 are auCdl, auLvs,cdsSpice, hspiceSspectre sprectreS symbol etc
for Sample, they are cdl hspice ivpcell lvs saber spectre spice symbol symlvs etc.
and click the properties for nmos4 or pmos4 in analogLib , there is a "choice" labele as " analog pin annotate" might be the key point.

but i want to use sample library and still need the annotate function, how to solve this?

thks all

xinyu

Back to top

IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: about "annotate" function in spectre
Reply #1 - Apr 4^th, 2005, 11:26pm

The annotation requires you to have special labels on the symbol, which are of a type "ILLabel". This means that the label is actually a SKILL function call, which is evaluated at display time.

There are three main label functions that are used:

cdsName() - which can display the cell name or instance name
cdsTerm("termName") - which can display terminal name, net name, net voltage, or terminal current
cdsParam(num) - which can display instance parameter, model parameter, operating point param etc.

You'll find that the symbols in analogLib have these parameters (open the symbol and take a look) whereas those in sample don't. The sample library was really not intended for use with the analog tools - which is why you see the stopping views are rather different than those components in analogLib. However, the spectre netlister is designed to work in both "digital" and "analog" mode, and so will netlist the components from the sample lib.

Note the magic labels mentioned above can also be controlled via the Edit->Component Display in the schematic editor, and also via the labels section of the CDF for each component.

So, my advice would be to use the analogLib components if you want to have backannotation, or to build your own primitive component library. Without editing the sample library components, you won't be able to get the backannotation to work, since they were never set up for use with ADE.

Best Regards,

Andrew.

Back to top

IP Logged

wangxy829 New Member Offline Posts: 2	Re: about "annotate" function in spectre Reply #2 - Apr 5^th, 2005, 1:57am Hi, Andrew your tips really help me a lot, I added cdsName cdsTerm and cdsParam to the instance in the Sample library, the dc node voltages are displayed, but how to display" dc operation points" there, i tried the component display, but doesn't work, could you find a final way to help me out?? bests xinyu
Back to top	IP Logged

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: about "annotate" function in spectre
Reply #3 - Apr 7^th, 2005, 1:29pm

So did you add labels:

cdsParam(1)
cdsParam(2)
cdsParam(3)

to the symbol? Are they ILLabel type?

Then you would normally do Results->Annotate DC Operating
Points from ADE (something like that). You can do it with the edit component display, but it's easier using the ADE menus.

Ah, the trouble is you need to define the default set of parameters to display if you use the above approach. You can do that by doing Tools->CDF->Edit in the CIW, setting the choice the "Base" rather than Effective, selecting the cell you're modifying (the nfet or pfet), and then modifying the label display part of the CDF down the bottom. You can choose which operating point parameters are picked by default there.

These can be overridden with the edit component display form.

Sorry for not being precise, but I'm out of the office and didn't have time to work through it (which I'd have to do to give a precise step by step answer).

Regards,

Andrew.

Back to top

IP Logged