The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> help on error msg
https://designers-guide.org/forum/YaBB.pl?num=1175244600

Message started by rankati on Mar 30^th, 2007, 1:49am

Title: help on error msg
Post by rankati on Mar 30^th, 2007, 1:49am

hi Gurus, Im a new user to cadence. I use NCSU libraries in cadence to simulate my analog circuits. when adding voltage sourses as inputs I got an error "wave form type must be specified if any wave form parameters are given" as problem found in hyrarchical flaterning. Could you pleasehelp me to overcome this error and simulate my circuits.

thanx and best regards
Awantha

Title: Re: help on error msg
Post by Ken Kundert on Mar 30^th, 2007, 9:33am

Spectre is different from SPICE in that it allows you to specify the parameters for several waveshapes at the same time, but then it also requires you to specify which waveshape you want. To do so, you use the "type" parameter. Possible values are "type=dc", "type=sine", "type=pulse", "type=pwl", etc.

This feature is convenient because it allows you to quickly switch between input waveshapes by changing the value of a single parameter, which can manually between runs or using the alter statement within a single run (oh yes, Spectre also allow you to have multiple transient analyses).

-Ken

Title: Re: help on error msg
Post by Andrew Beckett on Apr 11^th, 2007, 8:04am

This problem occurs if you forget to set "CDS_Netlisting_Mode" and are using things like vsin, vpulse etc from analogLib. What happens is that it misses out any "default" parameters (such as the type), and you end up with this kind of error message.

Before you start DFII, ensure that you have done:

setenv CDS_Netlisting_Mode Analog (if using csh)
export CDS_Netlisting_Mode=Analog (if using ksh or bash)

or if you're using sh (Bourne Shell), you need to od:

CDS_Netlisting_Mode=Analog
export CDS_Netlisting_Mode

Regards,

Andrew.