Andrew Beckett
Senior Fellow
![* *](https://designers-guide.org/forum/Templates/Forum/default/starsilver.gif) ![* *](https://designers-guide.org/forum/Templates/Forum/default/starsilver.gif) ![* *](https://designers-guide.org/forum/Templates/Forum/default/starsilver.gif) ![* *](https://designers-guide.org/forum/Templates/Forum/default/starsilver.gif) ![* *](https://designers-guide.org/forum/Templates/Forum/default/starsilver.gif)
Offline
![](https://designers-guide.org/forum/avatars/elmerfudd.gif)
Life, don't talk to me about Life...
Posts: 1742
Bracknell, UK
|
1. You must be using an old version of the IC tools. The message comes from the quantity.spectre in the ahdLib - this is auto-included in the spectre netlist in order to support spectreHDL models, which required quantity definitions in the spectre netlist. In years gone by, the quantities in this file conflicted with those defined by default for VerilogA. This was fixed in October 2004, and so anything after IC5141 USR1 should not have this problem. 2. I've normally seen this occur if you have a vsource/isource/port in your schematic, and when you look at the netlist, the type of the source is missing. This usually happens because you didn't do "setenv CDS_Netlisting_Mode Analog" before starting icfb. See sourcelink.cadence.com solution number 1838670 3. Well, if you've not set CDS_Netlisting_Mode to Analog, the chances are that your circuit is completely wrong - so I'd fix that first. May well be that these will go away. What it's telling you is that the auto-inserted gmin resistors are large enough to affect the DC solution. You could try reducing gmin. Also search in this forum, because I think there are a number of posts on this. 4. It failed to compile the VerilogA models. This should not cause you any real problems, but almost certain the best bet could be to use a more recent simulator version (I don't know what you're using). Try the latest MMSIM71 version, and see if that solves it.
Regards,
Andrew.
|