Jon wrote: > I often wonder if anyone from Synopsis bothers to monitor this list. I > don't > recall ever > seeing any advice from them, ... Actually, I'm fairly certain I have recognized one or two names responding to mail on this list who are in HSPICE support and have been since before Synopsis took over. I wouldn't blame them if they don't advertise that fact, as they could get inundated with e-mails from everyone on this list who uses it and has ever had a problem. After all, their job is to support a commercial product, through proper support channels, not necessarily to offer free advice to everyone on this list. Julia, re: "internal timestep too small" messages: This is one of the most common and perplexing errors in SPICE, and it pre-dates HSPICE. There is no one cause, nor is there one "fix". Start to get more adventurous with the .OPTIONs. Try loosening up the various *TOL options (some of which go by different alias names in Hspice). Open them up by several orders of magnitude, and if this lets your simulations work, then go back and tighten them up. They WILL cause bogus and misleading results if left very loose. You've already tried Gear. Things that work for one person's circuit, may do nothing in another's. Component values spanning a very wide range tend to not do well in Spice. So if you have micro or milliohm and megohm resistors in the same simulation, see whether you really need the tiny ones. If someone added tiny resistors to make "connections" between nodes, replace them with shorts or 0V voltage sources. This may go against your conscience or your gut feelings, but lots of 0V voltage sources are usually much better in Spice than lots of 1e-6 resistors are! There are Hspice options that will add a small capacitor, or a small conductance, at every node, not just a few. Try playing with these too if you haven't already. Don't be afraid to use values much larger than actually exist. Your first job is to get the darned thing to converge; then you can go back and tweak things until it just doesn't break. Try simulating the connector model and everything else separately, as a sanity check. Or try different drivers and receivers with the connector model. Alas, many Spice problems don't show up until you connect things together, as if the elements are somehow "incompatible" in some way. If it is a complex connector model, maybe there is something wrong, either with the model or how you are using it, so make sure to try it with different connections (terminated or open or short circuited on the various pins) to see if one of them causes ill behavior. There could be issues with grounds on the two sides of the connector model; make sure you fully understand how it is supposed to be used in that regard. If node 0 appears on both sides, might that be an unrealistic sneak path short-circuit around the connector? Some models are meant to be used that way, some aren't, and some models probably don't handle grounds right anyway. Regards, Andy ------------------------------------------------------------------ To unsubscribe from si-list: si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field or to administer your membership from a web page, go to: //www.freelists.org/webpage/si-list For help: si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field List technical documents are available at: http://www.si-list.org List archives are viewable at: //www.freelists.org/archives/si-list or at our remote archives: http://groups.yahoo.com/group/si-list/messages Old (prior to June 6, 2001) list archives are viewable at: http://www.qsl.net/wb6tpu