OK, a few things are wrong here: I'm not sure why you created a schematic from the hspiceText view, because this will just contain the pins. The schematic creation using create cellView from cellView only creates an empty schematic other than the pins. I'm sure you didn't really mean to do this. When the schematic view is created using create cellView from cellView, it is saved, but not check-and-saved. That's why you are getting the net listing error (the error would go away if you did a check-and-save of the schematic with the three pins, but you'd then not get a sensible simulation because you'd just be simulating an empty schematic!) So what you really want to do is add the text view into the switch view list in Setup->Environment. However, hspiceText views are not supported with spectre as the simulator - they netlist, but there's no inclusion of the resulting netlist (not sure why this is the case - it's probably an oversight - although perhaps it's only designed to work with hspice). So instead, create a "spice" text view (default name "spiceText") and paste in the same model text that you had. Then add spiceText into the switch view list on Setup->Environment (near the beginning - certainly before any schematic view). If you then simulate, it will netlist and include this view, but fail because of the line: .MODEL RTEMP RES (TC1=9E-3 TC2=5.5E-6) Change the "RES" to "R" in that line in the spiceText view and all will be OK Regards, Andrew.
↧