Hi @Stefan Schippers, one question. I am trying to set up all the xschem testcases we already provided in IHP-Open-PDK using Xyce simulator. Since our mosfets use PSP103 Verilog-A model it have to be compiled to either to

osdi

(for ngspice) file or

so

library (for Xyce). In the case of ngspice is simple because you can inform it using

.spiceinit

where the actual

osdi

file is. Xyce does not have it so you have to run the netlist calling

Xyce -plugin ../../../admslibs/Xyce_Plugin_PSP103_VA.so nmos_id_vg_vb.cir

My question is if it is possible to define it on schematic and then pass to xyce this

-plugin path_to_file/plugin.so

It is possible to change the simulation command. Go to Simulation->Configure simulators and tools-> locate the Xyce batch line and change the command, adding the required -plugin options. You can do this programmatically:

# Setup the default simulation commands if not already set up
set_sim_defaults
# Check the name of the 4th (0,1,2,3) spice simulation command:
puts $sim(spice,3,name)
# --> Xyce batch
# get the command
puts $sim(spice,3,cmd)
# --> Xyce "$N"
# Change the command
set sim(spice,3,cmd) {Xyce  -plugin /.../.../... \"$N\"} 
# Change the simulator to be used (Xyce)
set sim(spice,default) 3
# run netlist and simulation
xschem netlist
simulate

You can place a launcher (launcher.sym) in the schematic and trigger the above commands by ctrl-clicking it (Left button click on the launcher by holding down the Ctrl key). The attributes in the image are copied here:

name=h8
descr="Simulate with Xyce" 
tclcommand="
# Setup the default simulation commands if not already set up
# for example by already launched simulations.
set_sim_defaults

# Change the Xyce command. In the spice category there are currently
# 5 commands (0, 1, 2, 3, 4). Command 3 is the Xyce batch
# you can get the number by querying $sim(spice,n)
set sim(spice,3,cmd) {Xyce -plugin /.../.../... \"$N\"}

# change the simulator to be used (Xyce)
set sim(spice,default) 3

# run netlist and simulation
xschem netlist
simulate
"