To annotate the schematic with operating point data (on recent xschem versions) go to

Waves -> OP annotate

, then choose the right raw file. To load the DC simulation go to

Waves->DC

and load the appropriate file. The launcher command

xschem raw_read $netlist_dir/tb_bg_dc.raw dc

loads the DC simulation. If there are multiple simulations in one file it is better to specify the simulation (dc, ac, tran) To annotate the operating point the command is:

xschem annotate_op $netlist_dir/tb_bg_op.raw

Net labels and I/O pins will show the voltage value, voltage sources, resistors, ammeters will show the current. (for resistors add .

option savecurrents

)

Thanks, i forgot to use

annotate_op

. If i have a bandgap curvature in DC sweeping the temperature, why this command is not working in DC?

.measure dc ymax MAX v(vbg) from=-40 to=150

The name of the net is

vbg

, in transient

tran

it fine, where is the problem?

It seems there is a problem when a measure is used in a

dc temp

sweep. ngspice is looking for a

v-sweep

variable, while for temp sweeps the variable is called

temp-sweep

. Try to forward this to the ngspice devs.

Error: no such vector as time, frquency or v-sweep.

Error: measure  ymin  min(TRIG) : out of interval
 meas dc ymin min v(outm) from=-40 to=150 failed!

I open a ticket, and the guys has already resolved this kind of bug. Will be resolved in versione 42 of ngspice.

Thank you! 👍

commit 3b38125afd5dfee2b7661789773becd650c5ad78
Author: Holger Vogt <holger.vogt@uni-due.de>
Date:   Fri Dec 8 10:32:15 2023 +0100

    Enable measurements with ?-sweep (v, i, temp, or res).
    Improve error messages.
    Prevent crash is compüdata is not available.
    Add to examples for measure failures.