Hi @Stefan Schippers, thanks for developing xschem, I really enjoy using it. Recently I began exploring the graph function and have the following two questions: 1. In your tutorial video you plot the power lines. I am trying to plot both VDD and GND in a graph (see image). VDD was no issue, but for GND ngspice returns "vector GND is not available or has zero length". 2. If I try to save all raw signals ("write inv.raw all") and load the raw file no data is shown and the scale is off when I press "f" on the horizontal bar. There is also an empty signal loaded (see image). When I write specific signals ("write v(din) v(out) v(vdd)") the graph function shows the correct signals. Attached are two binary encoded raw files inv_writeSome.raw and inv_writeAll.raw and their SPICE files. Any idea how to resolve these? Thanks!

@Steven Bos 0 or GND (they are the same thing in ngspice) are not saved. These are '0'. If you need a '0' reference in the graphs simply add this: "GND; 0" This creates an expression with label 'GND' and value 0 I use this trick to draw reference levels, like:

"VREF; vcc 2 /"

to draw aline at VCC/2. To save all signals do this:

.control

.save all

tran .... (or dc ... or ac ...)

write <schematic_name>.raw

.endc

save all should be before the analysis line (tran, ac, dc). If you need all device currents add a

.option savecurrents

outside (and before) the .control block.

That is a great tip! I added the gnd label.

@Steven Bos I have created a 'test_inv.sch schematic that produces and identical netlist as yours (i have not drawn the circuit, i have pasted your netlist as text), ran simulation, loaded graphs all went fine. No waves disappear if i press 'f' and no empty node is present in the list. I see you load the .lib file from the open_pdks directory. This is not correct. After building open_pdks with

make

yous should do a

make intall

. This installs the pdk and the .lib file you need is there, under

..../share/pdk/sy130A/libs.tech/ngspice

. Numerous corrections are done in installed files.

@Stefan Schippers thank you very much! That was the issue.

@Steven Bos about the

"GND; 0"

trick to show a 0V level, the space in the quoted expression is very important. A space is used by xschem to detect an expression, like:

VREF;  VCC 2 /"

If you remove the space the

"GND;0"

is knot recognized as an expression. The reason is that (integer) numbers are valid spice nodes, so for example:

"TEST;5"

means "draw the waveform of node

5

,while: "`TEST: 5"` means "draw a line at y value `5`"

Check! Good to know that easy to overlook detail. The embedded graphing feature is very convenient, happy to skip the installation of yet another tool 😄

I ran myself into this problem. I entered some

"LEVEL;1"

and i didn't see any waveform, until i realized xschem was right, it was looking for a saved node named

1

. This is because for convenience you can reference (in xschem graphs) node names as

out

,

in

,

bias

in addition to

v(out)

,

v(in)

,

v(bias)

. The space is the best candidate do discriminate expressions from node names, since space is not allowed in node names. Most other characters are possible in the spice node syntax.

Ah that is also useful. I realize that learning more about the SPICE syntax parsing and execution will speed up my simulations (and put more confidence in my results). I am now exploring the use of parallel xyce since a simple 10 bit DAC simulation with ngspice took near 10 hours. Looking forward to switching to xyce in xschem, already found your instructions in the xyce channel.