Hello, How could i simulate the corners (ss, sf, fs and ff) with the tt and plot it in same graph? C...

Hugo Dias

07/09/2022, 10:35 PM

Hello, How could i simulate the corners (ss, sf, fs and ff) with the tt and plot it in same graph? Could i do it just using ngspice+gaw or ngspice only?

Pranav Lulu

07/10/2022, 2:23 AM

What do mean by with tt and plot in the same graph?

Stefan Schippers

07/10/2022, 5:11 AM

@Hugo Dias Run multiple simulations with different corners, use the write nsgspice command to save in different .raw files, then use gaw and load these files. Picture shows ring oscillator simulated with ss and tt corners. 2 raw files loaded into gaw.

🙌 1

Hugo Dias

07/10/2022, 7:12 PM

@Stefan Schippers It works, thanks! But how to export to raw files more than voltages and currents (like variables)?

Juan Andres

07/11/2022, 5:40 AM

Hello, How can I do all the simulations with all the corners? Do I have to do many simulations or can I do that in one

Stefan Schippers

07/11/2022, 5:51 AM

@Juan Andres Yes you have to run more simulations. you can write all data in a single raw file if you want, by doing

set appendwrite

before issuing the write command. Check the ngspice manual for this.

Stefan Schippers

07/11/2022, 5:53 AM

@Hugo Dias ngspice saves all voltages and voltage source currents if command

save all

is given before the tran , dc, ac command. If you give

.option savecurrents

ngspice saves everything including all device currents (gate, drain, source currents for MOS etc).

.option savecurrents

.control

save all

save @m.xm2.msky130_fd_pr__nfet_01v8_lvt[gm]

tran 1n 100n

remzerovec

write test.raw

.endc

If you want additional variables (transistor gm for example) you must explicitly save it as shown above for mos

m2

. The remzerovec is a quirk that eliminates zero vectors to prevent errors from ngspice when writing the raw file (see https://sourceforge.net/p/ngspice/bugs/596/)

Juan Andres

07/11/2022, 6:12 AM

But I can join all the files at the end? I ask because in the manual it presents during the simulation

Stefan Schippers

07/11/2022, 6:18 AM

@Juan Andres I don't know what you want to do, however if you have 2 raw files you can append these 2 files into a new raw file: on linux:

cat test_gm_id1.raw test_gm_id2.raw > test_gm_id.raw

and you can see the 2 traces in a waveform graph:

Juan Andres

07/11/2022, 3:21 PM

Yes I want that but with set appendwrite .raw1 .raw2 > .rawnew I will can to get a one file?

Stefan Schippers

07/11/2022, 9:14 PM

@Juan Andres

set appendwrite

does exactly what it says, simulation data is appended to the existing raw file. If you run 1st simulation with no

set appendwrite

and all next sims with

set appendwrite

you get a unique raw file with all sims 1st simulation:

Copy code

.control
  save all
  tran ...
  write file.raw
.endc

next simulations:

Copy code

.control
  save all
  set appendwrite
  tran ...
  write file.raw
.endc

At the end

file.raw

contains all simulations.

Hugo Dias

07/12/2022, 2:47 AM

@Stefan Schippers But if i want to export variables which was created by "let" command. Like in my case, i want to export "tc" and tc is: "let tc=deriv(v(vts))". What i need to do? (vts is a node and i ran the temperature sweep)

Hugo Dias

07/12/2022, 2:51 AM

@Juan Andres Lopez Cubides I changed the final of the .lib content. Change tt to ss, sf, fs and ff and run diffrent simulations. In each simulation, i go to xschem simulation path and change manually the .raw file name. But i will try the Stefan suggestion.

3 Views

Open in Slack

Previous Next

What is Linen?

Linen is a search-engine friendly community platform. We offer integrations with existing Slack/Discord communities and make those conversations Google-searchable.