#490 Plot issue with shared library

[Fabrice Salvaire]

For this particular desk

.title Pulse
Bsource in 0 v=time^4*exp(-1000*time)
R1 in out 9kOhm
R2 out 0 1kOhm
.options TEMP = 27°C
.options TNOM = 27°C
.ic 
.tran 0.001ms 20ms 0s
.end

that plot No. of Data Rows : 20008 in ngspice cli

PySpice https://github.com/FabriceSalvaire/PySpice is know to retrieve correctly plots but for this desk the plot is wrong see https://github.com/FabriceSalvaire/PySpice/issues/172

I checked for data truncation issue since the plot looks like the beginnning of the expected one.
I dumped the C array from ngspice api to check for PySpice issue.

It looks like there an issue with the API.

[Holger Vogt]

This is unfortunately not enough information to check for any bug.

What part of the ngspice api are you using to transfer the data to the host program?

[Holger Vogt]

shared ngspice simulates correctly. I have succsessfully tranferd the netlist to ngspice.dll (ngspice-32, Windows 10) and retrieved the data back to the caller. Adding a gnuplot command shows the correct output.

What the OP has shown in his 'wrong' plot is not the beginning of the plot, but is the result of a truncated input line
Bsource in 0 v=time^4 ; *exp(-1000*time)
Please check if pyspice is sending the complete input line to ngspice. You may check the ngspice input parser by sending a command 'listing' and reading the response. If the line
set ngdebug
is put into .spiceinit, then a debug output debug-out.txt is generated to show the input file after parsing in ngepice.

[Fabrice Salvaire]

I supect '*' ...

debug-out.txt is

**************** uncommented deck **************

     1       1  Pulse
     0       2  .global gnd
     2       4  bsource in 0 v= time ^   4,0000000000e+00 * exp (  -1,0000000000e+03 * time )
     3       5  r1 in out 9kohm
     4       6  r2 out 0 1kohm
     5       7  .options temp=27°c
     6       8  .options tnom=27°c
     7       9  .ic
     8      10  .tran 0.001ms 20ms 0s
    10      12  .end

****************** complete deck ***************

     1       1  Pulse
     0       2  .global gnd
     2       3  *source in 0 v=time^4*exp(-1000*time)
     2       4  bsource in 0 v= time ^   4,0000000000e+00 * exp (  -1,0000000000e+03 * time )
     3       5  r1 in out 9kohm
     4       6  r2 out 0 1kohm
     5       7  .options temp=27°c
     6       8  .options tnom=27°c
     7       9  .ic
     8      10  .tran 0.001ms 20ms 0s
     9      11  *end
    10      12  .end

[Fabrice Salvaire]

listing is

Pulse
1 : pulse
2 : .global gnd
4 : bsource in 0 v= time ^   4,0000000000e+00 * exp (  -1,0000000000e+03 * time )
5 : r1 in out 9kohm
6 : r2 out 0 1kohm
9 : .ic
10 : .tran 0.001ms 20ms 0s
7 : .options temp=27__c
8 : .options tnom=27__c
12 : .end

[Holger Vogt]

Just one glimpse, and it is obvious:

ngspice expects something like
-1.0000000000e+03
and it gets
-1,0000000000e+03
The difference is the dot versus the comma.

ngspice does not set locale itself, it expects settings as are obtained by using
setlocale(LC_NUMERIC, "C");

standard ngspice executable does this setting automatically (as all C coded executable without explicit locale settings), shared ngspice does not.

[Fabrice Salvaire]

oh, but why we didn't encounter this issue before ? PySpice send the string time^4*exp(-1000*time) thus something strange happen in ngspice

[Fabrice Salvaire]

I got the same result for bsource in 0 v= time ^ 4,0000000000e+00 ** ** exp ( -1,0000000000e+03 * time ) very suspicious

[Holger Vogt]

As a shared library ngspice adopts the locale setting of the calling program. This may have changed, or is even user depending. So it might be advisable to set the locale LC_NUMERIC to "C" directly before calling ngspice. This is what KiCAD is doing right now. One could of course think about other solutions, but this is by no means a short term activity.