Yet when I remove the external cap and put it inside the amp

Question

Yet when I remove the external cap and put it inside the amp instead it gives me the response I expect without complaining about a singular matrix See images below Does anyone know what might be going on here if this could be an ngspice bug I ve attached the netlist too

Stefan Schippers · Answer

< Tom> i can not simulate the netlist as there is an undefined subcircuit sev2diffv It is called in the netlist and it is probably defined in some include file EDIT I found this component in a previous thread Will look forward

Stefan Schippers · Answer

< Tom> after inserting the sev2diffv and pointing the pdk includes to my installation i got simulation running without singular matrix warning ```schippes mazinga ~ xschem simulations$ ngspice bgr amp test spice ngspice 34 Circuit level simulation program The U C Berkeley CAD Group Copyright 1985 1994 Regents of the University of California Copyright 2001 2020 The ngspice team Please get your ngspice manual from Please file your bug reports at Creation Date Sat Jan 30 12 16 19 UTC 2021 Compatibility modes selected hs Circuit subckt bgr amp test Doing analysis at TEMP = 27 000000 and TNOM = 27 000000 Warning include has no value DC 0 assumed Note Starting true gmin stepping Trying gmin = 1 0000E 03 Note One successful gmin step Trying gmin = 1 0000E 04 Note One successful gmin step Trying gmin = 1 0000E 05 Note One successful gmin step Trying gmin = 1 0000E 06 Warning Further gmin increment Trying gmin = 5 6234E 06 Note One successful gmin step Trying gmin = 2 3714E 06 Note One successful gmin step Trying gmin = 6 4938E 07 Warning Further gmin increment Trying gmin = 1 7154E 06 Note One successful gmin step Trying gmin = 1 0554E 06 Note One successful gmin step Trying gmin = 5 0937E 07 Warning Further gmin increment Trying gmin = 8 7970E 07 Note One successful gmin step Trying gmin = 6 6940E 07 Note One successful gmin step Trying gmin = 4 4433E 07 Note One successful gmin step Trying gmin = 2 4029E 07 Note One successful gmin step Trying gmin = 9 5562E 08 Note One successful gmin step Trying gmin = 2 3967E 08 Note One successful gmin step Trying gmin = 3 0102E 09 Note One successful gmin step Trying gmin = 3 0102E 10 Note One successful gmin step Trying gmin = 3 0102E 11 Note One successful gmin step Trying gmin = 3 0102E 12 Note One successful gmin step Trying gmin = 1 0000E 12 Note One successful gmin step Note True gmin stepping completed Reference value 0 00000e+00 No of Data Rows 1 Reset re loads circuit subckt bgr amp test ``` Did you compile ngspice with the XSPICE feature

Tom · Answer

Did you < Stefan Schippers> Thank you for trying it out sorry about the missing sev2diffv I forgot about that I m not sure if I have the XSPICE feature let me check What is it

Stefan Schippers · Answer

< Tom> Xspice is an extension to Spice3C1 that provides code modelling support and simulation of digital components through an embedded event driven algorithm Some devices are simulated by the Xspice subsystem B sources devices with equations etc

Tom · Answer

Ah ok but why would that be required in order for my sim to work with the cap external

Stefan Schippers · Answer

< Tom> build with configure with x enable xspice disable debug enable cider with readline=yes enable adms

Stefan Schippers · Answer

I am not sure it is needed in your case but if anything else fails try building in xspice if not already in

Tom · Answer

I ll give that a try

Stefan Schippers · Answer

< Tom> the voltage controlled voltage source is simulated with xspice if the gain is set with an expression uses a B source EP vop vc vi vc 0 5 gain try setting it to a number EP vop vc vi vc 0 5 In this case the native vcvs devices is used

Tom · Answer

I m building it now with ` configure with x enable xspice disable debug enable cider with readline=yes enable openmp enable adms` so it s what you said plus ` enable openmp` as per the section entitled A fully featured ngspice on LINUX may be obtained with the following commands

Tom · Answer

Which I m fairly sure is what I did last time If it fails I ll remove the openmp to get exactly what you had and try again

Tom · Answer

That still fails for me < Stefan Schippers> This is what I tried I built with ` configure with x enable xspice disable debug enable cider with readline=yes enable adms` as you suggested removed the ` 0 5 gain ` expressions and just used `0 5` and I still get the same error What is the commit of your build of ngspice I want to try that next so we re on exactly the same page and if that fails I m going to try and boil it down to a simple failing test case ``` ngspice 34 Circuit level simulation program The U C Berkeley CAD Group Copyright 1985 1994 Regents of the University of California Copyright 2001 2020 The ngspice team Please get your ngspice manual from Please file your bug reports at Creation Date Tue Feb 9 17 19 56 UTC 2021 No compatibility mode selected Circuit subckt bgr amp test Scale set to 1e 06 Doing analysis at TEMP = 27 000000 and TNOM = 27 000000 Warning include has no value DC 0 assumed Warning singular matrix check nodes net1 and net1 Note Starting true gmin stepping Trying gmin = 1 0000E 03 Warning singular matrix check nodes net1 and net1 Warning Further gmin increment Trying gmin = 5 6234E 03 Warning singular matrix check nodes net1 and net1 Warning Further gmin increment Trying gmin = 8 6596E 03 Warning singular matrix check nodes net1 and net1 Warning Further gmin increment Trying gmin = 9 6466E 03 Warning singular matrix check nodes net1 and net1 Warning Further gmin increment```

Tom · Answer

That was with sev2diffv ``` single ended to differential voltage buffer subckt sev2diffv vi vc vop von PARAMS gain=1 EP vop vc vi vc 0 5 EN von vc vi vc 0 5 ends```

Tom · Answer

and ngspice git hash `279edff5d9877b13ddd7708285553ea20d6f14cd`

Stefan Schippers · Answer

< Tom> the only diffs i see in the logs is that you dont have the set ngbehavior=hs in a spiceinit file Create a spiceinit file in your home or in the directory where you run ngspice with this line in it set ngbehavior=hs

Tom · Answer

Ah good point Let me add that and get back to you

Tom · Answer

Where does xschem run ngspice from

Tom · Answer

I d rather put it in there if that would make it part of my project

Stefan Schippers · Answer

in the ~ xschem simulations directory by default To check click Simulations gt set netlist dir

Stefan Schippers · Answer

this is what i do indeed a spiceinit file in ~ xschem simulations

Tom · Answer

perfect so I have that set to a netlist folder in my project so putting it in there should be ok right

Stefan Schippers · Answer

yes create the spiceinit file where the spice file is generated and ngspice run

Tom · Answer

ok trying it now The only reason I didn t have that before is because I remember we tested it and it didn t seem to be required if the option was set correctly to use the models based on fingers

Tom · Answer

< Stefan Schippers> that doesn t seem to be the issue either actually This is so bizarre As you can see it s picked up the hspice compatibility directive correctly ``` ngspice 34 Circuit level simulation program The U C Berkeley CAD Group Copyright 1985 1994 Regents of the University of California Copyright 2001 2020 The ngspice team Please get your ngspice manual from Please file your bug reports at Creation Date Tue Feb 9 17 19 56 UTC 2021 Compatibility modes selected hs Circuit subckt bgr amp test Scale set to 1e 06 Doing analysis at TEMP = 27 000000 and TNOM = 27 000000 Warning include has no value DC 0 assumed Warning singular matrix check nodes net1 and net1 Note Starting true gmin stepping Trying gmin = 1 0000E 03 Warning singular matrix check nodes net1 and net1```

Tom · Answer

This is my netlist for refrence I ve removed my `analoglib` and the `sev2diffv` component with the same result What git hash did you build ngspice from < Stefan Schippers> ``` ngspice 34 Circuit level simulation program The U C Berkeley CAD Group Copyright 1985 1994 Regents of the University of California Copyright 2001 2020 The ngspice team Please get your ngspice manual from Please file your bug reports at Creation Date Tue Feb 9 17 19 56 UTC 2021 Compatibility modes selected hs Circuit subckt bgr amp test Scale set to 1e 06 Doing analysis at TEMP = 27 000000 and TNOM = 27 000000 Warning include has no value DC 0 assumed Warning singular matrix check nodes net1 and net1 Note Starting true gmin stepping Trying gmin = 1 0000E 03 Warning singular matrix check nodes net1 and net1```

Stefan Schippers · Answer

< Tom> can you try the netlist i am running you need to change the prefix of the pdk includes according to your installation

Stefan Schippers · Answer

just do ngspice bgr amp test spice

Tom · Answer

That worked Even without hs compatibility since i was running it from a different folder I noticed that I hadn t updated my lib symbol to the one which replaces ` inc` with ` include` so I m goint to see if that makes my netlist work all of a sudden What s your theory

Tom · Answer

Unsurprisingly < Stefan Schippers> replacing ` include` with ` inc` in your netlist doesn t break it

Stefan Schippers · Answer

so at the end < Tom> was the singularity due to the inc vs include hard to believe but with ngspice i have had more strange surprises like this some don t have a rational explanation i just managed to accept life the way it is

Tom · Answer

haha no it wasn t < Stefan Schippers> I m actually just about to dive in and try and figure it out I suspect that it may be to do with the `lib` statement since it looks like you don t have that in your version the passing version of the netlist but let s see I ll get back to you with an update shortly

Tom · Answer

< Stefan Schippers> I ve got to the bottom of it I m sorry for the trouble and thank you for the help The issue was that the amp labels the net connected to the `vcomp` pin `v1` and that was the cause of the singularity since the `vcomp` pin in the ` subckt` definition wasn t actually connected to a subcircuit net as the net in the subcircuit was called `v1` So in the top level the cap was connected to an amp pin which didn t actually go anywhere in the ` subckt` I just noticed that the ERC info window actually reports this short so I ll be sure to check that next time The netlist which was passing was the one with the cap inside the amp so that was actually a red herring That s my fault for uploading so many netlists

Amro Tork · Answer

< Eslam Morsie>