Hi Excuse me I was simula

Question

Hi < Stefan Schippers> < Tim Edwards> Excuse me I was simulating a single OTA circuit with simulation result as shown in fig1 however when i added an other OTA without any connection i get different results as depicted in Fig 2 I do not know how come can you please explain it to me Thanks

Stefan Schippers · Answer

In the second example ngspice prints the warning `Warning singular matrix check node net3` when this happens you must resolve the singularity This is caused by floating nodes with no DC path fo ground If you connect supplies and inputs of the second ota to GND the simulation will match the one of the 1st example

Tim Edwards · Answer

< Ahmed Reda> If one of the netlists is a full R C extraction and it is generating parasitic entries for floating nodes that can cause singular matrices That can be resolved by ` option RSHUNT` in ngspice The value of RSHUNT can be something ridiculously high like 1E20 which wil not affect the simultion but will satisfy ngspice s matrix solver

Tim Edwards · Answer

Whether or not the full R C extraction is producing floating capacitors that aren t real is an entirely different discussion

Stefan Schippers · Answer

< Ahmed Reda> I confirmed < Tim Edwards> advice Adding ` options RSHUNT=1e15` Adds one PetaOhm resistor to ground to all nodes resolves the singularity and simulation results are correct in second netlist

Stefan Schippers · Answer

However always be suspicious about singular matrix warnings expecially if not using PEX netlists Usually there is something wrong or indeterminate in the circuit

Ahmed Reda · Answer

< Tim Edwards> < Stefan Schippers> Thanks you Your advice fixed this issue