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.

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.

@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.

@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.

@Tim Edwards @Stefan Schippers Thanks you. Your advice fixed this issue.