I ran the resistor temperature simulations va

Question

< U01BJBTNN9E> I ran the resistor temperature simulations varying the temperature ` temp 27` and the parameter ` param temp 27` and still see no temperature effect on those suffix devices So my hunch was wrong and it must be something else happening

Tim Edwards · Answer

< yrrapt> What does your netlist look like The devices all have `tc1` and `tc2` defined e g `sky130 fd pr res high po 0p35 model spice` has ` model resbody r tc1 = tc1rpolybody tc2 = tc2rpolybody tnum = 30 0` and `sky130 fd pr model r+c model spice` has `tc1rpolybody = 0 514E 3` and `tc2rpolybody = 0 122E 5` Are you getting any warnings out of ngspice

yrrapt · Answer

< Tim Edwards> this is the netlist basically the same as < Patrick Van Oosterwijck> original one I tried to do the for loop in ngspice control structure but couldn t get it working so in the end used a Python script that modifies the netlist to change the temperature param and temp before each run

yrrapt · Answer

I ve been looking further into it and believe I may have found the reason it s not working I ve distilled it down to this simple test ``` Simplified test param temp=27 Rnov 0 r nov 0 resbody r = 10e3 Rv 0 r v 0 resbody r = 10e3 1 + v 0 r v 1e 6 model resbody r tc1=1e 3 tc2=1e 6 tnom = 30 0 VRnov 0 r nov dc 1 VRv 0 r v dc 1 control dc temp 40 120 10 plot 1 i VRnov 1 i VRv endc end``` When the resistor value includes a voltage measurement the temperature coefficients don t have any effect The no suffix model uses a different resistor model which is based on physical dimensions w l sheet resistance which is why it s not affected So it seems to me that either the temperature coefficient needs to be added algebraically to the resistor value expression and not count on setting separate tc s and or ngspice probably needs to be changed to avoid this behaviour

Patrick Van Oosterwijck · Answer

Thanks for confirming < yrrapt>