@User an update about the ngspice fixes regarding resistor temperature coefficients: what they have done so far (and i think they will not do further actions) is the ability to resolve a parameter (Just a parameter, not an expression!) for tc1 and tc2: this is OK:

r1 node1 node2  r={...expr...} tc1=PAR1 tc2=PAR2

this is not OK (resolves tc1 and tc2 to 0):

r1 node1 node2 r={...expr...} tc1={...expr1...} tc2={...expr2...}

so if you have an expression for tc1/tc2 you need to declare an additional parameter:

.param PARTC1={...expr1...}

.param PARTC2={...expr2...}

r1 node1 node2 r={...expr...} tc1=PARTC1 tc2=PARTC2

I also verified that putting tempco parameters in a resistor model card does NOT work for non linear resistors (where r={...expr...}. I don't even think this is allowed, it's probably a Spectre/HSPICE extension. This will NOT work:

r1 node1 node2 resmod r={...expr...}

.model resmod r tc1=-1.47e-3 tc1=1e-5

To make the long story short, let's keep the sky130 patches as they are right now.

That's great news. Thanks for following up with the ngspice maintainers. They're very quick to fix bugs.