< U01BJBTNN9E> I ran the resistor temperature simulations va open-source-silicon.dev #analog-design

<@U01BJBTNN9E> I ran the resistor temperature simu...

yrrapt

10/03/2020, 12:06 PM

@User 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

10/03/2020, 1:23 PM

@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

10/03/2020, 2:40 PM

@Tim Edwards this is the netlist https://github.com/xorbit/sky130-power-blocks/blob/yrrapt_resistors/primitive-test/resistor-tc.spice. 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

10/03/2020, 2:46 PM

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:

Copy code

** 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

10/04/2020, 4:47 AM

Thanks for confirming @yrrapt

2 Views

Open in Slack

Previous Next