Time Variable Resistor

A couple of ways. One is just to use a voltage-controlled-resistor. You can use the vccs component from analogLib for this - and change the "Type of Source" to "vcr". See "spectre -h vccs" at the UNIX prompt for details.

Another way is to set the value of the resistor via a design variable, and then use the Dynamic Parameters option on the Transient analysis form in ADE to change the value at particular times. Note however that this is not continuous - it will do a step change in the parameter values at each time you specify. 

Clearly this second approach isn't very physical - I'm guessing you're trying to model some voltage dependent resistor, and so I'd expect the first approach would be better.

Kind Regards,

Andrew

Hi Nicolas,

Can you provide your netlist (the VCR instance and the vsource driving it, together with the tran analysis) so that I can take a look? Otherwise I'll have to guess what you've done.

Can you also let me know which simulator version you're using? (probably doesn't matter, but easier to ask now rather than later).

Regards,

Andrew

Hi Andrew,

Thank you for the reply.

Here is the tool version:

mmsim/15/15.10.385

ic/IC617/IC_617_702

Here is the netlist:

// Generated for: spectre
// Generated on: May 18 09:15:47 2016
// Design library name: scratch
// Design cell name: tb_nb_test_vpwl
// Design view name: schematic
simulator lang=spectre
global 0
parameters iload_high_val=1m vout_val=3.3
include "$PDKROOT/xh035/cadence/v6_0/spectre/v6_0_3/mos/top.scs" section=all_typical

// Library name: scratch
// Cell name: tb_nb_test_vpwl
// View name: schematic
source_iload_tran (net2 vss) vsource dc=vout_val/iload_high_val type=pwl \
pwlfilter=none wave=[ 0 (vout_val/1u) 5m (vout_val/1u) 5.001m \
(vout_val/50m) 10m (vout_val/50m) 10.001m (vout_val/100m) 15m \
(vout_val/100m) 15.001m (vout_val/50m) 20m (vout_val/50m) 20.001m \
(vout_val/1u) 25m (vout_val/1u) 32.5m (vout_val/100m) 40m \
(vout_val/1u) 45m (vout_val/1u) 45.001m (vout_val/100m) 50m \
(vout_val/100m) 50.001m (vout_val/1u) ]
V0 (net05 vss) vsource dc=vout_val type=dc
source_vss (vss 0) vsource dc=0 type=dc
G0 (net05 vss net2 vss) vccs gm=1.0 type=vcr
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
checklimitdest=psf
tran tran stop=55m write="spectre.ic" writefinal="spectre.fc" \
annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts where=rawfile
saveOptions options save=allpub

Hi Nicolas,

Everything is correct here. It's because you have a linear sweep on the controlling voltage and hence a linear sweep of the resistance - and so if you're plotting the current, that will have a 1/x response on that linear sweep.

I added save G0:oppoint to the netlist so I could plot the G0:lx0 parameter (and hence see the resistance changing). I then computed (in the calculator) both -3.3/v("net2" ?result "tran") and -3.3/getData("G0:lx0" ?result "tran") and plotted these. You can see that these two calculated currents overlay exactly with the current from the simulator. The top strip shows both the controlling voltage and the VCR value (the lx0) - again, they overlay exactly.

Here's a zoomed in (in the y-direction) plot of the current - you can see it is gradually changing:

This is not surprising - if you see the last red cross (at this zoom level) before the end of the ramp down, it's at about 0.5MV, which corresponds to 0.5MOhm in the VCR. Then the current will be 3.3/0.5M which is about 6uA. The scale of the current means  you hardly see this change. If you were to change the y-axis to a log scale for the current, this would be much more evident without the need to zoom in.

So everything is working as it should - the results are correct.

Regards,

Andrew.

Hi Nicolas,

Don't worry - when I first looked at it, I thought - that's very strange. I was just about to file this as a bug and then I wondered where the step in the current was coming from at 10ms to 15ms. Then I twigged what was going on!

BTW, it's probably a wise idea to scale your voltages to not be in the megaVolt range - instead use typical voltages in a similar range to your supplies, and then use the gm on the VCR to convert to a resistance with the right magnitude. Big voltages (when using transient with relref=allglobal) can compromise the time step control mechanism for your typical signals). That can be improved by using relref=alllocal (e.g. errpreset=conservative) but that's more expensive for simulation.

Regards,

Andrew