Channels

#analog-design

Title

# analog-design

s

Sudharsan S

01/05/2022, 1:26 PMI am trying to perform a parametric sweep with ngspice(following Section 17.8.8 of ngspice manual) as shown in the code below for nfet_01v8

`.dc V1 0 1.8 0.01`

`.control`

`let start_WN1 = 1e-6`

`let stop_WN1 = 100e-6`

`let delta_WN1 = 10e-6`

`let actual_WN1 = start_WN1`

`while actual_WN1 le stop_WN1`

`alter m.xm1.msky130_fd_pr__nfet_01v8 W = actual_WN1`

`dc V1 0 1.8 0.01`

`* plot v(Vout)`

`let actual_WN1 = actual_WN1 + delta_WN1`

`end`

`plot dc1.v(Vout) dc5.v(Vout) dc10.v(Vout)`

`.endc`

But running this simulation I get:
`*Error:* no model available for w=1.100000e-6 l=1.500000e-7`

and so on for all the values iterated.
I understand that only certain parameter combinations are available and any other sizes result in interpolated models.
Any help regarding on how I can perform such a parametric sweep type simulation would really help.t

Tim Edwards

01/05/2022, 2:39 PMThe Sky130 device models have a

`.option scale`

line built into the library files. W and L (and all dimensions of length) need to be specified in microns, not meters (and area needs to be specified in microns squared, not meters squared).s

Sudharsan S

01/05/2022, 3:51 PMThanks for clarifying **@Tim Edwards**. But I get similar errors when I specify W in terms of microns too. Additionally I am getting a few more errors that I don't fully understand too, I have attached screen shot.

t

Tim Edwards

01/05/2022, 6:04 PMWhat I see in the screenshot is that a model has been specified at W=1 (correct) and L=1.5E-7 (not correct).

f

Felipe Vianna

03/02/2022, 9:49 PMHi everyone.
I get the same result as **@User** described here when performing parametric sweeps in ngspice 35 for MOSFET W or L.
e.g. ngspice will output the following:
**@User** reported.
I'm only sweeping W in this case:
*seems* that the alter statement has *some* effect, because I get different results that are appropriate in between each other.
I wouldn't have worried much about the error, but apparently, for a given width Wx, I'm getting slightly different (but non-negligible) results in a single DC simulation in comparison to multiple DC simulations that sweep the width with alter param (in which Wx is included).
Is anyone aware of this and can help? Thanks in advance

`Error: no model available for w= 9.0000000e+00 l= 1.5000000e-07.`

I am aware that parameters must be supplied in microns, hence W is specified as 9, L is specified as 0.15. Still, the error changes the decimal for both parameters - seems to be the same as `alter @m.xm1.msky130_fd_pr__nfet_01v8[w] = wn_loop`

Even though the error happens, it Upgraded to ngspice **36** - issue remains.

s

Stefan Schippers

03/03/2022, 9:44 AMCan you share the complete netlist?

t

Tim Edwards

03/03/2022, 1:45 PMf

Felipe Vianna

03/04/2022, 12:46 AM`xm0 ... w=1.6`

) has some strange effect over the DC response of my inverter. Even though I alter the transistor width Copy code

```
'CMOS Inverter DC analysis'
**********************************
* Models
**********************************
.lib "/home/frbvianna/sky130/skywater-pdk-libs-sky130_fd_pr/models/sky130.lib.spice" tt
**********************************
* Parameters
**********************************
* .param <param>=<value>
.param wp = 1.5
.param wn = 0.6
**********************************
* Options
**********************************
.option temp=27C
* .option scale=1e-6
**********************************
* Circuit
**********************************
Vdd vdd gnd dc=1.8
xm0 out in vdd vdd sky130_fd_pr__pfet_01v8
+ w={wp} l=0.15
xm1 out in gnd gnd sky130_fd_pr__nfet_01v8
+ w={wn} l=0.15
**********************************
* Control
**********************************
.control
destroy all
* Loop Wp and Wn (op), ratio 1 to 5
let wp_step = 0.05
let wn_begin = 0.6
let wn_end = 1.8
let wn_step = 0.15
let wn_loop = wn_begin
while wn_loop le wn_end
let wp_loop = 1*wn_loop
alter @m.xm1.msky130_fd_pr__nfet_01v8[w] = wn_loop
while wp_loop le 5*wn_loop
alter @m.xm0.msky130_fd_pr__pfet_01v8[w] = wp_loop
op
let v_diff = v(out) - v(in)
let ratio = wp_loop/wn_loop
* $W_P/W_N$ $V_{OUT}-V_{IN}$
echo
+ $&ratio
+ $&v_diff
+ >> inverter/v_diff_w_l.dat
let wp_loop = wp_loop + wp_step
end
let wn_loop = wn_loop + wn_step
echo >> inverter/v_diff_w_l.dat
end
.endc
**********************************
* EOF
**********************************
.end
```

`v_diff`

gives `v(out) - v(in)`

which would be near 0 for a symmetric inverter with an optimal Wp/Wn ratio.
First Wp/Wn ratio of the sweep is 1, given by Wp = Wn = 0.6.
By changing to `.param wp=1.5`

in the circuit definition (larger than the initial sweep value of `wp_loop=0.6`

) you can already see `v_diff`

changing in that ratio 1 iteration.
Furthermore, even if wp and wn defined in `.param`

match the values for the first parametric sweep iteration, in my nested loop scenario, `wn`

is then altered and it seems that the subsequent iterations (wn != 0.6) will then yield incorrect results.
I am working on a Python wrapper to perform this same simulation without nested whiles to see if I can get the expected results.t

Tim Edwards

03/04/2022, 1:41 AM👍 1

✅ 1

f

Felipe Vianna

03/04/2022, 10:50 PMAlso, I'm guessing the reason we see this kind of error when altering the MOSFET width/length is because it doesn't precisely match a device bin?

`Error: no model available for w= 4.0500000e+00 l= 1.5000000e-07.`

s

Stefan Schippers

03/05/2022, 10:10 AMf

Felipe Vianna

03/05/2022, 4:41 PM👍 1

s

Stefan Schippers

03/05/2022, 9:23 PMThanks Felipe, i missed in the error message also W has e-6 so both quantities are in micron. Forgive me.

f

Felipe Vianna

03/05/2022, 9:28 PM`4.05u`

) the simulation will actually fail