1

问题：

如何在 Monte Carlo 迭代循环中将修改后的器件模型参数（如 W、L、Tox）传递给子电路？

工具版本：

[boris@E7440 inverter]$ ngspice -v
ngspice compiled from ngspice revision 23
Written originally by Berkeley University
Currently maintained by the NGSpice Project

Copyright (C) 1985-1996,  The Regents of the University of California
Copyright (C) 1999-2008,  The NGSpice Project
[boris@E7440 inverter]$ uname -a
Linux E7440.DELL 4.4.13-200.fc22.x86_64 #1 SMP Wed Jun 8 15:59:40 UTC 2016 x86_64 x86_64 x86_64 GNU/Linux
[boris@E7440 inverter]$

测试用例：

这是一个演示问题的小型独立测试用例；通过改变晶体管通道的宽度和长度，对简单的反相器门执行蒙特卡罗分析。

SPICE3 file

.GLOBAL VDD VBP
V0DD VDD 0 1.1
V0BP VBP 0 1.1
.GLOBAL VSS VBN
V0SS VSS 0 0.0
V0BN VBN 0 0.0

X1 VDD VSS VBP VBN X A INV1

V1 A 0 DC 0 PWL( 2501.80p 1.10 2503.02p 1.10 2504.24p 1.10 2505.46p 1.10 2506.68p 1.10 2507.90p 1.09 2509.12p 1.09 2510.34p 1.09 2511.56p 1.09 2512.78p 1.08 2514.00p 1.07 2515.22p 1.06 2516.44p 1.05 2517.66p 1.03 2518.88p 1.01 2520.10p 0.98 2521.32p 0.94 2522.54p 0.88 2523.76p 0.79 2524.98p 0.67 2526.20p 0.55 2527.42p 0.43 2528.64p 0.31 2529.86p 0.22 2531.08p 0.16 2532.30p 0.12 2533.52p 0.09 2534.74p 0.07 2535.96p 0.05 2537.18p 0.04 2538.40p 0.03 2539.62p 0.02 2540.84p 0.01 2542.06p 0.01 2543.28p 0.01 2544.50p 0.01 2545.72p 0.00 2546.94p 0.00 2548.16p 0.00 2549.38p 0.00 2550.60p 0.00 )
C1 X 0 12.3f

.OPTIONS NOACCT

.control
    save A X
    let mc_runs = 25
    let run = 0
    set curplot = new
    set plot_out = $curplot

    define unif(nom, var) (nom + (nom*var) * sunif(0))
    define aunif(nom, avar) (nom + avar * sunif(0))
    define gauss(nom, var, sig) (nom + (nom*var)/sig * sgauss(0))
    define agauss(nom, avar, sig) (nom + avar/sig * sgauss(0))

    dowhile run <= mc_runs
        alter @M1[W] = gauss(0.72u, 0.1, 3)
        alter @M1[L] = gauss(0.18u, 0.1, 3)
        alter @M2[W] = gauss(0.36u, 0.1, 3)
        alter @M2[L] = gauss(0.18u, 0.1, 3)

        tran 3p 3n 2n

        set run ="$&run"
        print run

        linearize A X
        set plot_tmp = $curplot
        setplot $plot_out
        if run=0
            let time={$plot_tmp}.time
            let vin={$plot_tmp}.A
        end
        let vout{$run}={$plot_tmp}.X
        setplot $plot_tmp
        let run = run + 1
    end
    plot {$plot_out}.allv
.endc

.END

.MODEL NFET NMOS(LEVEL=14 VERSION=4.6.5)
.MODEL PFET PMOS(LEVEL=14 VERSION=4.6.5)

.SUBCKT INV1 VDD VSS VBP VBN X A
M1 X A VDD VBP pfet W=0.72u L=0.18u AD=3.6p PD=2.34p AS=3.6p PS=2.34p
M2 X A VSS VBN nfet W=0.36u L=0.18u AD=1.8p PD=1.62p AS=1.8p PS=1.62p
.ENDS

SPICE 输出如下：

[boris@E7440 inverter]$ ngspice simulate_mc2.sp
******
** ngspice-23 : Circuit level simulation program
** The U. C. Berkeley CAD Group
** Copyright 1985-1994, Regents of the University of California.
** Please get your ngspice manual from http://ngspice.sourceforge.net/docs.html
** Please file your bug-reports at http://ngspice.sourceforge.net/bugrep.html
** Creation Date: Tue Jul  8 03:06:23 UTC 2014
******

Circuit: simulation file

Error: no such device or model name m1
Error: no such device or model name m1
Error: no such device or model name m2
Error: no such device or model name m2
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

OpenMP: 2 threads are requested in BSIM4
%100.00

No. of Data Rows : 501
run = 0.000000e+00
Error: no such device or model name m1
Error: no such device or model name m1
Error: no such device or model name m2
Error: no such device or model name m2
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

OpenMP: 2 threads are requested in BSIM4
%100.00

No. of Data Rows : 501
run = 1.000000e+00
Error: no such device or model name m1
Error: no such device or model name m1
Error: no such device or model name m2
Error: no such device or model name m2
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

OpenMP: 2 threads are requested in BSIM4
%100.00

No. of Data Rows : 501
run = 2.000000e+00
Error: no such device or model name m1
Error: no such device or model name m1
Error: no such device or model name m2
Error: no such device or model name m2
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

OpenMP: 2 threads are requested in BSIM4
%100.00nce value :  2.55551e-09

No. of Data Rows : 501
run = 3.000000e+00

显然，将参数传递给子电路时出了点问题。我还尝试了以下语法变体：

alter X1.@M1[W] = gauss(0.72u, 0.1, 3)
alter X1:@M1[W] = gauss(0.72u, 0.1, 3)
alter X1/@M1[W] = gauss(0.72u, 0.1, 3)
alter @X1.M1[W] = gauss(0.72u, 0.1, 3)
alter @X1:M1[W] = gauss(0.72u, 0.1, 3)
alter @X1/M1[W] = gauss(0.72u, 0.1, 3)
alter @X1.@M1[W] = gauss(0.72u, 0.1, 3)
alter @X1:@M1[W] = gauss(0.72u, 0.1, 3)
alter @X1/@M1[W] = gauss(0.72u, 0.1, 3)
alter @X1[M1[W]] = gauss(0.72u, 0.1, 3)
alter @X1(M1[W]) = gauss(0.72u, 0.1, 3)
alter @X1{M1[W]} = gauss(0.72u, 0.1, 3)

没有任何作用...

顺便说一句，当我在主网表中移动子电路内容时，模拟工作正常......

例子：

SPICE3 file

.GLOBAL VDD VBP
V0DD VDD 0 1.1
V0BP VBP 0 1.1
.GLOBAL VSS VBN
V0SS VSS 0 0.0
V0BN VBN 0 0.0

M1 X A VDD VBP pfet W=0.72u L=0.18u AD=3.6p PD=2.34p AS=3.6p PS=2.34p
M2 X A VSS VBN nfet W=0.36u L=0.18u AD=1.8p PD=1.62p AS=1.8p PS=1.62p

V1 A 0 DC 0 PWL( 2501.80p 1.10 2503.02p 1.10 2504.24p 1.10 2505.46p 1.10 2506.68p 1.10 2507.90p 1.09 2509.12p 1.09 2510.34p 1.09 2511.56p 1.09 2512.78p 1.08 2514.00p 1.07 2515.22p 1.06 2516.44p 1.05 2517.66p 1.03 2518.88p 1.01 2520.10p 0.98 2521.32p 0.94 2522.54p 0.88 2523.76p 0.79 2524.98p 0.67 2526.20p 0.55 2527.42p 0.43 2528.64p 0.31 2529.86p 0.22 2531.08p 0.16 2532.30p 0.12 2533.52p 0.09 2534.74p 0.07 2535.96p 0.05 2537.18p 0.04 2538.40p 0.03 2539.62p 0.02 2540.84p 0.01 2542.06p 0.01 2543.28p 0.01 2544.50p 0.01 2545.72p 0.00 2546.94p 0.00 2548.16p 0.00 2549.38p 0.00 2550.60p 0.00 )
C1 X 0 12.3f

.OPTIONS NOACCT

.control
    save A X
    let mc_runs = 5
    let run = 0
    set curplot = new
    set plot_out = $curplot

    define unif(nom, var) (nom + (nom*var) * sunif(0))
    define aunif(nom, avar) (nom + avar * sunif(0))
    define gauss(nom, var, sig) (nom + (nom*var)/sig * sgauss(0))
    define agauss(nom, avar, sig) (nom + avar/sig * sgauss(0))

    dowhile run <= mc_runs
        alter @M1[W] = gauss(0.72u, 0.1, 3)
        alter @M1[L] = gauss(0.18u, 0.1, 3)
        alter @M2[W] = gauss(0.36u, 0.1, 3)
        alter @M2[L] = gauss(0.18u, 0.1, 3)

        tran 3p 3n 2n

        set run ="$&run"
        print run

        linearize A X
        set plot_tmp = $curplot
        setplot $plot_out
        if run=0
            let time={$plot_tmp}.time
            let vin={$plot_tmp}.A
        end
        let vout{$run}={$plot_tmp}.X
        setplot $plot_tmp
        let run = run + 1
    end
    plot {$plot_out}.allv
.endc

.END

.MODEL NFET NMOS(LEVEL=14 VERSION=4.6.5)
.MODEL PFET PMOS(LEVEL=14 VERSION=4.6.5)

结果：

[boris@E7440 inverter]$ ngspice simulate_mc1.sp
******
** ngspice-23 : Circuit level simulation program
** The U. C. Berkeley CAD Group
** Copyright 1985-1994, Regents of the University of California.
** Please get your ngspice manual from http://ngspice.sourceforge.net/docs.html
** Please file your bug-reports at http://ngspice.sourceforge.net/bugrep.html
** Creation Date: Tue Jul  8 03:06:23 UTC 2014
******

Circuit: simulation file

Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

OpenMP: 2 threads are requested in BSIM4
%100.00

No. of Data Rows : 501
run = 0.000000e+00
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

OpenMP: 2 threads are requested in BSIM4
%100.00

No. of Data Rows : 501
run = 1.000000e+00
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

OpenMP: 2 threads are requested in BSIM4
%100.00

No. of Data Rows : 501
run = 2.000000e+00
Doing analysis at TEMP = 27.000000 and TNOM = 27.000000

OpenMP: 2 threads are requested in BSIM4
%100.00nce value :  2.52249e-09

No. of Data Rows : 501
run = 3.000000e+00

然而，这不是一个实用的解决方案。我也想模拟其他单元，但是将不同子电路的内容复制粘贴到主网表中既麻烦又容易出错。

4

1 回答 1

2

我可以推荐 ngspice 论坛来发布这样的问题吗？会有一个更快的答案，而不是像这里发生的那样偶然。

交互式运行输入文件后，输入命令“listing expand”，您将看到子电路扩展后的电路结构。

m1 变成了 m.x1.m1，m2 变成了 m.x1.m2。alter 命令作用于扩展电路。因此，通过在 alter 语句中将 m1 替换为 m.x1.m1 并将 m2 替换为 m.x1.m2，您将获得合适的结果。

霍尔格

于 2016-09-07T16:11:13.193 回答