SPICE TEAM¶

Some tips for piece(Ngspice) user (by Kramer)¶

For the hspice or other spice user, in-house spice simulator piece has many triky usags and I list some of them here.

1. About easurement

Both meas line at control block and outside of control block are supported, but both cannot support any complex expression as below

.meas tran vtest find par('v(n1)-v(n0)') at=40n
.meas tran ttest when v(n1) = 'v(0)+vdd'

The right way is

.control
let vdiff = v(n1)-v(n0)
let vtest = v(0)+vdd
meas tran vtest find vdiff at=40n
meas tran ttest when v(n1) = vtest
.endc

There are more useful measurement statements for example.

.control
* rhs of let statement cannot use the golbal parameter outside of control block while vdd is a special case!
let halfvdd = 'vdd/2'
let trans = {v(q)*v(cp)/vdd}
meas tran tran01 when tranx = 'halfvdd' rise=1
meas tran delay1 trig v(in) val='halfvdd' fall=1 targ v(zn) val = 'halfvdd' rise=1
print tran01 delay 1 > trans.txt
.endc

2. some useful options

.opt noopac  ; skip op when do ac analysis
.opt numdgt=9 ; set the output data's digital number to 9 (must set in control block, as *.control numdgt=9 .endc*)
*#set nobreak ; set output data file without page break
.opt maxord=1 method=trap trtol=1  ; options to get stable waveform without some ring (more accuracy)

The following lines to set autostop when v(zn) cloase to zero

.opt autostop
.meas tran tend when v(zn)='vss+1e-5' fall=1

3. about output file format

In control block, we can use print or wrdata to dump data to file.

print i(vp) i(cl_t) v(q) > dat1.txt
wrdata dat2.txt i(vp) i(cl_t) v(q)

The dat1.txt(left) and dat2.txt(right) as below:

4. alter usage

Wrong usage for altering C1's capacitance:

C1 1 0 'cload'
.control
alter C1=1p
tran 1p 10n
alter C1=1.2p
tran 1p 10n
.endc

The right way as below, in the above case, the latter simulation will be impacted by the former.

c1 1 0 'cload'
.control
alterparam cload = 1p
reset
tran 1p 10n
alterparam cload = 1.2p
reset
tran 1p 10n
.endc

##Development Environment:
New spice engine "piece" is located in pub2018/bin/rhelx-64/analog. (2021/7/12 historical moments!!!)

piece update can flow below procedure Tool_lib_organization

Reference SPICE center (Repository in 10.30.100.22/spice)¶

ngSPICE¶

Reference: http://ngspice.sourceforce.net/docs.html
User manual: ngspice-34-manual.pdf
Binary and library install guidance: ngspice_install.pptx
ngspice git clone: git clone ssh://git@10.30.100.22:222/analog/spice.git
Local build binary with ngSpice 34: /rnd1/jchen/ngspice34/agigaspice/release/bin/bin/ngspice
Example spice file: /rnd1/jchen/ngspice34/agigaspice/examples
Ngspice compiling method enhancement (SiQi)

spice3f5 元祖SPICE¶

spice3f5.tar.gz

cuSPICE, (CUDA ver. ngSPICE)¶

CuSPICE.pdf
Reference: SPICE on GPU: http://ngspice.sourceforge.net/cuspice.html

xyce¶

Xyce install method (Langyun): 基于WSL的Ubuntu系统Serial Xyce编译整理.docx
Reference: https://xyce.sandia.gov/

SPICE 历史¶

SPICE_history.docx