Xschem cheatsheet

Most often used bindkeys in Xschem^[1]

Commonly used cells

Symbol properties

type=nand
tedax_format="footprint @name @footprint
device @name @device"
template="name=U1 device=CD4011B footprint=\"dip(14)\" numslots=4 power=VCC ground=GND"
extra="power ground"
extra_pinnumber="14 7"

Pin properties

name=A dir=in pinnumber=1:5:8:12

Bus and multiple instances^[2]

Line, arc, circle, polygon properties

fill=true
dash=10
bus=true

Text properties

layer=6
hcenter=true
vcenter=true
weight=bold
slant=oblique
font="Liberation Sans"

Save gm, id, vgs, vds, vdsat, cgg for backannotation

name=NGSPICE
only_toplevel=true
value="
.control
save all
save @m.xm11.msky130_fd_pr__pfet_01v8[gm]
save @m.xm11.msky130_fd_pr__pfet_01v8[id]
save @m.xm11.msky130_fd_pr__pfet_01v8[vgs]
save @m.xm11.msky130_fd_pr__pfet_01v8[cgg]
save @m.xm11.msky130_fd_pr__pfet_01v8[vds]
save @m.xm11.msky130_fd_pr__pfet_01v8[vdsat]
save @m.xm11.msky130_fd_pr__pfet_01v8[vth]
save @m.xm11.msky130_fd_pr__pfet_01v8[gds]
save @m.xm1.msky130_fd_pr__nfet_01v8[gm]
save @m.xm1.msky130_fd_pr__nfet_01v8[id]
save @m.xm1.msky130_fd_pr__nfet_01v8[vgs]
save @m.xm1.msky130_fd_pr__nfet_01v8[vds]
save @m.xm1.msky130_fd_pr__nfet_01v8[cgg]
save @m.xm1.msky130_fd_pr__nfet_01v8[vdsat]
save @m.xm1.msky130_fd_pr__nfet_01v8[vth]
save @m.xm1.msky130_fd_pr__nfet_01v8[gds]
dc Vin 0 1.8 1m
write Sim_inv.raw
set appendwrite
*op
write Sim_inv.raw
.endc
"

Add more proporties in symbol

tcleval(vgs=[to_eng [ngspice::get_node [subst -nocommand {v(\@m.${path}@spiceprefix@name\.msky130_fd_pr__@model\[vgs])}]]], vds=[to_eng [ngspice::get_node [subst -nocommand {v(\@m.${path}@spiceprefix@name\.msky130_fd_pr__@model\[vds])}]]])

tcleval(vdsat=[to_eng [ngspice::get_node [subst -nocommand {v(\@m.${path}@spiceprefix@name\.msky130_fd_pr__@model\[vdsat])}]]] )

tcleval(cgg=[to_eng [ngspice::get_node [subst -nocommand {\@m.${path}@spiceprefix@name\.msky130_fd_pr__@model\[cgg]}]]] )

Derivative to calculate capacitance

Usage: 100e-9 is because that we are sourcing 100nA current into the cap. g1 is the voltage across the capacitor.

"Varactor cap;100e-9 g1 deriv0() /"

Load/unload simulation data

Usage: right click to load/unload simulation data. Symbol: devices/launcher.sym

name=h1 
descr="Select arrow and 
Ctrl-Left-Click to load/unload
simulation .raw file" 
tclcommand="
xschem raw_read $netlist_dir/[file tail [file rootname [xschem get current_name]]].raw
"

name=h4 
descr="Select arrow and 
Ctrl-Left-Click to load/unload
simulation .raw file" 
tclcommand="
xschem raw_read $netlist_dir/[file tail [file rootname [xschem get current_name]]].raw dc
"

If you have multiple simulation results in the same file, we can use the following command.

name=h1 
descr="Load tran waves" 
tclcommand="
xschem raw_read $netlist_dir/[file tail [file rootname [xschem get current_name]]].raw tran

"

name=h17 
descr="Load dc waves" 
tclcommand="
xschem raw_read $netlist_dir/[file tail [file rootname [xschem get current_name]]].raw dc

"

Append write

Usage: write multiple simulation results into the same file

name=COMMANDS1
simulator=ngspice
only_toplevel=false 
value="
.control
save all
dc i1 1p 50u 0.1u 
write test_diode.raw
set appendwrite
tran 100p 22n
write test_diode.raw
.endc
"

Calculate BJT beta

Usage: from folder xschem_library/devices import ngspice_get_expr.sym symbol. Change its property to the following content:

name=r1 
node="[format %.4g [expr { 
      [ngspice::get_node {i(@q.xq1.qsky130_fd_pr__pnp_05v5_W3p40L3p40[ic])}] 
      /
      [ngspice::get_node {i(@q.xq1.qsky130_fd_pr__pnp_05v5_W3p40L3p40[ib])}] 
}]]"
descr="Beta="

Backannotation operating point

Usage: from folder xschem_library/devices import launcher.sym symbol. Change its property to the following content:

name=h1
descr="Annotate OP" 
tclcommand="set show_hidden_texts 1; xschem annotate_op"

Save BJT Vbe information

Usage: from folder xschem_library/devices import code_shown.sym symbol. Change its property to the following content:

name=NGSPICE
only_toplevel=true
value="
.option savecurrents
.control
save all
save @q.xq1.qsky130_fd_pr__pnp_05v5_W3p40L3p40[vbe]

dc i0 5n 100u 0.05u

* plot vc1#branch / vb1#branch
* plot e1
write test_bipolar.raw
set appendwrite
op
write test_bipolar.raw


.endc
" 

Save current

Usage: from folder xschem_library/devices import ammeter.sym symbol. Put the ammeter in series with the device whose current you are interested. The current will be saved and you can add it to the plot from waveform graph.

Or you can automatically plot the current as follows by using the code_shown.sym stimulus.

name=NGSPICE
only_toplevel=true
value="
vp P 0 1.8
vm M 0 0
vb B 0 0
.control
save all
* dc vp 0 3 0.01
dc temp -40 140 1
*plot v(p,m) / vr1#branch
*plot v(p,m) / vr2#branch
*plot v(p,m) / vr3#branch
plot v(p,m) / vr4#branch
plot v(p,m) / vr5#branch
plot v(p,m) / vr6#branch
*plot v(p,m) / vr7#branch
*plot v(p,m) / vr8#branch
plot v(p,m) / vr9#branch
plot v(p,m) / vr10#branch
*plot v(p,m) / vr11#branch
*plot v(p,m) / vr12#branch
plot v(p,m) / vr13#branch
write test_res.raw
.endc
" 

Temperature sweep

Usage: from folder xschem_library/devices import code_shown.sym symbol. Change its property to the following content:

name=NGSPICE
only_toplevel=true
value="
vp P 0 1.8
vm M 0 0
vb B 0 0
.control
save all
* dc vp 0 3 0.01
dc temp -40 140 1
*plot v(p,m) / vr1#branch
*plot v(p,m) / vr2#branch
*plot v(p,m) / vr3#branch
plot v(p,m) / vr4#branch
plot v(p,m) / vr5#branch
plot v(p,m) / vr6#branch
*plot v(p,m) / vr7#branch
*plot v(p,m) / vr8#branch
plot v(p,m) / vr9#branch
plot v(p,m) / vr10#branch
*plot v(p,m) / vr11#branch
*plot v(p,m) / vr12#branch
plot v(p,m) / vr13#branch
write test_res.raw
.endc
" 

Nested DC sweep

dc vd 0 1.8 0.005 vg 0 1.8 0.2

Monte carlo simulation

• Step1: import corner.sym from xschem/sky130_fd_pr folder. Change its content as follows:

name=CORNER only_toplevel=true corner=tt_mm

• Step 2: import code_shown.sym from xschem_library/devices folder. Change its content as follows. The below stimulus basically will have a 30 runs of simulation.

For each run, it is going to use the tt_mm mismatch model and a new temperature as well.

name=stimulus 
only_toplevel=false 
place=end

value="
.option chgtol=4e-16 method=gear
.param TEMPGAUSS = agauss(40, 30, 1)
.option temp = 'TEMPGAUSS'

.control
  option seed = 8
  let run = 1
  save all
  op
  write SIM_current_mirror.raw
  reset
  set appendwrite
  dowhile run < = 30
    save @m.xm1.msky130_fd_pr__nfet_01v8[gm] 
    + @m.xm1.msky130_fd_pr__nfet_01v8[id]
    + @m.xm1.msky130_fd_pr__nfet_01v8[vgs]
    + @m.xm1.msky130_fd_pr__nfet_01v8[cgg]
    + @m.xm1.msky130_fd_pr__nfet_01v8[vds]
    + @m.xm1.msky130_fd_pr__nfet_01v8[vdsat]
    + @m.xm1.msky130_fd_pr__nfet_01v8[vth]
    + @m.xm2.msky130_fd_pr__nfet_01v8[gm] 
    + @m.xm2.msky130_fd_pr__nfet_01v8[id]
    + @m.xm2.msky130_fd_pr__nfet_01v8[vgs]
    + @m.xm2.msky130_fd_pr__nfet_01v8[cgg]
    + @m.xm2.msky130_fd_pr__nfet_01v8[vds]
    + @m.xm2.msky130_fd_pr__nfet_01v8[vdsat]
    + @m.xm2.msky130_fd_pr__nfet_01v8[vth]
    * save all
    tran 1n 1u uic
    write SIM_current_mirror.raw
    let run = run + 1
    reset
  end
.endc
"

Netlist and run

Usage: import launcher.sym from xschem_library/devices library and change the property as follows:

name=h3
descr="Netlist & sim" 
tclcommand="xschem netlist; xschem simulate"

Plot magnitude in db

Usage: in waveform graph, add "Vout db20()". This will plot signal Vout magnitude in dB format.

Plot phase

Usage: in waveform graph, add ph(Vout). This will plot signal Vout phase.

References and materials

[1] Xschem editor commands

[2] Ngspice cheatsheet