Backannotation of operating point in Xschem

In this tutorial, we will keep using the SIM_inv.sch schematic test bench. In the previous blog post^[1], we use Ngspice to view the simulation results. Another alternative to view the simulation results is to use the built-in waveform viewer from Xschem.

Show hidden text

Go to View => enable Show hidden text option. This will allow us to see gm and id from the MOSFET symbol.

Fig. 1Show hidden text in Xschem

Modify stimulus

In code_shown.sym block, modify the stimulus as follows:

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.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]
dc Vin 0 1.8 1m
op
write Sim_inv.raw
.endc
"

Basically, we will save gm, id, vgs, vdsat into the operating point.

Add additional probe

You can add addtional probe, such as ngspice_get_value.sym and ngspice_probe.sym from xschem_library/devices folder.

In my case, I placed two ngspice_get_value.sym probes in the schematic with the following contents:

name=r14 node=v(@m.xm11.msky130_fd_pr__pfet_01v8[vgs])
descr="vgs="

name=r1 node=v(@m.xm11.msky130_fd_pr__pfet_01v8[vds])
descr="vds="

Modify NMOS and PMOS symbol

I prefer to check the vgs, vds, cgg, vdsat directly from the symbol, similar to Spectre. What we can do is that we can modify the NMOS and PMOS symbol by adding more properties.

By default, after Skywater130 PDK installation, the NMOS and PMOS symbols are read only. To enable the write, we can use the following command:

sudo chmod a+rwx nfet_01v8.sym
sudo chmod a+rwx pfet_01v8.sym

Here I only enabled the write for 1.8V NMOS and PMOS. You can follow the same procedure to enable the write for other symbols as well.

Then click NMOS symbol and press bindkey i to decend to its symbol. We can add the following properties:

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]}]]] )

Fig. 2Modified 1.8V NMOS symbol

Similarly, we can follow the same above procedure to add more properties for 1.8V PMOS symbol as well.

Fig. 3Modified 1.8V PMOS symbol

Backannotation

Click Netlist and then Simulate button. After the simulation is done, go to Simulation => Annotate Operating Point into schematic.

Fig. 4Backannoate operating point

The backannotation results are shown in Fig. 5.

Fig. 5Completed schematic

Live annotate

• Another way to do the back annotation is to use the Live annotate option. To do so, add a waveform graph in the schematic.

• change the NMOS width W=1 and multiplier mult=1 as well.

• Then, modify the stimulus as follows:

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.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]
dc Vin 0 1.8 1m
write Sim_inv.raw
set appendwrite
*op
write Sim_inv.raw
.endc
"

• At waveform graph, press bindkey b to show the b cursor

• Click Netlist => Simulate

• Click waveform graph and then choose the net Vin. Press bindkey option-g to send Vin waveform into the waveform graph. Similarly, we can send the Vout data to waveform graph as well.

• Go to Simulation => Load/unload spice .raw file. In the meanwhile, enable the Live annotate probes with 'b' cursor as well.

• When you move cursor b, you can see that the annotation results change at the same time.

Fig. 6Live annotation with cursor b

References and materials

[1] Backannotation of NGSPICE simulation operating point data into an XSCHEM schematic

[2] Xschem - 101

[3] Sim_inv.sch - download