Different simulation results between ngspice and Xyce

[dbm-174]

Hi all,
I tried to do a small simulation with the npn13G2, where I plot Ic vs Vce. In my simulation ngspice (blue) and Xyce (red) show different results.

Does anyone know what could be the reason for this behavior?

Thank you very much in advance

ngspice netlist

*Qucs 24.4.1 /home/bastian/.qucs/lna_prj/dc_hbt_13g2.sch
.INCLUDE "/foss/tools/qucs-s/current/share/qucs-s/xspice_cmlib/include/ngspice_mathfunc.inc"

.SUBCKT IHP_PDK_nonlinear_components_npn13G2 gnd c b e bn Nx=1
X1 c b e bn npn13G2 Nx={Nx}
.ENDS

*.LIB cornerHBT.lib hbt_typ
.LIB /foss/pdks/IHP-Open-PDK/ihp-sg13g2/libs.tech/xyce/models/cornerHBT.lib hbt_typ

Vbe _net0 0 DC 1
VPrIc _net1 _net2 DC 0
VPrIb _net0 _net3 DC 0
Vce _net1 0 DC 1.5
Xnpn13G1 0 _net2 _net3 0 gnd IHP_PDK_nonlinear_components_npn13G2 Nx=1

.control

op
print i(VPrIb) i(VPrIc) > spice4qucs.dc1.ngspice.dc.print
destroy all
reset

dc vce 0 2 0.00666667
write spice4qucs.sw1.plot i(VPrIb) i(VPrIc)
destroy all
reset

exit
.endc
.END

Xyce netlist:

*Qucs 24.4.1 /home/bastian/.qucs/lna_prj/dc_hbt_13g2.sch

.SUBCKT IHP_PDK_nonlinear_components_npn13G2 gnd c b e bn Nx=1
X1 c b e bn npn13G2 Nx={Nx}
.ENDS

*.LIB cornerHBT.lib hbt_typ
.LIB /foss/pdks/IHP-Open-PDK/ihp-sg13g2/libs.tech/xyce/models/cornerHBT.lib hbt_typ

Vbe _net0 0 DC 1
VPrIc _net1 _net2 DC 0
VPrIb _net0 _net3 DC 0
Vce _net1 0 DC 1.5
Xnpn13G1 0 _net2 _net3 0 gnd IHP_PDK_nonlinear_components_npn13G2 Nx=1

.dc vce 0 2 0.00666667
.PRINT dc format=raw file=spice4qucs.dc.plot I(VPrIb) I(VPrIc)
.END

[dwarning]

It's not the root cause, but you should use ngspice lib in ngspice simulation. And first subckt node for ground is obsolete. In my opinion ngspice result is correct.

[dwarning]

The xyce lib is wrong. Thermal node t in the subckt is floating and selfheating is on. Please look for the messages by Xyce in the beginning of simulation (hope it is shown in qucs-s).

[KrzysztofHerman]

@dbm-174

What I suppose is that the last IIC-OSIC-TOOL docker image does not include the update we have made recently in PR #283 related to the PR #261 where models and symbols for Xyce and ngspice where introduced.

Here I provide you the netlists generated by xschem for ngspice and Xyce.
There i no difference in the simulation results,

Ngspice

**.subckt dc_hbt_13g2
Vce net3 GND 0.0
I0 GND net1 0.0
Vc net3 net2 0
.save i(vc)
XQ1 net2 net1 GND GND npn13G2 Nx=1
**** begin user architecture code
.lib cornerHBT.lib hbt_typ
.param temp=27
.control
save all
dc Vce 0 1.2 0.01 I0 0 5u 0.1u
write dc_hbt_13G2.raw
.endc
**** end user architecture code
**.ends
.GLOBAL GND
.end

Xyce

**.subckt dc_hbt_13g2
Vce net3 GND 0.0
I0 GND net1 0.0
Vc net3 net2 0
XQ1 net2 net1 GND GND npn13G2 Nx=1
**** begin user architecture code
.preprocess replaceground true
.option temp=27
.step I0 0 5u 0.1u
.dc Vce 0 1.2 0.01
.print dc format=raw file=dc_hbt_13G2.raw I(Vc)
.lib  your_location/IHP-Open-PDK/ihp-sg13g2/libs.tech/xyce/models/cornerHBT.lib hbt_typ
**** end user architecture code
**.ends
.GLOBAL GND
.end

@dwarning could you please review it ?

[dbm-174]

Many thanks for the fast and very helpful replies.
I did not use the docker image. I used the main branch of the IHP repository and switched to the most recent dev. Now the output is the same (ngspice=blue stars).

Thanks again and sorry to bother!