Can not run HBT example from Qucs-s using Xyce simulator
Closed this issue · 13 comments
Environment
Qucs-s 24.3.1
Xyce 7.8
Expected Behavior
The examples given in "sg13g2/libs.tech/qucs-s/exampels" does not run using Xyce.
But the examples given in "sg13g2/libs.tech/xyce/examples" run without any trouble, when I run the cir files from Terminal, and I can plot them using Gnuplot.
Can anyone help me how can I run schematics from Qucs-s using Xyce?
Actual Behavior
Steps to Reproduce the Problem
- Open Qucs-s.
- Projects > IHP-Open-PDK-SG13G2-Examples_prj > Schematics > dc_hbt_13g2.sch
- Change Simulator to Xyce.
- Change Model Library Directory from Ngspice to Xyce.
- Simulate
@rupokdas147 Could you please share the netlist please
@KrzysztofHerman Here is the Netlist file...
- Qucs 24.3.0 /home/rf/QucsWorkspace/IHP-Open-PDK-SG13G2-Examples_prj/dc_hbt_13g2.sch
.SUBCKT IHP_PDK_nonlinear_components_npn13G2 gnd c b e bn t Nx=1
.INCLUDE ../../.qucs/IHP-Open-PDK-main/ihp-sg13g2/libs.tech/xyce/models/sg13g2_hbt_mod.lib
X1 c b e bn t npn13G2 Nx={Nx}
.ENDS
.LIB /home/rf/IHP-Open-PDK/ihp-sg13g2/libs.tech/xyce/models/cornerHBT.lib hbt_typ
VPr1 _net0 _net1 DC 0
V2 _net0 0 DC 1
I1 0 _net2 DC 0
Xnpn13G2 0 _net1 _net2 0 gnd IHP_PDK_nonlinear_components_npn13G2 Nx=1
.dc v2 0 1.5 0.005
.step i1 0 5e-06 5.55556e-07
.PRINT dc format=raw file=spice4qucs.dc._swp.plot I(VPr1)
.END
This line automatically becomes ngspice. Don't know why
- Qucs 24.3.0 /home/rf/QucsWorkspace/IHP-Open-PDK-SG13G2-Examples_prj/dc_hbt_13g2.sch
.SUBCKT IHP_PDK_nonlinear_components_npn13G2 gnd c b e bn t Nx=1
.INCLUDE ../../.qucs/IHP-Open-PDK-main/ihp-sg13g2/libs.tech/ngspice/models/sg13g2_hbt_mod.lib
X1 c b e bn t npn13G2 Nx={Nx}
.ENDS
.LIB /home/rf/IHP-Open-PDK/ihp-sg13g2/libs.tech/xyce/models/cornerHBT.lib hbt_typ
VPr1 _net0 _net1 DC 0
V2 _net0 0 DC 1
I1 0 _net2 DC 0
Xnpn13G2 0 _net1 _net2 0 gnd IHP_PDK_nonlinear_components_npn13G2 Nx=1
.dc v2 0 1.5 0.005
.step i1 0 5e-06 5.55556e-07
.PRINT dc format=raw file=spice4qucs.dc._swp.plot I(VPr1)
.END
I changed every "ngspice" to xyce and tried to run it from terminal using "xyce [netlist]" command. Here are the errors:
`*****
***** Welcome to the Xyce(TM) Parallel Electronic Simulator
***** This is version Xyce Release 7.6-opensource
***** Date: Fri Nov 01 06:28:17 EDT 2024
***** Executing netlist /home/rf/QucsWorkspace/IHP-Open-PDK-SG13G2-Examples_prj/dc_hbt_13g2.cir
***** Reading and parsing netlist...
Netlist error: Number of nodes for subcircuit instance XNPN13G2 does not agree
with number of nodes in subcircuit IHP_PDK_NONLINEAR_COMPONENTS_NPN13G2
Simulation aborted due to error. There are 0 MSG_FATAL errors and 1 MSG_ERROR
errors
*** Xyce Abort ***
Simulation aborted due to error. There are 0 MSG_FATAL errors and 1 MSG_ERROR
errors
*** Xyce Abort ***
MPI_ABORT was invoked on rank 0 in communicator MPI_COMM_WORLD
with errorcode 1.
NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.
You may or may not see output from other processes, depending on
exactly when Open MPI kills them.
`
Then I tried run the files from "libs.tech/xyce/examples" they run smoothly without any error.
@rupokdas147 so there is an issue with the binding to a valid model.
In this #241 PR we provide some solution for xschem and ngspice, which binds symbols to valid models.
This is still not working with Qucs-S
As you can see this HBT is a 5 terminal device and the symbol is 4 terminal in Qucs-S so the t terminal is floating.
.SUBCKT IHP_PDK_nonlinear_components_npn13G2 gnd c b e bn t Nx=1
.INCLUDE ../../.qucs/IHP-Open-PDK-main/ihp-sg13g2/libs.tech/ngspice/models/sg13g2_hbt_mod.lib
X1 c b e bn t npn13G2 Nx={Nx}
.ENDS
You could try to copy the sg13g2_hbt_mod.lib file from the #241 PR and place it in
../../.qucs/IHP-Open-PDK-main/ihp-sg13g2/libs.tech/ngspice/models/sg13g2_hbt_mod.lib. Then
use this netlist subckt to simulate
.SUBCKT IHP_PDK_nonlinear_components_npn13G2 gnd c b e bn Nx=1
.INCLUDE ../../.qucs/IHP-Open-PDK-main/ihp-sg13g2/libs.tech/ngspice/models/sg13g2_hbt_mod.lib
X1 c b e bn npn13G2 Nx={Nx}
.ENDS
Validate also if you have the recent version of the PDK.
Your symbol entry in .qucs/user_lib/IHP_PDK_nonlinear_components.lib should look like this:
<Component npn13G2>
<Description>
Author: Mike Brinson, Feb 2024
mbrin72043@yahoo.co.uk, or m.brinson@londonmet.ac.uk.
</Description>
<Model>
.Def:IHP_PDK_nonlinear_components_npn13G2 c b e bn Nx="1"
.Def:End
</Model>
<Spice>*
.SUBCKT IHP_PDK_nonlinear_components_npn13G2 gnd c b e bn Nx=1
X1 c b e bn npn13G2 Nx={Nx}
.ENDS
</Spice>
<VerilogModel> </VerilogModel>
<VHDLModel> </VHDLModel>
<Symbol>
<Line 0 20 0 30 #ff0000 4 1>
<Line 0 -50 0 30 #ff0000 4 1>
<Line 0 -20 -10 10 #ff0000 4 1>
<Line -10 -20 0 40 #ff0000 4 1>
<Line -10 10 10 10 #ff0000 4 1>
<Line -10 0 -20 0 #ff0000 4 1>
<Line 10 0 -10 0 #ff0000 4 1>
<.PortSym 10 0 4 180>
<Arrow -10 10 10 10 6 3 #ff0000 3 1 1>
<.PortSym 0 50 3 0>
<.PortSym -30 0 2 0>
<.PortSym 0 -50 1 0>
<.ID 10 64 npn13G2 "1=Nx=1">
</Symbol>
</Component>
@KrzysztofHerman The Qucs-s working fine with Ngspice. I want to design Power Amplifier. So I need large signal analysis, which doesn't support by Ngspice. I will try the solution you given above and inform you if the Xyce is working or not in the next comment.
The issue we are trying to solve with PR #241 is exact binding between a device symbol and model. The *.cir netlists with examples for Xyce use 5 terminal HBT device. The PR introduces two version of each device npn13G2 and npn13G2_5t where the difference is the number of terminals (additional t output which is correlated with device temperature and self heating ).
I have just added xyce support for 4 and 5 terminal devices, See last commit in PR #241.
There is a difference in VBIC model level ngspice supports level 9 and Xyce level 12. We still do not have a 5 terminal symbol for HBT's in Qucs-S
@KrzysztofHerman If I change "IHP_PDK_nonlinear_components_npn13G2" to "npn13G2" the netlist simulates from terminal using Xyce.
`* Qucs 24.3.0 /home/rf/QucsWorkspace/IHP-Open-PDK-SG13G2-Examples_prj/dc_hbt_13g2.sch
.SUBCKT IHP_PDK_nonlinear_components_npn13G2 gnd c b e bn t Nx=1
.INCLUDE ../../.qucs/IHP-Open-PDK-main/ihp-sg13g2/libs.tech/ngspice/models/sg13g2_hbt_mod.lib
X1 c b e bn t npn13G2 Nx={Nx}
.ENDS
.LIB /home/rf/IHP-Open-PDK/ihp-sg13g2/libs.tech/xyce/models/cornerHBT.lib hbt_typ
VPr1 _net0 _net1 DC 0
V2 _net0 0 DC 1
I1 0 _net2 DC 0
Xnpn13G2 0 _net1 _net2 0 gnd IHP_PDK_nonlinear_components_npn13G2 Nx=1
.dc v2 0 1.5 0.005
.step i1 0 5e-06 5.55556e-07
.PRINT dc format=raw file=spice4qucs.dc._swp.plot I(VPr1)
.END
`
I don't know why Qucs-s adding the library name with the component name. I am actually a newbie in this sector. Removing the "IHP_PDK_nonlinear_components" from the above-highlighted line also helps to simulate the netlist in Ngspice. I have removed the exact phrase from a Ngspice generated Netlist and the netlist simulated in Ngspice smoothly.
@rupokdas147 unfortunately this is the way you can define custom symbols in Qucs-S. You have to wrap it using
subcircuit and additionally reference the spice library with the model of the device you use. In this particular case the device is npn13G2, the wrapper sub-circuit is IHP_PDK_nonlinear_components_npn13G2 and finally the instance name is
Xnpn13G2. There is a discussion on Qucs-S discussion space where we discuss enhancements of Qucs-S so maybe you could drop there your suggestions if you have any.
@rupokdas147 please update the PDK and run your testcase again.
@KrzysztofHerman Thanks, Worked