Stats

  • Locked Locked
  • Replies 13
  • Subscribers 126
  • Views 12213
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

Running the power sic MOSFET model using the spectre simulator

liangqunshan

I used onsem's sic mosfet model （NTHL040N120M3S）for double  pulse test simulation which will generates  large voltage and current, but the simulation results were not satisfactory，just  as follows：

This is the schematic diagram I built:

the NTHL040N120M3S model was downloaded from this website ：  Case: 00451022 (site.com)

the datasheet download website for this device ：Silicon Carbide (SiC) MOSFETs (onsemi.com)

The corresponding netlist is as follows：

// Design view name: schematic
simulator lang=spectre
global 0
include "/home/student1/PDK/csmc600v/Docs/Spice_Mode/10HVCSDST60V19/10HVCSDST60V19/s10hvcsdst60v19.scs" section=tt_20v
include "/home/student1/model_stage2/NTHL040N120M3S_spectre/NTHL040N120M3S_Rev1.scs"

// Library name: qsliang_sic
// Cell name: NTHL040N120M3S_3P_DPT
// View name: schematic
V10 (net012 GND) vsource dc=18 type=dc
V9 (inv_in GND) vsource dc=0 type=dc
V8 (net011 GND) vsource dc=-5 type=dc
V7 (inv_in GND) vsource dc=0 type=dc
V6 (net014 VD) vsource dc=-5 type=dc
V5 (GND 0) vsource dc=0 type=dc
V0 (net016 GND) vsource dc=800 type=dc
V2 (net6 GND) vsource dc=15 type=dc
V1 (net4 GND) vsource dc=-5 type=dc
M4 (Tj inv_in net011 net011) mn20v m=1 mt=100 w=10u l=1.4u as=12.625p \
ad=80.64p ps=22.725u pd=40u
M0 (Tcase inv_in net4 net4) mn20v m=1 mt=100 w=10u l=1.4u as=12.625p \
ad=80.64p ps=22.725u pd=40u
M3 (net016 net014 VD Tj Tcase) NTHL040N120M3S_5P
M2 (VD VGS GND Tj Tcase) NTHL040N120M3S_5P
M5 (Tj inv_in net012 net012) mp20v m=1 mt=200 w=10u l=1.6u as=12.5625p \
ad=72.8p ps=22.6125u pd=38.4u
M1 (Tcase inv_in net6 net6) mp20v m=1 mt=200 w=10u l=1.6u as=12.5625p \
ad=72.8p ps=22.6125u pd=38.4u
L0 (net016 VD) inductor l=200u
V4 (in GND) vsource dc=0 type=pwl \
file="/home/student1/qsliang/sic/qsliang_sic/doupul.txt"
C0 (net016 GND) capacitor c=660u
R0 (in VGS) resistor r=10.00
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 diagnose=yes \
maxnotes=5 maxwarns=5 digits=5 cols=80 dc_pivot_check=yes pivrel=1e-3 \
sensfile="../psf/sens.output" checklimitdest=psf
tran tran stop=10u errpreset=moderate write="spectre.ic" \
writefinal="spectre.fc" annotate=status maxiters=5
finalTimeOP info what=oppoint where=rawfile
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
primitives info what=primitives where=rawfile
subckts info what=subckts where=rawfile
save M2:1
saveOptions options save=allpub

The version of spectre I use is 19.1.0.496.isr12 64bit -- 16 Oct 2020

Does' The results calculated by Spectre may be incorrect because the junction current model has been linearized ' mean that the current value is not correct ？

What impact will those "Top 10 Residue Convergence failure counts accumulated from the beginning of `dc gmin stepping' analysis、warnings and notices" have on the simulation results? Do I need to do something to eliminate them?

Additionally, do I need to set "bin-relref=yes, highvoltage=yes" ？ If so, how do I set it ？

  • in reply to liangqunshan

    Dear liangqunshan,

    liangqunshan said:
    The reason why I said " I added the “hz1 dyn_highz node=["*"] duration=2e-09 time_window=[1e-09 1e-08] ” command to the file called highvoltage_enable.scs，but it does not work" is that the simulation results for adding this command are the same as those for not adding this command. the simulation results did not provide high impedance nodes, even though I adjusted the duration time and time window,

    I understand and am happy to read you tried a few options. Thank you for your explanation.

    liangqunshan said:

    But I didn't see such a table.

    The simulation results are as follows：

    The motivation for using that check was to assist in the DC operating point simulation which occurs prior to the transient analysis. If you examine the log file you just provided, your DC operating point analysis was successful.

    In addition, looking at the output log of the DC operating point suggests the operating points of devices M0, M4, and M5 are contributing to the DC operating simulation time and difficulty. These conventional MOS devices have very large gate source voltages across them (5V or more!). They also appear to be quiescent in your circuit. I am not sure if they are needed as you seem to be focused on the performance of your SiC devices M2 and M3. Perhaps if you remove them from your netlist or change their operating points to something more reasonable (much lower vgs voltages) that will ease the DC operating point analysis.

    liangqunshan said:
    Protected devices exist and are not included in the circuit inventory.

    Since you are using protected devices, I am not sure if spectre can inspect their internal nodes to determine if they possess high-impedance states during the transient simulation.

    In any case, it appears your simulation is now converging and completing - which is good. Good luck!

    Shawn

  • in reply to ShawnLogan

    Hello，ShawnLogan ，thank you very much for your help, and now I can concentrate on the follow-up design work, thank you very much！

  • in reply to liangqunshan

    Dear liangqunshan,

    You are most welcome! I am just happy you've made some progress, I can tell you have learned a lot and that is all that matters!

    Shawn

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.