https://open-source-silicon.dev logo
Channels
aa
abcc
activity
adiabatonauts
analog-design
announce
announcements
b2aws
b2aws-tutorial
bag
basebands
beagleboard
bluetooth
board-respin
cadence-genus
cadence-innovus
cadence-spectre
cadence-virtuoso
caravan
caravel
caravel-board
chilechipmakers
chip-yard
chipignite
chipignite2206q_stanford_bringup
chisel
coalition-for-digital-environmental-sustainability
community_denmark_dtu
containers
courses
design-review
design-services
dffram
digital-design
digital-electronics-learners
discord-mods
dynamic-power-estimation
efabless
electric
events
fasoc
fault
foss-asic-tools
fossee-iitb-esim
fossee-iitb-google-sky130
fpga
funding
fuserisc
general
generative-ai-silicon-challenge
genius-vlsi
gf180
gf180mcu
hardware-beginners
help-
ieee-sscs-cac-23
ieee-sscs-dc-21q3
ieee-sscs-dc-22
ieee-sscs-dc-23
ihp-sg13g2
images
infiniband
j-core
japan-region
junk
klayout
latam_vlsi
layouteditor
lvs
lvs-analysis
magic
magical
maker-projects
maker-zone
microwatt
mpw-2-silicon
mpw-one-clean-short
mpw-one-silicon
neuro-mem
nydesign
open_pdks
open-pdk
openadiabaticlogic
openfpga
openhighqualityresonators
openlane
openlane_cloudrunner
openlane-development
openocd
openpositarithmetic
openpower
openram
openroad
opentitan
osu
pa-test-chip
paracells
pd-openlane-and-sky130
picosoc
pll
popy_neel
power
private-shuttle
rad-lab-silicon
radio
rdircd
reram
researchers
rf-mmw-design
rios
riscv
sdram
serdes
shuttle
shuttle-precheck
shuttle-status
silicon-photonics
silicon-validation
silicon-validation-private
sky130
sky130-ci
sky130-pv-workshop
sky65
sky90
skywater
sram
stdcelllib
strive
swerv
system-verilog-learners
tapeout-job
tapeout-pakistan
team-awesome
timing-closure
toysram
travis-ci
uvm-learners
vendor-synopsys
venn
verification-be
verification-fe
verilog-learners
vh2v
vhdl
vhdl-learners
vliw
vlsi_verilog_using_opensource_eda
vlsi_verilog_using_opensoure_eda
vlsi-learners-group
vlsi101
waveform-viewers
xls
xschem
xyce
zettascale
Powered by
Title
g

Greg Warwar

03/01/2023, 6:51 PM
Hi, I'm currently working with the spice models from the git repository : globalfoundries-pdk-libs-gf180mcu_fd_pr/models/... and I see there are "ngspice" and "xyce" model files which are slightly edited from each other. Does anyone know if the original model files from GF are accessible anywhere?
t

Tim Edwards

03/01/2023, 7:36 PM
The original models are in Hspice format (also Spectre) and are considered proprietary. However, the "ngspice" files are only lightly edited, since there are relatively few differences between Hspice and ngspice formats (Spectre is a whole other bundle of issues). @Amro Tork did the conversion and can perhaps provide some details of the conversion, but I think there is not much beyond the device name changes imposed on us by Google (I also did a conversion but Amro's is the one that is currently in the PDK).
a

Amro Tork

03/01/2023, 7:42 PM
@Greg Warwar I don't believe we could release the HSPICE version at least from our end.
But I could try any other question you might have.
g

Greg Warwar

03/01/2023, 7:43 PM
Super! That makes sense, and these files should work fine. Thanks very much
t

Tim Edwards

03/01/2023, 7:43 PM
Actually I can just run a quick diff on the two and tell you what else was changed: Hspice uses tref, ngspice uses tnom. (Some of the) monte carlo parameters have been commented out, although I'm not sure why. Some parameter names were changed, like
r_length
and
r_width
for resistors, which is news to me because I still have the original parameter names being extracted from magic.
a

Amro Tork

03/01/2023, 7:44 PM
@Tim Edwards all the changes to make sure that models will function properly inside ngspice.
Many failures happened because the equations for MC for example.
ngspice
doesn't parse it correctly. We ended up changing it.
t

Tim Edwards

03/01/2023, 7:45 PM
@Amro Tork: But I used to use
r_length
and
r_width
parameters without any issue in ngspice. Right now it's broken because nobody told me it was changed.
@Amro Tork: I guess capacitor
c_length
and
c_width
was also changed?
a

Amro Tork

03/01/2023, 7:46 PM
@Tim Edwards Could you please create a ticket and we could discuss that further there?
t

Tim Edwards

03/01/2023, 7:49 PM
a

Amro Tork

03/01/2023, 7:50 PM
Thanks @Tim Edwards I'll take a closer look and give you feedback why we did this.
t

Tim Edwards

03/01/2023, 7:52 PM
I don't really care why as much as I care that it gets fixed in the magic tech file and that I have caught all the changes that were made.
a

Amro Tork

03/01/2023, 7:53 PM
That's great. Anything is required from my end then?
t

Tim Edwards

03/01/2023, 7:56 PM
Just confirm that I've caught all the changes. But I just looked at the file again and realize that MiM caps still have parameters
c_length
and
c_width
. Why were resistor parameters changed but capacitor parameters not changed?
a

Amro Tork

03/01/2023, 7:56 PM
If I remember correctly, resistance parameters caused the problem with resistor simulation.
t

Tim Edwards

03/01/2023, 7:57 PM
(@Greg Warwar: You opened a can of worms. Sorry for spilling all over your thread. I can move the unrelated conversation elsewhere if you like.)
g

Greg Warwar

03/01/2023, 7:57 PM
@Tim Edwards @Amro Tork Thanks again for the model file information. I'm sure the model files will work fine. I saw something funny in my first simulation, like it was running MC because I was getting a slightly different answer each time I ran the sim, but I need to debug this further. Thanks again for the help and if I find any issues, I will let you know. thanks
a

Amro Tork

03/01/2023, 7:58 PM
@Greg Warwar It is
And we fixed this
MC was enabled by default
g

Greg Warwar

03/01/2023, 7:59 PM
Haha, That's great! Now I'm feeling better 🙂! Thanks
a

Amro Tork

03/01/2023, 7:59 PM
@Tim Edwards Could you please update the files from: https://github.com/efabless/globalfoundries-pdk-libs-gf180mcu_fd_pr
?
@Greg Warwar To fix this you need to replace this file.
g

Greg Warwar

03/01/2023, 8:01 PM
Ok, great! Thank you!
t

Tim Edwards

03/01/2023, 8:01 PM
@Amro Tork: How recently updated? I ran an update on the repository just yesterday.
a

Amro Tork

03/01/2023, 8:02 PM
It was fixed in Jan
@Tim Edwards About why we removed r_length and r_width
in section 3.3.4
This miss up everything, we removed all unused parameters fundmentally.
we didn't do the same for Caps
because we didn't have the same problem.
It's only for resistors.
t

Tim Edwards

03/01/2023, 8:08 PM
I still don't get why that's a problem. There's nothing in the manual that states why you would not be able to use the name
r_width
in an equation, as opposed to
rw
. It's just a parameter name passed to the subcircuit, and then passed to the resistor model. I used it without issue when I was simulating the power-on-reset circuit for Caravel.
a

Amro Tork

03/01/2023, 10:27 PM
It's not the name, it's just using an equation based resistor doesn't work properly with ngspice. We could keep the
r_width
but it won't affect the simulation as we can't use it in the equation anymore. That's why I removed it all together to make sure it's not confusing anyone to try to use it and find that it doesn't affect the simulation.