Comments (8)
There is no (to my knowledge) schematic or picture showing the standard cell implementations. The standard cell instances point directly to a spice netlist.
I have reverse engineered some spice netlists of these standard cells to get the transistor level schematic, but this is a extremely boring work.
from xschem_sky130.
Hi @StefanSchippers ,
Thank you for your message.
To provide some context regarding my original post: I am teaching an introductory VLSI design course for undergraduate students at my university. I was hoping to have my students see/learn what is "underneath" each standard cell symbol block (as opposed to simply taking them for granted).
Based on your message, is my understanding correct that by looking at the spice netlist to which a standard cell instance points to, someone can "see" all the constituent transistors and corresponding connections?
And for reference purposes, are you able to provide some guidance on how someone can find the spice netlist of a standard cell instance given its name? For instance, in your test_stdcells.sch
there are instances of dfrtp_1
and nand2_1
. Where can someone find their corresponding spice netlists (and corresponding file names)?
Thank you!
from xschem_sky130.
Of course you can see the transistor netlist. Take for example the simplest one, inv_2.sym
. You may look into the file:
.../share/pdk/sky130A/libs.ref/sky130_fd_sc_hd/cdl/sky130_fd_sc_hd.cdl
and locate the inv_2 subcircuit:
.SUBCKT sky130_fd_sc_hd__inv_2 A VGND VNB VPB VPWR Y
*.PININFO A:I VGND:I VNB:I VPB:I VPWR:I Y:O
MMIN1 Y A VGND VNB nfet_01v8 m=2 w=0.65 l=0.15 mult=1 sa=0.265
+ sb=0.265 sd=0.28 topography=normal area=0.063 perim=1.14
MMIP1 Y A VPWR VPB pfet_01v8_hvt m=2 w=1.0 l=0.15 mult=1 sa=0.265
+ sb=0.265 sd=0.28 topography=normal area=0.063 perim=1.14
.ENDS sky130_fd_sc_hd__inv_2
You see there is a cmos pair with gate terminals connected to A and drains connected to Y. Source and body of the N-channel connected to VGND/VNB (usually ground nodes) and P-channel source and body connected to VPWR/VPB (usually VCC)
from xschem_sky130.
Thank you @StefanSchippers !
To make sure that I understand the conventions used in the file:
Is there some sort of implied scaling factor for the transistor widths and lengths? For instance, in your inv_2.sym
example, are the widths and lengths assumed to be in units of micro-meters?
And when it comes to the meaning of m=2 in your inv_2.sym
example, does it translate to equivalent NMOS and PMOS transistors whose widths are 2*0.65
micro-meters and 2*1.0
micro-meters, respectively?
Thank you!
from xschem_sky130.
sky130 has a scale=1e-6
set in the model file. This means a transistor specified with W=1 and L=0.15 has width equal to 1um (1e-6m) and length equal to 150nm (0.15e-6m).
For the inv_2 subcircuit, m=2 means there are two devices working in parallel (m is a multiplier factor)
so the actual sizes you deduced are correct.
from xschem_sky130.
Thank you @StefanSchippers !
And is there a difference in meaning between the m
parameter versus mult
?
Thank you!
from xschem_sky130.
no, m and mult are the same thing. xschem sets them to the same number. mult
is simply needed because mult
(like any generic parameter) is available from inside the spice models, while m
is not. This is a spice limitation. The number of parallel devices must be known to the model equations to estimate mismatch parameters. The more the parallel devices the lower the mismatch. More precisely the sigma of variation of parameters (like Vth, Tox etc) is proportional to 1/sqrt(W * L * mult)
from xschem_sky130.
Thank you @StefanSchippers !
I will close this thread.
from xschem_sky130.
Related Issues (17)
- Error running xshem from xschem_sky130 directory HOT 4
- ./bin/xschem not working while running from xschem_sky130 directory HOT 1
- patch problem for sky130 in xschem HOT 2
- Directions to import other librariers (spice or verilog) HOT 4
- Resistor models contain an error. Fix provided. HOT 6
- ngspice run error HOT 1
- Can't find sky130_fd_sc_hd.spice HOT 2
- test_inv.sch references $::SKYWATER_MODEL but when you run a NGSPICE simulation it does not exist HOT 4
- .xschemrc is not present after installing skywater HOT 4
- issue in xschem and Ngspice using sky130 process HOT 1
- is there an example of a circuit, ready for layout? HOT 1
- Installation of magic and skywater pdk HOT 1
- Simulating sky130_stdcells in xschem & ngspice HOT 4
- `XSCHEM_LIBRARY_PATH` issue with default symbols HOT 10
- PDK_ROOT environment variable path not found HOT 5
- Symbol error found HOT 4
Recommend Projects
-
React
A declarative, efficient, and flexible JavaScript library for building user interfaces.
-
Vue.js
🖖 Vue.js is a progressive, incrementally-adoptable JavaScript framework for building UI on the web.
-
Typescript
TypeScript is a superset of JavaScript that compiles to clean JavaScript output.
-
TensorFlow
An Open Source Machine Learning Framework for Everyone
-
Django
The Web framework for perfectionists with deadlines.
-
Laravel
A PHP framework for web artisans
-
D3
Bring data to life with SVG, Canvas and HTML. 📊📈🎉
-
Recommend Topics
-
javascript
JavaScript (JS) is a lightweight interpreted programming language with first-class functions.
-
web
Some thing interesting about web. New door for the world.
-
server
A server is a program made to process requests and deliver data to clients.
-
Machine learning
Machine learning is a way of modeling and interpreting data that allows a piece of software to respond intelligently.
-
Visualization
Some thing interesting about visualization, use data art
-
Game
Some thing interesting about game, make everyone happy.
Recommend Org
-
Facebook
We are working to build community through open source technology. NB: members must have two-factor auth.
-
Microsoft
Open source projects and samples from Microsoft.
-
Google
Google ❤️ Open Source for everyone.
-
Alibaba
Alibaba Open Source for everyone
-
D3
Data-Driven Documents codes.
-
Tencent
China tencent open source team.
from xschem_sky130.