https://open-source-silicon.dev logo
#analog-design
Title
# analog-design
m

Matt Venn

09/16/2021, 4:27 PM
I'm trying to simulate an extracted spice netlist of about 50 cells. I'm trying for 5 clock cycles over 20ns. It's taking forever! Are there any techniques to speed up spice simulation of larger designs?
m

Matthew Guthaus

09/16/2021, 4:48 PM
Xyce! You can also do things like increase the time step in the .tran statement. ngspice can also be told to run in parallel by adding this to a .spiceinit: set num_threads=4
m

Matt Venn

09/16/2021, 4:49 PM
can you recommend a Xyce tutorial?
m

Matthew Guthaus

09/16/2021, 4:49 PM
This will only speed up the BSIM model evaluation if you have it compiled with OpenMP. So, the more devices the better. However, it doesn't speed up the matrix solve
No, I don't know of any
We have been pretty active in #xyce though
Although, 50 cells shouldn't take "forever" so it is likely a setting
m

Matt Venn

09/16/2021, 5:19 PM
well, my patience is limited. I'm only waiting 20 minutes till I kil it
it loads the libraries, prints the message about timescale and then sits there eating memory
m

Matthew Guthaus

09/16/2021, 5:21 PM
Are you using an old version of ngspice? There were bugs that prevented library reading in early versions
m

Matt Venn

09/16/2021, 5:21 PM
ngspice-34
m

Matthew Guthaus

09/16/2021, 5:21 PM
That should be fine
t

Tim Edwards

09/16/2021, 6:12 PM
@Matt Venn: If you are simulating a digital standard cell circuit, then ngspice will get bogged down because its methods are much better suited to smooth signals and not the sharp edges of digital signaling. Xyce may do better. If you are doing a mixed-signal design, then the best method is to simulate the digital part using xspice, which is a digital event-driven simulator inside ngspice.
e

Eric Smith

09/16/2021, 8:13 PM
Where is it hanging? Did it find the DC operating point?
m

Matt Venn

09/17/2021, 11:12 AM
I was just trying a transient simulation. Hangs after printing 'timescale'
but I only left it 20 minutes.
@Tim Edwards problem with doing a digital simulation is that I'm wanting to explore this hardware trojan idea further. So I want to change a pfet to an nfet in a standard cell and check it breaks the operation in the expected way.
hence why I'm doing a full extraction rather than blackbox
t

Tim Edwards

09/18/2021, 1:42 AM
One problem with that is that the trojan is creating things that are not recognizable to magic as devices. The changing of, say, the p+ implant to n+ implant does not turn the p-FET into an n-FET; it turns the p-FET into a varactor. (I've forgotten the details of the paper, which layers were modified.)
m

Matt Venn

09/18/2021, 5:12 PM
Yes so my plan is extract the cells then manually change the pfet/nfet in the spice file
I'll make the GDS mod with magic but I don't expect to extract that mod
j

J. Scott Elder

09/19/2021, 1:59 PM
@Matt Venn If you can solve the problem of speeding up SPICE, any SPICE, by 10x, call Cadence; they will buy your solution for $100 Million USD. In the meantime, keep your simulations down to about 100 or so transitions per run. Alternatively, you can do what experts do in semiconductor companies: design all digital using an HDL flow and a mixed signal simulator or run simulations for days, and sometimes a week or more, using the highest compute platforms available.
🤣 1
m

Matt Venn

09/19/2021, 2:04 PM
Yep I'll let them know!
I'm trying to get a handle on what's a realistic size of circuit. So 40 odd cells takes more than 20 mins for 5 clocks
I'm expecting slow but wasn't expecting that slow
j

J. Scott Elder

09/19/2021, 2:09 PM
@Matt Venn It has been that way for decades. No one has come up with a fast way to invert a circuit node matrix. So companies play tricks like breaking a circuit apart and running the pieces in parallel. This is not as precise as SPICE, but in the hands of experts, they know when the results are wrong and revert to the ages old SPICE matrix solvers.
e

Eric Smith

09/23/2021, 9:40 AM
Try looking this over. Lots of important advice
Most especially, make sure you use ngspice-34
m

Matt Venn

09/23/2021, 10:04 AM
thanks Eric
e

Eric Smith

09/23/2021, 10:20 AM
Copy code
ngbehavior=hsa
in the spiceinit seems important.
I just simulated a design with 60 cells and thistran 10ps 4ns 0 20p UIC
Took ~15s on my machine
m

Matt Venn

09/23/2021, 10:22 AM
could you share it somewhere?
e

Eric Smith

09/23/2021, 10:39 AM
add.example.tgz
8 Views