New Fet parameter annotator is added in sky130. Shows

gm, gds, vth, vdsat, cgg, cgdo, cgso

and

ft

, calculated as

ft = gm / [2π (Cgg + Cgdo + Cgso)]

All the necessary procedures are in the sky130

xschemrc

file, since all this is pdk-specific (plus the

sky130_fd_pr/annotate_fet_params.sym

symbol). Next step is to add similar functionality for the IHP PDK if there interest. @Harald Pretl I have verified thet the

ft

calculated with the above formula is correct (of course i was not questioning the formula but the ngspice

cg*

parameters), i have run an AC analysis and let ngspice show the point where unity current gain occurs. The frequency value matches with the formula as shown in the video.

This is great! I am a little surprised that his works, though. I complained a few months ago that the overlap caps are not written out by the model, was this fixed? Looks like I need to try again... https://open-source-silicon.slack.com/archives/C0750383B2M/p1721240399826509

@Stefan Schippers this is great, thanks for implementing this. Yes, there is great interest to have this in IHP as well 😀

@Boris Murmann, I had provided a patch for updating the BSIM4 parameter table:https://sourceforge.net/p/ngspice/patches/116/

@Harald Pretl @Boris Murmann I was looking at the IHP pdk (updated my workspace to latest IHP-Open-PDK

dev

branch). The mos models are based on Verilog-A

pspnqs103va

model. (at least the 1st one I am looking at,

sg13_lv_nmos

). As such they are completely different from BSIM4 regarding the observable parameters. What are the equivalents for the common ones I need, like

id, gm, gds, vdsat, vth

and the gate (

cg*

)capacitances? in bsim4, adding

.options savecurrents

I get all the MOS [id] values, like:

i(@m.xm_bias.msky130_fd_pr__nfet_01v8_lvt[id])

and from this syntax it is easy to get all the other parameters by adding the

.save

lines.

Here is a list: https://github.com/bmurmann/EE628/blob/main/4_Technology/src/tb_sg13_lv_nmos_save.spice

@Boris Murmann Thank you for the tip. The vdsat equivalent is

vdss

. There is also a parameter

vsat

which is

vds - vdss

, it tells you how far the transistor is in saturation region. BTW, the IHP parameters are much simpler than the long sky130 bsim4 equivalents.

That's odd. I'll try to duplicate this.

@Stefan Schippers @Boris Murmann yes, the Vth=f(L) is pretty strong in IHP.

Yes I thought the same yesterday night. At higher Vgs values the short channel has higher currents. Didn't realize the dc sweep was at low Vgs values.

Hi, how can I get those features, since Xschem V3.4.6 (get by

git clone <https://github.com/stefanschippers/xschem.git>

) does not have it?

@Toni Tejada The above additions are process specific so they are in the development branch of the IHP pdk: https://github.com/IHP-GmbH/IHP-Open-PDK/tree/dev

Thanks Stefan for the quick response. I mean that the PDK menu does not appear to me. I am running xschem from

/usr/local/share/pdk/sky130A/libs.tech/xschem

to load the pdk´s

xschemrc

file.

@Toni Tejada did you run

make update

in the open_pdks repository after git pull to update the imported repositories? If everything fails get the complete

sky130_tests/

and

sky130_fd_pr/

directories from here and replace your installed copy in

.../libs.tech/xschem/

Thank you very much @Stefan Schippers, now I got accessfully the PDK menu and the schematic examples are updated. What I did:

cd ~/repos/open_pdks

make distclean
./configure --enable-sky130-pdk --enable-reram-sky130
make -j"$jobsize"
sudo make install

Doing

make distclean

the command

make update

return error because the complete cleaning of the previous command, and all the repositories were downloaded from the last version.

@Toni Tejada yes sometimes updates fail. If this happen I delete everything and start over again with a git clone. The

make update

should be issued after a

make veryclean

.

make distclean

clears too much

Hi every one, I am trying to simulate the behavior of nfet_03V3_nvt in sky130PDK. but its simulations are successful only if the L<0.6, for any value of L>0.6 simulation ends with error "could not fine device modelname" Can some one guide me here, @Stefan Schippers I tried to use the W/L combinations that you mentioned but cant get it worked beyond L>0.6. Actually I am looking for a positive VT to reduce leakage current while working with 3V supplies.