open-source-silicon.dev

Hi <@U016EM8L91B>, I have few questions more regarding the caravan pad frame. The 18 analog pins in caravan wrapper which have ESD protection, how are the ESD diodes connected to power supply or ground? Are they using  VDDA? And what is  the maximum current specification of QFN pins of package provided by efabless? One more issue, I have extracted the netlist of GPIO pad from *`sky130_ef_io__gpiov2_pad.mag`* . Then fed the netlist to a GPIO pad symbol and tried simulating it for analog connect for ESD. I have used PAD_A_ESD_0_H as input and pad pin as output. I am getting following errors during simulation :  see attachment. Can you please help me with the issue. I have attached the extracted netlist and test bench as well.

I wonder if this has anything to do with the `generic_po` devices being modeled as subcircuits in the combined models but as discrete models in the binned versions? magic extracts `generic_po` devices as discrete models.

magic tech file `version 1.0.470-0-g6d4d117`
``` device resistor sky130_fd_pr__res_generic_po rmp *poly
 device resistor sky130_fd_pr__res_generic_po mrp1 *poly```
`libs.tech/combined/continuous/models_resistors.spice`
```.subckt  sky130_fd_pr__res_generic_po r0 r1 mult=1
+
.param  w = 1 l = 0 r = 0 tc1 = {tc1rsgpu} tc2 = {tc2rsgpu}
+ r_tot = {sw_rp1*l/(w-1e6*(sw_polycd*4-poly_dw))+r}

Rsky130_fd_pr__res_generic_po r0 r1 r = {r_tot*(1+sw_mm_sky130_fd_pr__res_generic_po*mismatch_factor*MC_MM_SWITCH*AGAUSS(0,1.0,1)/sqrt(w*l*mult))}
+ tc1 = {tc1} tc2 = {tc2}


.ends sky130_fd_pr__res_generic_po```
`libs.tech/ngspice/sky130_fd_pr__model__r+c.model.spice`
```.model sky130_fd_pr__res_generic_po       r tc1r=tc1rsgpu   tc2r=tc2rsgpu   rsh=rp1   dw="-tol_poly/2-poly_dw/2" tnom=30```
<@U06JDGN07LM> For a quick and dirty possible solution, you might try putting an `X` at the beginning of the `generic_po` `R` lines. This should work and create a `.bak` backup of the file just in case.
```sed -i.bak '/sky130_fd_pr__res_generic_po/s/^R/XR/' pad_flat.spice```


<@U017X0NM2E7> Thank you so much for your answer. I replaced R with XR but still have some issue. If I use ngspice models instead of combined models, the ESD transistors are not recognized. Please find the updated netlist as well.

Looks like you might have changed all your `R` resistors to `X` devices.
```XR0 m2_12329_34611# a_12068_29431# sky130_fd_pr__res_generic_m2 w=0.65 l=10m```
My suggestion was just to change the `generic_po` resistors to `X` devices. I don’t think there are subcircuit models for the `generic_m*` resistors in the combined models, so you should probably leave those as `R` devices.

Ok. Sorry for my mistake. The resistor issue is fixed but *`esd_nfet_g5v0d10v5`* transistors are not recognized as well.

<@U06JDGN07LM> I’m not absolutely certain, but I think the only difference between the esd nfets and the corresponding non-esd nfets is a non mask recognition layers. As a temporary solution, you might try replacing `sky130_fr_pr__esd_nfet` with `sky130_fr_pr__nfet`.

I think this problem should be reported though. Can you log an issue on <https://github.com/RTimothyEdwards/open_pdks>?