Hi @Stefan Schippers I remember we were talking about the resistance value for sky130 pdk a while ago. I have another quick question regarding the layout aspect of

res_xhigh_po

which is a generic version high resistance polysilicon resistor that takes more generic geometric

W

values. When I go to magic and try to find out the layout for

res_xhigh_po

I do not think I have found any pcell for that, only the ones available are those 0.35, 0.69, 1.41, etc. However, those pcells the

W

seems editable and can take other values. I have not done any LVS yet but wondering what is the most convenient way to have a resistor layout that is LVS/DRC clean but can take arbitrary

L

and

W

values? Thanks. Also, I know you can make

mult

to be some integers meaning they are placed in parallel, how about if I want multiple of them in series?

I can answer that: (1) There are only fully officially characterized models for the

res_high_po

at those specific widths, which correspond to the exact device width that precisely fits 1 to 5 contacts on the terminals. The idea, I think, is that it is hard to gauge the exact resistance of the terminal area for any arbitrary contact geometry, so they fabricated and measured five devices and produced models to match what they measured. The

res_xhigh_po

device, on the other hand, was introduced with sky130 and was only experimental in s8, and I expect has not been completely characterized (at least not in the sky130 PDK). Its model is not as sophisticated as

res_high_po

, and the width-specific models just call the generic model with a specific width. Out of concern for the fact that the sky130 DRC rules insist that

res_xhigh_po

devices must exist in only the five "approved" widths, I followed that convention. The simple

res_xhigh_po

device model divides the device width by the contact pitch to get the number of contacts, but it does not try to determine the effect of the remainder of poly on the sides of the contact when the width does not exactly match the contact pitch, so the value will be slightly off if the device width isn't one of the "approved" widths. I could easily add the generic base model to magic's device generator script. But if you just draw the layer type

xpolyres

in magic and contact both ends with layer type

xpc

, then it will extract as generic type

res_xhigh_po

. (2)

M

is the SPICE parameter for multiple devices.

mult

is a parameter used for mismatch simulation, for the obscure reason that you can't use the value

M

inside model equations in SPICE. So

mult

is supposed to be set equal to

M

and is multiplied by the square root of the device area to get the variance for mismatch calculation. I think that there are versions of SPICE that understand

S

as a series multiplier, or maybe it's just dependent on a subcircuit model being defined with an

S

parameter, but regardless, ngspice and the sky130 models don't support that. However, if you use netgen for LVS, it will combine resistors in series to match layout against schematic, so you can just specify the total length in xschem (but, going back to the discussion of terminal resistance above, the total resistance of ten resistors in series can be quite different from the resistance of one resistor multiplied by ten, so be aware of that in your design).

This is very informative, thanks a lot! Despite not being characterized, I do have applications where I have to use very high-resistance resistors so

res_xhigh_po

becomes my choice. I am using

res_xhigh_po_0p35

with a

L

equals 20. Are there any concerns regarding having too big of

L

? Thanks.