The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Geometry parameters in Spice/Spectre simulation.
https://designers-guide.org/forum/YaBB.pl?num=1290800136

Message started by Taimur Gibran on Nov 26^th, 2010, 11:35am

Title: Geometry parameters in Spice/Spectre simulation.
Post by Taimur Gibran on Nov 26^th, 2010, 11:35am

Hello. Maybe this would sound a little bit stupid to the more experienced command-line spice/spectre users. I know that making the schematic in a GUI (e.g. Virtuoso) and then generating the netlist, the geometry parameters from the pcell are passed to the netlister, and the netlist will contain parameters such as AS, PS, AD, PD (areas and perimeters of drain/source). But what about running simulations from a manually typed netlist? Should I manually calculate these parameters? Doesn't sound like a straightforward approach. Spectre help is not completely clear about it. So I searched in BSIM3.3 and BSIM4 user manuals, and it's not also clear. So, from your experience, can I rely on a netlist with no explicit as, ad, ps and pd parameters???

Title: Re: Geometry parameters in Spice/Spectre simulation.
Post by pancho_hideboo on Nov 26^th, 2010, 11:11pm

Taimur Rabuske wrote on Nov 26^th, 2010, 11:35am:

But what about running simulations from a manually typed netlist?
Should I manually calculate these parameters?

Yes, you should use same equations for calculating them as PDK.

Taimur Rabuske wrote on Nov 26^th, 2010, 11:35am:

So, from your experience, can I rely on a netlist with no explicit as, ad, ps and pd parameters???

No, it is not appropriate.

Each simulator have default values for as, ad, ps and pd.
If you don't specify them in MOS FET instance stament, simulator use default values.

Title: Re: Geometry parameters in Spice/Spectre simulation.
Post by ywguo on Nov 27^th, 2010, 1:09am

Hi Taimur,

First of all, we need non-zero value of AS, AD, PS, PD, NRS, NRD. It tends to transient non-convergence for some circuits if those values are zero.

Second, we depend on schematic entry software and good PDK to calculate those parameters automatically nowadays. I say good PDK because not all foundries provide PDK that calculate those parameters or calculate those parameters correctly.

Third, even if you have a schematic entry software and good PDK, you cannot always rely on them. For example, the MOSFETs in I/O cells may have very large drain diffusion to meet ESD design rule. It causes bigger non-linear parasitic capacitance, please be careful if you design a very high performance circuit.

Fourth, if unfortunately you do not have any schematic entry software and PDK. There is some parameters in the MOSFET model for estimation of the area and perimeter of drain and source. For BSIM3, there are hdif and ldif, acm and so on. Please read simulator manual, and model manual for details.

The last, you'd better to check your SPICE/Spectre model before you begin to simulate.

Best Regards,
Yawei

Title: Re: Geometry parameters in Spice/Spectre simulation.
Post by ontheverge on Dec 5^th, 2010, 7:03am

Hi Yawei,
If possible, could you name one or two schematic entry software (other than Virtuoso)? that would do a lot help to me.
thanks,
Steve

ywguo wrote on Nov 27^th, 2010, 1:09am: