choosing correct component for particular model file

I'm trying to simulate a circuit using Spectre (6.1.0) and I'm
confused about choosing the correct component from the
NCSU_Analog_Parts library to match my model file. I want to simulate
45nm technology, so I downloaded the Berkeley PTM for 45nm.

The model must be a spice model because the first line looks like
this:
..model nmos nmos level = 54

I'm under the impression that spectre can read hspice models.

My question is: what component should I place in my schematic...
"nmos" or "nbsim4"?
The simulation seems to work with the "nmos" component because that is
the name in the model file, but it seems to me like I should really be
using the "nbsim4" component. I downloaded this model from the BSIM4
website, so why am I not using the nbsim4 component?
How is the actual component you chose related to the model you use?
I'm concerned that using the "nmos" component will ignore certain
parameters in my model file.

If any one can shed some light on this confusion it would be much
appreciated!

 

[S. Badel]

Renee.St.Amant@gmail.com wrote:

I'm trying to simulate a circuit using Spectre (6.1.0) and I'm
confused about choosing the correct component from the
NCSU_Analog_Parts library to match my model file. I want to simulate
45nm technology, so I downloaded the Berkeley PTM for 45nm.

The model must be a spice model because the first line looks like
this:
.model nmos nmos level = 54

I'm under the impression that spectre can read hspice models.

That's correct.

My question is: what component should I place in my schematic...
"nmos" or "nbsim4"?
The simulation seems to work with the "nmos" component because that is
the name in the model file, but it seems to me like I should really be
using the "nbsim4" component. I downloaded this model from the BSIM4
website, so why am I not using the nbsim4 component?
How is the actual component you chose related to the model you use?
I'm concerned that using the "nmos" component will ignore certain
parameters in my model file.

Both are extremely similar. The fact that your model is named nmos does not imply the need to use
the nmos component. Both components have a 'model' parameter which you set to the name of the device
model you want to use, and that's what'll appear in your netlist. They have plenty of other
parameters that, if set, will appear also on the instance statement in the netlist.

From what I can see, parameters are the same for both components, except the first has
'degradation' parameter which the second doesn't have, while the second has 'nqsmod'.

Basically, what's important is the end result : what gets netlisted. For most common uses, you will
only set the parameters w,l,m,as,ad,ps,pd, so it really doesn't matter which component you're using.

If I may, I'd recommend using components with explicit bulk pin (ie, (n,p)mos4 and (n,p)bsim4).


Cheers,

Stéphane

 

[Andrew Beckett]

On Tue, 18 Sep 2007 10:03:09 +0200, "S. Badel"
<stephane.badel@REMOVETHISepfl.ch> wrote:

Renee.St.Amant@gmail.com wrote:
I'm trying to simulate a circuit using Spectre (6.1.0) and I'm
confused about choosing the correct component from the
NCSU_Analog_Parts library to match my model file. I want to simulate
45nm technology, so I downloaded the Berkeley PTM for 45nm.

The model must be a spice model because the first line looks like
this:
.model nmos nmos level = 54

I'm under the impression that spectre can read hspice models.

That's correct.

My question is: what component should I place in my schematic...
"nmos" or "nbsim4"?
The simulation seems to work with the "nmos" component because that is
the name in the model file, but it seems to me like I should really be
using the "nbsim4" component. I downloaded this model from the BSIM4
website, so why am I not using the nbsim4 component?
How is the actual component you chose related to the model you use?
I'm concerned that using the "nmos" component will ignore certain
parameters in my model file.

Both are extremely similar. The fact that your model is named nmos does not imply the need to use
the nmos component. Both components have a 'model' parameter which you set to the name of the device
model you want to use, and that's what'll appear in your netlist. They have plenty of other
parameters that, if set, will appear also on the instance statement in the netlist.

From what I can see, parameters are the same for both components, except the first has
'degradation' parameter which the second doesn't have, while the second has 'nqsmod'.

Basically, what's important is the end result : what gets netlisted. For most common uses, you will
only set the parameters w,l,m,as,ad,ps,pd, so it really doesn't matter which component you're using.

If I may, I'd recommend using components with explicit bulk pin (ie, (n,p)mos4 and (n,p)bsim4).


Cheers,

Stéphane

Indeed. I believe the idea of the nbsim4 etc is to allow netlisting of the
different instance parameters that bsim4 supports, which the nmos4 knows nothing
about.

In practice these additional parameters are fairly esoteric, and usually anyone
using a particular design process would have their own library relevant to that
process, which netlists the parameters (and constrains the model names) relevant
to the model used.

Regards,

Andrew.
--
Andrew Beckett
Senior Solution Architect
Cadence Design Systems, UK.