Bob Cordell's Power amplifier book

[Edmond Stuart]

Hi Stein,

MC complains about these models. Are they written in LTSpice format?
Anyway, thanks for the effort.

Cheers,
E.

[magnoman]

Edmond

For Cadence Orcad I at least had to remove the mfg=.... (last line in each model) information from Bob's files.

Hope this helps
-Antonio

[stinius]

Originally Posted by Edmond Stuart

Hi Stein,

MC complains about these models. Are they written in LTSpice format?
Anyway, thanks for the effort.

Cheers,
E.

Hi Edmond

As Antonio is saying, you have to delete the mfg= to make Bob's models workable in Cadence or MC. I had to do that with all of Bob's models.

Cheers
Stein

[Edmond Stuart]

Hi Antonio & Stein,

These are the models (no mfg=... ):

* 2SJ162C VDMOS copyright Cordell Audio December 6, 2010
.model 2SJ162C VDMOS(pchan Vto=-0.08 Kp=0.6 Lambda=0.1 Rs=0.55 Rd=0.1 Rds=1e7 Cgdmax=215p Cgdmin=10p a=0.25 Cgs=900p Cjo=1200p m=0.7 VJ=2.5 IS=4.0E-06 N=2.4)
*
* 2SK1056C VDMOS copyright Cordell Audio December 6, 2010
.model 2SK1056C VDMOS(nchan Vto=0.02 Kp=0.85 Lambda=0.02 Rs=0.62 Rd=0.1 Rds=1e7 Cgdmax=100p Cgdmin=5p a=0.25 Cgs=600p Cjo=1080p m=0.7 VJ=2.5 IS=4.0E-06 N=2.4)

Clearly a proprietary LT format. Not compatible with standard spice.
BTW, WTF 'copyright Cordell Audio'? Has Bob extracted all these parameters?


Cheers,
E.

[stinius]

Originally Posted by Edmond Stuart

Hi Antonio & Stein,

These are the models (no mfg=... ):

* 2SJ162C VDMOS copyright Cordell Audio December 6, 2010
.model 2SJ162C VDMOS(pchan Vto=-0.08 Kp=0.6 Lambda=0.1 Rs=0.55 Rd=0.1 Rds=1e7 Cgdmax=215p Cgdmin=10p a=0.25 Cgs=900p Cjo=1200p m=0.7 VJ=2.5 IS=4.0E-06 N=2.4)
*
* 2SK1056C VDMOS copyright Cordell Audio December 6, 2010
.model 2SK1056C VDMOS(nchan Vto=0.02 Kp=0.85 Lambda=0.02 Rs=0.62 Rd=0.1 Rds=1e7 Cgdmax=100p Cgdmin=5p a=0.25 Cgs=600p Cjo=1080p m=0.7 VJ=2.5 IS=4.0E-06 N=2.4)

Clearly a proprietary LT format. Not compatible with standard spice.
BTW, WTF 'copyright Cordell Audio'? Has Bob extracted all these parameters?


Cheers,
E.

Hi Edmond
You have to replace VDMOS in the model with NMOS or PMOS

like this:
.model 2SK1056C NMOS(nchan Vto=0.02 Kp=0.85 Lambda=0.02 Rs=0.62 Rd=0.1 Rds=1e7 Cgdmax=100p Cgdmin=5p a=0.25 Cgs=600p Cjo=1080p m=0.7 VJ=2.5 IS=4.0E-06 N=2.4)


"BTW, WTF 'copyright Cordell Audio'? Has Bob extracted all these parameters? "

I'm confused as well, Bob claimed somewhere that he had spent a lot of time measuring a lot of transistors to make his models.

Cheers
Stein

[Edmond Stuart]

Originally Posted by stinius

Hi Edmond
You have to replace VDMOS in the model with NMOS or PMOS

like this:
.model 2SK1056C NMOS(nchan Vto=0.02 Kp=0.85 Lambda=0.02 Rs=0.62 Rd=0.1 Rds=1e7 Cgdmax=100p Cgdmin=5p a=0.25 Cgs=600p Cjo=1080p m=0.7 VJ=2.5 IS=4.0E-06 N=2.4)

Hi Stein,

Also the text nchan or pchan has to be removed. Nevertheless I got warnings about unknown parameters:
CGDMAX, CGDMIN, A CGS, CJO, M and VJ. As a result, capacitances are not modeled at all. I wish I could buy such MOSFETs.
Happily, here I found models that do work: (p)spice models 4 2sk1058 & 2sj162 , that is, I don't get warnings.

I'm confused as well, Bob claimed somewhere that he had spent a lot of time measuring a lot of transistors to make his models.

Cheers
Stein

That would have been a huge job. Anyhow, Bob, chapeau !

Cheers,
E.

[Bob Cordell]

Originally Posted by stinius

Hi Edmond
You have to replace VDMOS in the model with NMOS or PMOS

like this:
.model 2SK1056C NMOS(nchan Vto=0.02 Kp=0.85 Lambda=0.02 Rs=0.62 Rd=0.1 Rds=1e7 Cgdmax=100p Cgdmin=5p a=0.25 Cgs=600p Cjo=1080p m=0.7 VJ=2.5 IS=4.0E-06 N=2.4)


"BTW, WTF 'copyright Cordell Audio'? Has Bob extracted all these parameters? "

I'm confused as well, Bob claimed somewhere that he had spent a lot of time measuring a lot of transistors to make his models.

Cheers
Stein

Hi Stein,

First of all, let me apologize to everyone here for putting the mfg= into my model files. I did not realize that it causes problems with other simulators.

With regard to my set of models, every model was created by hand, and a sample of every device was actually measured by me. This did indeed take an excrutiatingly long time. In general, I used the techniques that I described in my book. Having said that, not all parameters in each model were derived from measurements. For some parameters, I fitted the models to information in the datasheets, where that information was reasonable. Examples would be some parameters like Ccb and ft. For each device, I also used one or more manufacturer's SPICE models as a starting point. If some of the more obsure parameters looked reasonable, I used that value or a similar value.

Cheers,
Bob

[dchisholm]

Bob,

I , for one, admire and commend your approach and your decision to include the LTSpice-specific parameters such as "mfg=", "Vceo=", etc.

Questions of compatibility and library portability deserve a serious answer, not a cursory dismissal. In this case, Mike Engelhardt (the LTSpice author & architect) has chosen to "extend" the standard SPICE syntax, now roughly 40 years old and created for use in a computing environment that is barely recognizable from today's world. He is not unique in this regard: the encrypted models of HSPICE, and Multisim's method of mapping the nodes of a SPICE model to the pins of a schematic symbol come to mind. In my mind, making an LTSpice ".model" statement (containing the LTSpice-unique parameters) portable to other simulators is a very straightforward, and rather obvious effort. It requires only a very basic text-editor - in many cases adding a semicolon (introduced, as I recall, by PSPICE as the delimiting symbol for in-line comments) is all that's needed.

I think there's value in retaining the "mfg=" information. It's not just the fact that, as one of Edsel Murphy's corollaries states, "Interchangeable parts won't.". This Forum, of all places, appreciates that there are often subtle differences among interchangeable parts. Knowing the origins of a model's parameter values is at least a first step toward understanding those differences.

Bob, thanks for making the effort to develop those models and share the results. At least we know your methodology. In most cases you simply receive a model with no hints as to whether it was developed from purely theoretical considerations; from published (or perhaps unpublished) Data Sheet values; from measurements on a batch of components; or from measurements across several batches. You don't know if the model is intended to represent "typical" performance, or "worst-case" behavior, or a mixture. If the model was verified against physical measurements you don't know what operating conditions or applications were tightly controlled and which were allowed to simply fall "in the ballpark". With Bob Cordell's name on his work we at least know where to start looking for answers to these questions.

Dale

[Edmond Stuart]

Nevertheless I got warnings about unknown parameters:
CGDMAX, CGDMIN, A CGS, CJO, M and VJ. As a result, capacitances are not modeled at all. I wish I could buy such MOSFETs.

[dimitri]

CGDMAX, CGDMIN, A CGS, CJO, M and VJ

I'll try to search here: LTspice : LTspice/SwitcherCAD III