Forums » General Electronics Discussion

Is there a listing somewhere describing or defining the MOSFET parameters that can be changed. For instance, placing the cursor on:

"C_OSS" displays "Output Capacitance (GS short @AC)" "C_ISS" displays "Input Capacitance (DS short @ AC)" "C_RSS" displays "Reverse Transfer Capacitance (GS short @ AC)"

Precisely, what do these mean?

Terms like "Threshold Voltage" (="V_TO"); and Source, Gate, and Drain Ohmic Resistance (= R_S, R_G, and R_D) are understandable.

Thanks.

About datasheet parameters etc.

To edit models see:

https://www.circuitlab.com/docs/faq/#q_add_custom_models

https://www.circuitlab.com/forums/modeling-and-simulation/topic/sq59q7zy/model-a-low-leakage-schottky-diode/

Note that there are some unanswered questions about editing CL model parameters (which may not affect you anyway):

https://www.circuitlab.com/forums/feature-requests/topic/6k7v65fx/questions-about-editing-model-parameters/

You cannot simply map datasheet parameters onto a device simulation model.

However, if you can find a spice model for your target device, then you can edit the relevant parameters of one of the built-in CL models and use that in your circuit.

SPICE parameters for devices have little to do with datasheet specifications. They are much more to do with semiconductor physics and the particular process under which a given device is manufactured at the foundry. Consequently it is not always a simple task to map datasheet information onto the model parameters.

If you want to try to understand more about what the SPICE - and hence CL - parameters mean in diodes, bipolar transistors and MOSFETs, then you might like to have a look at:

http://www3.imperial.ac.uk/pls/portallive/docs/1/56133736.PDF

with individual slide sets:

http://www3.imperial.ac.uk/pls/portallive/docs/1/7292571.PDF

http://www3.imperial.ac.uk/pls/portallive/docs/1/7292572.PDF

http://www3.imperial.ac.uk/pls/portallive/docs/1/7292573.PDF

For more detailed information about bjt's in particular, have a look at this book:

http://ieeexplore.ieee.org/stamp/stamp.jsp?arnumber=01480193

available from:

http://www.lulu.com/spotlight/iangetreu

and

http://www.amazon.com/Modeling-Bipolar-Transistor-Ian-Getreu/dp/B000EYPQLU

Another excellent (and free) book about transistor modelling, go to:

http://www.aeng.com/spice_modeling.htm

and register to get a copy of:

Definitive Handbook of Transistor Modeling

I'm sorry - How does this answer my question??

Have you read any of the links I pointed you to?

"Is there a listing somewhere describing or defining the MOSFET parameters that can be changed."

&

"Precisely, what do these mean?"

CL models are stripped down spice models.

Google:

"spice mosfet parameters"

and you will find that there are many different types of spice MOSFET models.

Some are supersets of others, some are defined by pretty much unique parameter sets.

CL does not defined exactly which model their MOSFETs are based on so it is not clear exactly what each parameter means.

They are probably based on the "simplest" NMOS and PMOS .model statement descriptions.

Clarification: "Is there a listing somewhere describing or defining the MOSFET parameters that can be changed." My question was specifically related to CircuitLab. I know about MOSFET and about the various parameters of MOSFETs.

The generalized model is preferable over that of a specific MOSFET.

Within CL, one can pop-up the MOSFET parameter window which displays the parameters that can be changed within CL. Of these, I am/was asking about clarification of the following three that are on the MOSFET parameter change window within CL:

Placing the cursor on the indicated items within the parameter window

"C_OSS" displays "Output Capacitance (GS short @AC)" "C_ISS" displays "Input Capacitance (DS short @ AC)" "C_RSS" displays "Reverse Transfer Capacitance (GS short @ AC)"

Ah, OK.

Each capacitance is measured at with the device biased at some specified Vgs (gate to source voltage) and Vds (drain to source voltage) but with either:

i) the other two terminals shorted at AC by connecting a large very low inductance and low effective series resistance capacitance across those two pins;

or;

ii) one of the terminals connected directly or decoupled to an AC ground by connecting a large very low inductance and low effective series resistance capacitance from the pin to the AC ground.

C_oss is drain to gate capacitance with gate shorted to source at AC. C_iss is gate to drain capacitance with drain shorted to the source at AC. C_rss is drain to gate capacitance (with source connected to ground).

See:

2.5 Capacitances and Gate Charges

in:

http://www.ixys.com/Documents/AppNotes/IXAN0065.pdf

and:

2.6.2.2 Capacitances

on pages 19 & 20 of:

http://www.nxp.com/documents/application_note/AN11158.pdf

CL quoting:

"C_RSS" displays "Reverse Transfer Capacitance (GS short @ AC)"

is a bit misleading but is probably OK as a shorthand notation.

K_P seems as "transconductance" but its unit is A/V^2. The unit of transconductance is A/V. If you build a simple NMOS circuit such as a diode connected one with an ideal current source where Vgs=Vds, you never get the correct value of Vgs for a fixed current by using gm=2Id/(Vgs-Vth).

Any comments?

For instance:

The circuit in https://www.circuitlab.com/circuit/besfqw/nmos-bias/

results in a Vgs of 0.85 V for a fixed drain current of 1 mA and a supply voltage of 1.8V when K_P is set to 0.01, V_TO to 0.4 and all other parameters are set to zero for convenience.

The theoretical value of gm = 0.01 = 2*1e-3/(Vgs-0.4) does not yield a Vgs of 0.85V. It yields 0.6 V.

Also the unit of gm is not A/V^2 as I pointed in my previous comment.

Comments?

I just found that K_P is actuallu MobilityCoxW/L. It is not transconductance as it says in the properties window.

Unit is correct which is A/Vˆ2 .

@ertanzencir,

K_P in CL is equivalent to the KP parameter in spice.

In spice, KP is defined to be the MOSFET transconductance parameter.

Please refer to the MOSFET model in:

http://www3.imperial.ac.uk/pls/portallive/docs/1/7292573.PDF

or any other spice model description resource such as:

http://bwrcs.eecs.berkeley.edu/Classes/IcBook/SPICE/UserGuide/elements_fr.html

(see also my earlier post in this thread for more:

https://www.circuitlab.com/forums/modeling-and-simulation/topic/f2j5jq2a/mosfet-parameters/#comment_5001)

:)

Hello Signality,

True. K_P is named as transconductance and given by Mobility*Cox.

The way CL uses it is MobilityCoxW/L.

Spice model has W/L but no W/L parameter in CL.

If you click on the link I sent simulate that circuit for DC you will see that Id=1/2MobilityCoxW/L(Vgs-Vth)ˆ2 is satisfied if K_P is defined as MobilityCoxW/L by CircuitLab different from Spice..

I wonder what your feedback is after you simulate the circuit. Just change Id and measure Vds=Vgs you will see that the numbers make sense only when K_P parameter is thought as MobilityCoxW/L rather than the conventional Spice way.

It is also questionable why there is no W and L as design parameters. It should be included..

It is nice to have quick feedbacks btw. Highly appreciated.

Regards EZ

Thanks.

I'm struggling to get a grip on K_P. If I drag & drop an N-Channel MOSFET The default value is 5. Using the default parameters, the simulation is reasonably close to the actual performance of the circuit on the bench. However, the value of K_P from the Spice model for the actual MOSFET I am using is 1.04E-6, but if I enter that in the parameter box I get absurd results. In fact if I enter 11, which is the typ Gfs from the datasheet I get even closer results. I understand that Gfs from the datasheet is in A/V whereas K_P is A/V[squared]. Can anyone explain this? Thanks.

@abenton3

"However, the value of K_P from the Spice model for the actual MOSFET I am using is 1.04E-6, but if I enter that in the parameter box I get absurd results. "

What MOSFET model are you trying to use?

Are you importing it into CL?

Is it a .model or a .subckt? (AFAIK CL will only import .model and will not import .subckts models.)

Can you post a link to it?

Can you make your example public?

I don't know why, but the URL on the Ixys web site does not change as I drill down to the actual Spice model file. Anyway, if you feel inspired, the basic URL is: http://www.ixys.com/TechnicalSupport/pspice.aspx Then select DISCRETE MOSFETs and N-Channel Depletion-Mode MOSFETs. You can then download the PSPICE file. Thanks.

Thanks for you help, Signality!

I am trying to import a SPICE Model into CL but there is some format I am missing. I tried to just copy the .MODEL string into CL but get various error messages. Is there some special way to import and existing .MODEL into CL?

The key point to note about MOSFET models in CircuitLab is that only LEVEL 1 models are accepted. Most manufacturer-provided SPICE models for MOSFETS I have encountered are LEVEL 3.

LEVEL 1 (Schichman-Hodges Model) is limited in capability, but simulate quickly and are supposed to be good for timing calculations (good for the typical hobbyist switching application, maybe).

LEVEL 3 is a semi-empirical model, taking into consideration several effects that are ignored in LEVEL 1. There are many parameters in the LEVEL 3 model that have no correspondence to the parameters in LEVEL 1.

A detailed discussion of the differences is here:

https://e2e.ti.com/cfs-file/__key/communityserver-discussions-components-files/234/MOSFET_5F00_MODELING.PDF

There is no straightforward way to take the parameters from a manufacturer's LEVEL 3 model and use them in the LEVEL 1 model of CircuitLab.

You may get decent results using the SPICE default parameters in the above linked article, and adjusting K_P and VTO to match the datasheet.