Hi,

I would like to perform a simulation on LTspice about a switching MOSFETs.

In particular on how the parasitic inductance and capacitance affect the switching transient.

In order to perform this analysis I need a MOSFET model of SCT3022AL from Rhom semiconductor. Please find attached the datasheet.

Unfortunately it is not avaiable the LTspice model of this MOSFET.

I could create my own model but I saw that the information needed are:

- L (channel length)
- W (channel width)
- VT0 (zero-bias threshold voltage)
- KP (transconductance, µn/pCox)
- LAMBDA (channel-length modulation coefficient)

These information are not avaiable in the datasheet.

How can I do to create my own model? Alternatively, do you know if this model is avaiable?

Thank You.

 

How can I do to create my own model? Alternatively, do you know if this model is avaiable?

Thank You.

I'd use a model from the same company for a MOSFET with similar ratings – they off a bunch of models. Then maybe tweak the parameters in that existing model, if I could figure out how their model relates to the datasheet specs.

 

It's not straight-forward to convert from data sheet info to a Spice model since they use entirely different parameters.
The easiest might be to look for a MOSFET model already in LTspice that close the the transistor you are interested in.
Three important parameters for switching simulations, that should be reasonably matched, are the gate charge, the gate-source threshold voltage, and the ON resistance.
The other MOSFET parameters are generally more important for linear operation, and don't have much effect on the switching behavior.

Using a comparable Spice model from Rhom, as wayneh suggested, could possibly give you a better match.

Internal parasitic MOSFET inductance is usually very small and is likely dominated by the external wiring inductance.

 

Hi,

I would like to perform a simulation on LTspice about a switching MOSFETs.

In particular on how the parasitic inductance and capacitance affect the switching transient.

In order to perform this analysis I need a MOSFET model of SCT3022AL from Rhom semiconductor. Please find attached the datasheet.

Unfortunately it is not avaiable the LTspice model of this MOSFET.

I could create my own model but I saw that the information needed are:

- L (channel length)
- W (channel width)
- VT0 (zero-bias threshold voltage)
- KP (transconductance, µn/pCox)
- LAMBDA (channel-length modulation coefficient)

These information are not avaiable in the datasheet.

How can I do to create my own model? Alternatively, do you know if this model is avaiable?

Thank You.

Hi

Rohm actually does have a spice model for this part. You can download it from their web site.

Otherwise, I will download and post a symbol and model file in a few hours.

eT

 

Hello,

Model attached.
You can use it with the standard LTspice nmos symbol.

1. Copy the .lib file to the schematic folder.
2. Place the nmos symbol on the schematic.
3. Alt-Rht-Click on the symbol to edit symbol attributes.
4. Change "Prefix" to "X" without quotes.
5. Change "Value" to "SCT3022AL_LT" without quotes.
6. Click OK to close Attribute editor.

7. Click anywhere on schematic, then press letter T, to activate text popup window.
8. Click "Spice directive" radio button, then click in the text area and type:

.lib sct3022al_LT.lib

This is the name of the model file.

9. Click OK, then drop the text on the schematic.

10. done.

11. Finish schematic and test.

Note:

There are two different model files. I'm not sure of the difference but you can try each one.
To try the other model file:

1. redo steps 3,5,6. Use "SCT3022AL" without quotes for the Value.
2. Rht-click on the "Spice directive" (step 8) and change to "SCT3022AL.lib" without quotes. click OK
3. Done

eT

 

Hi

Rohm actually does have a spice model for this part. You can download it from their web site.

Otherwise, I will download and post a symbol and model file in a few hours.

eT

It should be very helpfull.
Thank You.

 

It should be very helpfull.
Thank You.

I added to my collection of models of all such SiCMOSFET transistors from ROHM.
https://forum.allaboutcircuits.com/...nents-models-of-ltspice-free-download.133690/
See lib.zip