Three spice files for one MOSFET

[Wilson__]

New to this.  Planning to use MOSFET for switching LED at tens of mA with "Arduino style" PWM dimming (seems low hundreds Hz???).

LTSpice was recommended in this forum.  One MOSFET has one spice file and stimulation result looking good.

For another MOSFET, factory web has three spice files, namely, HS, PS, PS_RC.  Which one should we use?

https://www.vishay.com/en/product/70300/tab/designtools-ppg/

Many thanks

[tooki]

I’m gonna go out on a limb and guess that HS and PS stand for HSPICE and PSpice, and that RC means a model that includes the thermal modeling described in the separate PDF on the product page titled “R-C Thermal Model Parameters Models”.

[PGPG]

Planning to use MOSFET for switching LED at tens of mA with "Arduino style" PWM dimming (seems low hundreds Hz???).

I don't know what is "Arduino style" but PWM dimming means that you use MOSFET simply as switch.
Hundreds Hz are very slow frequency for MOSFETs so nothing to worry about.
I would just check in datasheet if this MOSFET will be correctly switched on and off by PWM signal you have and not spend time on any simulation.

Simulation can cheat you, as model you will use will certainly be using typical parameters of the MOSFET but when you order element you have no guarantee to get one with typical parameters but you have guarantee to get one with parameters within specified in datasheet value ranges.
So checking these data in datasheet is the right way of designing circuits and not simulating the circuit.
Simulation could be acceptable if you can check circuit behavior with specified by you worst case MOSFET paramaters.

[Ian.M]

I answered this for you for another Vishay MOSFET two months ago: https://www.eevblog.com/forum/projects/which-file-to-use-for-ltspice/

TLDR: Vishay HSPICE models typically are incompatible with LTspice and you cant use the thermal model without a lot of work, so for Vishay parts always go for the plain PSPICE model as a first choice.

[Wilson__]

Many thanks.  My bad in slip of mind on other things happening.

[Wilson__]

Would you please mind some advises on the stimulation software.  Should I stay with LTSpice or get another stimulation softwre that reads Vishay model better?   

I had just started using and work fine for my simple switching MOSFET at low freq and low current, nothing too demanding.

[RoGeorge]

If you compare the txt models, all the files are the same model, except they are packed in different formats.

LTspice is my preferred flavor of SPICE, free and with no software limitation, easy to use, fast simulation and with the biggest community, so easy to find answers online.

[Ian.M]

If you compare the txt models, all the files are the same model, except they are packed in different formats.

The problem is although the models are basically the same, the format matters.   
Lets take a look at what LTspice expects for a resistor:

R. Resistor

Symbol Names: RES, RES2

Syntax: Rxxx n1 n2 <value> [tc=tc1, tc2, ...] [temp=<value>]

The resistor supplies a simple linear resistance between nodes n1 and n2. A temperature dependence can be defined for each resistor instance with the parameter tc. The resistance, R, at will be

   R = R0 * (1. + dt * tc1 + dt**2 * tc2 + dt**3 * tc3 + ...)

where R0 is the resistance at the nominal temperature and dt is the difference between the resistor's temperature and the nominal temperature.

and lets take a look at the first resistor in the model - SiUD412ED_HS.TXT line 18:

Code: [Select]

R1 D 3 2.099e-01 3.635e-03 9.966e-06 and SiUD412ED_PS.TXT line 19:

Code: [Select]

R1 D 3 2.099e-01 TC=3.635e-03,9.966e-06
Its obvious that the PSPICE resistor is in LTspice compatible format and the HSPICE resistor isn't.  Both are 0.2099 ohms between nodes D and 3, but the temperature coefficients are in different formats.  Open the attached LTspice sim to see what it makes of HSPICE format resistors.  Inspect the netlist and you will see that apart from the _HSPICE and _PSPICE tags appended to the R1 component designator, they are the spice lines above.  R1_HSPICE throws an error when you run the sim:

Code: [Select]

Error on line 2 : r1_hspice d 3 2.099e-01 3.635e-03 9.966e-06
Unknown parameter "9.966e-06"
and gives the wrong result!

Code: [Select]

       --- Operating Point ---

V(d): 1 voltage
V(3): 0 voltage
I(R1_pspice): 4.76417 device_current
I(R1_hspice): 275.103 device_current
I(V2): 0 device_current
I(V1): -279.867 device_current


LTspice is my preferred flavor of SPICE, free and with no software limitation, easy to use, fast simulation and with the biggest community, so easy to find answers online.

+1