Can this spice model work with LTSPICEs' spice engine

Status
Not open for further replies.
I think you added the thermal model of the spice subcircuit, those the 2 extra pins, probably it doesn't like it.
Delete of the thermal model section maybe can solve it. Otherwise I don't know, the subcircuit should have 3 terminals, in the model the 2 1 3 nodes after the name of it.
(strange that the MOS in the model have a width of 1.08m.... but probably good, if it is fairchild's model)
 
Reactions: Zak28

    Z

    Zak28

    Points: 2
    Helpful Answer Positive Rating

Removing the thermal part did nothing and using the thermal model gave same original issue.
 

Hmm... Maybe the model terminal names are different of the symbol. You should check that the symbol has the same 2 1 3 terminal names and are they refer to the correct pin. By the linked description: 2=drain, 1=gate, 3=source
But the model description seems OK. LTSpice should handle it.
 
Reactions: Zak28

    Z

    Zak28

    Points: 2
    Helpful Answer Positive Rating
I vaguely recall having problems with LTSpice trying to use
the geometry params, LTSpice being for discrete and IC use
and not wanting the low down width, length, multiplier type
params that pertain to free-for-all IC design. I think it's the
geometry params after D G S B that are being complained
about ("fifth node" when there are only 4, plus params).
 
Reactions: Zak28

    Z

    Zak28

    Points: 2
    Helpful Answer Positive Rating
LTSPICEs' spice engine gives 'Only a level 9 bssoi can have 5 nodes' for nmos model FQP6N90C
Click to expand...
You don't show the model instantiation that gives the said error. Please ask complete questions.
 
Reactions: Zak28

    Z

    Zak28

    Points: 2
    Helpful Answer Positive Rating
I simulated a simple circuit with the above model and it works for me. There are quite good video tutorials about how to use a subcircuit model in LTSpice, I suggest to watch one.
 
Reactions: Zak28

    Z

    Zak28

    Points: 2
    Helpful Answer Positive Rating
I cannot get it to simulate maybe there is a particular video you recommend.
 

Zak28 said:
I cannot get it to simulate maybe there is a particular video you recommend.
Click to expand...

I recommend you to generate with LTspice a symbol for your sub-block:
1, copy the spice model of the transistor in a mosModel.txt file to the same folder where your testbench (= the .asc file) is
2, open with LTSpice the mosModel.txt file, and click with the right mouse mouse button on the highlighted name of the transistor (= FQPF6N90C). Choose "Create symbol", save this (The generated pins should be 1 2 3 = Gate Drain Source).
3, open your testbench (= the .asc file), press F2 and add the FQPF6N90C symbol from the AutoGenerated directory, from the sym library.
4, on your testbench place a spice directive (at the toolbar click on the .op), type in .include mosModel.txt
5, be sure on your testbench the name of the symbol is the same as the name of the transistor in the mosModel.txt.
6, run a simulation
 

The fault is in not referencing the subcircuit model correctly.

It should be done like below:



Doing so reveals that Ltspice doesn't like this model


Commenting parameter FC removes the error, there are warnings, nevertheless the circuit achieves a reasonable operation point.
 

Status
Not open for further replies.

Similar threads

Menu
Log in
Register
Cookies are required to use this site. You must accept them to continue using the site. Learn more…