Can this spice model work with LTSPICEs' spice engine

[Zak28]

LTSPICEs' spice engine gives 'Only a level 9 bssoi can have 5 nodes' for nmos model FQP6N90C

**broken link removed**

https://www.fairchildsemi.com/datasheets/FQ/FQP6N90C.pdf

I don't write spice and am not familiar with it. Is the file beyond repair or is it a simple fix?

 

[frankrose]

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)

 

[Zak28]

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)

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

 

[frankrose]

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.

 

[dick_freebird]

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).

 

[FvM]

LTSPICEs' spice engine gives 'Only a level 9 bssoi can have 5 nodes' for nmos model FQP6N90C

You don't show the model instantiation that gives the said error. Please ask complete questions.

 

[Zak28]

You don't show the model instantiation that gives the said error. Please ask complete questions.

You probably meant the circuit which gives the error.

View attachment issue.zip

 

[frankrose]

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.

 

[Zak28]

I cannot get it to simulate maybe there is a particular video you recommend.

 

[FvM]

You probably meant the circuit which gives the error.

You didn't yet post CC-Source-MOSFET.asc

 

[Zak28]

You didn't yet post CC-Source-MOSFET.asc

I missed the actual circuit and included an error log instead. Here is the circuit.

View attachment issue-circuit.zip

 

[frankrose]

I cannot get it to simulate maybe there is a particular video you recommend.

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

 

[FvM]

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

Error on line 808 : .model m1:bsim3 nmos (level=7 version=3.1 mobmod=3 capmod=2 paramchk=1 nqsmod=0 tox=970e-10 xj=1.4e-6 nch=1.7e17 ua=1.6e-9 u0=700 vsat=1.0e5 drout=3.0 pvag=5 delta=0.10 pscbe2=0 rsh=1.0e-3 pdiblc2=1e-7 vth0=4.10 voff=-0.1 nfactor=1.1 lint=5.90e-7 dlc=5.90e-7 fc=0.5 cgso=9.32e-10 cgsl=0 cgdo=8.65e-12 cgdl=9.23e-10 cj=0 cf=0 ckappa=0.13 kt1=-2.07 kt2=0 ua1=1.02e-10 nj=10 )
* Unrecognized parameter "fc" -- ignored
Warning: Pscbe2 = 0 is not positive.
Warning: Pd = 0 is less than W.
Warning: Ps = 0 is less than W.
Direct Newton iteration for .op point succeeded.

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