+ Post New Thread
Results 1 to 13 of 13

1st October 2018, 01:01 #1
 Join Date
 Aug 2016
 Posts
 236
 Helped
 2 / 2
 Points
 1,256
 Level
 8
Can this spice model work with LTSPICEs' spice engine
LTSPICEs' spice engine gives 'Only a level 9 bssoi can have 5 nodes' for nmos model FQP6N90C
http://dpaste.com/0QDAYRJ
https://www.fairchildsemi.com/datash...Q/FQP6N90C.pdf
I don't write spice and am not familiar with it. Is the file beyond repair or is it a simple fix?

Advertisment

1st October 2018, 09:57 #2
 Join Date
 Nov 2013
 Posts
 416
 Helped
 90 / 90
 Points
 2,911
 Level
 12
Re: Can this spice model work with LTSPICEs' spice engine
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)"Try SCE to AUX." /John Aaron/
1 members found this post helpful.

1st October 2018, 10:06 #3
 Join Date
 Aug 2016
 Posts
 236
 Helped
 2 / 2
 Points
 1,256
 Level
 8

1st October 2018, 10:42 #4
 Join Date
 Nov 2013
 Posts
 416
 Helped
 90 / 90
 Points
 2,911
 Level
 12
Re: Can this spice model work with LTSPICEs' spice engine
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."Try SCE to AUX." /John Aaron/
1 members found this post helpful.

1st October 2018, 18:05 #5
 Join Date
 Mar 2008
 Location
 USA
 Posts
 5,977
 Helped
 1732 / 1732
 Points
 37,041
 Level
 47
Re: Can this spice model work with LTSPICEs' spice engine
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 freeforall 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).
1 members found this post helpful.

Advertisment

2nd October 2018, 06:43 #6
 Join Date
 Jan 2008
 Location
 Bochum, Germany
 Posts
 43,128
 Helped
 13123 / 13123
 Points
 247,995
 Level
 100
Re: Can this spice model work with LTSPICEs' spice engine
LTSPICEs' spice engine gives 'Only a level 9 bssoi can have 5 nodes' for nmos model FQP6N90C
1 members found this post helpful.

Advertisment

2nd October 2018, 06:56 #7
 Join Date
 Aug 2016
 Posts
 236
 Helped
 2 / 2
 Points
 1,256
 Level
 8
Re: Can this spice model work with LTSPICEs' spice engine
You probably meant the circuit which gives the error.
issue.zip

2nd October 2018, 19:03 #8
 Join Date
 Nov 2013
 Posts
 416
 Helped
 90 / 90
 Points
 2,911
 Level
 12
Re: Can this spice model work with LTSPICEs' spice engine
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.
"Try SCE to AUX." /John Aaron/
1 members found this post helpful.

3rd October 2018, 05:47 #9
 Join Date
 Aug 2016
 Posts
 236
 Helped
 2 / 2
 Points
 1,256
 Level
 8
Re: Can this spice model work with LTSPICEs' spice engine
I cannot get it to simulate maybe there is a particular video you recommend.

3rd October 2018, 09:16 #10
 Join Date
 Jan 2008
 Location
 Bochum, Germany
 Posts
 43,128
 Helped
 13123 / 13123
 Points
 247,995
 Level
 100
Re: Can this spice model work with LTSPICEs' spice engine
You probably meant the circuit which gives the error.

Advertisment

3rd October 2018, 09:31 #11
 Join Date
 Aug 2016
 Posts
 236
 Helped
 2 / 2
 Points
 1,256
 Level
 8
Re: Can this spice model work with LTSPICEs' spice engine
I missed the actual circuit and included an error log instead. Here is the circuit.
issuecircuit.zip

3rd October 2018, 11:23 #12
 Join Date
 Nov 2013
 Posts
 416
 Helped
 90 / 90
 Points
 2,911
 Level
 12
Re: Can this spice model work with LTSPICEs' spice engine
I recommend you to generate with LTspice a symbol for your subblock:
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"Try SCE to AUX." /John Aaron/

3rd October 2018, 12:11 #13
 Join Date
 Jan 2008
 Location
 Bochum, Germany
 Posts
 43,128
 Helped
 13123 / 13123
 Points
 247,995
 Level
 100
Re: Can this spice model work with LTSPICEs' spice engine
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=970e10 xj=1.4e6 nch=1.7e17 ua=1.6e9 u0=700 vsat=1.0e5 drout=3.0 pvag=5 delta=0.10 pscbe2=0 rsh=1.0e3 pdiblc2=1e7 vth0=4.10 voff=0.1 nfactor=1.1 lint=5.90e7 dlc=5.90e7 fc=0.5 cgso=9.32e10 cgsl=0 cgdo=8.65e12 cgdl=9.23e10 cj=0 cf=0 ckappa=0.13 kt1=2.07 kt2=0 ua1=1.02e10 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.
+ Post New Thread
Please login