Diode STIEC45-30AS in LTSpice einbinden

[Volker (Gast)]

Hallo Forum,

ich versuche folgende Spice Datei in LTSpice einzubinden:

http://www.st.com/content/st_com/en/search.html#q=STIEC45-XXAS%20PSpice%20model%20(.lib%20&%20.olb)-t=keywords-page=1

Folgendes habe ich bereits versucht:

Datei STIEC.lib im Pfad abgelegt, in dem auch meine .asc Datei steht.
Datei mit Directive .lib STIEC.lib eingebunden.

Zener.asy (LT Symbol) nach Zener1.asy kopiert und die Pinnamen in Anode 
und Cathode umbenannt (weil sie in der lib Datei auch so benannt sind).

Zener1 Diode plaziert und mit rechter Maustaste den Value STIEC45-30AS 
eingetragen.

Wenn ich simulieren möchte kommt die Meldung:
"Can't find definition of model STIEC45-30AS"

Wäre nett, wenn mir jemand auf die Sprünge helfen könnte.

Vielen Dank

Volker

[hinz (Gast)]

RTFM:


Third-party Models
This section explains the basics to adding a third-party model to 
LTspice XVII.

Basically there are two types of third party SPICE models, those 
described with a .MODEL statement and those defined with a .SUBCKT.

Models given as .MODEL statements are for intrinsic SPICE devices like 
diodes and transistors. The .MODEL statement gives the parameters for 
the specific component. The behavior of the device is already known by 
SPICE, only the parameters need to be given to finish specifying the 
component's electrical characteristics.

On the other hand, models given by .SUBCKT statements define the modeled 
component by a collection of circuitry of intrinsic SPICE devices. For 
example, the SPICE model of an opamp would be given as a subcircuit.

The way how to include the model in LTspice depends on whether the model 
is given as a .MODEL statement or a .SUBCKT.

Example for an NPN transistor defined with a .MODEL statement:

1. Add an instance of the symbol NPN to your schematic.

2. Edit the value "NPN" to be "BC547C" to coincide with the name used in 
the target .MODEL statement.

3. Now either

3a) Add the .MODEL BC547C... statement as a SPICE directive on your 
schematic.

or

3b) If you have a file bipol.lib containing your .MODEL BC547C... (other 
models may be too in this file), then add the SPICE directive ".INCLUDE 
bipol.lib" on your schematic. Note that "bipol.lib" must be the complete 
name with any file extensions and that Windows Explorer defaults to not 
showing the file extension. So you if you have a file called 
"bipol.lib.txt", which you can edit/view in notepad, and Windows 
Explorer shows you the file exits as "bipol.lib" The SPICE directive to 
include this file is ".inc bipol.lib.txt" If you used, ".inc bipol.lib" 
you will get an error message that that file can't be found.

or

3c) You can alternatively add the .MODEL BC547C... statement to the file 
typically installed at 
%HOMEPATH%\Documents\LTspiceXVII\lib\cmp\standard.bjt. If you do that 
you will automatically see the model as a choice was editing the NPN 
transistor. If you edit this standard.bjt file outside of LTspice, you 
will have to restart LTspice for it to notice that the file has changed.

Example for a 5-pin opamp. This will be defined with a .SUBCKT 
statement:

1. Add an instance of symbol opamp2 to your schematic.

2. Edit the value "opamp2" to "TL072" on the schematic to coincide with 
the name of the .SUBCKT.

3. Either

3a) Paste the ".SUBCKT TL072 ..... .ENDS" definition as one multi-line 
SPICE directive to your schematic.

or

3b) If you have a file called "TI.lib" containing the definition of 
subcircuit TL072(It will look like a line that starts out as ".SUBCKT 
TL072...") add the SPICE directive ".INCLUDE TI.lib" to the schematic.

It is possible to create a new symbol and program it to automatically 
include the necessary model for the simulation whenever it is used on a 
schematic. See help section Schematic Capture=>Creating New Symbols.

It is possible to create an automatically generated symbol that netlists 
correctly against an arbitrary third party model and have it programmed 
so that it includes the necessary model for the simulation whenever it 
appears on a schematic. See help section Schematic Capture=>Creating New 
Symbols. For most users, this is the only method you should consider for 
adding new models defined as subcircuits since all the details are 
handled for you.

Example for a 3-pin NPN transistor but defined with a .SUBCKT statement:

1. Add an instance of symbol NPN to your schematic.

2. Move the cursor over the body of the newly-placed NPN symbol 
instance. Press <Ctrl>RightMouseButton. A dialog box will appear. Change 
Prefix: QN to Prefix: X. This causes this instance of the symbol to 
netlist as a subcircuit instead of an intrinsic bipolar transistor.

3. Edit the value "NPN" to be "BFG135" to coincide with the name given 
on the .SUBCKT line.

4. Then either

4a) Add the .SUBCKT BFG135 lines to your schematic

or

4b) If you have a file Phil.lib containing your .SUBCKT BFG135 .... 
(others may be too in this file) then you have to add a SPICE directive 
.INCLUDE Phil.lib

One aspect of adding a .SUBCKT model to LTspice is that you need have 
the symbol used to call the subcircuit and the model agree on the same 
pin/port netlist order. The above examples assume the 3rd party model 
you're adding follows popular pin order conventions.

Further related information is in the help sections Schematic Capture 
and LTspice. The basic idea is that the schematic capture program 
generates a netlist that the simulator, LTspice reads. Any aspect of 
importing 3rd party models can be resolved by understanding SPICE 
netlist syntax and how the schematic capture program generates that 
syntax. There are also tutorials prepared on this topic archived at the 
independent users' group at http://groups.yahoo.com/group/LTspice.

[Volker (Gast)]

Hi hinz,

vielen Dank, das einzige was mir gefehlt hat war den Prefix in "X" zu 
ändern. Jetzt funktioniert alles.

Nochmals vielen Dank.

Volker