Problem with component/library in OrCAD PSpice

[CataM]

I have tried to simulate the circuit showed below with thyristor from DISCRETE library but shows me the message: No PSpice Template for Q2 (also for Q1).
But it is not only with S2800 thyristor, with other thyristors from that library too like T106D1/TO or others..




But it works with thyristor 2N1595 from EVAL library for example.

Do anyone know why happens that or how to fix it or what to do ? I think the problem is the library...

If anyone uses Orcad please make a fast simulation using a thyristor from DISCRETE library and tell me if happens that issue.

 

[mvaseem]

Discrete.olb cannot be used for Simulation flow.
Only the libraries lying inside the following folder can be used for Pspice simulation - <install>\tools\capture\library\pspice

To make parts from discrete.olb simulate in Pspice, do following -
1) Add property PSPICETEMPLATE with the value (see the part from eval.olb to know about value). It basically tells the port order (by providing the pin names)
2) Property "Implementation Type" should be having value as "Pspice Model". Change it from dropdown.

 

[CataM]

For the EVAL.olb thyristor, the "value" is : X^@REFDES %A %G %K @MODEL

So for the discrete.olb thyristor should I write this? Q^@REFDES %ANODE %GATE %CATHODE @MODEL ?

It is important the order I write them ? Because on the eval.olb thyristor, when I place the arrow above 1 pin it says this /X1/A Number:0 and for the other pins Number:0 too.

But when I place the arrow above pins on eval.olb thyristor it says /Q1/ANODE Number:2 , for cathode Number:1 and Gate Number:3 ... see attached.

 

[mvaseem]

Yes you should write pin names as displayed when you put arrow on pin.
You should not write "Q^@REFDES...." because Q is reserved for BJT.
X is reserved for subckt, which could represent anything inside it. The subckt/model name is the name entered against IMPLEMENTATION property.
So if you want to use same model as used by eval.olb part, just use same name under IMPLEMENTATION property.
See attached screenshot
.

 

[CataM]

Ok but then for example, your S2008L will behave like a 2N1597 ? Or with its own characteristics ?

Other thing, its changes like adding PSpiceTemplate and all that will remain saved ? Because every time I erase it from the schematic, those properties disappear.

 

[mvaseem]

Yes it would behave like 2N1597.
If you have your own model/subckt, just change the implementation name to that model/subckt and provide that library Pspice simulation settings.
To make the changes permanent you should open olb in capture (using open->library). Then edit the part, modify/add properties and save olb.

 

[CataM]

It is possible to make it behave with its own characteristics? I mean, a S2008L behave like a S2008L :smile:

And one last thing, where can I see its internal parameters ? For example, threshold voltage, capacitance of junctions etc ?