[SOLVED] pspice mosfet simulation help!

[saqib.shah06]

I`m trying to simulate a square root domain filter using orcad capture...the design involves the use of MOSFETS operating primarily in saturation.
I used the library file accompanying the book "Microelectronics" by sedra and smith...they worked without any errors...however the circuit kinda behaved abnormally..so i decided to use a bsim3 model..i downloaded a bsimv3 library from somewhere...it has level 3 and level 7 MOSFETS...after creating capture parts from the lib file ..i used them in my circuit.

The problem is whenever i use an nmos model from the lib,it works fine but whenever i try to use a pmos model, pspice shows an error"missing model" on running the simulation.Can someone please help me out?

I have copied the netlist generated.


*********************************************************************

** Creating circuit file "test-schematic1-sa.sim.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:
* Local Libraries :
.LIB "C:\Program Files\Orcad\Capture\Library\PSpice\nom.lib"
* From [PSPICE NETLIST] section of C:\Program Files\Orcad\PSpice\PSpice.ini file:
.lib "C:\Program Files\Orcad\Capture\Library\PSpice\bsim3.lib"
.lib "nom.lib"

*Analysis directives:
.DC LIN V_V5 0 10 .1
.PROBE V(*) I(*) W(*) D(*) NOISE(*)
.INC ".\test-SCHEMATIC1.net"



**** INCLUDING test-SCHEMATIC1.net ****
* source TEST
V_V5 N247842 0 1Vdc
V_V4 N247893 0 2Vdc
R_R1 N247893 N250324 1k
V_V3 N250324 0 -5Vdc
M_Q2 N247893 N247842 0 M12L3P
------------------------------------------------$
ERROR -- Missing model

**** RESUMING test-schematic1-sa.sim.cir ****
.END


 

[abhajn]

MOS is a 4-node device:
M<name> <drain node> <gate node> <source node> <bulk/substrate node> <model name>.

Your netlist has only 3 node names, so the model name is getting interpreted as the 4th node name.
I suspect that the pmos model symbol has got generated wrongly, with 3 pins instead of 4.
You could check the lib file for any difference in pin syntax between nmos and pmos.

.. Abha

 

[sjamil02]

You can just use MOSFET from 'Breakout.olb' library for PMOS or NMOS devices. But you need to change the implementation for NMOS/PMOS to match your model file. Otherwise the simulator will not recognise the model you are using.

For example,
In your bsim3 model file PMOS device is denoted as --> .PMOS ...
Then when you instantiated PMOS from the library, right-click on the device, edit implementation to PMOS.

Hope this shed some light