[SOLVED] pspice mosfet simulation help!

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


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

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