Using Models from PSPICE in ISPICE
ISPice has a slighty different set of requirements on its models:

You can find a manual for this in C:/spice8/Adding_SPICE_Model.pdf.
The key parts are:


  1) ...separate each part by using  as delimiters. This means that
  the netlist will be enclosed by a line that starts with 5 or more
  asterisks. Therefore, add this to the top and bottom of your netlist
  (the line of ). Even if you are only adding one part, you still 
  need to implement this procedure...
  
  2) ... After the * line marking where your part begins, you will
  be adding a *SRC=  line to link to SpiceNet's part browser...
  
  ***** 
  *SRC=Part_Number;SubCkt;PartType;SubType;Notes


So you should have something like, in your library file.
The rest of your procedure is fine.

*From OrCad Eval (free to reuse)
*****
*SRC=PSpice_PMOS;MP4016A;MOSFETs P;Gen. Purpose;L2
.MODEL MP4016A PMOS LEVEL=2 VTO=-1.5 TOX=1000E-10 NSUB=7.6E15
+XJ=3U LD=1.5U UO=225 UCRIT=3E5 UEXP=.5 UTRA=0.25 RSH=15
+NEFF=2.5 VMAX=1E5 CGBO=3E-10 CGDO=10E-10 CGSO=10E-10 CJSW=1F
+NFS=1E12  GAMMA=1.8 LAMBDA=0.02
******

*From OrCad Eval (free to reuse)
*****
*SRC=PSpice_NMOS;MN4016A;MOSFETs N;Gen. Purpose;L2
.MODEL MN4016A NMOS LEVEL=2 VTO=1.45 TOX=1000E-10 NSUB=4.7E16
+XJ=3U LD=2U UO=625 UCRIT=1E5 UEXP=0.45 UTRA=0.25 RSH=15 
+NEFF=2.5 VMAX=1E6 CGBO=3E-10 CGDO=10E-10 CGSO=10E-10 CJSW=2F
+NFS=4E12  GAMMA=2.2 LAMBDA=0.02
******