(Help)PSPICE simulation error--unknown parameter

hello,can anyone help me to solve this error?i'm really running out of time. The PSPICE version that i'm using is 10.0, i downloaded the schemetic from ON Semiconductor .


** Creating circuit file "TRANS.cir"
** WARNING: THIS AUTOMATICALLY GENERATED FILE MAY BE OVERWRITTEN BY SUBSEQUENT SIMULATIONS

*Libraries:
* Profile Libraries :
* Local Libraries :
.LIB "../../../user library/onsemi ncp1608 rev0.lib"
* From [PSPICE NETLIST] section of C:\OrCAD\OrCAD_10.0\tools\PSpice\PSpice.ini file:
.lib "nom.lib"

*Analysis directives:
.TRAN 0 200m 0 SKIPBP
.PROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
.INC "..\TRANS.net"



**** INCLUDING TRANS.net ****
* source NCP1608 PSPICE MODEL
R_Ro1a N268246 VOUT 2MEG
V_Vin N268222 N268212
+SIN 0 {Vac_in*1.414} 50 0 0 0
C_Cparasitic 0 N268318 10p
I_Iout VOUT 0 DC 250m
X_U3 N2689320 VOUT DIODE_BHAVE PARAMS: VT=0.7
R_Rctup2 N268434 N269006 750k
X_Q1 N268262 0 N268148 N268064 TRANS_Q1
R_Rctup1 N269006 AC_RECT 750k
C_Cds N268064 N268148 50p
X_J1 N268068 N268056 Sw_topen PARAMS: TOPEN=199m TTRAN=1U RCLOSED=0.01
+ ROPEN={1/GMIN}
X_U2 N268148 N268104 ZCD_WINDING 0 XFMRLp PARAMS: LPRIM=400U TRATIO=0.1
X_B3 0 N268222 DIODE_BHAVE PARAMS: VT=0.7
R_RLESR AC_RECT N268104 100m
C_CIN 0 AC_RECT 0.1u
R_RZCD N268318 ZCD_WINDING 100k
X_B2 N268212 AC_RECT DIODE_BHAVE PARAMS: VT=0.7
R_RDRV N268142 N268262 10
R_RS 0 N268064 0.125
R_Ro1b N268068 N268246 2MEG
R_ROUT2A 0 N268068 25.5k
C_CBULK VOUT 0 68u IC=395
X_B4 0 N268212 DIODE_BHAVE PARAMS: VT=0.7
C_CCOMP N279338 0 1u IC=3
V_Vcc N268426 0 15
C_CT 0 N268434 1.33n
R_Rdiode N268148 N2689320 10m
X_U1 N268056 N279338 N268434 N268064 N268318 0 N268142 N268426 NCP1608B
+
X_B1 N268222 AC_RECT DIODE_BHAVE PARAMS: VT=0.7
C_Cgs N268064 N268262 1n
.PARAM Vac_in=85

.subckt TRANS_Q1 1 2 3 4
S_Q1 3 4 1 2 _Q1
RS_Q1 1 2 1G
.MODEL _Q1 VSWITCH Roff=1e6 Ron=0.4 Voff=2 Von=4
.ends TRANS_Q1

**** RESUMING TRANS.cir ****
.END


**** EXPANSION OF SUBCIRCUIT X_U1.X_COMPHYSOVP ****
X_U1.X_COMPHYSOVP.R_R5 0 X_U1.OVPHYS 100meg TC 0 0
X_U1.X_COMPHYSOVP.E_E1 X_U1.X_COMPHYSOVP.HYS1 N268056 VALUE { IF(V(2#)>
+ {(VHIGH+VLOW)/2},V(3#),0) }
X_U1.X_COMPHYSOVP.E_E2 X_U1.X_COMPHYSOVP.4 0 VALUE { IF(V(HYS1,1#) > 0,
+ {VHIGH}, {VLOW} ) }
X_U1.X_COMPHYSOVP.R_R7 0 X_U1.X_COMPHYSOVP.HYS1 100meg TC 0 0
X_U1.X_COMPHYSOVP.R_R6 0 X_U1.OVPREF 100meg TC 0 0
X_U1.X_COMPHYSOVP.R_R4 X_U1.X_COMPHYSOVP.4 X_U1.$N_9999 10 TC 0 0
X_U1.X_COMPHYSOVP.C_C1 0 X_U1.$N_9999 100p TC 0 0
------------------------------------------------$
ERROR -- unknown parameter


I only see one .param statement, and it does not include
such variables as VHIGH, VLOW. I am also suspicious
about a "100meg" resistor value syntax, that would depend
on the particular SPICE dialect / parsing.

Some SPICEs give you a more detailed context for their
complaints. Maybe you can find a more enlightening .out
or .log type file in the run directory?

"meg" is genuine Berkley SPICE and should be supported by any tool, that is claiming SPICE compatibilty, I think.
Due to the parsing order, part of the library isn't shown in the output file. It would be better to post the respective
design files to make the problem understandable (if someone is motivated to run the simulation).

The downloaded project file as below, can anyone try to run it to check whether there consist of same error as mine.Thanks

1. I opened the simulation profile (trans.sim) in PSpice. I had to add the onsemi ncp1608 rev0.lib in Library settings, and then simulation proceeded without any errors.
2. I directly ran psp_cmd on the cir file (trans\trans.cir). The downloaded file had the line:
.lib "C:\Documents and Settings\fftr6r\Desktop\1606_1271\NCP1606\NCP1608\PSPICE Model\Sent to iMIT\User Library\ONSemi NCP1608 rev0"
+ ".lib"
On modifying it to:
.lib "<...>\User Library\ONSemi NCP1608 rev0.lib",
simulation worked fine without any errors.

I couldn't get the same error as you, but my guess is that the space in lib name might be creating a problem here.

(However, I have a different version of PSpice.)

Also, Meg is totally valid syntax in PSpice, so that is definitely not an issue.