Help defining PSPICETEMPLATE for BAV99 component

Tue Jun 07, 2005 4:33 am   

I set up a circuit using part BAV99
(http://www.semiconductors.philips.com/acrobat/datasheets/BAV99_4.pdf).
I defined the following PSpiceTemplate property "D^@REFDES %A %C
@MODEL\nD^@REFDES %C %J @MODEL". When I run the simulator (pspice), I
find that the PSpiceTemplate property that I devised is not correct.

Because BAV99 is a double diode, the device itself has three terimals.
The pin properties for BAV99 are configured as A, C, J corresponding to
physical pins 1, 2, and 3 respectively on the device.

I devised PSPICETEMPLATE this way because I was trying to get the net
node assignment to substitute properly as they ought to for basic Spice
Diode. How should I revise the PSPICETEMPLATE variable so that the
expansion is correct during substitution?
Thanks

PSpiceTemplate: D^@REFDES %A %C @MODEL\nD^@REFDES %C %J @MODEL


PSpice console window output:


**** 06/06/05 21:15:01 ******* PSpice 10.3.0 (Jan 2004) ******* ID#
1111111111
** Profile: "SCHEMATIC1-bias" [
D:\DESIGN\test4\bav99-pspicefiles\schematic1\bias.sim ]


**** CIRCUIT DESCRIPTION


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




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

*Libraries:
* Profile Libraries :
* Local Libraries :
..LIB "../../../bav99-pspicefiles/bav99.lib"
* From [PSPICE NETLIST] section of
D:\OrCAD\OrCAD_10.3\tools\PSpice\PSpice.ini file:
..lib "D:\design\hb\humminbird2-PSpiceFiles\humminbird2.lib"
..lib "nom.lib"

*Analysis directives:
..PROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
..INC "..\SCHEMATIC1.net"



**** INCLUDING SCHEMATIC1.net ****
* source BAV99
X_DN1 N00185 N00220 N00207 SCHEMATIC1_DN1
V_V1 N00178 N00233 5Vdc
R_R1 N00178 N00185 1k
R_R2 N00233 N00207 2k
R_R3 N00233 N00220 3k

..subckt SCHEMATIC1_DN1 A C J
D_DN1 A C BAV99
D_DN1 C J BAV99
..ends SCHEMATIC1_DN1

**** RESUMING bias.cir ****
..END


**** EXPANSION OF SUBCIRCUIT X_DN1 ****
X_DN1.D_DN1 N00185 N00220 X_DN1.BAV99

ERROR -- Name "X_DN1.D_DN1" is defined more than onceX_DN1.D_DN1 1
------------$
ERROR -- Extra text on line

Tue Jun 07, 2005 7:25 pm   

Jim, thanks for replying! Your help set me forward about one light year
on the evolutionary scale .

In regards to your question the complete part description is as follows
(note this requires fixed font for viewing the ASCII diagram properly).

BAV99 part:

2 o--|<l--o--|<l--o 1
|
|
o
3

Where,

cathode o--|<l--o anode

Pins/terminals 1, 2, 3 correspond to net nodes A, C, J, respectively.

I discovered that my original circuit had no ground, which contributed
to part of pspice breakage. I revised my PSPICETEMPLATE property as
follows:

D1^@REFDES %A %J @MODEL \nD2^@REFDES %J %C @MODEL

Note I am using OrCAD v. 10.3 and although broken in some areas, I
learned to avoid some minor glitches by avoiding "doing that". I re-ran
the simulator and received the following results.
Thanks again.


**** 06/07/05 12:13:33 ******* PSpice 10.3.0 (Jan 2004) ******* ID#
1111111111
** Profile: "SCHEMATIC1-bias" [
D:\DESIGN\test4\bav99-pspicefiles\schematic1\bias.sim ]


**** CIRCUIT DESCRIPTION


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




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

*Libraries:
* Profile Libraries :
* Local Libraries :
..LIB "../../../bav99-pspicefiles/bav99.lib"
* From [PSPICE NETLIST] section of
D:\OrCAD\OrCAD_10.3\tools\PSpice\PSpice.ini file:
..lib "nom.lib"

*Analysis directives:
..OP
..PROBE V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
..INC "..\SCHEMATIC1.net"



**** INCLUDING SCHEMATIC1.net ****
* source BAV99
R_R3 0 N01535 3k
X_DN1 N00185 N01535 N00207 SCHEMATIC1_DN1
V_V1 N00178 0 5Vdc
R_R1 N00178 N00185 1k
R_R2 0 N00207 2k

..subckt SCHEMATIC1_DN1 A C J
D1_DN1 A J BAV99
D2_DN1 J C BAV99
..ends SCHEMATIC1_DN1

**** RESUMING bias.cir ****
..END

**** 06/07/05 12:13:33 ******* PSpice 10.3.0 (Jan 2004) ******* ID#
1111111111
** Profile: "SCHEMATIC1-bias" [
D:\DESIGN\test4\bav99-pspicefiles\schematic1\bias.sim ]


**** Diode MODEL PARAMETERS


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




BAV99
IS 2.783800E-09
N 1.8703
RS 1.3548
CJO 600.000000E-15
VJ .2
M .1
EG 1.0637
XTI 1.5


**** 06/07/05 12:13:33 ******* PSpice 10.3.0 (Jan 2004) ******* ID#
1111111111
** Profile: "SCHEMATIC1-bias" [
D:\DESIGN\test4\bav99-pspicefiles\schematic1\bias.sim ]


**** SMALL SIGNAL BIAS SOLUTION TEMPERATURE = 27.000 DEG C


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



NODE VOLTAGE NODE VOLTAGE NODE VOLTAGE NODE
VOLTAGE


(N00178) 5.0000 (N00185) 3.1320 (N00207) 2.4805 (N01535)
1.8833




VOLTAGE SOURCE CURRENTS
NAME CURRENT

V_V1 -1.868E-03

TOTAL POWER DISSIPATION 9.34E-03 WATTS


**** 06/07/05 12:13:33 ******* PSpice 10.3.0 (Jan 2004) ******* ID#
1111111111
** Profile: "SCHEMATIC1-bias" [
D:\DESIGN\test4\bav99-pspicefiles\schematic1\bias.sim ]


**** OPERATING POINT INFORMATION TEMPERATURE = 27.000 DEG C


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






**** DIODES


NAME X_DN1.D1_DN1 X_DN1.D2_DN1
MODEL BAV99 BAV99
ID 1.87E-03 6.28E-04
VD 6.52E-01 5.97E-01
REQ 2.59E+01 7.71E+01
CAP 9.96E-13 9.62E-13

JOB CONCLUDED

**** 06/07/05 12:13:33 ******* PSpice 10.3.0 (Jan 2004) ******* ID#
1111111111
** Profile: "SCHEMATIC1-bias" [
D:\DESIGN\test4\bav99-pspicefiles\schematic1\bias.sim ]


**** JOB STATISTICS SUMMARY


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



Total job time (using Solver 1) = .69