Issue with FPOLY (CCCS) in order to use poly(n), where n>1

I am not too sure what you are trying to achive with this model but a POLY(3) is a fairly complex way to handle this since the coefficients can rapidly get out of hand, unless you need to control "all" the coefficients, "regular" ABM expressions might be a better approach. In any case, for this:

.subckt SCHEMATIC1_F1 1 2 3 4  
F_F1         3 4 POLY(3) V_F1 V_VDT V_F1 0.0 0.0 1.0 0.0 0.0 0.0 0.0 0.0 0.0
+  0.0 0.0 0.0 0.0 0.0 0.0
V_F1         1 2  
V_VDT         N821065 0
.ends SCHEMATIC1_F1

The V_F1 is repeated so this is only a POLY(2) (?). The only coefficient is for 1.0*(V_VDT), V_CDT references node N821065 which is not part of the subcircuit, see  (X_F1.N821065)    0.0000 in the output file and hence the output.

I would have expected more nodes for the subcircuit, something like:

.subckt <name> 1 2 3 4 5 6 7 8

F_F1 7 8 POLY(3) VF1 VF2 VF3 <coefficients> 

VF1 1 2 0

VF2 3 4 0

VF3 4 5 0

.ends

 See the section in the pspcref.pdf, doc\pspcref directory of the installation, page 172 onwards.

 Hi

I have the problem when entering data in tab SCHEMATI..* [Property Editor] of the CCCS source

I enter the data as follows
COEFF             0.0 1.0 1.0 1.0
PSpice Template   F^@REFDES %3 %4 POLY(3) V_F1^@REFDES V_VF2^@REFDES V_VF3^@REFDES \n+ @COEFF \nV_F1^@REFDES %1 %2 0V \nV_VF2^@REFDES N821065 0 0V \nV_VF3^@REFDES N822098 0 0V

but I can't obtain a current output different to zero caused by second and third entry, i.e.,

VOLTAGE SOURCE CURRENTS
    NAME         CURRENT
    X_F1.V_VF2   0.000E+00      <----this value must be different to zero, because V_VF2  N821065 0 0.5
    X_F1.V_VF3   0.000E+00      <----this value must be different to zero, because V_VF3  N822098 0 0.8

Since COEFF are 0.0 1.0 1.0 1.0 then the results should be as follows

VOLTAGE SOURCE CURRENTS
    NAME         CURRENT
    X_F1.V_VF2   0.500         <----because R_R26  N821065 0  1 and V_VF2  N821065 0 0.5
    X_F1.V_VF3   0.800         <----because R_R27  N821065 0  1 and V_VF3  N822098 0 0.8

Therefore, the final value of the dependent current source CCCS should be 6.300A

I cannot increase the number of nodes in the subcircuit

.subckt <name> 1 2 3 4 5 6 7 8

F_F1 7 8 POLY(3) VF1 VF2 VF3 <coefficients>

VF1 1 2 0

VF2 3 4 0

VF3 4 5 0

.ends

Regarding pspcref.pdf file, where they are located currentsense and voltagesense, ammeter and voltmeter, respectively. They can be used in CCCS.

Please show me a procedure in order to know exactly how to resolve it. Here are the netlist.
Thank you very much


**** 06/04/14 00:21:10 ****** PSpice Lite (October 2012) ****** ID# 10813 ****

 ** Profile: "SCHEMATIC1-Converters"  [ C:\CCCS AveragedBuck\converters-pspicefiles\schematic1\converters.sim ]

 ****     CIRCUIT DESCRIPTION

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

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

*Libraries:
* Profile Libraries :
* Local Libraries :
* From [PSPICE NETLIST] section of C:\Documents and Settings\Administrador\Datos de programa\SPB_16.6\cdssetup\OrCAD_PSpice/16.6.0/P
.lib "nomd.lib"

*Analysis directives:
.TRAN  0 40ms 0 0.0001
.OPTIONS ADVCONV
.PROBE64 V(alias(*)) I(alias(*)) W(alias(*)) D(alias(*)) NOISE(alias(*))
.INC "..\SCHEMATIC1.net"

**** INCLUDING SCHEMATIC1.net ****
* source CONVERTERS
C_C1         N26126 0  50u  TC=0,0
E_E1         N26376 0 POLY(2) N26140 0 N821065 0 0.0 0.0 0.0 0.0 1.0
L_L1         N47845 N26126  25uH 
V_E         N26140 0 10Vdc
X_F1    N26376 N47845 N26140 N26376 SCHEMATIC1_F1
R_R1         N26126 0  1 TC=0,0
R_R26         N821065 0  1 
V_VF2         N821065 0 0.5
R_R27         N822098 0  1 
V_VF3         N822098 0 0.8

.subckt SCHEMATIC1_F1 1 2 3 4 
F_F1         3 4 POLY(3) V_F1_F1 V_VF2_F1 V_VF3_F1
+ 0.0 1.0 1.0 1.0
V_F1_F1         1 2 0V
V_VF2_F1         N821065 0 0V
V_VF3_F1         N822098 0 0V
.ends SCHEMATIC1_F1

**** RESUMING Converters.cir ****
.END

**** 06/04/14 00:21:10 ****** PSpice Lite (October 2012) ****** ID# 10813 ****

 ** Profile: "SCHEMATIC1-Converters"  [ C:\CCCS AveragedBuck\converters-pspicefiles\schematic1\converters.sim ]

 ****     INITIAL TRANSIENT SOLUTION       TEMPERATURE =   27.000 DEG C

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

 NODE   VOLTAGE     NODE   VOLTAGE     NODE   VOLTAGE     NODE   VOLTAGE

(N26126)    5.0000 (N26140)   10.0000 (N26376)    5.0000 (N47845)    5.0000    

(N821065)     .5000                   (N822098)     .8000                      

(X_F1.N821065)    0.0000              (X_F1.N822098)    0.0000             

    VOLTAGE SOURCE CURRENTS
    NAME         CURRENT

    V_E         -5.000E+00
    V_VF2       -5.000E-01
    V_VF3       -8.000E-01
    X_F1.V_F1_F1   5.000E+00
    X_F1.V_VF2_F1   0.000E+00
    X_F1.V_VF3_F1   0.000E+00

    TOTAL POWER DISSIPATION   5.09E+01  WATTS

          JOB CONCLUDED

**** 06/04/14 00:21:10 ****** PSpice Lite (October 2012) ****** ID# 10813 ****

 ** Profile: "SCHEMATIC1-Converters"  [ C:\CCCS AveragedBuck\converters-pspicefiles\schematic1\converters.sim ]

 ****     JOB STATISTICS SUMMARY

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

  Total job time (using Solver 1)   =         .02