F_CCC_POLYPolynomial current controlled current source, like SPICE2 
This information is part of the Modelica Standard Library maintained by the Modelica Association.
The polynomial source is a SPICE2 model, which is also known in other SPICE derivatives.
Nonlinear current controlled current source. The "right" port current at pin p2 (=p2.i) is controlled by the "left" port vector of currents at pin pc[:] via
p2.i = f(pc[2].i, pc[4].i,...)
The controlling port (left) voltage is zero for each pair: pc[2].v  pc[1].v = 0, ...
Furthermore the currents of each pair are pc[2].i + pc[1].i = 0, ...
f is a polynomial in N variables s1...sN of the following form with M+1 coefficients a0, a1, a2,...aM.
f = a0 + a1s1 + a2s2 + ... + aNsN + a(N+1)s1² + a(N+2)s1s2 + ... + a(.)s1sN + a(.)s2² + a(.)s2s3 + ... + a(.)s2sN + a(.)s3² + s3s4 + ... + a(.)s4sN + ... + a(.)sN² + a(.)s1³ + a(.)s1²s2 + a(.)s1²s3 + ... + a(.)s1²sN + a(.)s1s2² + a(.)s1s2s3 + ... + a(.)s1s2sN + ... + a(.)sN³ + ...
The Coefficients a(.) are counted in this order. Reaching M, the particular sum is canceled.
In Modelica the controlling pins have to be connected to the CCC in that way, that the required currents flow through the according pins of the CCC:
s1=pc[2].i, s2=pc[4].i, s3=pc[6].i,...
The pairs pc[1].i and pc[2].i, pc[3].i and pc[4].i...form ports with pc[2].i + pc[1].i = 0, pc[4].i + pc[3].i = 0, ...
The corresponding SPICE description of the CCC polynomial source is the following:
Fname A1 A2 POLY(N) V1...VN P0 P1...
where Fname is the name of the instance, A1 and A2 are the nodes between them the current source is arranged, whose current is calculated.
N is the number of the controlling currents, V1...VN are the voltage sources, that are necessary in SPICE to supply the controlling currents,
and P0, P1... are the coefficients that are called a0, a1, ... aM in the description of the polynomial f above.
To describe the SPICE line in Modelica, the following explanation would be useful:
Fname > F_CCC_POLY name A1, A2 > pins name.p2, name.p1 N > parameter N
V1 (...VN) is declared in SPICE:
V1 V1+ V1 type of voltage source (constant, pulse, sin...)
In Modelica the currents through V1...VN has to be led through the CCC. Therefore V1...VN have to be disconnected and additional nodes
V1_AD...VN_AD
have to be added. In the case, that the SPICE source is
V1 n+ n 0,
this source can be eliminated.
V1_AD > name.pc[2] V1 > name.pc[1] ... VN_AD > name.pc[N] VN > name.pc[N1] P0, P1 > polynomial coefficients name.coeff(coeff={P0,P1,...})
N 
Value: 1 Type: Integer Description: Number of controlling voltages 

coeff 
Value: {1} Type: Real[:] Description: Coefficients of polynomial 
p 
Type: PositivePin Description: Positive pin of the right port (potential p2.v > n2.v for positive voltage drop v2) 


n 
Type: NegativePin Description: Negative pin of the right port 

pc 
Type: PositivePin[2 * N] Description: Pin vector of controlling pins 