In a nut shell, my question is: what setting must be specified in order to use a voltage probe statement such as v(n1,n2) in a bsource parameter expression. for example, consider the netlist statement ...

R6 (vdd! net019) bsource r=v(26)*1000

is this statement enough to render component R6 a behavioral resistor whose resistance is a function of the voltage on net26 ??

It seems not to be because when i use it the v(X) statement consistently evaluates to zero.

I am using Virtuoso schematic editor spectre simulator IC5141 .. In the Spectre.out log file i see statements such as

Installed compiled interface for bsource_2
opening directory input.ahdlSimDB/bsource_1.input.ahdlcmi

Circuit inventory
              bsource_1 2
              bsource_2 1

so it seems that the bsource statement is being evaluated as a behavioral component but my probe statements are being ignored. Is there some setting that I am neglecting to specify before I use probe statement in component parameter expressions ... ?? Any suggestion would be helpful, Thank you .

Thanks a lot for your response - The thing is, that was the whole point of using bsource, because looking around this forum I have ran into multiple post where a voltage probe such as v(n1,n2) has been used in an expression passed onto a bsource parameter (r, c, i, v).

I know I cant use variable-containing expressions directly in a CDF Parameter. Such components need to be coded in Verilog A. However according to Andrew B, "bsource" was introduced into Cadence Spectre IC5033 and this enables the direct passing of simple expression (that may be a function a node signal) to parameters of components defined as a "bsource".

I am using IC5141 release which has "bsource" capability .. so it must be that I am not using it properly , I think ....  Or am I wrong in thinking that an expression (that is a function of a simulation signal) can be passed to a component parameter in general, "bsource" or not ...?

Wow ... Had almost given up on this .. i think it is working now . That is very exciting as I was completely stuck and unwilling to move past it, so now i can finally move on with my life .. Thanks*1M

Here is what I did .. following up on Geoffrey suggestion I changed the Subckt code as such

subckt b_r (PLUS MINUS CTRL)
Parameter r = 10
R1(PLUS MINUS) bsource r=r*v(CTRL)
ends b_r

If I use V(CTRL) I get an error during hierarchy flattening :"instance name.R1: parameter 'bs_par_1': Unknown parameter name 'CTRL' found in expression

I suppose bs_par_1 is short for behavioral source parameter 1

However if i use v(CTRL) which is the voltage probe notation the CTRL parameter is recognized and I get no error.

Then I have to add the new node, from the modified subckt code, (namely the 'CTRL') to the termOrder in CDF Simulation Information of my subcircuit symbol. termOrder: PLUS MINUS CTRL

Furthermore I have modify the subcircuit symbol itself by adding an extra port to it - Port Object Properties: Name=CTRL Direction=inputOutput  (I'm sure Direction=Input will also work)

Finally I have to connect the extra port that is now appearing on my b_r symbol component(sticking out of the side of the rectangular symbol shape) in my schematic to the node on which CDF parameter value depends on.

For example:
for my behavioral resistor I want  : r = 1K*v(26)

right click on the subcircuit symbol (b_r, as named above) and enter 1K for the CDF parameter r. Then connect the CTRL port of the symbol to net026 and simulate. Apparently there is no need to add the vprobe notation in the CDF parameter field as it is added in the subckt bsource statement : R1 bsource r = r*v(CTRL). In the CDF parameter field just add the r value which should be a constant part of the expression.  

some of the steps might be redundant but, judging by a cursory observation of the results I think it works.

I am very grateful for your guidance on this Geoffrey.