Rxxxxxxx

Resistor: This device is translated as a resistor device. For information on the resistor model, refer to [R_Model:Resistor Model].

Example SPICE Command Line:

r1 1 2 1k

SPICE dialect and netlist syntax:

Spice2/3:

rid n1 n2 [value] [mname] [l=l ] [w=w ] [ temp=temp ]

PSpice:

rid n1 n2 [ mname ] value [ tc= tc1 [, tc2 ]]

HSpice:

rid n1 n2 [mname] [r=]value [[tc1=]tc1 [[tc2=]tc2]]
+ [scale=s] [m=mult] [ac=ac] [dtemp=dtemp] [l=l] [w=w] [c=c]

ADS Netlist Syntax:

R:rid n1 n2 R=value [TC1=tc1] [TC2=tc2 ] [_M=mult]

ADS Schematic Symbol:

Instance Parameters:

rid = Resistor element name
mname = Model name. Use this name in elements to reference the model.
n1, n2 = Element nodes
value = Resistance value (in ohms). Reff=R*SCALE/M.
tc1 = First order temperature coefficient for resistor.
tc2 = Second order temperature coefficient for resistor.
scale = Element scale factor for resistance and capacitance. Default=1.0.
mult = Multiplier that simulates parallel resistors. For example, to represent two *parallel instances of a resistor, set M=2 to multiply the number of resistors by 2. Default=1.0.
dtemp = Temperature difference between the element and the circuit. Default=0.0
l = Resistor length. Default=0.0, if L is not specified in the model.
w = Resistor width. Default=0.0, if W is not specified in the model.
SHRINK is a model parameter.
Wscaled=W*SHRINK*SCALE(option)
dw = Width narrowing due to etching in specified units.
dl = Length narrowing due to etching in specified units.

Comments:

If SCALE is specified, Value=Value*scale.

In the netlist, as in ADS, the value of R may be positive or negative but not zero.

HSpice:
If the value of R is an expression which is a function of node voltages or independent variables, then the component is a dependent resistor. In ADS, the component is represented by a Symbolically Defined Device (SDD).

If one of the SDD parameters uses a variable containing node voltages, the translator needs to look up the node voltages on the resultant SDD to convert them to the correct ADS syntax and update the variable expression. For instance, the node voltage described as v(nodeX) in HSpice must be converted to _v1, if the first pair of nodes on the SDD is (node1, 0).

For translation purposes of this special case, the SDD and the variable used by it are expected to be defined in the same subcircuit, with the variable being used by only one SDD. If the variable were defined globally or used by different SDDs, the node voltage variables (_v1, etc.) might not match up correctly. For example, in the case described above one SDD might have (nodeX,0) as the first pair of nodes (_v1), while another SDD might have (nodeX,0) as the 2nd pair of nodes (_v2). The translator would not be able to replace v(nodeX) in the variable expression to define both SDDs correctly at the same time.

If this SDD is not found in the same subcircuit as the variable expression, a warning message will be written to the log file nettrans.log. Also, the expression will not be converted automatically, and it will have to be fixed manually before simulation is attempted.

If dtemp is provided, Temp=temp+dtemp

The Netlist Translator fails to recognize the resistor model in the following syntax:

r1 1 2 rmodel

The translator assumes that it is a variable name for the resistor value. To correct your imported schematic, manually move the model name to the parameter Model. To correct the ADS Netlist, use the following netlist syntax:

rmodel:r1 1 2 [param=value]*