


spice_raw(5)             spice raw format            spice_raw(5)


NAME
       spice_raw  -  ascii  file  is  outputed  by Spice to store
       results of simulation.


DESCRIPTION
       here is the example of file with comments in angle  brack-
       ets <...> :

       Title:  Circuit 1 <the circuit name>
       Date: Thu May 25 12:29:22  2000 <the date is here>
       Plotname: Transient Analysis <or other analysis>
       Flags: real <may be complex>
       No. Variables: 7 <the number of variables>
       No.  Points:  53505  <the  number of points - time or fre-
       quency>
       Command: version 3f5
       Variables:
       <varables follow:, name and type>
            0    time time
            1    V(3) voltage
            2    V(1) voltage
            3    V(2) voltage
            4    V(4) voltage
            5    lbranch current
            6    vbranch current
       Values:
       <values follow in groups. Each group represents one point.
       Group  is  started with integer - number of point.  Values
       follow: values in a group correspond to variables in  sec-
       tion Variables: . If variable is of COMPLEX type, then two
       comma separated values per line should be. >
       0         1.000006870302956e+01
            4.183917045036226e-01
            2.081480481818476e-01
            -1.058725840837939e-05
            2.080585895060827e-01
            2.099491815491466e-03
            -2.102436563217750e-03
       1         1.000016870302956e+01
            8.723517652443397e-01
            2.376136217706665e-01
            4.416169358174814e-04
            2.373435406906185e-01
            2.099563653771034e-03
            -6.347381434736731e-03
        ...
       53504          1.500000000000000e+01
            -3.673819061467132e-12
            2.003686205994584e-03
            -2.202131617294144e-03
            2.004538774476798e-03
            2.088272248371801e-03
            2.003686209668403e-05



Habala                     02-Aug-2000                          1





spice_raw(5)             spice raw format            spice_raw(5)


SPICE VARIABLES
       Names of variables in section "Variables" (see above)  are
       named  in accordance with some scheme.  On my (GS) mind it
       is the following:

              Spice variables naming scheme
              * for simply numbered nodes ( 1, 2, etc) node volt-
              age variables are V(1), V(2), V(3);
              * For named nodes ("in", "out", "feed", etc.)  node
              voltage variables are "in", "out", "feed";
              * for subcircuit "xsub1" node voltage variables are
              sub1:1, sub1:2, sub1:in;
              *  for  subcircuit "xfilter1" in subcircuit "xsub1"
              node  voltage   variables   are   "sub1:filter1:1",
              "sub1:filter1:2", "sub1:filter1:in";
              *  but  if subcircuit named as x1 or x2, then vari-
              ables are: V(1:1), V(1:2), V(1:in), V(1:sub1:in);
              * if subcircuit named as x1f or  x23cmp,  variablev
              will be: V(1f:1), V(1f:2), V(1f:in) or V(23cmp:fil-
              ter1:in).
              Summary:
              <full_name>  =  <firts_level_subcircuit_name>:<sec-
              ond_level>:<third>:<...>:<variable_number_or_name>.
              To <full_name> like "1",  "1:1",  "2v2:3:86:spiral"
              (if  full_name  starts  with digit) add "V(" before
              name  and ")" after.


SEE ALSO
       spice(1)


COMPOSED
       Composed by Gennady Serdyuk, gserdyuk@mail.ru























Habala                     02-Aug-2000                          2


