DESCRIPTION
Ext2spice will convert an extracted circuit from the hierarchical ext(5) representation produced by Magic to a flat spice file which can be accepted by spice2, spice3, hspice and other simulation tools. The root of the tree to be extracted is the file root.ext; it and all the files it references are recursively flattened. The result is a single, flat representation of the circuit that is written to the file root.spice .

The following options are recognized:

-o outfile

Instead of leaving output in the file root.spice, leave it in outfile.

-B

Don't output transistor or node attributes in the spice file. Usually the attributes of a node or a device are output as special comments **fetattr and **nodeatrr which can be processed further to create things such a initial conditions etc.

-F

Don't output nodes that aren't connected to fets (floating nodes). Normally capacitance from these nodes is output with the comment **FLOATING attached on the same line.

-tchar

Trim characters from node names when writing the output file. Char should be either "#" or "!". The option may be used twice if both characters are desired. Trimming "#" and "!" is enabled by default when the format is hspice.

-M|m

Merge parallel fets. -m means conservative merging of fets that have equal widths only (usefull with hspice format multiplier if delta W effects need to be taken care of). -M means aggresive merging: the fets are merged if they have the same terminals and the same length.

-y num

Select the precision for outputing capacitors. The default is 1 which means that the capacitors will be printed to a precision of .1 fF.

-f hspice|spice2|spice3

Select the output format. Spice3 is the the format understood by the latest version of berkeley spice. Node names have the same names as they would in a sim(5) file and no special constructs are used. Spice2 is the format understood by the older version of spice (which usually has better convergence). Node names are numbers and a dictionary of number and corresponding node is output in the end. HSPICE is a format understood by meta-software's hspice and other commercial tools. In this format node names cannot be longer than 15 characters long (blame the fortran code): so if a hierarchical node name is longer it is truncated to something like x1234/name where x1234 is an alias of the normal node hierarchical prefix and name its hierarchical postfix (a dictionary mapping prefixes to real hierarchical paths is output at the end of the spice file). If the node name is still longer than 15 characters long (again blame the fortran code) it is translated to something like z@1234 and the equivalent name is output as a comment. In addition since hspice supports scaling and multipliers so the output dimensions are in lambdas and if parallel fets are merged the hspice construct M is used.

-J hier|flat

Select the source/drain area and perimeter extraction algorithm. If hier is selected then the areas and perimeters are extracted only within each subcell. For each fet in a subcell the area and perimeter of its source and drain within this subcell are output. If two or more fets share a source/drain node then the total area and perimeter will be output in only one of them and the other will have 0. If flat is selected the same rules apply only that the scope of search for area and perimeter is the whole netlist. In general flat (which is the default) will give accurate results (it will take into account shared sources/drains) but hier is provided for backwards compatibility with version 6.4.5. On top of this selection you can individually control how a terminal of a specific fet will be extracted if you put a source/drain attribute. ext:aph makes the extraction for that specific terminal hierarchical and ext:apf makes the extraction flat (see the magic tutorial about attaching attribute labels). Additionaly to ease extraction of bipolar transistors the gate attribute ext:aps forces the output of the substrate area and perimeter for a specific fet (in flat mode only).

-j device:sdRclass[/subRclass]/defaultSubstrate

Gives ext2sim information about the source/drain resistance class of the fet type device. Makes device to have sdRclass source drain resistance class, subRclass substrate (well) resistance class and the node named defaultSubstrate as its default substrate. The defaults are nfet:0/Gnd and pfet:1/6/Vdd which correspond to the MOSIS technology file but things might vary in your site. Ask your local cad administrator.

The way the extraction of node area and perimeter works in magic the total area and perimeter of the source/drain junction is summed up on a single node. That is why all the junction areas and perimeters are summed up on a single node (this should not affect simulation results however).

Special care must be taken when the substrate of a fet is tied to a node other than the default substrate (eg in a bootstraping charge pump). To get the correct substrate info in these cases the fet(s) with separate wells should be in their own separate subcell with ext:aph attributes attached to their sensitive terminals (also all the transistors which share sensistive terminals with these should be in another subcell with the same attributes).

In addition, all of the options of extcheck(1) are accepted.

The awk filter spice2sim is provided with the current distribution for debugging purposes.

SEE ALSO
extcheck(1), ext2spice(1), magic(1), irsim(1), ext(5), sim(5)

AUTHOR
Stefanos Sidiropoulos.

BUGS
The areas and perimeters of fet sources and drains work only with the simple extraction algorith and not with the extresis flow. So you have to model them as linear capacitors (create a special extraction style) if you want to extract parasitic resistances with extresis.