Skip site navigation (1)Skip section navigation (2)

FreeBSD Manual Pages


home | help
EXT2SPICE(1)		    General Commands Manual		  EXT2SPICE(1)

       ext2spice - convert hierarchical	ext(5) extracted-circuit files to flat
       spice files

       ext2spice [ -B ]	[ extcheck-options ]  [	 -M|m  ]  [  -y	 num  ]	 [  -f
       hspice|spice3|spice2  ]	[  -J  hier|flat ] [ -j	device:sdRclass[/subR-
       class]/defaultSubstrate ] root

       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

       -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 pro-
		 cessed	further	to create things  such	a  initial  conditions

       -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 mul-
		 tiplier if delta W effects need to  be	 taken	care  of).  -M
		 means	aggressive  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	preci-
		 sion 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 con-
		 structs  are  used.   Spice2  is the format understood	by the
		 older version of spice	 (which	 usually  has  better  conver-
		 gence). 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 hierarchi-
		 cal node name is longer it is	truncated  to  something  like
		 x1234/name where x1234	is an alias of the normal node hierar-
		 chical	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 lamb-
		 das and if parallel fets are merged the hspice	construct M is

       -J hier|flat
		 Select	the source/drain area and perimeter  extraction	 algo-
		 rithm.	 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 back-
		 wards compatibility with version 6.4.5. On top	of this	selec-
		 tion you can individually control how a terminal  of  a  spe-
		 cific	fet will be extracted if you put a source/drain	attri-
		 bute. 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).   Addition-
		 aly to	ease extraction	of bipolar transistors the gate	attri-
		 bute 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) re-
		 sistance class	and the	node named defaultSubstrate as its de-
		 fault	 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	admin-

       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

       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.

       extcheck(1), ext2spice(1), magic(1), rsim(1), ext(5), sim(5)

       Stefanos	Sidiropoulos.

       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.

4th Berkeley Distribution					  EXT2SPICE(1)


Want to link to this manual page? Use this URL:

home | help