ext2spice, exttospice

Usage:

ext2spice [option]

where option is one of the following:

[run] [runtime_options]

Run ext2spice on current cell, with command-line options (see Summary, below).

default

Reset to default values

format hspice|spice2|spice3

Set output format. spice3 is the default, for compatibility with tclspice. This is a change from previous versions of magic, where the default was hspice.

rthresh [value]

Set resistance threshold value. Lumped resistances below this value will not be written to the output. The value is in ohms, or may be the keyword infinite to prohibit writing any lumped resistances to the output.

cthresh [value]

Set capacitance threshold value. The value is in femtofarads, or may be the keyword infinite to prohibit writing any parasitic capacitances to the output.

merge [merge_option]

Merge parallel devices/transistors. The valid merge options are:

conservative

Merge transistors and capacitors having the same device type and node connections and having the same width and length. Widths are summed in the final output for transistors. Capacitor values are summed in the final output.

aggressive

Merge transistors having the same node connections and having the same length. Widths are summed in the final output. Merge any capacitors having the same device type and node connections. Capacitance is summed in the final output.

none

Do not merge any devices.

extresist on|off

Incorporate output from the command extresist into the final SPICE file.

resistor tee [on|off]

Model resistor capacitance as a T-network. Each resistor device is split into two, with all substrate and overlap capacitance placed on the node between the two half-length devices. Without this option, resistor devices lose all parasitic capacitance information, and ext2spice may produce warnings about unknown nodes. However, use of this option may conflict with LVS (layout-vs.-schematic), when only one resistor is expected per drawn device.

subcircuits [on|off]

When set to on (the default), standard cells become subcircuit calls ("X") in the SPICE output. The contents of the standard cells are not output, and it is assumed that a pre-characterized SPICE deck exists modeling the behavior of each standard cell definition. Standard cells are defined by the use of the port method for labeling input and output ports. When set to off, ports are ignored, and the entire circuit hierarchy is flattened down to the device level.

help

Print help information.

Summary:

Without options, or with the option run, the ext2spice command converts the hierarchical extracted netlist information produced by the extract command in a series of .ext files into a flattened representation in SPICE format, used for detailed analog simulation.

runtime_options may be passed on the command line, and represent the original command-line options passed to the standalone version of ext2spice. A number of the original command-line options have been deprecated in the Tcl-based version, and some are duplicated by other ext2spice options. Valid runtime_options are:

-d

Distribute junction areas and perimeters. The Magic extractor computes area and perimter values per node, not per device. For devices that share a node, Magic cannot distinguish between the devices (for parasitic calculations, it's not necessary to distinguish between the devices). Normally, when generating device output, Magic writes the lumped area and perimeter values along with the first device attached to a node, and sets the area and perimeter values for all remaining devices on that node to zero. The -d option causes Magic to distribute the node area and perimeter evenly among all devices attached to that node.

-B

Don't output transistor or node attributes in the SPICE file. This option will also disable the output of information such as the area and perimeter of source and drain diffusion and the FET substrate.

-F

Don't output nodes that aren't connected to devices (floating nodes).

-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 require trimming.

-y num

Select the precision for outputting capacitors. The default is 1 which means that the capacitors will be printed to a precision of 0.1 fF.

-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 device in a subcell the area and perimeter of its source and drain within this subcell are output. If two or more devices 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 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).

With options, the command sets various parameters affecting the output format and content.

Implementation Notes:

ext2spice is implemented as a separate loadable Tcl package, but one which depends on the presence of the standard "tclmagic" package. magic is set up with a placeholder command for ext2spice, and will automatically load the Tcl package when this command is invoked.

exttospice is an alias for ext2spice, to satisfy the grammatically anal retentive. ext2spice is also implemented as a script to be run from the shell command line, where it executes magic in batch mode (i.e., using the -dnull option) and runs the ext2spice command automatically. With this usage, the syntax is:

ext2spice [ magic_options -- ] ext2spice_runtime_options ext_file

The double-dash separates command options passed to magic on startup (such as "-T technology" to specify the technology) from those runtime options (see above) passed to the ext2spice command.

See Also:

extract
ext2sim

Return to command index

Last updated: January 19, 2009 at 7:50am