PUTDEVMOD(1ICD)

NAME
putdevmod - put a device model description into the circuit database

SYNOPSIS
putdevmod [-e] file

OPTIONS

-e  Make an equivalence between the device and an existing object of viewtype 'layout' that has a similar name.

DESCRIPTION
Putdevmod(1ICD) places a device model description into the circuit database. A device model description contains a description of the name of the device, a description of its terminals and (optionally) some instance-specific information and a description of the parameters of a simulation model for the device (currently only SPICE models are supported). The device model description is used by other programs to detect which cells are network primitives (e.g. by the program that extracts a circuit description out of the database) and/or to collect simulation input.

The input file for putdevmod should at least contain the name of the device and a specification of its terminals. The other information that might be specified in the inputfile for putdevmod is (1) A possible bulk voltage for the device. (2) A prefix that should be used before an instance name of the device when the device is included in a SPICE description. (3) Values 'dw' and 'dl' that specify with which value the width and length of the device as specified in the database should be decreased in order to obtain the width and length that should be used for a SPICE network description. (4) A SPICE model description for the device.

The syntax of the input file for putdevmod is as follows: On the first line the keyword "device" is specified followed by the name of the device. On a next line the keywords "begin" and "spicemod" are specified to denote the beginning of the SPICE device information. The next lines are considered to be SPICE input that can directly be appended to a SPICE network description in order to form the model description of the device. The end of the SPICE model description is denoted by a line that contains the keyword "end". The specification of the terminals of the device, its bulk voltage etc. should be included as comment in the SPICE model description in order to prevent the occurrence of syntax errors when running the SPICE simulator. The terminals of the device are specified by the keyword "terminals" followed - on the same line and separated by spaces and/or tabs - the names of the terminals (The order in which the terminals are specified should agree with the order in which the terminals are required in the SPICE description). The bulk voltage (if appropriate) is specified by the keyword "bulk" followed by a floating point number. The values for dw and dl (if appropriate) are specified by the keywords "dw" and "dl" respectively, followed by a floating point number.

By using putdevmod the user can easily perform extraction of bipolar circuits and other circuits that contain devices that are not common n-mos and p-mos transistors. This is achieved by defining cells in the layout view that have names and terminal names that are identical to the names and terminal names of the corresponding devices that are stored with putdevmod in the circuit view. The layout to circuit extractor space will consider these devices to be leaf-cells whose contents should not be extracted, but that should be included as primitives in the network description instead.

EXAMPLE
An example of an input file for putdevmod is as follows:

device nenh
begin spicemod
* terminals	d g s
* bulk	0
* prefix	m
* dw	0.88e-6
* parameters for n_enhancement NMOS  w/l = 4/4
.model nenh nmos	level=2
+	vto=0.6838  	kp=32u    	gamma=0.2787
+	phi=0.55    	pb=0.84   	cgso=440p
+	cgdo=440p   	cgbo=100p 	rsh=25.3
+	cj=62u      	mj=0.73   	cjsw=340p
+	mjsw =0.20  	js=6.2u   	tox=0.07u
+	xj=0.35u    	ld=0.625u 	uo=650
+	ucrit=143000	uexp=0.154	utra=0
+	xqc=0.5     	fc=0.6          lambda=0.02269
+	vmax=6e4    	nsub=5.71e14
+	delta=5.5
end

Another example is

device npn
begin spicemod
* terminals	c b e
* prefix	q
end

SEE ALSO
xspice(1ICD), User's guide for SPICE.