**From:** abe riazi (*ariazi@serverworks.com*)

**Date:** Mon Apr 02 2001 - 10:55:28 PDT

**Next message:**Mike Hughes: "Re: [SI-LIST] : Jitter Measurement"**Previous message:**Khalid Ansari: "[SI-LIST] : Jitter Measurement"**Maybe in reply to:**abe riazi: "[SI-LIST] : Diode Modeling"

Joel:

Thanks for your response.

I was also informed today that new versions of XTK (for both UNIX and Windows NT platforms) to be released later this month include QSPICE simulation capabilities.

I look forward to utilizing it.

Abe

-----Original Message-----

From: Joel Amzallag [SMTP:amzallag@cisco.com]

Sent: Monday, April 02, 2001 9:37 AM

To: ARiazi

Cc: si-list@silab.eng.sun.com

Subject: Re: [SI-LIST] : Diode Modeling

Abe,

The latest version of XTK include a Spice simulator. If you want to avoid

all these translating steps, you could use the Spice models directly within

XTK but it will slow down the simulation speed.

Regards,

-Joel.

At 11:37 AM 3/31/2001 -0800, ARiazi wrote:

*>Dear All:
*

*>
*

*>In my recent post, the third paragraph includes:
*

*>
*

*>"IBIS specs [Reference 1] require for the [POWER Clamp] data to be Vcc
*

*>relative, as illustrated by Figure 3 which is a plot of current through D2
*

*>versus Vcc-Vx. A comparison of Figures 2 and 3 reveals a shift of I(D2) from
*

*>the first to the second Cartesian quadrant."
*

*>
*

*>D2 should have been D1.
*

*>
*

*>Also the I-V table of XTK diode example includes typographical error. The
*

*>POINTS should be replaced by POINT as corrected below:
*

*>
*

*>#Schottky diode to 5.0 Volts
*

*>LOADSPEC FAST_SCHOTTKY5
*

*>CEFF: 0
*

*>V-I: 5 POINTS
*

*># Voltage given in Volts, Current in mA
*

*>POINT V: 0 I: 0
*

*>POINT V: 5.0 I: 0.0
*

*>POINT V: 5.5 I: 3.0
*

*>POINT V: 5.6 I: 5.0
*

*>POINT V: 5.75 I: 30.0
*

*>#End of Model
*

*>
*

*>Best Regards,
*

*>
*

*>Abe
*

*>
*

*>
*

*>----- Original Message -----
*

*>From: abe riazi <ariazi@serverworks.com>
*

*>To: <si-list@silab.eng.sun.com>
*

*>Sent: Friday, March 30, 2001 7:35 PM
*

*>Subject: [SI-LIST] : Diode Modeling
*

*>
*

*>
*

*>Dear Scholars:
*

*>
*

*>The diode's PN junction and the base-emitter (or base-collector) junctions
*

*>of bipolar transistors are governed by similar physical laws. Subsequently,
*

*>diode model having numerous applications is regarded as fundamental to
*

*>models of other semiconductor devices. Several stages of creating IBIS,
*

*>SPICE and XTK diode models are described by this message.
*

*>
*

*>IBIS model of a diode can be generated via simulation or measurements.
*

*>Figure 1 is schematic for generating behavioral model of 1N4002 rectifier
*

*>diode by way of simulation. Using PSPICE program, DC sweep was carried out
*

*>from -15 to +15V to cover the (-Vcc to 2Vcc) voltage range recommended by
*

*>IBIS specs.
*

*>
*

*>Figure 2 presents simulation results for diode currents I(D1) and I(D2) as
*

*>function of applied voltage. When generating I-V (or V-T) curves for an
*

*>IBIS datasheet, higher accuracy is achievable by sampling more data points
*

*>in the non-linear regions (such as knee areas ) of the curve as opposed to
*

*>more linear sections . IBIS specs [Reference 1] require for the [POWER
*

*>Clamp] data to be Vcc relative, as illustrated by Figure 3 which is a plot
*

*>of current through D2 versus Vcc-Vx. A comparison of Figures 2 and 3 reveals
*

*>a shift of I(D2) from the first to the second Cartesian quadrant.
*

*>
*

*>A diode IBIS model can be produced by extracting the [POWER Clamp] table
*

*>from I(D1) vs. (Vcc-Vx) of Figure 3, the [GND Clamp] data from I(D2) Vs. Vx
*

*>of Figure 2, incorporating package/pin parasitic values, and inserting the
*

*>necessary keywords [Reference 1] such as [IBIS Ver], [File Name], [File
*

*>Rev], [Component], [Manufacturer], etc.
*

*>
*

*>Regarding procedure for creating SPICE diode macromodels, the major steps
*

*>[Reference 2] include: (i) Inspecting device data sheet for useable
*

*>modeling information. (such as, plots of forward diode current vs. voltage,
*

*>junction capacitance vs. diode voltage, etc.), (ii) conducting I-V and C-V
*

*>measurements to extract remaining parameter values, and (iii) performing
*

*>simulations to optimize model parameters.
*

*>
*

*>The SPICE diode macromodel can contain fourteen parameters: IS (Reverse
*

*>leakage current), RS (Diode series resistance), N (Emission coefficient), BV
*

*>(diode breakdown voltage), IBV (Diode breakdown current), CJO (Zero-bias
*

*>junction capacitance), VJ (Bulk junction potential), FC (Coefficient for
*

*>capacitance), M (Grading coefficient), TT (transit time), EG (Energy
*

*>band-gap), XTI (Temperature coefficient), KF (Flicker-noise coefficient),
*

*>and AF (Flicker-noise exponent)). Each of above parameters has a default
*

*>value assigned by SPICE program; however, it is frequently possible (based
*

*>on application) to produce a sufficiently accurate diode model using just a
*

*>subset of the 14 parameters. For instance, parameters KF, AF, EG and XT1 are
*

*>needed only for AC noise analyses and temperature sweeps; hence, unnecessary
*

*>if the diode model is intended for other types of simulations. As another
*

*>example, SPICE model of a 1N4002 diode suitable for numerous applications
*

*>[Reference 2] includes:
*

*>
*

*>IS = 46.5Pa, RS=123MohmS, N=1.35, CJO=51.5pF, M=0.333, VJ=0.381, FC=0.5,
*

*>TT=5.77uS.
*

*>(with remaining parameters at default values).
*

*>
*

*>It should be added that SPICE model parameters are scalar variables of diode
*

*>equation:
*

*>
*

*>Id = IS * [exp(qVd/Nkt) - 1]
*

*>
*

*>Where Id is diode DC current, q is electron charge, Vd is voltage across
*

*>diode, K is Boltzmann's constant, and t is the diode temperature in degrees
*

*>Kelvin ( IS and N as defined earlier).
*

*>Different forms of above equation exist (some being approximations) for
*

*>describing three regions of diode operation namely: forward conduction,
*

*>reverse conduction before breakdown, and reverse-bias breakdown .
*

*>
*

*>SPICE or IBIS models can not be directly utilized by some simulators. For
*

*>instance, XTK requires that models be in Quad format. A Quad diode model
*

*>can be created from the IBIS version using IBIS2XTK, or written manually.
*

*>A sample is presented:
*

*>
*

*>#Schottky diode to 5.0 Volts
*

*>LOADSPEC FAST_SCHOTTKY5
*

*>CEFF: 0
*

*>V-I: 5 POINTS
*

*># Voltage given in Volts, Current in mA
*

*>POINTS V: 0 I:0
*

*>POINTS V: 5.0 I:0.0
*

*>POINTS V: 5.5 I:3.0
*

*>POINTS V: 5.6 I: 5.0
*

*>POINTS V: 5.75 I: 30.0
*

*>#End of Model
*

*>
*

*>The above discussed models have contained data limited to only one
*

*>simulation corner, whereas a more complete model demands data for three
*

*>(i.e. MIN, TYP and MAX) corners. Simulations results based on TYP models
*

*>are often well suited for purpose of correlation with physical measured
*

*>data. However, Fast and Slow corner runs are also frequently necessary to
*

*>verify a design under all conditions.
*

*>
*

*>A finished model also needs a package/pin parasitic section. Nevertheless,
*

*>a model may lack parasitic portion mainly due to two reasons: (1) the model
*

*>developer leaves it to the user to ascertain what package type and parasitic
*

*>values are applicable, and (2) The model is intended for use at low
*

*>frequencies where parasitics have negligible effects.
*

*>
*

*>In conclusion, several phases of generating IBIS and SPICE diode models were
*

*>explained. A XTK model was also exemplified to emphasize that some
*

*>simulators do not directly employ IBIS or SPICE models and demand
*

*>translation to simulator's native model format. One logical order for diode
*

*>modeling consists of first creating SPICE diode via measurements, then IBIS
*

*>model by means of simulation and finally the Quad version using IBIS2XTK.
*

*>
*

*>REFERNCES:
*

*>1. IBIS (I/O Buffer Information Specification) Version 3.2, August 1999.
*

*>2. R. Kielkowski, "SPICE Practical Device Modeling", McGraw-Hill, Inc. 1995.
*

*>
*

*>Your response is highly appreciated.
*

*>
*

*>Respectfully,
*

*>
*

*>Abe Riazi
*

*>ServerWorks
*

*>2251 Lawson Lane
*

*>Santa Clara, CA 95054
*

*>
*

*>
*

*>
*

*>
*

*>
*

*>**** To unsubscribe from si-list or si-list-digest: send e-mail to
*

*>majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
*

*>si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
*

*>si-list archives are accessible at http://www.qsl.net/wb6tpu
*

*>****
*

**** To unsubscribe from si-list or si-list-digest: send e-mail to

majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE

si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.

si-list archives are accessible at http://www.qsl.net/wb6tpu

****

**** To unsubscribe from si-list or si-list-digest: send e-mail to

majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE

si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.

si-list archives are accessible at http://www.qsl.net/wb6tpu

****

**Next message:**Mike Hughes: "Re: [SI-LIST] : Jitter Measurement"**Previous message:**Khalid Ansari: "[SI-LIST] : Jitter Measurement"**Maybe in reply to:**abe riazi: "[SI-LIST] : Diode Modeling"

*
This archive was generated by hypermail 2b29
: Thu Jun 21 2001 - 10:11:24 PDT
*