Electronics II: SPICE Lab ECE 09.403/503 Team Size: 2-3 Electronics II Lab Date: 3/9/2017 Lab Created by: Chris Frederickson, Adam Fifth, and Russell Trafford Introduction SPICE (Simulation Program for Integrated Circuits Emphasis) was developed at the Electronics Research Laboratory of the University of California, Berkeley by Laurence Nagel with direction from his research advisor, Prof. Donald Pederson. SPICE1 was largely a derivative of the CANCER program, [1] which Nagel had worked on under Prof. Ronald Rohrer. At these times many circuit simulators were developed under the United States Department of Defense contracts that required the capability to evaluate the radiation hardness of a circuit. When Nagel s original advisor, Prof. Rohrer, left Berkeley, Prof. Pederson became his advisor. Pederson insisted that CANCER, a proprietary program, be rewritten enough that restrictions could be removed and the program could be put in the public domain. SPICE1 was first presented at a conference in 1973. SPICE1 was coded in FORTRAN and used nodal analysis to construct the circuit equations. Nodal analysis has limitations in representing inductors, floating voltage sources and the various forms of controlled sources. SPICE1 had relatively few circuit elements available and used a fixed-timestep transient analysis. The real popularity of SPICE started with SPICE2 in 1975. SPICE2 included many semiconductor device compact models: three levels of MOSFET model, a combined EbersMoll and Gummel-Poon bipolar model, a JFET model, and a model for a junction diode. In addition, it had many other elements: resistors, capacitors, inductors (including coupling), independent voltage and current sources, ideal transmission lines, active components and voltage and current controlled sources. SPICE3 added more sophisticated MOSFET models, which were required due to advances in semiconductor technology. In particular, the BSIM (Berkeley Short-channel IGFET Model) family of models were added, which were also developed at UC Berkeley. Commercial and industrial SPICE simulators have added many other device models as technology advanced and earlier models became inadequate. To attempt standardization of these models so that a set of model parameters may be used in different simulators, an industry working group was formed, the Compact Model Council, to choose, maintain and promote the use of standard models. The most common SPICE models being used are: SPICE3, the latest Berkeley offering. It has the advantage of being freely available, to support a wide variety of models, and to run on all UNIX platforms. HSPICE (from Avant!) offers a more robust, commercial version of SPICE. PSPICE is a popular version of SPICE, available from Orcad (now Cadence). AIM-spice is a pc-version of SPICE with a revised user interface, simulation control, and with extra models. 1
IV Curves Finding the MOSFET Characteristic Curve What use is a model if it does not actually behave like a real world device? You will be generating the MOSFET Family of Curves using just a power supply, DMM, and your bare hands. We will save you the literal hours of headache by giving you the correct datasheet, since there are many iterations of the 2N7000 N-Channel MOSFET. http://www.mouser.com/ds/2/149/2n7002-8405.pdf The characteristic curve is found by biasing a MOSFET to a specific Gate to source voltage, then comparing the drain current as you increase, as seen below. In case you were not tortured enough by it in Electronics I, the family of curves represents the relationship between these two quantities at multiple Gate-to-Source voltages. This can provide you great insight into the device parameters, mainly the transconductance. In terms of SPICE Modeling, we need to actually visit the model twice when dealing with circuits which are heavily dependant on the internal properties of a device. First, the initial design needs to be made such that none of the maximum parameters are not exceeded during normal operation as well as to go into the lab expecting your results. After you find the characteristics, it is normally good practice to come back to your simulation and tweak the different parameters to get closer to real world performance. One of the take-aways from this lab should be the impact of certain parameters in your simulation and what you as the designer should care about when choosing devices. PSPICE Commands PSPICE commands and syntax are organized by type, (C for Capacitor, D for Diode, M for MOSFET, etc...). For each model there are specific definitions that are required in order to run. You can find a summary of the commands available in PSICE here: http://algos.inescid.pt/ac06/downloads/labs/pspice.pdf M - MOSFET Format The following is the basic syntax for a MOSFET model: 2
name means required in definition {name} means optional in definition [a,b,c] means choice of a,b, or c in definition. (name) means parentheses required in definition... means multiple declarations of the same format General Format: M defines a MOSFET transistor. The MOSFET is modeled as an intrinsic MOSFET with Ohmic resistances in series with the drain, source, gate, and substrate(bulk). There is also a shunt resistor (RDS) in parallel with the drain-source channel. Positive current is defined to flow into each terminal. L and W are the channel s length and width. L is decreased by 2*LD and W is decreased by 2*WD to get the effective channel length and width. L and W can be defined in the device statement, in the model, or in.option command. The device statement has precedence over the model which has precedence over the.options. AD and AS are the drain and source diffusion areas. PD and PS are the drain and source diffusion parameters. The drain-bulk and source-bulk saturation currents can be specified by JS (which in turn is multiplied by AD and AS) or by IS (an absolute value). The zero-bias depletion capacitances can be specified by CJ, which is multiplied by AD and AS, and by CJSW, which is multiplied by PD and PS, or by CBD and CBS, which are absolute values. NRD, NRS, NRG, and NRB are reactive resistivities of their respective terminals in squares. These parasitics can be specified either by RSH (which in turn is multiplied by NRD, NRS, NRG, and NRB) or by absolute resistances RD, RG, RS, and RB. Defaults for L, W, AD, and AS may be set using the.options command. If.OPTIONS is not used their default values are 100u, 100u, 0, and 0 respectively. Examples: M1 1 2 3 0 MNMOS L=3u W=1u defines a MOSFET with drain node 1, gate node 2, source node 3, substrate node 0, channel length and width 3u and 1u respectively, and described further by model MNMOS (which is assumed to exist in the.model statements) M2 4 5 6 0 MNMOS defines a MOSFET with drain node 4, gate node 5, source node 6, substrate node 0, and described further by model MNMOS (which is assumed to exist in the.model statements) 3
SPICE Download the PSPICE Model In this section, we will construct the circuit from earlier using TINA-TI and investigate the impact of varying parameters of the manufacturers spice model. Download Fairchild Semiconductors PSPICE model for the 2N7000 MOSFET from the following link: https://www.fairchildsemi.com/products/discretes/fets/mosfets/2n7000.html# models Two versions of the SPICE model are given. The Thermal;Electrical model contains a subcircuit for the electrical simulation and a subcircuit for the thermal subcircuit that takes into account the device heating up. The Electrical model contains one subcircuit that models the MOSFET at a given input temperature. Download the Thermal;Electrical model. Inspect the Model File Take a look at the model file in a text editor.comment on the structure of the file. What resistances and capacitances are taken into account? What MOSFET model level is used? Import the Model TINA-TI supports using PSPICE models and new parts can be created from their corresponding PSPICE model. In this section, we will create a part for the 2N7000 MOSFET. In TINA-TI, select Tools New Macro Wizard.... Set the macro name to 2N7000. Select the source of the macro as the.lib PSPICE model downloaded from the manufacturer. Click next. Two subcircuits will be found in the file: the electrical subcircuit and the thermal subcircuit. Select the electrical subcircuit: F2N7000. Click next. We will use the NMOS shape from the library. Select load shape from library. Deselect show suggested shapes only. Do a search for NMOSE and select the NMOSE shape. Click next. The PSPICE model subcircuit contains three terminals: 20 - Drain 10 - Gate 30 - Source Drag the unconnected terminals to the pins on the shape. Click next. Save the created model and insert it into the schematic. 4
Construct the Circuit Construct the circuit from earlier. Apply a voltage source of 4 V to the NMOS gate with a label VGS. Apply a voltage generator and current meter to the drain of the NMOS with labels VDS and AD respectively. Set the voltage generator so that it outputs a sinusoid with that varies between 0 V and 10 V with a frequency of 50 Hz. Basic IV Curve Select Analysis Transient.... Start the transient analysis at 0 seconds and end at 50 milliseconds or 50m. Click OK. A plot will appear that shows the voltage VDS and current ID. In the window, select Edit Post-processor.... Click More >>. Select XY Plot. In Line Edit - X Part write VDS(t) to plot the drain to source voltage. In Line Edit - Y Part write ID(t) to plot the drain current. Click Preview to show the IV curve. Comment on the expected values? Based on the plot of these IV Curves, what currents should you be expecting when you build and test the circuit? Physical Circuit Setting Up Your Lab Bench There needs to be a few considerations before you begin powering these MOSFETs. First, you need to realize that you will be taking current measurements, introducing an easy way to break a piece of equipment. You need to read the manual on your DMM to see the current limits for its current measurements. The easiest way to ensure that you do not blow any fuses or explode a handful of MOSFETs is to liberally apply a heaping helping of current limits. Take a few minutes to run a basic simulation of the testing circuit to see roughly what currents you should be expecting at the gate as well as the drain. Compare this to the graphs given in the Datasheet to your results when using the generic models and the manufacturer given models. When setting up your power supplies, you should set your current limits to around what you expect so that you do not destroy your device or your instrumentation. It would be in your best interest to set up your voltages and currents while setting your limits and with the output off. Start out your experimentation with the lowest recorded V gs on the datasheet, and a V ds of around 0.5V. Running The Experiment If by this point you have not looked at the datasheet, we are going to put the link again so you can do it now: http://www.mouser.com/ds/2/149/2n7002-8405.pdf. You need to take a very close at the maximum output characteristics and realize that you will most likely push the limits on this device. Sustained operation above these points will damage the device and could cause it to fail. However, if you pulse the device with these relatively large voltages and currents, you can minimize the impact of the device. For each of the Vgs provided in the Datasheet, sweep Vgs from 0V up to around 5V in ample increments. When taking voltage and current measurements, it is highly recommended to utilize the Single Acquisition mode on the DMM. In this way, you can turn on the power, 5
take a measurement, and immediately turn off the power supply. Plot these points in your favorite program and compare them to the datasheet and the simulation. What is different? Why do you think there would be a difference? Do your testing conditions match that of the manufacturers? Would these differences make that much of an impact (*cough cough* check SPICE *cough cough*)? SPICE Parameters Temperature Sweep In low earth orbit, a satellite will be subjected to temperature swings between roughly -65 C to 125 C. It is important to understand how temperature will affect the electronics on the satellite. In this section, we will subject the MOSFET to varying temperatures and observe the impact on the IV curve. Select Analysis Mode.... Set the current mode to Temperature stepping with a start temperature of -65 and end temperature of 125 with 5 cases. Run the transient analysis. An error may appear as the post-processor is not configured properly. In the post-processor, five new curves will be available, ID[1] - ID[5]. These correspond to the MOSFET running at varying temperatures. Change the Y axis to plot each curve. What is the impact of changing the device temperature? Is this trend in line with what the datasheet says? MOSFET Model Level The SPICE MOSFET models levels 1-3 use the same model parameters and therefore the model can be changed between these levels by simply changing the level parameter. Right click on the part in your circuit and select Enter Macro. The PSPICE model will appear. Change the MOSFET model level between 1-3. In order to change the back to the schematic view, select the first named tab in the bottom left corner of the screen. Plot the IV curves for VGS = 4V and comment on the impact of changing the model. Vary Model Parameters The PSPICE model contains a number of resistances. Vary the resistance values in the model. Which resistances is the model sensitive to changes in? What is the impact of changing a particular resistance value on the IV curve? References [1] Nagel, L. W. & Rohrer, R. A. (August 1971). Computer Analysis of Nonlinear Circuits, Excluding Radiation. IEEE Journal of Solid State Circuits. SC6: 166182 6