ELEC3106 Electronics. Lab 4: EMI simulations with SPICE. Objective. Material. Simulations

Transcription

1 ELEC3106 Electronics Lab 4: EMI simulations with SPICE Objective The objective of this laboratory session is to give the students a good understanding of the possibilities a circuit simulator (as SPICE) offer for modelling electrical phenomena; in particular in relation to power-supply related EMI. Readily available SPICE component models often do not model all the electrical properties that are relevant for good circuit performance; however used correctly, SPICE can be a very powerful tool to model any circuit phenomena of relevance. These notes include a very brief step-by-step guide to running LTSpice; students are strongly encouraged to obtain their own copy of LTSPice and play around with circuit simulation in their own time. LTSpice is available for free from Linear Technology s website; it runs under Windows or Linux (using Wine). It is assumed for this laboratory session that the student is proficient in the use of Windows based PCs. Material For this laboratory exercise, you will need 1 PC with LTSpice installed lab-book Simulations Carry out the simulations in this section during your laboratory session in pairs of two students. Make sure that you show your result to the laboratory demonstrator, and that both of you record everything neatly in your lab-book. A diode-like element LTSpice has a good built-in voltage controlled switch, see Figure 1(a) which can have either hysteresis of a smooth transition between on- and off-states. This is a very useful component for analysis in the absence of suitable diode parameters, for instance, the switch can be used to model a diode-like element. To start LTSpice under Windows, simply choose LTSpice in the Start menu. Build the schematic shown in Figure 1(b) to simulate the model of the diode-like element implemented with a switch: In the LTSpice main menu, choose Edit - Component, find sw in the dialog box, click OK and place the element (i.e. the switch) on your schematic; this should be labelled S1. Right-click on the switch to change its attribute alue to this is the name of TL/lab4/May 16, 2016 ELEC3106/lab4 p. 1/5 School of Electrical Engineering and Telecommunication

2 the switch model the simulator use. To specify the switch model, choose Edit - SPICE Directive, enter.model SW(RON=1 ROFF=1e6 T=0.6 H= 0.1) in the dialog box, click OK and place the text anywhere convenient on your schematic. Remember the. in.model. Now place the DC voltage source 1 on the schematic by choosing Edit - Component in the menu, select voltage in the dialog blox, click OK and place the element on your schematic; right-click on the voltage source and change its DC value to 1. Also remember a ground in the schematic by choosing Edit - Place GND and place it on your schematic. Your schematic should now start to resemble Figure 1(b). To wire up your schematic, choose Edit - Draw Wire and make the required connections. To simulate the I/ characteristic of the diode-like element, set up a DC simulation: in the menu choose Simulate - Edit Simulation Cmd, click on the DC sweep tab and choose as the 1st Source to sweep 1 from 0 to 1 with an increment of 0.01 and place the command text anywhere convenient on your schematic. 1 Now, save 2 your schematic, and choose in the menu Simulate - Run to simulate the element; a window should pop up ready to show currents and voltages as function of the (independent) sweep variable, 1. To plot a node voltage, simply click on the node in the schematic; to plot a device current, click on the device (devices with more than two pins may have multiple currents associated with them click on the device near a pin to plot the current flowing into that pin). You can zoom in on the displayed waveform, place cursors on waveforms, and do all sorts of helpful things in the waveform display window (for more advanced waveform processing, you can export the waveform data and read them into Matlab or Python). Comment on the simulation result; will this work as a diode? How can you change its forward voltage? Make sure that you print the schematic for your report (choose File - Print... in the menu when the schematic sub-window is selected) as well as the simulation waveform (choose File - Print... when the simulation subwindow is selected)..model SW(RON=1 ROFF=1e6 T=0.6 H= 0.1) i S R OFF v S i S H 1 v C v S R ON T v C (a) 1 I S1.dc (b) Figure 1: LTSpice switch model (a). Diode simulation using switch; simulation setup (b). Modelling a nand gate A 74LS00 TTL nand gate can be modelled using switches and a resistor as shown in Figure 2(a). S1, S2, S4 and S5 are the diode-like elements from above, while S3 and S6 use different models 1 Remember that SPICE uses SI units; the units may be entered after the value, but is ignored; unit pre-fixed may be used but are case insensitive (usual gotcha: M means milli-; MEG means mega-; U means micro-). For example, 5µF could be entered as: 50e-7, 5u, 5UF, or 5uXQW. 2 Spice uses spaces and other exotic characters as part of its syntax structure for this reason such characters should never be used in names, including filenames restrict names to alphanumeric characters (including underscores). ELEC3106/lab4 p. 2/5

3 as shown on the figure. Using the 74LS00 data-sheet, find, and enter, suitable values for R1 and the RON model parameters for S3 and S6. Explain how the model works, and build the circuit in the schematic editor. To functionally test the model, embed the nand gate in the functional simulation setup (test bench) shown in Figure 2(b). 2 and 3 are pulse voltage sources: for 2 place a voltage element; right-click on this and click on the Advanced button; in the pop-up window under Functions click PULSE(...) and fill in the values in the dialog box: initial=0.2, on=3.5, Tdelay=0, Trise=10n, Tfall=10n, Ton=2u Tperiod=4u (the different voltage Functions are used in transient simulations). For 3 you need Ton=1u and Tperiod=2u. Prepare for running a transient simulation by in the menu choosing Simulate - Edit Simulation Cmd, click on the Transient tab and choose a Stop Time of 5µs. Run the simulation and plot the nand gate input and output voltages as well as the supply current; print the schematic and the simulation waveforms. Does the circuit work as a nand gate? what are rise- and fall-times, propagation delays and transient supply currents? Are these realistic values?.model SW(RON=1 ROFF=1e6 T=0.6 H= 0.1).model PUSW SW(RON=... ROFF=1e6 T=3.5 H= 0.5).model P SW(RON=... ROFF=1e6 T=2.5 H= 0.5) + PUSW R1 S3 A B symbol B A S1 + Y S2 S4 S5 P S6 Y (a) 1 I 5 C p PULSE( n 10n 2u 4u) PULSE( n 10n 1u 2u).tran 5us (b) Figure 2: Model of 74LS00 nand gate (a). Functional simulation setup (b). Simulating power supply noise and decoupling Power supply noise can be simulated by explicitly including supply line inductance in your schematic. Modify your simulation schematic as shown in Figure 3 (do not include C2 yet). L1 and L2 are the power supply inductances; L3 and L4 are the inductance in leads and tracks leading to the decoupling capacitor C2; L5 is the inductance leading to the load capacitance. Carry out the transient simulation again, but also make sure to plot the power supply pin voltages on the nand gate; print the schematic and the simulation waveforms. Does these supply pin voltages look reasonable compared with what what you know from previous labs? What is ELEC3106/lab4 p. 3/5

4 the peak supply voltage dip on the gate, and how does this compare with simple calculations when the gate rise/fall time is assumed to be unchanged from the previous simulation? Has the rise and fall time changed compared with the previous simulation? Now add a decoupling capacitor C2 of 5 nf, and carry out the transient simulation again; print the simulation waveforms. Has the supply voltage dip reduced to the expected level? What else do you observe (this is a real phenomena that can well happen due to the LC resonances; it is rectified by including a resistance (say 2Ω) in series with 1 try this)? L1 30n C2 L3 5n 1 5 I 3 PULSE(...) L4 5n L2 30n L5 10n C1 100p Figure 3: Nand gate power supply decoupling simulation setup. Going further A few hints for keen students that might want to play around with the simulation software (it is a great tool to get to understand electronics; do use it!). The Edit - Component component library has a number of useful component models already there; the components in the library are the ones available from Linear Technology, but component models from other vendors can easily be included in the simulations using SPICE directives (look at vendor websites for SPICE models of their components). The library also have many diodes (diode), transistors (npn and pnp) and other discrete components; simply right-click on the component and select Pick New Transistor (say) to choose your desired part. You can also create your own component models with parameters of your choice in the same manner as was done for the switch. Look in the program documentation for more things to do. Lab extension Create a circuit schematic that model some EMI effect observed in laboratory session 3, PCB EMI measurements (for instance the coupling of digital supply noise into the analogue circuit); simulate the circuit and compare with measurements obtained in laboratory session 3. It is possible to create meaningful simulations using just passive components and switches, but use of other components are welcome. It is left to the student to decide upon an appropriate circuit, which EMI effect to model and which simulations to carry out. Report A short report (5 pages max) on the laboratory exercise must be prepared and uploaded as a.pdf-file on the course Moodle site by Friday the week after the lab finishes. The report should ELEC3106/lab4 p. 4/5

5 include answers to all questions asked above, and brief comments on the results. Submit one report per two-student group and make sure that both students names and student ID appear clearly on the report. Plots of relevant simulations must be included in the report. If done, a 1 page full schematic of the optional extension simulation must be included in the report, not counting towards the page limit. ELEC3106/lab4 p. 5/5