EMC Menu

Generate Spice File

The command "Generate Spice File " (icon ) launches the electrical net extraction and creates a SPICE netlist from the schematic diagram, ready to be executed by WinSpice. Notice that IC-EMC has been made compatible with WinSpice (See www.winspice.com) a freeware SPICE for PC based on Berkeley Spice. The following window appears. The SPICE text appears on the left side of the screen. On the right side, different fields appear to configure:

• The type of analysis may be selected. The analysis may be forced and saved using a label (Click "A" icon) starting with ".AC" for AC analysis, ".DC" for DC analysis, ".TRAN" for Transient Analysis, etc…
• Options may be listed. Alternatively, a label on the editing window starting with '.OPT ' updates the options.
• The result is saved into a text file (*.txt), which is mandatory for post processing.
• When special devices as MOS or Diode are listed, a library containing SPICE models may be included. The default library is SPICE.LIB (included in system\lib subdirectory)
• A script may also be included. The script is Spice3 compatible. See the WinSpice documentation for script examples. An example of SPICE3 script may be found in script.txt
• A direct access is given to the windows of EMC tools (emission, near field scan, susceptibility, voltage vs time, impedance, S parameter). However, the user must invoke the WinSpice simulation manually, on the generated SPICE file.

Ibis Interface

The command "EMC -> Ibis Interface" (icon ) gives access to the current IBIS information related to circuit. Use File -> Load Ibis to load the information from a given IBIS file. The list of I/Os extracted from the IBIS file appears, as well as the buffer models and package information. In the IBIS window:

• One pin may be converted into RLC. Select the desired pin and click "One pin into RLC"
• Several supply may be merged into single R,L,C elements. Select the desired supply network and click "Supply merged into RLC"
• One model (input or output) may be converted into RLC and associated clamp devices. Select the desired model and click "Model into RLC"
• A basic 3D view of the package can be reconstructed. Click on the button "3D Draw"
• Access to the tool Tools -> Advanced SPICE and IBIS to translate the whole IBIS file into a symbol, with a shape that is deduced from the IBIS information, evaluate package model, generate advanced IBIS netlist including accurate evaluations of packge and lead elements, and generate sub-circuit containing all R,L,C sub-elements in a Spice-compatible format.

Emission dBµV vs Frequency

The voltage waveform computed by the analog simulator is translated by Fast Fourier Transform (FFT) into frequency domain energy. The X axis should cover the range 10-10,000MHz in logarithmic scale. The representation of the energy in Y axis is made in dBµV, equal to 20*log(V*1e6). 1µV should correspond to 0dBµV, 1mV to 60dBµV and 1V to 120dBµV.

In the EMC menu, click "EMC à Emission dBµV vs Frequency" or on the icon . A specific screen with Log/Log units configured to display energy vs frequency is proposed, as shown below.

In the item "SPICE simu", click the button and select the desired result file from WinSpice (.txt file). The corresponding spectrum appears. The FFT points are adapted to fit the information included in the simulation. The number of points may be adjusted manually. Several scaling buttons exist (Lin/log). Measurements may be also added to the figure. Several formats are supported. The most common is the simple tabulated dB vs freq (*.tab).

Susceptibility dBm vs Freq

Susceptibility simulations require a RFI source, a bidirectional coupler and a transient simulation .tran. The RF source (RFI) is a sinusoidal wave with programmable slope. The source is built from two voltage sources, one sinusoidal source and one ramp, that serve as inputs for a “B“ element, which performs V(RFI)= VRFI_sin* VRF_ramp. The bidirectional coupler is an ideal transmission line with a programmable delay and characteristic impedance and equations used to compute forward and reflected powers.

Click "EMC -> Susceptibility dBm vs frequency" or on the icon to open the RFI control window and the susceptibility graph window. The RFI control window is used to configure the susceptibility simulation and to extract the susceptibility threshold from transient simulation. The RFI control proposes three simulation modes: a manual mode where only the amplitude of the RFI source is swept, the frequency remains constant during the transient simulation. In the automatic mode, both the amplitude and the frequency of the RFI source are swept. The last mode is the list mode, where RFI frequency and amplitude, transient simulation duration and susceptibility criterion are predefined in a text file.

The user's interface for susceptibility is shown below. The RFI control of the SPICE generation appears on the left while the susceptibility graph appears on the right. Fix the parameter of the amplitude and or freqency sweep, create an update version of the CIR file, run the WinSpice simulation, and click "Get Power“ to extract the source power at which the voltage limit has been reached at the observation point. After clicking Add Forward Power, one or several simulation point corresponding to the user's frequency (X coordinates) and power in dBm (Y coordinates) appear. Susceptibility measurements in .tab file can be imported and compared with simulation results.

Impedance vs Freq

The software uses a specific probe called "Z probe" that can be found in the probe menu, close to the voltage probe. The Z probe is inserted between the two electrical nodes where the impedance needs to be measured. A ground should always exist in the schematic diagram in order to avoid instability. An AC simulation is performed with an AC source at the Z probe location. The ratio between the voltage and current is computed from 10MHz to 10GHz. The result is plotted as shown below.

An example of impedance simulation using IC-EMC is shown below. The supply impedance of an integrated circuit (C51 microcontroller) is represented by the on-chip decoupling C1, the access package inductance LVdd, LVss, as well as parasitic serial resistance Rvdd and Rvss. The corresponding file is "basic\impedance\Impedance_c51_supply.sch". The software uses a specific probe called "Z probe" that can be found in the probe menu, close to the voltage probe. The Z probe is inserted between the two electrical nodes where the impedance needs to be measured. We compare here the simulation with measurements based on [S] parameters. The conversion betwwen [s] and [z] parameters is described in the appendix of IC-EMC documentation.

Near-field Scan

The near-field scan window enables the comparison between measured and simulated scan. The near-field emission is based on "radiating inductances", a concept based on elementary current dipoles.

Radiating Inductances

The radiating elements are the inductances which are declared for near-field scan prediction (See figure below). The inductor coordinates are defined in the XoY plane in mm. Geometrical coordinates for inductances may be linked with package information, which can be deduced from IBIS description. In that case, the schematic diagram should be coupled to an IBIS file (See for example "near field\cesame\cesame_norm_scan.sch"), using the label ".IBIS <ibis_filename>". The list of I/Os as defined in the IBIS description appear in the inductance window: select the desired I/O and click "Update Value, coordinates". The gemetrical coordinates of the inductance updated the fields "X_start, Y_Start", "X_Stop, Y_Stop" and the Z coordinates ("Altitude" for an horizontal conductor). The geometrical coordinates can also be typed manually.

Note that inductances are oriented. The current is supposed to flow from the Start to the Stop point. Consequently, care should be taken in defining the Start and Stop point as it impacts the sign of the current. Power pins like VDD should have a Start point (Source of the current) situated at the outer part of the IC package. The Stop point should be near the center of ICs. VSS pins should have a start point near the center of the IC and a Stop point at the oupter part of the package.

Near-Field simulation

SPICE simulation must be performed in time domain in order to monitor all currents flowing in all inductances declared for near-field simulation. For each inductance current I(t), a Fast Fourier Transform is performed to extract the current amplitude I0 at a given frequency.

Click "EMC -> Near field scan" or on the icon to open the near field scan interface. IC-EMC computes the magnetic and electric fieldz generated by of each elementary current dipole, calculated from well known formulations as may be found in [Bendhia S., "EMC of ICs", Springer 2005]. The magnetic and electric field (Htotal, Hx, Hy or Hz) is the sum (in complex domain) of all elementary currents and charges flowing in the declared inductances. When dipole coordinates are very close, with opposite Start and Stop points (See Lvss and LVdd on the left upper side of the package in the figure below), the magnetic field tends to cancel at a certain distance above the surface of the integrated circuit.

The IC-EMC user interface shown above displays the position of the die, the package, and the position of four current dipoles, assigned to four inductances. The scan altitude can be changed. Measurements can be loaded, which are described in various formats, and especially a .xml format. More information about these formats may be found in the appendix of the software documentation.

Voltage vs. Time

The window "EMC à Voltage vs Time" (icon )is useful to display time-domain waveforms and to compare time-domain simulations with measurements. The window is also convenient to measure periods and signal amplitudes. Just click in the screen, keep the button pressed and release: if the given marker is horizontal, time and frequency will be displayed. If the marker is vertical, corresponding voltage will be computed. The button Distrib. gives access to a special screen used to extract the distribution of the amplitude signal in term of density of probability.

S parameters

The software uses a specific probe called "S probe" that can be found in the symbol palette, below the voltage probe, to compute S parameters between the N ports of a device. The S probe is inserted between the two nodes of each port of a device under test. A common ground should always exist between every ports. The S parameter analysis requires an AC simulation.

Click "EMC à S parameters" or on the icon . An example of s parameter simulation using IC-EMC is shown below. The interface proposes conversion between S and Z parameters and display under several forms: magnitude in linear or dB, real and imaginary part, phase in degree or radian. S parameters can be displayed in a Cartesian or a Smith chart. Simulation results can be exported in the standard Touchstone file *.sNp (N is the number of ports). Similarly, measurements in Touchstone file can be imported and compared with simulation results.

Parametric analysis

The command “EMC à Parametric analysis” opens a screen for the configuration of a parametric analysis. The parametric analysis consists in sweeping one to five parameters of the devices inserted in the schematic (passive or active devices, sources, temperature, model parameters included in a library (*.lib)). Select the option “Enable” to activate a parameter, select one component in the field ‘Component’ and one of its property in the field ‘Parameter’. Then, define the sweeping with the start and stop value, the type of sweep (Linear or logarithmic sweep, number of step (‘Point number’ field) or value of the step (‘Step’ Field)). Once all the parameters have been configured, click on the button ‘Generate SPICE’. A simulation type has to be preconfigured or detailed in the field ‘SPICE simulation’. Only AC, DC and transient simulation are supported. Although S parameter, susceptibility, emission and near-field scan simulations rely on AC, DC or transient simulations, they are not supported by the Parametric analysis tool.

The parametric analysis configuration is saved in a *.par file, defined in the field ‘Simulation profile’. This file is also required to find all the SPICE simulation result files corresponding to the sweep of the parameters. Each time the button “Generate SPICE” is pushed, the *.par file is updated. The name of the *.par must be the same as the schematic name (for example, for the schematic called ‘misc\rc_filter_parametric.sch’, the configuration of the parametric analysis is saved in the file ‘misc\rc_filter_parametric.par’). A pre-existing parametric analysis file can be imported by clicking on the button .

At the end of the SPICE simulation, click on the button ‘Display Results’ to plot the simulation results vs. parameter values.

Signal analysis

The command “EMC à Signal Analysis” opens a special window to extract statistical information about amplitude and timing characteristic of a signal. The tool is also available from “EMC à Voltage vs. Time” interface. The tool loads the transient simulation results contained in a .txt file. If a schematic is opened and have been simulated, the simulation results in *.txt file are automatically loaded (whatever the simulation type!). The simulation result file can also be imported, with the field ‘Simulation Data Source’. The tool offers two types of signal analysis:

· Tracking analysis (Time domain category): the transient evolution of the signal (i.e. its amplitude) or one of its timing characteristics

· Statistical analysis (PDF category): the statistical distribution of the signal amplitude or one of its timing characteristics, given in term of probability density function (PDF). Statistical properties such as minimum, maximum, mean values, peak-to-peak amplitude and standard deviation are also given under the graph.

The following timing properties can be extracted:

· Rise and fall time: the time required for the signal to go from 10% to 90% of the maximum amplitude (defined by High Level – Low Level fields defined by the user)

· Period and frequency of the signal: the period is measured between two adjacent instants when the signal crosses the Threshold limit defined by the user (by default, threshold = 0.5×(High Level + Low Level). The frequency is equal to the invert of the period

· Duty Cycle: the period ratio during which the signal exceeds the Threshold level

Phase, Period and Cycle-to-cycle jitter: three different definitions of the jitter. The phase, edge, timing or absolute jitter, or time interval error is the deviation in the transition of the signal from its ideal position (the ideal position is defined by an ideal clock which starts with the characterized signal and with a period defined by the field ‘Signal Period (ns)’). The phase jitter characterizes each signal period. The period jitter is related to the fact that the phase jitter tends to diverge with measurement time due to jitter accumulation in real oscillators, so that phase jitter is not the best figure of merit for jitter characterization. Period jitter is the deviation of the signal period with respect to the ideal clock period. Period jitter originates from two timing errors on both rising edge of two adjacent periods. Period jitter is the first jitter difference. Cycle-to-cycle jitter characterizes the variation of signal period between two adjacent periods. It describes the short-term dynamics of the period.

Back