Spice up your simulations: used together, electronic measurement tools and EDA tools can help create and tune circuit models when SPICE models can't be found.

Ed. For the full article with all figures, please see www.pcdandm.com/pcdmag/mag/0504/0504rae.pdf.

Hardware design engineers are increasingly using simulation to test their board designs while still in schematic form. Simulation helps designers to reduce time to market, find errors in their designs before they become costly mistakes, evaluate problems potentially caused by variations in real world component properties, and optimize their designs.

Historically, engineers have simulated circuits with models that are based on the electrical of physical characteristics of the components.

Simulations operate at speeds slower than real time, and as a result, it is not possible to directly take simulation output and use it to drive external circuitry. Some of the other limitations include: not being able to easily model all types of devices, such as sensors, in the design; not being able to produce simplified models for existing designs that the designer would like to interface with; uncertainty of the reliability of models; and an inability to find models of model makers for all parts in the design.

As designers continue to look for ways to reduce time to market, the crossover point between the design and the characterization and validation process of actual hardware has been neglected. By bridging the gap between the design and measurement area, users can iterate more tightly through the design process by identifying and addressing discrepancies and addressing them in the prototypes. The way to accomplish this is by having the ability to reuse and compare the signal data--simulated or measured--easily in either domain.

It has been difficult and time-consuming to accurately model real-world signals such as those from sensors or buses. But designers can now capture these signals with electronic measurement automation (EMA) tools and use them to drive simulations in their electronic design automation (EDA) tools. By importing simulation waveforms into EMA tools, the signals can drive existing interfaces to verify that the design is working according to specifications. They can also compare simulation waveforms to real-world waveforms in a direct format. As a result, they can verify models and designs, tighten simulations, and aid the debugging process.

We have cited a number of examples where the crossover between EMA and EDA tools will help to improve the design process. We will focus on the use of EMA tools in helping to produce and verify a model for a device for which no SPICE model was available. The part in question is a coaxial low pass filter with a 5 MHz passband.

Creating and Verifying SPICE Models

In order to create the simulation model, the engineers must undertake a series of steps. To begin, they need to find out as much as they can about the part by consulting datasheets and application notes. They then must get the part and connect it up to the test and automation equipment so that they can characterize the device and capture the characteristics on a computer for future analysis. Given the information they obtained from the data sheet, application notes and the device characterization, the engineer can now create a circuit approximation of the device. They are now ready to simulate the equivalent circuit.

The next step is to export the simulation results to the EMA tool so that they can directly compare the real-world and simulated results to ensure an adequate model. If the model is too far from the desired response they can return to the equivalent circuit and adjust the component values. If the results are very different, they may need to re-evaluate the circuit topology as well. Once the designer finds a suitable circuit equivalent for the model, he can create a SPICE model of the device and assign it to a schematic symbol and store it in a database for current and future use.

The list below summarizes the steps required to create a SPICE model for a part.

1. Research the part.

2. Create an approximation of the equivalent circuit model.

3. Characterize the part with real measurements.

4. Simulate the equivalent circuit.

5. Export the results from the EDA tool to the EMA tool.

6. Compare the results.

7. Adjust the component values or change circuit topology.

8. Re-iterate through steps 4-7 until a suitable match is found (should be valid over the range that the part will be used in the design).

9. Create an equivalent SPICE model from the circuit.

10. Create a component with schematic symbol and model and save it to the database for re-use.

Let us now look at the example of the 5 MHz low-pass filter.

Research the part. Information available for the part included a datasheet and an application note. The datasheet provided information on the passband, cutoff frequency, stop-band, VSVR for the passband and the stopband, and included a frequency response graph.

Details of the application note showed that the filter was a passive device that contained inductors and capacitors, and that they provided a matched 50W impedance within and outside the passband. It also stated that the filter designs utilized included modified Butterworth, modified Bessel-Thomson, and Elliptic function design.

Create an approximation. From the information gathered, an equivalent circuit was designed. The circuit had equivalent input and output impedances of 50W and matched the filter characteristics of the datasheet.

Characterize the real part. Before you can compare real and simulated values, you must acquire the data. Since this part is a coaxial filter, the engineer was able to connect the input and output of the filter directly to the test and measurement system cables. Under other circumstances we would simply build a small prototype circuit and connect the test leads to the relevant points in the circuit. The input of the filter was connected to a function generator through an SMB-BNC cable and the output of the filter was connected to the input of a data-acquisition card through a second SMB-BNC cable.

A couple of different measurements were taken, beginning with the frequency response of the filter. This can be done easily with EMA tools, since the engineer can programmatically send out sine waves and take measurements across a desired range of frequencies. The results of this characterization appear in FIGURE 3. The second type of measurement was a look at the transient response to a 500 kHz square wave.

[FIGURE 3 OMITTED]

Simulate the equivalent circuit, Using a SPICE simulator the engineer can now repeat the measurements made on the real-world device. Users can perform an AC analysis across the same frequency range and perform a transient analysis to find the response to a 500 kHz square wave. If possible, the user could also connect virtual test instruments to the circuit as shown in FIGURE 4.

[FIGURE 4 OMITTED]

Export simulation results. In the SPICE simulation tool the user can save the simulation results to a file or export them directly to an EMA tool, if their tool supports this feature. It is important to note that most SPICE simulators will store the data in X-Y pairs with one column indicating the time of frequency and the other column indicating voltage, current of gain. EMA tools work with fixed sampling rates and their data files have one line at the beginning to express the sampling rate and then a single column of sampled data points. In order to make comparisons the engineer needs to convert from one file type to the other. Check with your tool provider to see if utilities are available to do this file conversion for you. FIGURE 5 shows an example of a utility available in National Instruments' Lab-VIEW and Signal Express to read in simulation results from Electronics Workbench's Multisim simulation tool.

[FIGURE 5 OMITTED]

Compare the results. Once the data is in the EMA tool, the engineer can compare and contrast the results of real-world and simulated data. He can perform additional analysis at this point. FIGURE 6 depicts the simulated and real-world square wave excitations as well as the difference in the amplitude of the two signals. If the engineer is not satisfied with the model at this time, he can return to the EDA tool and adjust either the topology of the equivalent circuit to compensate for large differences or modify the component values to fine-tune the model.

[FIGURE 6 OMITTED]

Create part for EDA tool reuse. Once the equivalent circuit matches the real-world part within operating range and within the requirements, the engineer can create a SPICE model to attach to a schematic symbol and store the part in a database for future use. Creating a model from an equivalent circuit involves exporting the circuit file as a SPICE netlist and then creating a subcircuit model from the netlist. This involves inserting the following line at the top of the exported netlist:

.SUBCKT LPF_5 filter_input filter_output

* Multisim to SPICE netlist routine

*

* Generated by: Shauna

* Monday, February 28 13:03:37, 2005

*

*

IL2 1 filter_output 1.596e-006 IC=0

IL1 filter_input 1 1.596e-006 IC=0

cC5 filter_output 1 1.07e-010 IC=0

cC4 1 filter_input 1.07e-010 IC=0

cC3 filter_output 0 9.16e-010 IC=0

cC2 1 0 1.57e-009 IC=0

cC1 filter_input 0 9.16e-010 IC=0

The first line contains the information that this model is built as a subcircuit, ".SUBCKT," the name of the model, "LPF_5," and the two nets inside the subcircuit that will attach to the symbol of the part, "filter_input" and "filter_output."

Last, use the EDA tool's component creation function to create a symbol for the part and associate the symbol to the model, and finally store it in the database for future use.

Engineers can now sample real-world data and use it to drive simulation. They can export simulation results to an EMA tool and use that to drive external circuitry. They can also couple EMA and EDA tools together to tune simulation models for parts without readily available models. PCD&M

SHAUNA RAE is an applications engineer with Electronics Workbench; [e-mail]. GRETCHEN EDELMON is a senior software engineer at National Instruments; [e-mail].