Simulating the front-end of your ADC

-March 04, 2015

Successive-approximation, analog-to-digital converters (SAR-ADCs) are straightforward, right? You attach analog voltages to the inputs (AINP, AINN, REF), and you see an output digital code that represents the analog input voltage with respect to the reference. At this point, you may be tempted to analyze the converter’s specifications to verify that your converter operates up to datasheet standards. Not so fast! Are you sure that the converter has really received the correct analog signals internally?

You can anticipate and troubleshoot these types of problems by using simulation tools. The determination of the ADC analog input stage simulations rely on voltage and current accuracy. This is where the analog SPICE macro-models come in handy. The PCB digital signal-integrity relies on timing, voltage-current levels, and parasitics. This is where the digital IBIS model comes into play. The discussion about IBIS is coming next month, but let’s address the simulation environment with ADCs.

SPICE simulations for ADCs

A trial-and-error approach to sending signals into your ADC is time-consuming, and it may or may not work. If your analog input pins are not stable at the critical times when the converter is capturing the voltage information, it will be impossible to obtain the correct output data. The first step that the SPICE model allows you to do is verify that all analog inputs are stable so that there are no erroneous signals going into your converter.

Let’s look closely at a typical serial, pseudo-differential SAR-ADC like the ADS8860 (Figure 1).

Figure 1 The ADS8860 is a pseudo-differential input, 1 MHz, 16-bit SAR-ADC.

This device’s TINA-TI spice macro model allows you to simulate the effects of the analog signals going into the converter. With this model and the proper driver op amp models at AINP, AINM, and REF, you can determine whether a good conversion is possible before you go to the PCB. The importance of the ADC macro-model is that it characterizes the converter’s input terminals accurately. The op amps driving AINP, AINN, and REF must also model their open-loop output resistance (Ro) accurately.

Let's get busy in figuring out how this macro-model works. The converter macro-model samples both positive and negative inputs individually with 55-pF sampling capacitors. The device converts the voltage difference between the two sampled values at AINP and AINN. As you view the simulation results, the model must settle to at least half a LSB at the end of the acquisition period. For this 16-bit converter half a LSB equals REF / 216.

The voltage reference pin, REF, requires a stable voltage to be present during the conversion process, or after the CONVST pin becomes a high value (Figure 2). While CONVST is low, the converter is acquiring the input signal (acquisition mode). The SAR-ADC macro-model has a 1 MHz clock and does produce the CONVST signal. The voltage reference pin must settle at the end of the bit conversion periods throughout the entire conversion time of the converter to a half LSB level.

Figure 2 In this three-wire timing diagram with three-wire operations, CONVST functions as chip select.
Click to enlarge

The TINA-TI model for the ADS8860 in Figure 3 samples the input signals on AINP and AINN and presents the results on the model’s AINPsmpl and AINMsmpl.

Figure 3 Here is a TINA-TI macro-model of a SAR-ADC.

In Figure 4, the input at AINP is equal to 3V, and the reference voltage is equal to 4.096V. As you test the accuracy of the input signal, set the ADS8860 TINA-TI circuit to sense the difference between the output of the amplifier driver, AMP_OUT_sig, and its output signal, AINPsmpl. As you look at this difference, examine the region at the end of the acquisition time or just before the CONVST pin goes high. Verify that the signal is less than half a LSB.

Figure 4 This set-up is for the TINA-TI circuit to monitor the analog and reference inputs.
Click to enlarge

Once you have examined the analog input function for accuracy, examine the stability of the voltage reference pin. As you measure accuracy of the REF pin, measure the difference between the voltage reference output (VF1) and the THS4281 amplifier output (AMP_OUT_ref). Be sure to remove offset errors generated by the voltage reference (REF5040) and op amp (THS4281) with the value of VERR1. While doing this, examine the voltage level just prior to the current spikes using the iref1 current meter. Reference 1 provides good in-depth information for this simulation.

Simulation is a tricky thing when it comes to SAR-ADCs. Presently there is no complete converter model that accurately models the entire device. The resource you do have is an analog SPICE file that models the analog input pin stability. The good fortune of having this tool available is that you have a powerful utensil to address one of the most critical, difficult converter issues.

But, this is half the story. You have only simulated the analog part of the ADC. Next month we will talk about simulating the digital input / output of your converter.

  1. Using SAR ADC TINA Models: Much ado about settling,” Munikoti, Harsha, Precision Hub, Texas Instruments, December 12, 2014
  2. Download the ADS8860 datasheet.

Also see

Loading comments...

Write a Comment

To comment please Log In