Created by Tim Green, Art Kay Presented by Peggy Liska Finding the R-C Charge Bucket Values TIPL 4404 TI Precision Labs – ADCs Hello, and welcome to the TI Precision Lab covering component selection for SAR ADCs. In this video we will use the amplifier and data converter model from the two previous TI Precision Labs videos to optimize the RC charge bucket circuit. The optimization will be done using SPICE parameter stepping to find the optimal settling for the data converter. Created by Tim Green, Art Kay Presented by Peggy Liska

Agenda SAR Operation Overview Select the data converter Use the Calculator to find amplifier and RC filter Find the Op Amp Verify the Op Amp Model Building the SAR Model Refine the Rfilt and Cfilt values Final simulations Measured Results SAR Drive Calculator Algorithm This video covers step 7 of the process for selecting the external components for a SAR ADC.

Remember: ADS8860 example calculator results 1. Enter the information from the ADS8860 Data Sheet. 2. Results will be used in the simulation In this video, we will use TINA SPICE to optimize the RC charge bucket circuit and to verify that we meet the error target. As a reminder we selected the amplifier to be OPA320 based on the calculator results. The calculator also gives the range for the filter resistor values. In this case the filter resistor is split into two equal resistors denoted Rfilt/2. The range for Rfilt/2 given by the calculator is 4.1 ohms to 32.5 ohms. We will use parameter stepping to find the best resistance in this range. The calculator also gives the value of 1.1nF for Cfilt. This value will be used in simulation. If proper settling cannot be achieved with Cfilt equal to 1.1nF, the entire search procedure will be repeated with Cmin and Cmax.

Trick: Voltage controlled resistor In this slide we show how we will use parameter stepping to sweep the input resistor values. Parameter stepping doesn’t allow for two equal components to be simultaneously stepped. One way around this limitation is to use a voltage controlled resistor. This example shows two voltage controlled resistors controlled by the source Vcont. The resistance is equal to the control source so each resistor in this example is set to 1k ohm since Vcont is 1kV. You can observe by the voltage sources and ammeters that the voltage controlled resistor acts like a normal 1k ohm resistor. The resistance for both resistors is equal to Vcont.

Use Parameter Stepping on Rfilt 1. Click here to do Parameter stepping 4. Do a linear sweep type. Enter the start and end value from the calculator. Set number of cases to 10. From Calculator 3. Press this box to configure parameter stepping range. In this slide we will learn how to set up parameter stepping on the resistors in the charge bucket filter. Notice that Rfilt1 and Rfilt2 are both voltage controlled resistors and their resistance value is set by the voltage source V1. The voltage control will allow us to step both resistors simultaneously. [click] The first step to using parameter stepping is to click on the icon shown here. You could also do this using the “Analysis>select control object” option from the menu. Once you do this your mouse pointer will change to look like a resistor with an arrow. [click] Click on the voltage source V1 to make it a control object. [click] When you click on the control object, a window will pop up listing all the parameters for the selected device. Click on the box next to the parameter you want to step. In this case we have two parameters: voltage, and internal resistance. We want to click on the box next to voltage as that is what we want to step. [click] Next a window will pop up that will allow you to edit the start value and end value for parameter stepping. In this case we enter 4.1 ohms to 32.5 ohms as this is what the calculator recommended. Here you should also enter 10 for the “number of cases”. This will run 10 different simulations with resistor values ranging from 4.1 to 32.5. Finally, choose “linear” for the sweep type as this will set the stepping so that the resistance increments are equal. Once all these steps are completed you will notice an asterisk next to the object that is being controlled. Now any simulation performed will automatically run ten times generating ten different sets of curves. 2. Click on the schematic symbol you want to control V1 = Rfilt

Run a Transient analysis Select “Analysis>Transient…” set the time to view a few conversion cycles. Throughput = 1us in this example. Now let’s run the transient analysis. Select “Analysis>Transient” from the menu. Select a range of time that covers several conversion cycles. Throughput is 1us, so we will run 3 conversions or 3us. The displayed curves will contain ten sets of curves. One for each resistance value in the parameter step.

Adjust the X and Y axis In order to make the simulation results easer to look at you need to adjust the vertical and horizontal axis scaling. The main curves we want to look at here are the error curves. The error curves will ideally settle to 0V, so setting the vertical range to ±100mV is a good range for zooming in on the error. On the horizontal axis, you should always ignore the first cycle as some startup behavior will invalidate these results. Click on axis and change the vertical range to ±100mV Click on axis and change the horizontal range to show 1 acquisition cycle. Always ignore first cycle!

Error for R = 4.1 ohms…32.5 ohms End of the acquisition period. Delete curves with large overshoot. After adjusting the curves this is what the graphs look like. There is one error curve for each resistance value for a total of 10 different curves. The purple square wave that controls the acquisitions period identifies the end of the acquisition period. Notice that some of the curves have very large overshoot. You can click on the large curves and hit the delete key to eliminate them.

Large overshoot curves deleted Change vertical scale to ±10mV After deleting the curves with large overshoot, we can adjust the vertical scale to ±10mV. Deleting the curves that are obviously out of range will make it easer to inspect the good curves. Fewer curves will be easer to inspect.

Add a legend 1. Click here to set the cursor. Set the cursor at the end of the acquisition period. Cursor at 1.290us, tacq = 290ns 2. Use the legend feature to show the error at the end of the acquisition period for all resistors shown. After deleting curves and zooming in we need to add a legend. The legend will give the numerical value for each curve at a particular point in time. [click] First let’s set the point in time that we want to generate legend for. For ADC settling analysis, we want to look at error at the end of the acquisition period. We need to place a cursor at the time where the acquisition period ends. Press on the cursor icon shown here, and click on any curve. You can drag the cursor to the end of the acquisition period or type the time in directly. In this case the cursor needs to be dragged to 1.290us as conversion starts at 1us and the acquisition period is 290ns. [click] Next press the legend button. This will generate a legend for every curve. The legend will list the curve name, the parameter step value for that curve, the time, and value of the curve at that time. So, for example, the curve “Verror[5]” is the error voltage source measured with a 16.72 ohm resistor, at 1.29us, with an error of -546uV. Remember, the parameter being stepped is actually a voltage source that is used to set resistance, so the 16.72 ohm resistor shows up as a voltage.

Select the best three curves Add labels to the key curves using this feature. Also, double click on curves to change thickness. We will use 19.9 to 26.2 as the range for the next parameter step simulation Here you can visually inspect the error curves to look for the three best curves from a settling perspective. Also look at the errors listed in the legend. Select the three curves with the best settling. Generally, you will find that one of the three curves will have overshoot, one will be underdamped, and one will be in-between. You can use the label generation feature to identify the curves. Also, if you double click on the curves you can increase the thickness to make the selection more obvious. In this example, you can see that curves 6, 7, and 8 are the best curves. Looking at the legend, you can see that curve 6 shows the lowest error of -21.6uV. The important point here is that the resistance range for the best three curves will be used as the parameter stepping range in the next simulation. So the next simulation will use a resistance range of 19.9 ohms to 26.2 ohms.

Second Run: further refinement in Rflt value 1. Enter a new range for the Rfilt range based on last simulation (i.e. 19.9 and 26.2) Here we will repeat the parameter stepping procedure for the resistance range of 19.9 ohms to 26.2 ohms from the last simulation. Once the transient results are displayed you should adjust the voltage scale to ±1mV. Again use visual inspection as well as the legend to find the best three curves. These three curves will set the range for the next simulation. Notice that the polarity of the error transitions from +80.3uV to -73uV for the three curves. The idea is that some curve between this range will have an error near zero. 2. Find the three best curves to set the range for the next simulation. Typically the three curves will be overdamped, underdamped and critically dampened. Notice the polarity of the error switches. We will use 24.1 to 25.5 for next simulation.

Final Run: Use Standard Values 1. Use the “List” sweep type 3. Choose the curve with the best settling. Check to see if the error target from the calculator is met. Yes! 3.9uV << 38.15uV For Rfilt = 24.9 Ω ½ LSB For the final run we will perform another parameter step analysis. In this case however we will type in a list of standard value resistors that cover the range from the previous sweep. To enter a list select “list” under “sweep type” and press the “Set List” button. [click] To add items to the list press “add new”. Enter all the standard 1% resistor values using the range from the previous simulation. The Analog Engineer’s Pocket Reference has a copy of this list. You could use 0.1% resistors if desired if you want smaller increments in the list, but 1% is usually sufficient. The previous simulation range was 24.1 to 25.5. There are three standard resistors in this range: 24.3, 24.9, and 25.5. [click] After running a transient analysis, choose the curve with the best settling to determine the resistor used in the final circuit. In this case, the 24.9 ohm resistor settles to an error of 3.9uV. Confirm that this final settling error meets the half LSB error maximum target from the calculator. It does in this case as the error of 3.9uV is much less than the error target of 38.15uV. Thus for this design we will use 24.9 ohms in the final circuit. 2. Enter standard resistor values using the results of the previous sweep (i.e. 24.1 to 25.5)

Turn off Parameter Stepping 1. Click on the parameter stepping icon. To remove parameter stepping, first click on the parameter stepping icon. This will cause your cursor to change into the shape of a resistor. Second, click on the voltage source to access the parameter stepping details. Here you want to select “remove” to disable parameter stepping. 2. Click the source and press remove to remove the parameter stepping.

Final Circuit The goal of this presentation was to provide a method for selecting the amplifier, and RC charge bucket circuit to achieve less than one half LSB settling error. First we developed the ADC model based on it’s data sheet specifications. Second, we used the calculator to get amplifier bandwidth requirements as well as RC charge bucket initial values. For this example, we used the amplifier bandwidth and other amplifier requirements to select the OPA320. Next we used parameter stepping in TINA SPICE to refine the RC charge bucket values and verify settling. The values selected in this procedure are shown in red. Replace voltage controlled resistors with standard resistors

What if we didn’t meet the error target? 2. If no RC combination works, try an amplifier with wider bandwidth. 1. Try reiterating on Rfilt using Cmin. If Cmin doesn’t work try Cmax. What if the parameter stepping didn’t yield good settling for any resistor value? The calculator provided two optional capacitor values. A minimum and maximum capacitance. First try re-running all the simulations with the minimum capacitance using the same parameter stepping method as before. If this still doesn’t meet the error requirements, try the same procedure using the maximum capacitance. If this doesn’t work you will probably need to try an amplifier with a wider bandwidth. Output impedance also impacts settling, so an amplifier with a lower or flatter output impedance may also yield better results. In general, you should not need to go through the additional steps, but there are always a few difficult cases. Note 1: Typically step 1 and 2 will not be required. Note 2: Output impedance can also impact settling. Ideally open loop output impedance is low (R < 100Ω) and flat.

Measured results for example circuit ADS8860 Data Sheet (1Msps) Parameter Min Typ Max Unit SNR 92 93 dB THD (1kHz) -108 Measured SNR = 93.3dB THD = -113.1dB Circuit from TINA This slide shows the measured performance for the SAR input drive circuit that we selected the amplifier and RC charge bucket circuit for earlier in this presentation. The EVM software measures THD, SNR, and other AC figures of merit for the circuit. For comparison, we also provide the data sheet AC specifications for this device. In this example you can see that the measured performance actually exceeds the data sheet typical performance. This is a good indication that the design procedure we used worked well for selecting the input RC values.

Agenda – next video… SAR Operation Overview Select the data converter Use the Calculator to find amplifier and RC filter Find the Op Amp Verify the Op Amp Model Building the SAR Model Refine the Rfilt and Cfilt values Final simulations Measured Results SAR Drive Calculator Algorithm The next video will walk through step 8 of the process.

Thanks for your time! Please try the quiz. That concludes this video – thank you for watching! Please try the quiz to check your understanding of this video’s content.

© Copyright 2017 Texas Instruments Incorporated. All rights reserved. This material is provided strictly “as-is,” for informational purposes only, and without any warranty. Use of this material is subject to TI’s Terms of Use, viewable at TI.com