THS4551: Single ended source to ADS1288

Hello Lkhagvahantsan,

I am switching this thread to the ADC team so they can support your questions on modeling the internals of the data converter.

If you end up needing a fully-differential amplifier I can assist you further. In general, you can use PGA and FDA models to simulate internal ADC blocks as long as you understand the specifications of the internal amplifiers within the ADC.

As I do not know what type of amplifier is internal to the ADS1288, I will have the precision ADC (PADC) team give their input here first. 

Best,

Alec

Hi Lkhagvajantsan Damdinsuren,

As Mark mentioned in your other post (https://e2e.ti.com/support/data-converters-group/data-converters/f/data-converters-forum/1457609/ads1288-ads1288?tisearch=e2e-sitesearch&keymatch=%2520user%253A637038#), we do not have a model to share for the ADC input stage.

You should instead get the ADS1285EVM so you can perform any required testing and better understand the input stage characteristics.

-Bryan

Hello Lhagva,

I will work on simulation.  I will consider the need for a buffer between the ADXL354 output stage and the FDA circuit.

For EVMs, the D (SOIC), DGK (VSSOP), DGN (HVSSOP) are available on the DEM-FDA-xxx-EVM boards.  These are unpopulated boards which support these three FDA packages.  If you need to evaluate the RUN FDA package or would like to use the THS4551 / THS4567 EVMs, you can order those populated EVMs from those product pages.

As long as you confirm package pinout, the FDAs should function on an EVM which supports the FDA package of the IC.

Best,

Alec

Hello Lhagva,

Do you have a target noise value for 0.1Hz to 100Hz?  Are you asking for an extended curve showing more noise data or lower 1/f noise at low frequencies?

Please refer to the THS2630 noise curve for an example of a lower value voltage noise at low frequencies.

Best,

Alec

Hello Lhagva,

You can request samples of all three products at the following links:

https://www.ti.com/product/OPA209/part-details/OPA209AID?source=ooq

https://www.ti.com/tool/DIYAMP-EVM

https://www.ti.com/tool/ADS1285EVM-PDK?

You need to login with your TI account, scroll to 'Add sample to cart', and fill out your address information to check-out.

Best,

Alec

Hello Lhagva,

I am glad you received samples.

If you still require simulation support for THP210, I can change-over the thread to the team who owns the THP210.

If you would still like simulation support for one of the THS45xx or THS2630 devices, I can still assist.

Best,

Alec

Hello Lhagva, 

I am adding the THP210 HVA team to this thread.  Thank you for working with me and for trusting TI to help with your design.

Best,

Alec

Hi Lhagva,

Below is a preliminary circuit using the THP210 (FDA) and OPA2388 dual, zero-drift (Chopper amplifier) rail-to-rail input amplifier.

Comments:

- Since the sensor has a 32kOhm impedance, the sensor output needs to be buffered to drive the FDA.

- I chose the OPA2388 chopper amplifier, since chopper amplifiers virtually eliminate 1/f low frequency noise (choppers do not exhibit flicker noise)

- This amplifier circuit has very low noise at frequencies at the ~100Hz frequency range.

- Since the sensor has a 0.1V to 1.7V output centered at 0.9V, the FDA negative input is referred to 0.9V .

-  The 0.9V is derived using a voltage divider, derived from V1P8ANA from the accelerometer.

- I assumed you plan to use a 2.5 reference for the ADS1285.  Kindly let me know if this is not the case.

See Preliminary circuit below:

Questions:

1)  Do you know if the V1P8ANA from the accelerometer is able to drive the 10k-10k voltage divider? If not, I will need to add another OPAx388 buffer prior the 10k-10k divider.

2) Since the measurements are ratiometric with respect to V1P8ANA, we will need a circuit to gain up this voltage and drive the ADS1285 reference inputs for better noise performance.

This can be accomplished using another OPAx388 circuit in dual-feedback configuration to drive the ADC reference inputs and bypass capacitor.  Kindly let me know if using a ADC reference of 2.5V is acceptable; and if you want to proceed with this approach or you want to use a different ADC reference circuit on your side. 

3) I assumed that the THP210, ADS1285 and OPA2388 are powered by a 5V unipolar supply, let me know if this is acceptable or if you have a different supply in mind.

I can provide detailed simulations (and if you wish, the ADC reference drive circuit), once I get your confirmation on the questions above.

Thank you and Kind Regards,

Luis Chioye  

HI Lhagva,

I changed the front-end buffer amplifier from the OPAx388 to the OPAx187. The OPAx187 is also a chopper amplifier, with no flicker noise, but tends to be less sensitive to source impedance.

Chopper amplifiers offer very low offset drift, and no (1/f)  flicker noise. This performance is achieved through the use of an internal calibration circuit that uses MOSFET switches to commutate the inputs. However, the chopper calibration technique generates small current transients within the amplifiers input bias current. These transients will flow through the amplifiers source impedance generating very small transient noise tones.

The OPAx187 is also a chopper amplifier, but it is less sensitive to source impedance, and works without any issues with source impedances up to 500kOhms.  Since the application requires a 32kOhm +100pF low-pass filter at the accelerator output, and a voltage divider (we discussed on the post above, you may decide to adjust the voltage divider to higher impedance), Hence, I changed the buffer amplifier with the OPAx187 since this op-amp will be less sensitive to the source impedance, see table 5-1 below.  The application note below provides a more detailed explanation on chopper amplifiers.

Optimizing Chopper Amplifier Accuracy

Attached are the OPAx187 + THP210 front-end Simulation results and simulation files.

- OPAx187 + THP210 Total output noise.  The ADS1285 has a bandwidth (-3dB) of 0.413 x Fdata (due to the FIR digital filter). If the application requires a 200SPS sampling rate, the f(-3dB) BW is ~82.6Hz.  The simulated total output noise of the OPAx187 + THP210 at 82.6Hz is 1.056uVRMS (or ~6.3uVpp using a crest factor of 6x)

Modified Circuit OPA2187+THP210:

Noise Simulation Result:

- Transient Simulation:

- Small-Signal BW:

OPAx187 + THP210 TINA-TI simulation file:

THP210_OPA2187_Front_End_noise_transient_AC.TSC

- Regarding the voltage divider, you can use a 1MOhm + 1MOhm voltage divider, (assuming the accelerometer/sensor can drive this high impedance).  The total output noise of the circuit will increase to about 3uVRMS on the TINA simulation.  The OPAx187 will see a source impedance of ~500kOhms which is still acceptable (per table 5-1 at the top of this post).

- For the ADC questions, it is probably best to consult with the ADC Applications team directly by submitting a query on  the data converter forum; as they have up-to-date information of the ADC portfolio: https://e2e.ti.com/support/data-converters-group/

- I will certainly help with the Reference amplifier buffer simulations; I will look into using the OPAx187;  I will update with the reference buffer simulation soon.  I expect by Tuesday evening US time.

Thank you and Kind Regards,

Luis

HI Lhaghva,

The OPAx388 and OPAx187 chopper amplifiers are difficult to compensate driving the large REFIN ADC bypass capacitor.

A good reference drive circuit is below, using the OPA210.  The OPA210 is a bipolar input amplifier that offers very good DC accuracy and low 1/f noise.  The op-amp can work at 5V unipolar supply, but the input common-mode requires a 1.5V headroom from the supplies, which is met in the circuit below.

The circuit uses the V1P8ANA from the accelerometer, and produces a 2.5V reference to drive the ADC.

The reference circuit is stable, and offers very low noise at 58nVRMS at 82.6Hz.

Noise Simulation of OPA210 reference drive:

 Reference_drive_OPA210_Noise.TSC

Thanks,

Luis

HI Lhagva,

On PSPICE, to simulate and plot the total integrated noise, you need to use the function shown on the slides below.

See attached:

Noise PSpice-for-TI.pdf

Thank you and Best Regards,

Luis 

HI Lhaghva,

The circuit requires the R3 4.02-ohm resistor for stability. R4 (200mOhm) is optional, sometimes this resistor helps with transient response while driving the REF input on other more demanding un-buffered SAR ADC refence inputs. In this case, it is not required on the Delta-Sigma ADS1285 application. You could populate with a 0-ohm resistor or eliminate if you are concerned with area/cost. If you wish, you could consider adding an RC filter at the input, to filter any potential EMI or high-frequency noise, depending on the noise environment present in the application.

The tolerance and drift of the THP210 input and feedback resistors (R1, R2, R3, R4) needs to be selected depending on the gain error and gain temperature drift accuracy requirements in this application.  These resistors will contribute to gain error and gain error drift.  Also, the matching of the V1P8ANA voltage divider resistors will affect the accuracy 0.9V reference that tracks the V1P8ANA regulator.  For the R-C-R filter at the output and the rest of the resistors, a 0.1% tolerance 25ppm/C is typically sufficient. 

When using ceramic capacitors, choose C0G high-grade capacitors for the RC filters and feedback capacitors on the front-end signal chain. Among ceramic surface-mount capacitors, COG (NPO) ceramic capacitors provide the best capacitance precision and lowest distortion. The type of dielectric used in COG (NPO) ceramic capacitors provides the most stable electrical properties over voltage, frequency, and temperature changes.

You could estimate the initial gain error using Monte-Carlo analysis on PSPICE-for-TI. For example, on a different circuit with two separate gain stages, using 0.05% tolerance resistors at room temperature, will provide a typical (mean ±1-std deviation OR mean ±1 sigma) gain error of ~ ±0.05% (approx); and worst case (assuming ±3-sigma distribution) of ~0.15%. 

 Attached is a pdf file with a different Monte-Carlo analysis circuit example. The pdf file documents the basic procedure.

Monte-Carlo_Circuit_Example_PSPICE-for-TI.pdf

Thank you,

Kind Regards,

Luis Chioye

Hi Lhagva,

I have not tried the Monte Carlo on this specific circuit. TheTHP210+OPA210 example on the pdf file worked without issue, but it is possible that the OPA187+THP210 combination could present issues converging.

On one case, when performing an AC Monte Carlo simulation on a different amplifier circuit, I modified some of the analysis parameters to help the circuit converge: All simulations convergence parameters were set to default, except for PTRANABSTOL (1e-5) and PTRANVNTOL(1e-4) under the “AC Analysis MonteCarlo”  Simulation Profile, under “Options”, and “Bias Point”.  These changes in parameters help speed up that circuit simulation. 

On your circuit case, the simulation may be a transient simulation. Nevertheless, the PSPICE prompts on the “Output window” often provide suggestions for changes on the simulation parameters to improve, or speed up convergence. 

Thank you and Best Regards,

Luis 

Hi Lhaghva,

If you decide to use a single op-amp, consider (if possible) using wide short traces on these connections with a symmetrical layout in attempt to reduce the trace connection  resistance to a few 10s of milliohms and minimize errors on the 0.9V reference potential seen by the THP210. Each THP210 input could sink/source about ~700µA in simulation, depending of the input signal voltage level. 

The OPAx187 can drive the 1kΩ input impedance of a single THP210.  When a single buffer amp drives 3x THP210s, the amplifier will see a lower 1/3 input impedance load.  Assuming this application is for 0.9V reference, a single may drive them as long this is a very low frequency 100s Hz signal.

Thanks,

Luis