I am working on Fluid Level Detection using Texas Instruments MSP430L092 Mixed Signal Microcontroller with Texas Instruments TDC1000 AFE. They are connected via SPI Bus and in its datasheet there is reference PCB design, as seen in screenshot: Recommended PCB Design for TDC1000 As you can see, there are resistors placed in SPI Bus and regarding them I have following question:

  1. What is their purpose?
  2. What is their recommended type?
  3. What is their recommended value?

The resistors on the SPI bus are placed in a manner where they are located close to the source driver of the trace. In case of the SPI bus here one of the drivers (SDO) is located in the TDC1000 whilst the others are in the master device. The three resistors for the master belong over close to the master driver outputs.

These resistors are used to match the driver output impedance to the trace impedance so as to optimize the signal integrity of the waveform. As a rule of thumb the value of the resistor plus the actual output impedance of the driver should be equal to the trace impedance. Typical resistor values could range from 10 ohms to 50 ohms. That said there could be requirement for different values based upon the actual trace impedance and the routing topology. Trace impedance is determined by trace width, board stackup definition and adjacency to other traces. The resistor is typically selected to minimize reflections on the trace and limit ringing at the signal edges. At the same time trying to ensure that edge transitions are smooth and monotonic.

Small physical size resistors of the SMT type are the most ideal type of resistor to use for these. They eliminate the need for extra vias and through holes. I find that the 0402 size work well as a trade off with the modern pin pitch on packages and the typical artwork design rules used today. The really ideal situation is to have the connection from the driver to the resistor be short and without any intervening vias.

  • \$\begingroup\$ Ok, but I've checked out some other schematics like Better SPI Bus Design in 3 Steps and according to this webpage I also must add pull-up resistor to Chip Select Line and pull-up/pull-down resistor pairs on MISO Line. Are these resistors also a strong recommendation? \$\endgroup\$ – KernelPanic Mar 20 '16 at 11:18
  • 2
    \$\begingroup\$ I answered your questions relative to the diagram that you placed into the posting you made. The other things you are looking at are really out of scope for my answer. A ChipSel pullup resistor may be needed when the driver is an Open Drain type connection. Pull-Up and Pull-Down resistors on MISO would presumably be placed at the master for destination termination of the line for in cases where the slave SPI bus does not have the series back-match termination at its driver. Under most cases of reasonably short traces it is not necessary to have both types of terminations on a line. \$\endgroup\$ – Michael Karas Mar 20 '16 at 11:29
  • \$\begingroup\$ A chip select pull up resistor would not be needed if the driver of the signal is able to pull the CS line high quickly. If the driver is a weak one or an open drain type then it can take a long time for the signal to go high. Most SPI devices will reset their SPI interfaces when the CS line goes high. This is often needed between transactions to ensure that the interface is fully re-initialized for the next transaction. If it takes a long time for the signal to go to a valid high level then the device may not be reset when the next transaction is started. The pullup speeds the rise time. \$\endgroup\$ – Michael Karas Mar 20 '16 at 11:47

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.