Just wondering what these characters are doing:
http://ww1.microchip.com/downloads/en/DeviceDoc/103-00398-R2.pdfThey put 100 ohm resistors on all the digital signals, and 10 ohms on the power rails. I've never seen that before. Would be nice to know that I can safely ignore that before I send the gerbers to the board house...
Limiting maximum current to prevent gross overloads? 100 ohm 3.3V comes to 33mA. Don't forget you can always populate the 0603 pads with 0-ohm (zero) resistors if it doesn't function as it should be.
Are the traces long (or, if before PCB layout, expected to be)? Series resistors are very common as source termination (assuming the resistors are each placed closest to the output driver pin on that node), reducing ringing on long traces without having to pay attention to signal quality (assuming the logic thresholds are relatively high, and the bitrate low, which should be fine for a 3.3V CMOS chip in the low MHz, like that).
Tim
On the power lines, they form an RC filter with the decoupling capacitors, isolating the power rail from the chip's transients (and likewise providing some additional power filtering). This is commonly done for low or constant quiescent current devices with an appropriately sized resistor; ferrites are also often used to similar effect.
This is a 24-bit DAC, noise considerations really matter and it looks like that's what they're targeting here, trying to slow down the digital edges and keep the digital transient currents off the power rail where it can affect the analog frontend.
They limit unwanted ringing caused by parasitic inductance of the traces and parasitic capacitance of pcb and receiving end of the line. They also limit higher frequency components from square wave, which reduces interferences to other parts of the circuit.
Not all chips are forgiving of I/O shorts, so yeah, my guess would be protection from misconfiguration inputs as outputs and shorts.
Shouldn't noon obvious design decision like this be documented on the schema? This is what I do when I write software.
The MCP3911 is specified as a high-speed SPI device with data rates of up to 25 MHz. At these frequencies you need to terminate the data and clock lines or otherwise you will get problems with reflections.
I tried to find some general source to share here on the concept - the best I could find was this technical document from Fairchild:
http://www.fairchildsemi.com/an/AN/AN-610.pdfWhat the schematics doesn't tell you is that the resistors need to be placed close to the source of the respective signal to be effective...
They limit unwanted ringing caused by parasitic inductance of the traces and parasitic capacitance of pcb and receiving end of the line. They also limit higher frequency components from square wave, which reduces interferences to other parts of the circuit.
this is a good explanation.
in digital audio, its very common to see small valued (50 or 200) ohms as series R elements from the clock and data lines going to a dac or i2s transmitter.
it does not have to be 'documented' on the schematic since most digital designers will see that and immediately know what they are there for. its very common.
its not about limiting current; its about reducing ringing.
Most excellent, signal integrity makes perfect sense. Thanks everyone.
Now to wiggle out some room to scatter a bunch of 0603s... So long tight layout!
You can always use resistor arrays.
on very tiny dac modules, they certainly do use arrays. I opened a FIO dac (spdif in or usb in, I forget; and analog out) and on its i2s lines went 3 traces thru a small chip that I'm sure was an R network. its where I tapped in, just to go to my own dac (using this as a receiver).
when I wired things up without resistors (just haywire, airwired or quick perf boarding) and left out resistors, things went ok. but its good design practice and if you look at the wave, I'm sure you will see a before/after that is obvious. some circuits care less, but that's beside the point, right?
Most excellent, signal integrity makes perfect sense. Thanks everyone.
Now to wiggle out some room to scatter a bunch of 0603s... So long tight layout!
As source termination resistors for signal integrity, then they should really be located as close as possible to the driver output pins.
I notice they have them on inputs *and* outputs. That, and the fact that the values are a bit high for termination resistors tells me it's more about noise suppression than series termination. They are probably trying to limit edge/transient currents into the IC, so as not to corrupt measurements of the input signal by developing transient voltages on the IC's internal ground reference.
Usually, when series terminating a PCB transmission line (trace), you'd add them at the source, or at the destination, but not both. Also, MOS outputs have typical output impedance of around 10-20 ohms. If you add that to the 100 ohms, then the traces would need to have a 110-120 ohm characteristic impedance for these to be proper termination values. That would be a *very* narrow trace, and/or a *very* thick dielectric layer. Typical traces are in the 50-75 ohm range, so series terminators are usually in the 30-50 ohm range (taking into account MOS output impedance).
Well... the resistors don't HAVE to be physically placed beside the chip, like they are in the schematic...
Tim