DSS w/o resistors

Fernando,

The series resistors are there to help match the trace impedances of the signals. If the impedances are not matched then you start to get reflections on the signals which can cause over/undershoot and corruption of the signals.

Having said this the requirement really depends on the signal path, trace impedances, connectors etc...

I would not expect the series resistors to be critical at lower frequencies and with short traces (implied by your space requirements).

BR,
Steve

Steve,

Have I to check trace width for 50 Ohm wave impedance like for DDR2 interfaces or this will not be so important for around 60-70 MHz? Can it replace necessity of dedicated series resistors?

Why series resistors was not recommended for HS USB PHY interface where frequencies are similar?

As Steve said, the resistors are to absorb reflections. This is known as series termination.  If the buffers of the chip are matched with the trace impedance they are not needed, but generally the chip buffers have a much lower impedance than the traces.

To avoid using resistors you can do two things.  First, you can make the traces really short.  For trace lengths less than the length where they are considered "lumped" loads (as defined by PCB high speed experts like Howard Johnson, Eric Bogatin, etc.) then resistances are not required.  Second, you can widen the traces or lower the height from the ground plane so they are on the lower side of the normal impedance required.  45 ohms or lower is what I'd recommend for this.

For 60-70 MHz operation I don't expect the resistors to be that important, but the trace impedance should be on the low side as mentioned above.

If you keep the trace length as short as possible and you are running 60-70 MHz with ~45 ohm traces, I don't think you'll run into trouble, however sometimes the lack of series resistors makes it difficult to tune the circuit if you have EMI requirements should it not pass the first time.

The USB phy has it's own special buffers (and input loads when receiving) that are very different from the buffers in other interfaces.  They are more like limited current sources rather than voltage driving buffers that normal interfaces like DDR etc. has.

I have traces from 11 to 35 mm. With generaly 0.1 mm clearance between each other. All are around 50 Ohm. Can I avoid resistors in this case?

The best way to check this is through simulation. TI provide an IBIS model for the processor and you'll need an IBIS model for whatever you are connecting to. If you specify 50 ohm trace impedance to your PCB manufacturer and run simulations of the board with 45, 50 and 55 ohm trace impedance you should get some idea of how the design will work (or not work). Once you are happy with the simulation and get the board manufactured according to the simulation results you need to check that real life corresponds with the simulation.

Unless I'd seen another design without the series termination I would not just remove it without simulating it first. A safer option would be to change the PCB technology to something like Blind and Buried vias (unless you are already using them) to increase the available real estate so you could add in the termination.

Regards

Andy

For 60-70 MHz, this should be O.K., but I would lower the impedance to closer to 45 ohms to reduce EMI and enhance signal integrity.  It should work either way, but lowering the impedance will help.

Keven