0
\$\begingroup\$

I'm trying to figure out how to correctly connect 200MHz LVDS oscillator (DSC1103CE1-200.0000T Datasheet) to ICE40LP1K-QN84 FPGA. After reading Lattice's guide to differential signals (Link) this is the routing I've come up with.Current routing CLK_N and CLK_P are connected to IOL_6A and IOL_6B_GBIN7 respectively as recommended in the guide. They are also connected through 100 Ohm resistor (R6). Due to the manufacturing limitations I'm unable to breakout double row QFN-84 package on the single layer, that is why I've routed the signals on the bottom layer.

I would like to know if my routing is acceptable or not. Should I also length-match these two clock inputs? Right now they are 5.39mm and 4.65mm.

Thanks for any advice, it's much appreciated.

\$\endgroup\$
8
  • \$\begingroup\$ I'd try to length match. Possibly loop in towards the via's from the top left diagonal and split out (so that it is symmetrical) \$\endgroup\$ May 9, 2017 at 21:04
  • 1
    \$\begingroup\$ Although to be fair for 6mm of trace you are looking at <lambda/16 for a 200MHz clock (up to 7th harmonic) - transmission line affects are pretty negligible, so I imagine it will work absolutely fine. \$\endgroup\$ May 9, 2017 at 21:07
  • \$\begingroup\$ @TomCarpenter, that is the recommended layout (latticesemi.com/~/media/LatticeSemi/Documents/ApplicationNotes/…). The only other place I could move these two vias is the center of landing pad, which I would rather not do. Besides, it would make little difference. I can try looping it from the left diagonal, thank you! \$\endgroup\$
    – Lee Brown
    May 9, 2017 at 21:15
  • \$\begingroup\$ That's fine, couldn't tell if there would be space. I agree about not sticking the vias in the centre of the pad. \$\endgroup\$ May 9, 2017 at 21:21
  • \$\begingroup\$ What is track width to gap to gnd plane ratio, thus Zo? If. no gnd plane then interleaved gnd with a design for differential impedance coplanar tracks. Multiple micro bias can reduce inductance, but generally poor for Zo \$\endgroup\$ May 9, 2017 at 22:00

1 Answer 1

2
\$\begingroup\$

Signal Critical Length

How long a PCB Trace can be before we MUST pay attention to Impedance Control.

Function of Frequency (1/16th Wavelength)

\$ l_{critical} = \frac {c}{f} * \frac{1}{ 16* \sqrt{ε_{eff}}} \$

example

  • At 1 GHz = approx .425” = 10.8mm (Microstrip- FR4)

  • At 1 GHz = approx .375” = 9.5 mm (Stripline - FR4)

- since rise time BW (-3dB)= 3 /Tr for 10~90%

  • and your 200MHz clock has rise time 0.2ns , BW = 15GHz

However your impedance is not controlled so one can only guess how many cycles of ringing will occur if the tracks were several hundred ohms reactance The Q can be determined and then amount of overshoot/undershoot.

If the undershoot crosses gate threshold then that gate will experience jitter of about 10~20% on the edge of that gate. If undershoot ringing did not reach Vss/2 then no possible edge jitter would occur.

Your design needs more care in Zo design as it is marginally ok, but I would need a 3D model of the clock path with more details.

So all I can say is it is marginal.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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