If you have up to 16 differential line pairs and you have to go through a connector to terminate the differential signals on a daughter card, what is the best signal to gnd ratio and pattern one should consider?
In this case the connector is a high density pin connector. If the differential impedance is 100 ohms do I need a special Ground pattern, as the signals go through the connector, to maintain the differential impedance close to 100 ohms?
Thanks for your interest in high-speed digital design.
Regarding your correspondence, there is no general formula for the number of grounds required, as it depends on the spacing and sizes of the connector pins, and how they are bent.
Here are a few general rules you may want to consider.
Put the two elements of each differential pair on the same row of the connector. That will ensure that they get the same pin lengths, and go through the same pattern of elbow bends.
On a synchronous bus, if you have enough time to wait for the crosstalk to settle, you may not need to isolate the differential pairs from each other.
If isolation between pairs is required (for a good, low-crosstalk bus or for a clock or asynchronous interrupt signal), place the pairs so they are never adjacent to any other pair. (This implies that you will be using AT LEAST as many grounds as signal pins to separate the pairs, and probably more.)
The differential impedance of most open-pin-field connectors is probably going to be a little higher than you want. You can measure this. You will need a pair of test boards on which you can mate the connector halves. The boards don't use any traces. They can be solid copper with holes drilled for the connector pins. Ground all the pins that will be grounded in your application. Use two RG- 174 50-ohm coax cables to route a differential, 100- ohm signal into the designated signal pin pair. Let this signal go through the connector to the far side. On the far side, terminate the signal differentially with 100 ohms.
For any signal speed that will work with an open- pin-field connector you will find that a 1/8th watt axial 100-ohm resistor works fine as a terminator.
Blast in a differential signal from your 100-ohm source. Make a record of the resulting waveform AS MEASURED AT THE SOURCE. This should show the source waveform going out, and a first reflection coming back (you've made a crude TDR instrument). Use a step risetime commensurate with what you are going to be using in the real system.
Don't mess around with fancy 35-ps step edges. They will just show you a bunch of fine-structure detail that isn't going to matter in the real system.
Now disconnect the coax cables from the connector. Place the 100-ohm termination directly across the coaxial cable outputs, with the coaxial grounds tied together. Repeat the measurement. You should (ideally) see no reflection.
Looking at the difference between the first measurement and the second, if the reflected waveform bumps up in the positive direction (same polarity as the step input), the connector impedance is a little too high. If it bumps negative, the connector impedance is too low.
Adding more ground pins around the signal pair lowers the impedance.
Spacing the signal pins further away from ground raises the impedance.
Adding a little lumped-element capacitance from signal to ground on each side will lower the effective impedance. This may be implemented in the PCB layout by just using larger- than-normal via pads. Experimentation and re- measurement is required to get this idea to work. The 'big-pad' concept works when the connector through-delay is less than 1/6th of the signal risetime, and the connector is acting like a lumped- element inductor (too high an impedance).
Thanks for taking the time to write.
Dr. Howard Johnson