Re: [SI-LIST] : Multi-drop backplane trace, with Z0=50 ohms - but my TDR says 40 ohms (fwd)

About this list Date view Thread view Subject view Author view

From: David Instone ([email protected])
Date: Mon Feb 19 2001 - 05:51:31 PST

Comments embedded below


Dave Instone. Compliance Engineer Storage Systems Development, MP24/22 Xyratex, Langstone Rd., Havant, Hampshire, P09 1SA, UK. Tel: +44 (0)23-92-496862 (direct line) Fax: +44 (0)23-92-496014 Tel: +44 (0)23-92-496000

Salvador Aguinaga jr wrote: > > Subject: Multi-drop backplane trace, with Z0=50 ohms - but my TDR says 40 ohms > > Hello All, > > A backplane trace that was designed to have a characteristic impedance of > 50 ohms registers at 40 ohms when I measure it with a TDR scope. Clearly > it's the capacitance of the equally spaced vias (or pin holes) that is > lowering the > impedance of the trace. Or, is it that the trace between two slots is so > short that the TDR cannot resolve the actual impedance of the trace from > slot to slot? If you can't see the individual dips in impedance at each via then: The risetime of the TDR pulse is too big. However, if you are using a TDR risetime equal to the shortest risetime of the signal that will actually use the trace, or you're maths filtering the TDR display to simulate that risetime, then in both those cases what you see on the TDR is what your signal will see.

If you want to see the tracks between the vias then you must use a shorter risetime TDR pulse. Generally the TDR risetime must be shorter than the flight time between vias (and other discontinuities).

> > Taking a step back, the impedance coupons on this board say that the trace > with x width should be 50 ohms. However, this impedance test coupon only > has vias (or pin holes) at each end of the trace. So, naturally the > impedance registers at 50 ohms. But, as I mentioned before, on a real > application the trace is going to have pin holes at every slot.

True, but also coupons tend to be on the edge of PCBs. Traces/coupons at the edges of boards tend to get etched more than traces near the center of the board. Therefore the traces on the board read lower, (they are physically wider). However a 10 ohm difference is a bit big unless your traces are narrow to start with. Variations in solder mask thicknesses of only a few 10ths of a mil can cause a difference also, but again only in the order of a couple of ohms. So yes I would think it is the vias that's causing the drop. > > If I absolutely have to have a 50 ohm trace, should I increase the > impedance of the traces between slots to compensate for the added > capacitance of the via? YES > Or should one reduce the parasitic capacitance of > the via, by reasonably increasing the anti-pads on internal layers? ALSO YES > And, > no I can't make the backlane any thinner! > > Please, let me know what your thoughts are on this, especially if you'd > ran into similar situation. > > Thanks a lot! > > -- Sal

**** To unsubscribe from si-list or si-list-digest: send e-mail to [email protected] In the BODY of message put: UNSUBSCRIBE si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP. si-list archives are accessible at ****

About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:30:53 PDT