Zig-Zagged Traces on PCBs

Discussion in 'General Electronics Chat' started by TrevorP, Mar 26, 2010.

  1. TrevorP

    Thread Starter Active Member

    Dec 8, 2006
    55
    0
    I'm currently working on a PCB for work so in an attempt to learn the best techniques/tricks I was looking at an old (2001) video card. One thing I noticed was there is a lot of little zig-zagged traces. I'm just wondering why someone would do that? My guess is it increases the length of the trace, thus increasing capacitance with the ground plane, as well as resistance. So would this be used for a low current DC line? Or maybe is it some sort of noise removal technique?

    There is a whole bunch of them on the left side of this image: http://www.smye-holland.com/SmyeHolland_ImageLibrary/Copy of Printed circuit board.jpg

    Thanks,

    Trevor
     
  2. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    The zig-zags can be used to match the lengths of a data bus so they all have approximately the same length.

    When you're dealing with a high-speed data buss, it's important that all data bits arrive at the same time. If you match the propagation delays for all of the bits, your chances of achieving that increases dramatically.
     
    Last edited: Mar 27, 2010
    TrevorP likes this.
  3. TrevorP

    Thread Starter Active Member

    Dec 8, 2006
    55
    0
    Wow. That's awesome. Thanks!
     
  4. kkazem

    Active Member

    Jul 23, 2009
    160
    26
    Hi,

    I've got to disagree with the SGT here. If you have a ground plane under the trace and zig-zag it, you are increasing both the trace inductance and capacitance to ground at the same time. That's called a transmission-line and has nearly constant impedance, depending on the trace width and other factors. Also, it usually isn't critical to have all data bits arrive at the same time. The datasheets for any uProcessor or other similar chip have a setup-time where the data must be valid by a certain period of time with respect to the clock, and then the data read line gets pulsed.
    There could be a lot of reasons for zig-zagged traces, not the least of which is getting the last 10% of connections hooked-up which takes 90% of the time. And it gets worse the more dense the board is. It also could be microstrip inductors or perhaps the layout guy wasn't very experienced. It is certainly not sometime to strive for in a layout except for a few very good reasons and should in general be minimized.

    Regards.
    Kamran Kazem
     
  5. rjenkins

    AAC Fanatic!

    Nov 6, 2005
    1,015
    69
    The zigzag tracks are very specifically delay sections.

    The zigzag does not increase the inductance particularly as the alternate reverses in direction cancel out the magnetic field. (look up designs of 'non-inductive resistors' if you doubt this).

    The frequency limit on a wide (ie. 32 bit) bus is largely down to how accurately the timing spread over all the data lines can be controlled.

    (That's why peripheral i/o is shifting toward serial busses like PCI Express & SATA, as each interface deals with a single signal that does not have to be checked or timed against any other signal.)

    If you look where the zigzags are, you will usually find they are in the tracks that would otherwise be the shortest of a group & the zigzag brings them to equal electrical length.
     
  6. R!f@@

    AAC Fanatic!

    Apr 2, 2009
    8,754
    760
    U know what. I also wondered about the zig zag.
    I have to disagree with Kazem partially.
    It's not connected with the one who traced that particular PCB.
    I have seen this on plenty of mobo's.
    So that means zig zagging is important feature in HF applications.

    I really donno why the traces a zig zaged, but I pretty much like to know
     
  7. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    I sit corrected.

    The reason for the zigzags is so that the lengths of all the traces in the data bus are the same; not the impedance.

    I halfway got that crossed up with another post.
     
  8. kubeek

    AAC Fanatic!

    Sep 20, 2005
    4,670
    804
    I bet that over the left border of the picture sits a memory bank. The speed the memory bus is operating makes these delay adjustments pretty important in the overall design of the card.
     
  9. Darren Holdstock

    Active Member

    Feb 10, 2009
    262
    11
    There's another reason for wiggling tracks, and that's to increase the EMC performance of the circuit. rjenkins quite correctly pointed out that the conductor doubling-back on itself cancels out any inductance created by the winding, but here the secret is in the corners. A sharp bend in a PCB track increases the local inductance of that section by squashing all the flux lines together. Adding some corners in a PCB track is a free way of attenuating high-frequency noise, and is particularly effective at very high frequencies where discrete inductors are less effective due to higher parasitic self-capacitance of their windings and limitations of the core material.

    An even more effective method is a square spiral going to a through-hole component leg or a via, as this also has a bit more inductance from its wound nature. Effective, but often inconvenient, so they're not often seen.

    And as SgtWookie stated, meandering PCB tracks are often used to equalise clock and data lines to prevent skew, or to add a bit of free delay if that's needed for reasons of timing. As a rough rule of thumb, a foot (30 cm) of wiring adds a 1 ns delay.

    I'm not sure why the PCB of the OP has these traces. It could be for EMC reasons, in which case the corners could be squarer and more numerous for better effect, or it could be for timing equalisation, in which case the traces look a bit too 'organic' to be carefully determined lengths as they fill the available gaps a bit too neatly.
     
  10. elliott614

    New Member

    Jan 4, 2016
    1
    0
    Also, on high-speed data lines, there is an effect from the glass weave that creates skew imbalances. Zig zagging can average the skew between the differential lines to be similar, rather than two straight traces that could be half the glass weave pitch apart, causing potentially a 180 degree phase difference between the two. http://www.oldfriend.url.tw/HFSS/PCB Glass Weave Effect.htm (there's some pictures there)

    The picture at the beginning of the thread is gone, but I'm assuming the zig-zagging was something like what's shown here: http://techdocs.altium.com/display/ADOH/Tuning+Route+Lengths
    That shows just how easy design tools make this. The purpose (as explained in the link) is to control both impedance and (moreso) timing. Even though it was said earlier by somebody else that the signals don't necessarily have to arrive at the same time, if they arrive too differently, your opportunity window of all the bits being correct at the same time gets smaller and smaller. So they really do need to arrive at the same time, since the signals are constantly changing from one bit to the next.
     
  11. dl324

    Distinguished Member

    Mar 30, 2015
    3,250
    626
    Your inaugural post. Welcome to AAC @elliott614!

    Normally I chastise posters who resurrect old threads, but yours is one of the exceptions. Be mindful of the warning that pops up on old threads though; necroposting is generally discouraged because the OP has likely moved on.
     
Loading...