Connect with us

Why Are There No Right Angle Traces?

Discussion in 'General Electronics' started by BM, Jun 27, 2003.

  1. BM

    BM Guest

    I was told the other day that there are no right angle traces on PCBs (the
    traces go to something like 45 degrees between perpendicular traces) because
    of something to do with something or other. Could something please explain
    this or point me to some resources so I can book up.

    Thanks

    -BM
     
  2. My guess is that it has to do sharp edges (right angles) radiate at high
    frequencies.

    Charles Perry P.E.
     
  3. John Larkin

    John Larkin Guest

    It's mainly a stylistic thing nowadays. Once upon a time, Mil Specs
    prohibited right angles on the theory that the traces might peel
    easier; that's not an issue with modern decent PCB material. People
    also cite resolution losses or contamination buildup in the corner,
    which aren't really problems these days either. The oft-cited claim
    that fast signals don't turn corners well is not an issue below maybe
    5 GHz.

    Dense ("memory") routing can be impossible using right angles, where
    it's a lot easier with diagonals.

    So do it if you like the way it looks. Most professional layout people
    don't. There are a lot of style issues in PCB layout.

    John
     
  4. Al

    Al Guest

    The metallization has a different coefficient of expansion from the PCB
    material. Sharp corners introduce stress risers. Most of the time it
    doesn't matter.

    Al
     
  5. There used to be a significant undercutting issue in right angle bends.
    This could be reduced by mettal filling unused areas or by avoiding
    right angle bends or both. In modern board processing, I rarely see
    undercutting anywhere. BTW, the same difficulty exists in some IC
    processes and metal fill is used to reduce the problem.

    Chuck
     
  6. John Larkin

    John Larkin Guest

    Well, it is if "above 180 MHz" means "way, way above 180 MHz". I've
    scoped test boards with a 20 GHz TDR system, and right angles are just
    tiny blips; vias are a much bigger abberation.

    John
     
  7. Tom Grqyson

    Tom Grqyson Guest

    I was told the other day that there are no right angle traces on PCBs (the
    That was a good question
    Thanks for asking because I also wondered the same thing
     
  8. Ben Bradley

    Ben Bradley Guest

    In sci.electronics.design, "BM"
    I see lots of good answers, but the reason I recall hearing many
    years ago is that the outer corner could have some 'flash' on it, a
    thin line of copper that didn't get etched off, that extends from the
    corner to connect to another trace. Now that I think about it, it
    sounds like BS to me, but it points out another more legitimate
    (-sounding) reason:
    If a trace has high voltage on it, there will be a high
    concentration of voltage potential at a sharp (90 degree) corner
    (think of electric lines of force extending out, much like magnetic
    lines of force from a magnet. Lines will hit the edges of the
    conductors in many places, but many lines will meet at one point: the
    corner). This can cause problems with corona discharge, dust
    collection and such, eventually causing arcing to another trace. A
    less-sharp angle (such as the 'standard' 45 degrees) won't have as
    high a concentration of potential for the same voltage, and so will
    have less of a problem.
    Furthermore, 45-degree angles just "look a lot more professional"
    than 90-degree angles.
     

  9. If ESD sparks between isolated circuit sections are an issue, then
    sharp corners cause problems. Where a 0.1" separation between
    parallel traces might ordinarily give plenty of hi-volt isolation,
    you'd better double it or triple it if one trace has a very sharp
    bend or if a ground plane has a 90deg corner. No room on the board?
    Then use nice shallow bends on any neighboring traces which experience
    high-volt pulses.

    This is a big issue in phone line interfaces. ALso in tiny industrial
    sensors where 120VAC and comm lines are adjacent, and are also right
    next to the analog front end... and all must survive for years in an
    environment with rubber conveyor belts travelling across nylon drive
    rollers.


    (((((((((((((((((( ( ( ( ( (O) ) ) ) ) )))))))))))))))))))
    William J. Beaty http://staff.washington.edu/wbeaty/
    Research Engineer
    UW Chem Dept, Bagley Hall RM74
    206-543-6195 Box 351700, Seattle, WA 98195-1700
     
  10. EEng

    EEng Guest

    Yes, in high speed circuits vias are indeed the bigger problem for
    signal reflection. As far as what frequency does signal reflection
    become a problem....this is dependant on trace width, weight of
    copper, through board configuration, trace length between bends, board
    material, and many MANY other factors that all tie in....however it is
    accepted without explanation that as a general rule of thumb 180MHz
    signals along a 1mil trace of 1/2oz copper (not realistic for layout)
    is the MINIMUM frequency at which signal reflection becomes a
    problem.. This then is used as a base line reference to guesstimate
    the most likely reflection problems i.e., 2mil traces/360MHz,
    4mil/720MHz and so on so that 10mil traces show significant right
    angle signal reflection beginning somewhere in the 1.8GHz range.
    Again, this is an ideal dependant on many factors but a good rule of
    thumb for designers. Personally, I only use 45s and curved traces
    regardless what I'm working on. Vias are a whole 'nuther issue.
    Blind vias tend to create the most problems.
     
  11. Robert Baer

    Robert Baer Guest

    To begin with, a large majority of PCBs in "consumer electronics" are
    made with right angle transitions.
    Curved or 45 degree transistions become necessary near microwave
    frequencies.
    As a circuit operates at frequencies above (say) 1GHz, these
    transitions become more useful.
    Essentially any abrupt transistion in wire (trace) size and/or
    curvature can give problems.
    "Abrupt transistion" is (to paraphrase Einstein) relative - on the
    wavelength as compared to the transition.
    Just consider the trace to be a transmission line and the why and
    wherefore become more clear.
     
  12. John Larkin

    John Larkin Guest


    At 180 MHz, wavelength is around 2 meters, a bit less inside a PCB. A
    corner bend of a 1 mil trace is then 1/80000 of a wavelength wide,
    which is absolutely inconsequential.

    In FR4, 50 ohm microstrip, 5 GHz range, the fiberglass weave shows up
    on TDR more than corners do.

    Your scaling rule - that wider traces show corner effects at higher
    frequencies - is backwards.

    I don't use right angles - except on very fat power traces - because I
    don't like the way they look. But that's the only reason.

    John
     
  13. onestone

    onestone Guest

    It's because they can't see where they're going!

    Al
     
  14. DarkMatter

    DarkMatter Guest

    Not really. Pretty much every layout person I ever knew avoids
    them, even on low frequency switching designs. I have not seen a
    right angle laid out in quite a few decades.
     
  15. onestone

    onestone Guest


    Nearly right! The ones on the outside of any corner have to travel
    faster than the ones on the inside. If the corner is 45 degrees or less
    this is OK, since the outside ones don't have to travel faster than C
    unless the track is wider than 100mils. But the transition is so sharp
    on a right angle corner that the outside ones have to break the C
    barrier on any track wider than 6 mils. The problem is that this is no
    longer legal, having been banned by Albert E. Thus the outside electrons
    are forced to crowd the inner lanes. Since they have already been
    accelerated more than the inner electrons they carry more inertia, and
    it's actually the inside electrons that get bumped. They then scramble
    around to the other side of the track and try to jump back on, hence the
    illusion that they have slipped from the outer edge.

    Al
     
  16. DarkMatter

    DarkMatter Guest


    Then, there is all that heat, generated from the hustle and the
    bustle.
     
  17. Jim Thompson

    Jim Thompson Guest

    Not quite ;-) But current crowding does occur in corners. There was
    a paper by Jim Dunkley on this subject, rigorously deriving the
    current density in corners, clear back in the mid 1960's.

    ...Jim Thompson
     
  18. DarkMatter

    DarkMatter Guest

    Very true, but for some circuits, even at low frequencies, it makes
    a difference. I will attempt to illustrate why the details matter in
    electronics with a couple examples. One directly topic related, and
    one closely related, but more toward workmanship in the industry.

    Take a small HV supply, and lay out two PCBs, one with right angle
    traces, and one with curved transitions or 45s utilized. Both PCB
    assemblies get potted, so corona at the corners will not be an issue
    here.

    Testing the two boards will indicate noise characteristics in the 90
    degree PCB that are greater in amplitude than the other two PCB
    choices for the second board.

    The reason is crosstalk. Another would be trace path lengths.

    Either way, the 90 degree board will exhibit poorer, noisier
    performance. If it is a regulated circuit, the likelihood of that
    noise getting injected into the control loop(s) of the circuit are
    high, causing poorer operation.

    Another example of why the details matter:

    A tester could not determine why he had higher leakage currents on
    an assembly after it was potted than before.

    Our chief engineer said "That's easy... Clean the board."

    The guy couldn't believe it. I said that so much as breathing
    "coffee breath" onto an HV assembly can cause failure modes and
    particularly leakage (I learned it from the master tho). After
    utilizing a vapor phase degreasing method for cleaning the unit in
    question, the leakage currents read pre and post pot were reported by
    him to be identical. He was "flabbergasted" (whatever/wherever that
    comes from). I knew it, as I too didn't believe them to be so
    sensitive some years back in my early HV realm experiences.

    It is always important to clean PCB assemblies that involve high
    impedance control or monitoring loops as it is quite easy to introduce
    stray flows into places where they are not desired. Merely touching a
    1G Ohm resistor with one's finger will render it useless.

    SMD assemblies are of particular importance in control loops. Make
    sure any resistor changes are followed by thorough spot cleaning with
    a dabber, then a solvent, then forced air. One can spend hours trying
    different value resistors, wondering why the math isn't working.

    One only wants the electrons to flow in only the desired places, and
    only in the desired ways. :-] *THEN* the math works... (mostly).

    Anyway, today's PCB plot methods use round spots such that corners
    even at right angles have a radius on the outside edge that matches
    the trace width usually. 90 degree corners would probably not suffer
    the same etch process problems, but would most assuredly still posses
    many of the electrical gremlins associated with such structural shapes
    where current flow is concerned.

    I have taken the time to lay out boards with curved transitions all
    around, yet still following the shortened path 45 methods for the most
    part. Absolutely no sharp inside or outside corners were on it
    though.

    Great for HV stuff. Don't forget to "Bump Solder" all of your cap
    and diode nodes on your HV multiplier boards! Round solder ball
    shapes are a good thing. :-]
     
  19. John Larkin

    John Larkin Guest

    NASA insisted on it, at least for the stuff on Saturn V. They were
    concerned about tape creeping or peeling. It was amazingly tedious,
    worse than tape-on-mylar if you can imagine that. Everything was
    nicely curved and filletted, too.

    What a pain. I still like to draw schematics with a Berol Turquoise on
    vellum (then I let the kids CAD it for me) but I'll never get
    nostalgic about taping boards. I remember two, three weeks of leaning
    over a hot light table, holding my breath every time I had to lay a
    line between two IC pads. I remember discovering that we'd have to
    move a whole section left 150 mils. I love PADS... I can slouch in my
    chair, latte in one hand and mouse in the other.

    John
     
Ask a Question

Want to reply to this thread or ask your own question?

You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day

-