Maker Pro
Maker Pro

Why Are There No Right Angle Traces?

B

BM

Jan 1, 1970
0
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
 
C

Charles Perry

Jan 1, 1970
0
BM said:
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

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

Charles Perry P.E.
 
J

John Larkin

Jan 1, 1970
0
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

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
 
A

Al

Jan 1, 1970
0
BM said:
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

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
 
C

Chuck Simmons

Jan 1, 1970
0
BM said:
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.

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
 
J

John Larkin

Jan 1, 1970
0
This is the correct answer!

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
 
T

Tom Grqyson

Jan 1, 1970
0
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.
That was a good question
Thanks for asking because I also wondered the same thing
 
B

Ben Bradley

Jan 1, 1970
0
In sci.electronics.design, "BM"
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.

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.
 
W

William J. Beaty

Jan 1, 1970
0
BM said:
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.


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/
[email protected] Research Engineer
[email protected] UW Chem Dept, Bagley Hall RM74
206-543-6195 Box 351700, Seattle, WA 98195-1700
 
E

EEng

Jan 1, 1970
0
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
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.
 
R

Robert Baer

Jan 1, 1970
0
BM said:
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

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.
 
J

John Larkin

Jan 1, 1970
0
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.


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
 
O

onestone

Jan 1, 1970
0
EEng said:
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.

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

Al
 
D

DarkMatter

Jan 1, 1970
0
To begin with, a large majority of PCBs in "consumer electronics" are
made with right angle transitions.

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.
 
O

onestone

Jan 1, 1970
0
R. Steve Walz said:
------------
Because the electrons slide off the copper if they take the corners
too fast! ;-> No, it's because chemical etching rounds off sharp
corners quite destructively, as it presents more side of the trace
to the etchant per lineal than a rounded one does.


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
 
D

DarkMatter

Jan 1, 1970
0
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.


Then, there is all that heat, generated from the hustle and the
bustle.
 
J

Jim Thompson

Jan 1, 1970
0
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

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
 
D

DarkMatter

Jan 1, 1970
0
People tend to be lazy when judging something a PCB technically, so they go
for the appearance. An aesthetically pleasing PCB gives the impression that
who ever layed it out is intelligent enough to lay it out correctly.
Jason

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. :-]
 
J

John Larkin

Jan 1, 1970
0
This an old thread but I can't resist adding my 2 cents.

1. Don't know about when they did PCB artwork with Pen and Ink,

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.

2. When laying out a PCB using moderate to high voltage, the last thing
you wanted was a sharp point or corner in your artwork "unless" you
desired to create a spark gap.

3. It made for ugly artwork

4. In the old days when you hand taped an artwork, it usually took two
people to check the artwork for errors. One would read the schametic and
one would verify traces went to the correct points. Tracing nested
square corners was very hard on the eyes.

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
 
Top