Why Are There No Right Angle Traces?

[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.

Thanks

-BM

 

[Charles Perry]

"BM" <brandon(underscore)melland@hotmail.com> wrote in message
news:1L0La.1667$7e.1222@nwrddc04.gnilink.net...

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.

 

[John Larkin]

On Fri, 27 Jun 2003 19:17:17 GMT, "BM"
<brandon(underscore)melland@hotmail.com> wrote:

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

 

[Al]

In article <1L0La.1667$7e.1222@nwrddc04.gnilink.net>,
"BM" <brandon(underscore)melland@hotmail.com> wrote:

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

--

Reverse address to reply.

 

[C what I mean]

This is the correct answer!

--
Conquip/Logic Systems, Inc.
Ph: (916) 387-5661
Fx: (916) 386-1730
www.lsione.com
www.conquipinc.com
"EEng" <unmaileeng@budget.net> wrote in message
news:i4cpfvcgco450c84mhn1vt1gubnejsfig4@4ax.com...

On Fri, 27 Jun 2003 19:17:17 GMT, "BM"
brandon(underscore)melland@hotmail.com> wrote:

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

High speed signal reflection is reduced by not using right angles.
This becomes particularly true above 180MHz and is profoundly reduced
in microwave, however at those speeds you're better off going with the
old fashioned ECL approach to layout....curved traces.

 

[Chuck Simmons]

BM wrote:

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
--
... The times have been,
That, when the brains were out,
the man would die. ... Macbeth
Chuck Simmons chrlsim@webaccess.net

 

[John Larkin]

On Fri, 27 Jun 2003 22:51:04 GMT, "C what I mean" <pythan@pacbell.net>
wrote:

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

 

[Tom Grqyson]

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

 

[Ben Bradley]

In sci.electronics.design, "BM"
<brandon(underscore)melland@hotmail.com> wrote:

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.

Thanks

-BM

 

[William J. Beaty]

"BM" <brandon(underscore)melland@hotmail.com> wrote in message news:<1L0La.1667$7e.1222@nwrddc04.gnilink.net>...

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/
beaty@chem.washington.edu Research Engineer
billb@eskimo.com UW Chem Dept, Bagley Hall RM74
206-543-6195 Box 351700, Seattle, WA 98195-1700

 

[EEng]

On Fri, 27 Jun 2003 17:42:49 -0700, John Larkin
<jjlarkin@highSNIPlandTHIStechPLEASEnology.com> wrote:

On Fri, 27 Jun 2003 22:51:04 GMT, "C what I mean" <pythan@pacbell.net
wrote:

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
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.

 

[Robert Baer]

BM wrote:

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.

 

[John Larkin]

On Fri, 27 Jun 2003 23:43:41 -0700, EEng <unmaileeng@budget.net>
wrote:

On Fri, 27 Jun 2003 17:42:49 -0700, John Larkin
jjlarkin@highSNIPlandTHIStechPLEASEnology.com> wrote:

On Fri, 27 Jun 2003 22:51:04 GMT, "C what I mean" <pythan@pacbell.net
wrote:

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
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

 

[onestone]

EEng wrote:

On Fri, 27 Jun 2003 17:42:49 -0700, John Larkin
jjlarkin@highSNIPlandTHIStechPLEASEnology.com> wrote:

On Fri, 27 Jun 2003 22:51:04 GMT, "C what I mean" <pythan@pacbell.net
wrote:

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
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

 

[DarkMatter]

On Sat, 28 Jun 2003 07:38:33 GMT, Robert Baer
<robertbaer@earthlink.net> Gave us:

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.

 

[onestone]

"R. Steve Walz" wrote:

BM wrote:

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
------------
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

 

[DarkMatter]

On Sat, 28 Jun 2003 17:28:59 GMT, onestone <onestone@bigpond.net.au>
Gave us:

"R. Steve Walz" wrote:

BM wrote:

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
------------
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.

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

 

[Jim Thompson]

On Sat, 28 Jun 2003 17:28:59 GMT, onestone <onestone@bigpond.net.au>
wrote:

"R. Steve Walz" wrote:

BM wrote:

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
------------
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

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
--
| James E.Thompson, P.E. | mens |
| Analog Innovations, Inc. | et |
| Analog/Mixed-Signal ASIC's and Discrete Systems | manus |
| Phoenix, Arizona Voice480)460-2350 | |
| Jim-T@analog_innovations.com Fax480)460-2142 | Brass Rat |
| http://www.analog-innovations.com | 1962 |

For proper E-mail replies SWAP "-" and "_"

Get Lolita Out of Debt... Add Three Inches to Your Mortgage!

 

[markp]

"Jim Thompson" <Jim-T@analog_innovations.com> wrote in message
news:j6rrfvcc01pfb6goslqtjrsjpder58clr0@4ax.com...

On Sat, 28 Jun 2003 17:28:59 GMT, onestone <onestone@bigpond.net.au
wrote:

"R. Steve Walz" wrote:

BM wrote:

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
------------
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

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

Indeed, that is to be expected. The electrons are charged, so they repel
their neighbours. They can only change direction or move if there is an
inbalence in forces, so they will tend to bunch up at the corner and push
adjacent electrons around it. There is therefore an increased density of
electrons at the corner, and a high electric field as a result.
Notwithstanding this the direction is being changed as they turn 90 degrees
which is an acceleration, and accelerating electrons radiate. Anyway, that's
how I look at it!

Mark.

 

[Blake Leverett]

John Larkin wrote:

The two best PCB layout people I've known were both women. And they
were very concerned about how the boards looked.

I have done layout on a lot of boards. To me, looks really do count, both
on placement and routing. No self-respecting layout person would create an
ugly board. They don't call it "artwork" for nothing. Also, having
unnecessary vias is just plain wrong. Even though it really doesn't matter
most times, I spend times to make the board look like it was purposefully
designed. If it looks "pooped out" it probably was.

I remember once the boss was going to lay out a board himself. It was all
in 90deg traces. Ugly as hell, and didn't work - not because of traces,
but because of other errors.

Blake