Thermal reliefs in plane connections

J

Joerg

Guest
While checking a layout for a client I saw this for the umpteenth time:
Trace connections to a plane via thermal relief, not in a solder area
where it would thermally matter.

Question: Was it taught once upon a time that thermals must be used
everywhere? Or is there some other reason why it's done so often?

--
Regards, Joerg

http://www.analogconsultants.com/
 
Joerg,
I would have to believe that it is the old problem of a little knowledge
being misapplied by the uninitiated. A general comment on a rule or practice
then being taken to further extremes and actually misapplied. Sometimes it
may be software initiated, some packages actually have default rules that
start out your design with thermals on 'all' plane connections. i.e. Protel
P99SE (quite possibly the current AD software also), the default plane
connection style rule on a new PCB is for "Board" (everything, vias and
pads) to be thermally relieved. So the less knowledgable and experienced get
introduced to the silly practice by their acceptance of software package
defaults.

Certainly seems silly doesn't it? Then there is the problem of all the
discontinuities caused in the planes by these unnecessary thermal reliefs.
It is fairly common to see required thermal reliefs that are actually
starved connections because of all the unecessary reliefs impeding a good
connections to those required points.

--
Sincerely,
Brad Velander.

"Joerg" <notthisjoergsch@removethispacbell.net> wrote in message
news:n_xlj.1883$EZ3.344@nlpi070.nbdc.sbc.com...
While checking a layout for a client I saw this for the umpteenth time:
Trace connections to a plane via thermal relief, not in a solder area
where it would thermally matter.

Question: Was it taught once upon a time that thermals must be used
everywhere? Or is there some other reason why it's done so often?

--
Regards, Joerg

http://www.analogconsultants.com/
Click to expand...
 
Joerg wrote:
While checking a layout for a client I saw this for the umpteenth time:
Trace connections to a plane via thermal relief, not in a solder area
where it would thermally matter.

Question: Was it taught once upon a time that thermals must be used
everywhere? Or is there some other reason why it's done so often?
Click to expand...
It is easier to have a consistent style of trace to plane (or to
polygon) connection throughout the board. For many types of board,
thermal reliefs are just as good as direct connections - they are only a
problem if the relief wires are very thin, or if you are working at very
high frequency, high currents, or with high accuracy analogue signals.
Personally, I use thermals everywhere if I am doing a simple card, and
direct connections everywhere if it is higher speed or has smaller
geometries.

mvh.,

David
 
Joerg <notthisjoergsch@removethispacbell.net> writes:
Question: Was it taught once upon a time that thermals must be used
everywhere? Or is there some other reason why it's done so often?
Click to expand...
Makes it easier to wire in a fix later.
 
On Tue, 22 Jan 2008 18:52:56 -0800, Joerg
<notthisjoergsch@removethispacbell.net> wrote:

While checking a layout for a client I saw this for the umpteenth time:
Trace connections to a plane via thermal relief, not in a solder area
where it would thermally matter.

Question: Was it taught once upon a time that thermals must be used
everywhere? Or is there some other reason why it's done so often?
Click to expand...
I would guess that the layout person is inexperienced. In Orcad
Layout, you need to specifically check off a box to get rid of thermal
connections for a particular pad stack.

---
Mark
 
Brad Velander wrote:
Joerg,
I would have to believe that it is the old problem of a little knowledge
being misapplied by the uninitiated. A general comment on a rule or practice
then being taken to further extremes and actually misapplied. Sometimes it
may be software initiated, some packages actually have default rules that
start out your design with thermals on 'all' plane connections. i.e. Protel
P99SE (quite possibly the current AD software also), the default plane
connection style rule on a new PCB is for "Board" (everything, vias and
pads) to be thermally relieved. So the less knowledgable and experienced get
introduced to the silly practice by their acceptance of software package
defaults.

Certainly seems silly doesn't it? Then there is the problem of all the
discontinuities caused in the planes by these unnecessary thermal reliefs.
It is fairly common to see required thermal reliefs that are actually
starved connections because of all the unecessary reliefs impeding a good
connections to those required points.
Click to expand...
Yes, I've had one case where a supply plane split open into four parts
because the fab house took the liberty to "improve" the clearances. They
ended up doing another free blitz run for us.

--
Regards, Joerg

http://www.analogconsultants.com/
 
DJ Delorie wrote:
Joerg <notthisjoergsch@removethispacbell.net> writes:
Question: Was it taught once upon a time that thermals must be used
everywhere? Or is there some other reason why it's done so often?

Makes it easier to wire in a fix later.
Click to expand...

Not really anymore. Most boards have this all covered and vias are so
small anyway. Plus, don't we all design perfectly so no rework is ever
needed ... ?

--
Regards, Joerg

http://www.analogconsultants.com/
 
My CAD software automatically has an underlap from the power plane to
the pads.
SO the only connection to the pwoerplane is via a normal track.
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top