Searching \ for '[OT] PCB layout questions' in subject line. ()
Make payments with PayPal - it's fast, free and secure! Help us get a faster server
FAQ page: techref.massmind.org/techref/pcbs.htm?key=pcb
Search entire site for: 'PCB layout questions'.

Exact match. Not showing close matches.
PICList Thread
'[OT] PCB layout questions'
1999\02\27@232631 by Rob Santello

flavicon
face
I marked this as off-topic (just to be safe) even though this is for a
16F84 PIC project and since you guys know everything ;-)  I just have to
ask...  I am trying to do PCB layout of a small 2 layer, through-hole,
3"x4" board.  I've followed the previous discussions about the crystal/caps
related to the PIC as well as the suggestion concerning a separate ground
"protect" loop around those components.   But several other questions arise
as I try to do this.  I've seen examples of all of my questions in use so
I'm not sure which (if any) way is best.  I know the answers are very
dependant on the circumstances, but just general suggestions (if possible)
would be useful.

1) Is it good to put both power and ground on the same layer, or better to
put ground on the bottom layer and power on top?

1A) If on different layers, is it best to place them directly over each
other for effectively added capacitance or keep them apart.

1B) If on the same layer, run close together (for capacitance reasons) or
keep apart?

2) Is it good to surround the entire bottom layer with a ground trace
(creating a loop of sorts) or is it better to not complete the circle?

3) Is it a good idea to fill in all blank areas (especially on the
bottom/ground side) with a ground fill? If so, is it best to be solid or a
hatch pattern of some sort?

4) For general signal runs, is it better to keep traces short by using VIAs
or complete the routing with longer traces when possible?

5) Again for general signal runs, is wider better,  I'm using .020" for
most runs but if I can fit a wider trace, should I use it?

Thanks!
--rob--

1999\02\28@031914 by Vincent Deno

flavicon
face
Without addressing each of your questions here, I would start by referring
you to:

http://www-s.ti.com/sc/psheets/sdya011/sdya011.pdf

Most other semiconductor manufacturers have similar datasheets on board
layout stratigies.

Hope this is of help.

-Vincent Deno

{Quote hidden}

--------------
Vincent Deno
Design Engineer
Theta Digital Corp.
http://www.thetadigital.com
spam_OUTdenovjTakeThisOuTspamemail.uc.edu
_____________
| ____   ____ |
|/| | | | | |\|
| | |/| |\| | |
| | | | | | | |
| |_/ | | \_| |
| |   | |   | |
|_/  /___\  \_|


'[OT] PCB layout questions'
1999\03\01@103420 by Lawrence Lile
flavicon
face
-----Original Message-----
From: Rob Santello <.....rmsanteKILLspamspam@spam@NS.NET>




>
>3) Is it a good idea to fill in all blank areas (especially on the
>bottom/ground side) with a ground fill? If so, is it best to be solid or a
>hatch pattern of some sort?


I don't do this a lot, but it is good practice esp. as frequencies increase.
I have seen a lot of boards with a hatch pattern, presumably to keep large
copper areas from delaminating due to differential expansion.


>5) Again for general signal runs, is wider better,  I'm using .020" for
>most runs but if I can fit a wider trace, should I use it?


0.020" is about the SKINNIEST trace I use, but I am designing my circuits to
be built by a fairly low tech assembly house.  I use .060" if I can get away
with it for any power and ground trace.  I have to run a lot of high current
traces (10-12 amps) so I'm used to seeing 0.120" to 0.250" traces once in a
while.  Most other people would consider such a trace to be a ground plane,
not a trace.

Depending on who will build your board,  0.020" might be a fat trace or a
skinny trace.  If you are building it yourself save yourself some trouble
and don't go much smaller unless you really have to.

1999\03\01@104114 by Harrison Cooper

flavicon
face
I have several .pdf files that answer quite a few questions dealing with pcb
layouts (can't recall the site where I got them from, so thats why I saved
them).  Considering bandwidth issues that some have...I won't post on here.
If interested in them...send me a private message with subject of "PCB pdf
files".  I will filter these out and respond toward the end of the week.
Anything else in the subject...like RE:PCB pdf files, etc.....won't get
them.  I don't have time to read thru.  I just delete without reading unless
the subject matter is of interest.

My experiance with PCB boards range from simple single sided, double sided,
to 12 layer boards.  Everything from analog to 100Mhz SDRAM stuff.

1999\03\01@110432 by Harrison Cooper

flavicon
face
I marked this as off-topic (just to be safe) even though this is for a
16F84 PIC project and since you guys know everything ;-)  I just have to
ask...  I am trying to do PCB layout of a small 2 layer, through-hole,
3"x4" board.  I've followed the previous discussions about the crystal/caps
related to the PIC as well as the suggestion concerning a separate ground
"protect" loop around those components.   But several other questions arise
as I try to do this.  I've seen examples of all of my questions in use so
I'm not sure which (if any) way is best.  I know the answers are very
dependant on the circumstances, but just general suggestions (if possible)
would be useful.


OK...I am responding, and this is based on MY experience...and by no means
am I an expert...


First off...it depends on how much you want to spend. A single sided board
is typically cheaper than two sides,
and often charge per hole.  More holes ya got...more $$$.  Double sided
would also require plated thru holes.
If you are trying to do a proto on the cheap, you can sometimes get them to
just drill and etch, and you solder the feedthrus.  Can sometimes get with
no tin plating as well.  I have a place that used to do that for me, but
found it was just as cheap and easy to get it done the right way...solder
mask and silk screen.  Typically didn't add that much cost to it.  Most the
time, for a small run, the cost is in the tooling or setups.

Now to answer:

1) Is it good to put both power and ground on the same layer, or better to
put ground on the bottom layer and power on top?

Double sided card....I will usually put power and ground on the bottom side,
and signals on top, easier to debug and troubleshoot.  If you are doing
rework and sending to a customer, do the rework on the lower side...makes it
look nicer at least.  Multi layer cards stackup typically have the inner
layers for power and ground dedicated.

1A) If on different layers, is it best to place them directly over each
other for effectively added capacitance or keep them apart.

Stackup will also affect impedance of the traces.  Signals want to find a
path back to ground.  Critical signals should be placed near a return
path...be it a ground plane on the next layer, or a guard band, or both.

1B) If on the same layer, run close together (for capacitance reasons) or
keep apart?

run what close together...power, ground, signals?  Depends on the frequency
of the signals as well.
Power...should be static. There should be no noise on either plane.  So
really doesn't matter so much on where these lay next to...other
than...signals NEED a low impedance path back to ground.

2) Is it good to surround the entire bottom layer with a ground trace
(creating a loop of sorts) or is it better to not complete the circle?

Again, it depends on the frequency of clocks, etc.  I've never done this,
other than guardbands on some clocks


3) Is it a good idea to fill in all blank areas (especially on the
bottom/ground side) with a ground fill? If so, is it best to be solid or a
hatch pattern of some sort?

not really....large areas of no etch doesn't hurt, but typically done a
cross hatch in these.  Some devices indicate a power plane under them, some
a ground plane (typically these are PLL types...)


4) For general signal runs, is it better to keep traces short by using VIAs
or complete the routing with longer traces when possible?

depends on the signals....speed....what its driving (capacative loads, etc).
One of the documents I have did a study on this...does via's really affect
the quality of the signals?  Basically said no...they don't.  But many clock
drivers always play it safe by stating to keep the number of via's to a min.


5) Again for general signal runs, is wider better,  I'm using .020" for
most runs but if I can fit a wider trace, should I use it?

trace width affects impedance, and depending on the stackup (if multilayer)
can affect ringing on the signals.
Double or single sided cards...probably does not affect it that much.  Other
than power traces. Don't skimp on these. AND...if you are passing power from
one layer to another...don't use just one via.  Use as many as you can fit
in the area.  Remember...you are passing current thru a small hole, so don't
try to squeeze 10 amps thru a .005 hole...
Just be sure that you have enough copper on the trace to pass the amount of
current.  There are online calculators for this.  Also...on small
widths...sometimes small run proto houses have hard time not overetching.
For lower frequency designs, I opt to make them wider rather than narrow,
just for that reason.  Nothing worse than having to run wires because the
trace was etched out.


One last comment.  Many vendors offer app notes about grounding and such.
Don't skimp on bypass caps. And follow the notes as far as values and
placements.  If a chip has several ground pins, most indicate NOT to tie
them together but bring each one out and tie to a common plane or point.
For most low frequency circuits, allot of this is not that critical.  If you
have ringing on a signal to an clocked input, but the ringing will settle
long before the clock, then its not allot to worry about.  If you are
running a 10ns clock.....whole different story.

1999\03\01@154053 by Reginald Neale

flavicon
face
Lawrence said:

>
>Depending on who will build your board,  0.020" might be a fat trace or a
>skinny trace.  If you are building it yourself save yourself some trouble
>and don't go much smaller unless you really have to.

 I'd go even further. For low-tech DIY stuff, make everything as big as
 possible. A very common beginner's mistake is to make the pads too small.
 Especially when your layout program allows you to zoom in, it's easy
 to lose perspective. Single-sided boards are particulary vulnerable,
 Without a through-hole to anchor the pad, little ones will peel right
 off the board when you go to solder your component in place.

 Reg Neale

More... (looser matching)
- Last day of these posts
- In 1999 , 2000 only
- Today
- New search...