Paul Cooper - Myrica wrote:

>       Am trying to layout my 1st board since college and have a few
> general
>       PCB layout questions. Board will be about 2x3", and max Frequency
> is
>       about 100Mhz, althoug most much slower.
>
>       This is a test board, which will be made in the 10's, not a
> production
>       board (which is why a chip designer is doing it)
>
>       1) Is there a standard or rule of thub that can be applied to the
>       seperation for a split plane ?

Your board fabricator usually has a spec for this.  I generally use
a 20 mil track around each split plane region (this becomes a 20-mil
gap in the actual copper), and with 2 of them next to each other,
it causes about a 40-mil gap between the two voltage areas.

>       2) For plated pads and vias, is hole size in layout before or
> after
>       plating. ie if i set hole size to be 50mil, will it compensate for
>
>       fact hole will be plated and compensate drill size so hole is
> 50mil
>       after plating?

Again, your board house has specs for how much oversize they drill
the holes, so the plating brings them back to your desired dimension.
Some outfits will drill the hole as you specify, and plating will reduce it

3 or more mils.  So, you need to work out with your fabricator what
you intend your hole size spec to mean.

>       3) Is there a standard or rule of thumb for dimensions of pad in
>       relation to hole size ? From most of the library components I
> looked
>       at, it seems hole is about 2/3 pad size.

In the most general sense, the accuracy of drill position and layer
stackup in the laminating process set a minimum "annular ring"
that you need to maintain to prevent the drill from going through the
edge of the pad.  This varies with process, number of layers, and total
panel size (as well as the quality of their equipment and procedures).
They should tell you what annular ring they need (both for outer and
inner layers) to make your board manufacturable.

>       4) Is there a standard via size/sizes ?
>
>       5) For a given size diameter component lead is there a guidline
> for
>       hole size ?

Umm, I usually want about .003" plus the worst case variation in hole
size.  Advanced Circuits has really large hole size tolerances of +/- .005"

so I try to spec the hole at .013" over the lead size so I won't have to
ram the leads in with pliers.  Some outfits have much tighter controls.

>       6) for a component with square pins, .025mil (+- .005) mil on a
> side,
>       I was going to use pads of diameter 80, hole 52. This sound
>       reasonable.

I usually use .038" for these.  If you use 80 mil pads for things that are
on
.1" centers, that doesn't leave much room between pads.  I use .060"
pads with .038" holes and it comes out fine.

>
>       7) For a thick track, say 30mil to 50mil, is it normal to use
> multple
>       small vias ?

If you really need the lowest possible impedance or DC resistance,
then thisa schem can be used.  Remember that the conductive cross
section of a via goes way down as the diameter goes down.  Very
roughly, it approximates the circumference of the hole.

Jon

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
*
* Browse or Search previous postings:
* http://www.mail-archive.com/proteledaforum@techservinc.com
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to