Suggestions follow each related paragraph of the original message:

At 03:02 PM 5/19/02 -0700, you wrote:
>I'm working on laying out my first board with power
>planes and I have a few questions.
>
>1. I placed an arc on the plane (my board is circular)
>to form a circle all the way around the edge of the
>board.  The idea is to keep the plane away from the
>edge of the board.  The assigned net for the arc is
>"No Net".  Is this the correct procedure for keeping
>the plane away from the edge of the board?

It is one way - and I have used it myself.  Since the arc is a void, the 
"No Net" designation has no meaning.  Remember that planes are shown 
negative.  Any lines you place on the plane are void so they have no net 
connection.  More related to this at the last paragraph following.

>2. The arc is 50 mils wide.  Since I placed the arc
>directly on top of the board outline, I expect to get
>25 mils of clearance from the board edge to the plane.
>  In general, is that enough clearance?

I generally leave at least 50 mils to the copper from the board 
edge.  There is no magic rule or reason - it just works well.  I've been 
doing it that way for over 40 years and it hasn't gotten me into 
trouble.  You can leave more or less, as long as you remember that signal 
traces on other layers need a good overlap (about 2-3 trace widths worth) 
for the signal return path on the nearest plane - power or ground.

>3. I have split the plane into multiple nets.  The
>tracks that indicate the boundaries are 45 degree and
>90 degree tracks.  Recall I have an arc on my board
>edge.  Because the 45/90 tracks and the arc are not
>"compatible", the tracks extend outside of the arc to
>avoid tiny slivers of plane near the board edge.  Is
>there a better way to do this?  For example, can I
>define the regions with mostly 45/90 tracks but add an
>arc at the board edge to complete the region?  Will
>the way I have done this likely confuse the board
>house?

Your way will not confuse the board house.  In the old days before the 
wonderful GUI EDA packages, we laid out plane segments with radials that 
extended beyond the edge of the board.  The fab is going to physically cut 
that area off, so anything outside the board perimeter you tell them you 
want will be discarded during fab.

  As for another, perhaps better, way - Protel gives you the ability to 
place split planes, and to define to what net the copper in the split area 
belongs.  Go to the "Design" menu in PCB and look for "Split Planes".  The 
menu item will allow you to add a split area with the width of boundary 
void you choose.

If you use something on the order of 20-30 mils for the split plane 
boundary, you can follow inside the 50 mil outline arc with line segments 
defining the outer edge ot the split plane.  It looks tidy, and it 
works.  The way the split plane boundary segments are laid down works just 
like laying a track - you can choose right angle, 45 degree, arc, or free 
form with a combination of space bar and shift key while laying down the 
boundary line.


* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* 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