At 01:45 PM 6/15/01 -0700, Jim McGrath wrote:
>By Manipulating the plane clearences by say a mil I get a separate Dcode
>for the desired pads and can modify the gerbers to thermals where
>required.
That's an interesting workaround. I'd think of using component classes to
determine the connection type and then I'd place blowout pads to disconnect
the appropriate pads according to layer. These blowout pads could be part
of the footprints for this customer. I'd probably make them 12 mils radial
oversize beyond the hole size. (Pads can be placed on the inner plane layers.)
>I have been meeting these requirements for many years and their boards
>always work so who am I to question their reasons.
Mr. McGrath is a professional printed cirucit board designer. This means
that he needs to know why the client wants something, if the client is
willing to disclose the information.
And if it turns out that what they want is foolish, in his opinion, it is
his obligation as a professional -- in my view -- to disclose to them what
he knows about the matter.
Notice that the first approach is couched in terms of expanding his
professional knowledge; the engineer should take this as a compliment.
Which indeed it might be.
Then, as a professional, I would share the knowledge [or claims] with other
professionals, some of whom may know a great deal about what they want and
why it is a good idea, or why it is not.
If it is a good idea, then, of course, it is another opportunity to thank
the engineer. Most people like being thanked.
And if it is bad idea, what one has learned (or already knew) might be
gently conveyed to the engineer.
There are a *lot* of black magic practices that are nothing more than
voodoo that seemed like a good idea at the time the practice was initiated.
That the board work might mean that all this effort is *harmless*. But it
is expensive to add two layers.
If I know what they are doing, however, it would be this: they are using
the inner power/ground pair for power distribution; these layers are close
to each other to gain the substantial benefits of the distributed plane
capacitance.
Then the outer pair of grounds is placed in the stack such that it provides
ground return and impedance control for signals on outer signal layers.
This is confirmed by the usage of ground return vias that will communicate
return currents with minimal disturbing inductance from one of the outer
ground layers to the other.
Now, what is wrong with this picture? I'm interested in the comments of
others, but here is my first pass:
Keeping the planes isolated, such that the return via, for example, only
connects to the outer planes, is *probably* useless, or maybe worse than
useless, but not a lot worse. The return currents are going to follow the
path of least impedance, which will, if the copper exists, be in the ground
plane paired with the signal layer involved. If the single jumps such that
another plane becomes the reference plane, the current will flow through
the nearest via. In my practice, if such a via exists within an inch or so,
I'd add no special via, but the higher the edge rate involved, the closer
I'd want it to be.
If I were working for the client here, I'd suggest that they have a board
fabbed both ways, one as described and the other without manipulation: the
vias connect to all layers, as do the bypass caps and other parts. One
experiment is worth a thousand engineers theorizing until their heads hurt.
[EMAIL PROTECTED]
Abdulrahman Lomax
P.O. Box 690
El Verano, CA 95433
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
*
* To leave this list visit:
* http://www.techservinc.com/protelusers/subscrib.html
* - or email -
* mailto:[EMAIL PROTECTED]?body=leave%20proteledaforum
*
* Contact the list manager:
* mailto:[EMAIL PROTECTED]
*
* Browse or Search previous postings:
* http://www.mail-archive.com/[email protected]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
